ESR Meter Adapter Design and Construction

[Jay_Diddy_B]

Hi,
I am going to share the design and construction of an ESR Meter adapter design and construction. The plan is to end up with a design that is similar in appearance to Dave's ucurrent that will allow a DMM to be used as an ESR meter. At this point in time I have not built the circuit.

The requirements are:

• To have a simple design that can be constructed on a single-sided circuit board.
• Operates at 100kHz.
• Be a true ESR meter as oppose to an impedance meter.
• Work in either the 2-Wire or 4-Wire mode.
• Be well protected from charged capacitors and applied voltages.

I will be using LTspice to verify the design goals.

Simulation Basic Functionality



This the LTspice model configured for normal operation. U3 is configured as a 100 kHz square wave oscillator. 1/3 of a CD74HC4053 analog Mux / Demux  is used to provide a current to the capacitor under test through R3, R9 and C5. The voltage across the capacitor under test is sensed via R5 and C5. Another 1/3 of the CD74HC4053 is used as a synchronous detector. U4 provide gain, resulting in a scale of 1V=10 Ohms.
R16 and R17 are included in the model to explore the effect of lead resistance.

If I plot Vout versus ESR, I get:



Simulation of a Charged Capacitor

I wanted to make sure that the adapter is not damaged if it is connected to a charged capacitor. To demonstrate this a switch is used to connect the adapter to a charged capacitor, the charged capacitor is connected at t=2ms:



Results



After a very brief transient the meter actual reads the correct value of ESR.



There is a brief impulse of current in R9. A special 'pulse withstanding' resistor will be selected for the R9 location.


Application of Line Voltage

Although not recommended, it would be nice to know that the adapter will survive being connected across the line. In this test 240V ac at 60 Hz is applied to the input.



Results of applying line voltage


The upper trace shows the dissipation in R5. (930uW average power)
The middle trace shows the dissipation in R9. (18.6mW average power)
The lower trace is the line voltage across the terminals of the adapter.


Real Schematic



This is the real schematic. It is very similar to the simulation schematic. The 74HC4053 has been broken up into four parts to make the schematic easier to read.

J1 and J2 are used for 2-wire measurements. J1-J4 are used for 4-wire measurements. J5 and J6 are the voltage output to the DMM.

Board Layout

Here is a picture of the board layout:



I need to add a switch for the power.

I will add more details after I have built the prototype. The LTspice models are attached if you want to play with the circuit.

Parts are on order.... to be continued....

Jay_Diddy_B

[Harvs]

Nice, looks like it should be easy to build as well. 

Hope to see some pictures of the prototype.  Assuming it all works well, any chance of getting either a gerber of the artwork or scale PDF?  Looks like a nice project to etch and assemble, but it doesn't look like I use the same CAD package as you.

[dannyf]

Nice work. Keep it up.

[ElectroIrradiator]

Nice design. Have you considered that the 4053 is quite slow to switch on or off? At +5V supply voltage the switching time is about 0.5uS, which might cause non-linear indication at 100 KHz sampling frequency / 5 uS half period.

[Jay_Diddy_B]

Have you considered that the 4053 is quite slow to switch on or off? At +5V supply voltage the switching time is about 0.5uS, which might cause non-linear indication at 100 KHz sampling frequency / 5 uS half period.

Thank you for your input, this is the kind of feedback that I was hoping to get by posting my design.

I have considered the delay from the select pin, to the switch opening and closing.

The 74HC4053 is about an order of magnitude faster than the CD4053 with maximum switching times of around 50ns (I checked TI and NXP).

The 74HC4053 in the source will compensate for the delays in the sense circuitry.

I will be building the circuit soon.

I am looking for a suitable enclosure. There are some advantages to keeping the board dimensions less than 100mm x 50mm, so that the board can be made cheaply at places like itead. The other requirement is that the box is deep enough to hold a 9V battery.

I have found the UB5 Jiffy Box from altronics

http://www.altronics.com.au/download/Datasheets/H0151.pdf

This the same box that was used by Dave in the uCurrent. It was also suggested by Harvs in a PM. This box seems to be Australian design and manufacture.

Does anybody know of a box like this with worldwide availability?

Jay_Diddy_B

[BravoV]

Finally, a DIY ESR measuring circuit which is hobbyist's grade friendly and capable of 100KHz, also looks like its accurate enough at ESR < 100 miliOhm, cmiiw. 

Thank you ! 

The requirements are:

• To have a simple design that can be constructed on a single-sided circuit board.
• Operates at 100kHz.
• Be a true ESR meter as oppose to an impedance meter.
• Work in either the 2-Wire or 4-Wire mode.
• Be well protected from charged capacitors and applied voltages.

I think you also forget another feature point which in circuit testing since the test voltage is so low. I would say specifying that its capable of test voltage at < 100 miliVolt is not too overly ambitious.

To others, the various test voltages span across the above sweep, maxed out at 40 miliVolt P-P, again, CMIIW. 

Although not recommended, it would be nice to know that the adapter will survive being connected across the line. In this test 240V ac at 60 Hz is applied to the input.

This too in the features list, but I guess you should word it more carefully. 

J1 and J2 are used for 2-wire measurements. J1-J4 are used for 4-wire measurements. J5 and J6 are the voltage output to the DMM.

If I'm going to use or build two coaxial cables for 4-wires measurements, how are the connections setup for the coax outer shield and it's core for both cables ?

Parts are on order.... to be continued....

Damn, this reminds me of your cool LPKF ProtoMat machine there, an instant PCB in just a few minutes, feeling so jealous. 

[matkar]

Very nice design! I have tried to add another opamp on the output to scale up the output by a factor of 10. The idea is to magnify the reading in the region I mostly use (measuring faulty low ESR caps). One benefit is also no 10x multiplication of the reading is needed. Unfortunately I'm unable to get good results...
@Jay_Diddy_B
Anyway it might be a nice addition to your device to add a range switch to switch between 1:1 and 1:10 scale.

[Jay_Diddy_B]

Hi,
The construction has started.

Printed Circuit Board

I have milled a prototype board on my LPKF Protomat c60:



Outside View

Here is a picture of the outside of the box. The 4mm jacks are Keystone Electronics 575-4.



Let the soldering begin.

To be continued ....

Jay_Diddy_B

[Jay_Diddy_B]

Hi,

I can now report that the ESR meter works.

Here is a picture of the assembled board:




I connected all 4 wires together to make a short and the adapter reads 7.3mV which is equivalent to 73m Ohms.



I can use the relative button on the DMM to zero the reading



I am now measuring a 470uF 16V capacitor. The adapter reads 132m Ohms. My HP 4274A LCR meter gives me a value of 125 m Ohms 5.6% difference.




I am now measuring a 47uF capacitor. The adapter reads 1.185 Ohms. My HP 4274A LCR meter gives me a value of 1.15 Ohms 3% error.



I have noticed that the frequency is around 77 kHz. This can be corrected by changing R3 to 4.7K, otherwise the circuit is the same as the LTspice model.


It is looking good.

Jay_Diddy_B

[w2aew]

Ooooooh, LPKF, nice! 

Congrats on the working proto, looks real nice!

[Spikee]

Could you post the Gerber files ?
I want to etch and test this circuit @ college.

[Fraser]

Impressive .... a working and pretty accurate prototype at the ALPHA stage. Excellent work.

[Jay_Diddy_B]

Hi group,

Spikee asked:

Could you post the Gerber files ?
I want to etch and test this circuit @ college.

Well here are the files. There are two set of Gerber files, one for the Hammond box that was used in the prototype, the other is for the UB5 Jiffy box. The layouts are the same. I changed the outline and the mounting holes.

Consider this experimental.

Jay_Diddy_B

[BravoV]

JDB, on zeroing the offset, does it help if using an opamp that has the offset adjutment using external potentiometer ?

About the opamp, I can see you are using different one at the proto than the one in the schematic, what is the minimum specifications if using different opamp ? I guess this particular question will come sooner or later. 

[Jay_Diddy_B]

Hi,
The op-amp used on the prototype is the same as the one used in the LTspice models. I used the LTC6241. The op-amp on the 'real' schematic was a place keeper. It has the same pin out.

The LTC6241 op-amp has the right combination of GBW, Slew rate and Vos.

http://www.linear.com/product/LTC6241

The Vos for this op-amp is 125uV max, 40uV typical.

The Vos is multiplied by the high gain of the DC amplifier stage x55.

So we can up to 6mV from the Vos, typically 2mV.

There are lots of other sources for the non-zero reading.

The reading of 7mV is 0.35% of full scale.

I considered adding a zero pot. There were three considerations:

• I needed a dual op-amp. Dual op-amps don't normally have offset pots. It would be tricky to design a stable offset adjustment circuit.
  
  
• When used in the 2W mode for troubleshooting, It is necessary to zero the leads, which might be 0.2 Ohms or more. This would need a wide range on the zero pot.
  
  
• Most of the better DMM have a Relative button. So I decided to take advantage of this feature and keep my circuit as simple as possible.
  
  

These were choices that I made during the design process. You can experiment with modifications. One modification would be to take the output and the meter 0V and measure these with an Arduino. This would make a nice self-contained unit. This would take care of the x10 scaling and deal with the zero adjustment.

Jay_Diddy_B

[quarks]

Looks very good, thanks for sharing

[Spikee]

Does anybody know if it is possible to get that UB5 box in europe ?
I have looked on the Altronics website but they don't list any dealers outside AUS.

I have also a uCurrent pcb laying around that needs a nice box =/

[dannyf]

Quick thoughts:

1) the switches on the front end (oscillator's output) aren't needed.
2) the unused switch can be utilized to introduce an automated zeroing function potentially.
3) you can build a stand-alone version with a mcu (that has a PGA): the mcu will generate pulse output, and the rectified output is then amplified by the mcu and digitalized via its onboard adc to drive a lcd, or to control a pwm pin to drive an analog meter. The autozeroing function can be implemented here.

The basic architecture of the meter is good and flexible.

[Jay_Diddy_B]

Hi,
The switches on the output of the oscillator perform three functions:

1) they have the same thresholds as the switches in the synchronous detector and the same propagation delays from the select input to the switches opening and closing.

2) The switches also increase the slew rate of the source. The op-amp has a minimum slew rate of 5V/us and a typical slew rate of 10V/us.

3) The switches also ensure rail to rail performance of the source.

I would be interested to see how the unused switch can be used to generate an auto zero function. Can you post a schematic?

Jay_Diddy_B

[dannyf]

Sure. Cut open the wire between the dut and the resistor to its right. Insert a switch there. When zeroing is off, the switch reconnects the resistor to the dut (as it is now); When on, the switch connects the resistor to the virtual ground.

So when zeroing is on, the output on the opamp would be outputing a drift that needs to be netted out. When a mcu is utilized, it would periodically turn on zeroing, and measure the output of the opamp.

When the zeroing is off, the mcu can measure the opamp's output and then subtract from it the drift -> you have zero'd out the drift.

[dannyf]

This approach doesn't zero out the drift from the front-end (especially if you use an opamp as an oscillator or have asymmetrical up/down slopes).

A "better" approach is to use a low Rds mosfet as a switch to short out the dut periodically and measure the overall drift, in a similar fashion. It has the disadvantage of requiring a DC voltage / constant current source across the dut.

[BravoV]

The Vos is multiplied by the high gain of the DC amplifier stage x55.

Ok, noted.

How about others specs, like minimum GBW ? Slew rate ? Noise ? Other else ? Will a cheap jelly bean fet amp like LF411 is "good enough/decent" as replacement ?

I have a limitation here, its not like I don't want to use those Linear op-amp as your recommendation, actually I can afford to purchase op-amp like LTC6241 say like $2 to even $5 a piece which is no big deal, but its just my location that most distributors and also like a direct purchase through Linear Tech, these guys will hammer me like $70 to $90  just for the shipping cost alone, which is not funny at all. 

So please understand me, finding for an alternative op-amp is the only way, and don't worry, even though I'm a electronics noob, but not that noob enough that I will blindly ask if I could use a 741 or LM324 as the replacement for this circuit.   

I wish I'm not alone here.

There are lots of other sources for the non-zero reading.

Such as ? Asking this cause I may ended up with low accuracy discrete components, just the critical parts that will affect the performance or accuracy, the plan is to use through hole parts.

Also about the gain, will a single voltage divider at the op-amp output will some how "temporarily" fix the gain error if I happened to use less accurate component ? I know, the best part is still use the exact components as your circuit, please bear with me here. 

When used in the 2W mode for troubleshooting, It is necessary to zero the leads, which might be 0.2 Ohms or more. This would need a wide range on the zero pot.

Say I will use only 4W mode, the op-amp zeroing pot still feasible ?

[BravoV]

Sure. Cut open the wire between the dut and the resistor to its right. Insert a switch there. When zeroing is off, the switch reconnects the resistor to the dut (as it is now); When on, the switch connects the resistor to the virtual ground.

So when zeroing is on, the output on the opamp would be outputing a drift that needs to be netted out. When a mcu is utilized, it would periodically turn on zeroing, and measure the output of the opamp.

When the zeroing is off, the mcu can measure the opamp's output and then subtract from it the drift -> you have zero'd out the drift.

This approach doesn't zero out the drift from the front-end (especially if you use an opamp as an oscillator or have asymmetrical up/down slopes).

A "better" approach is to use a low Rds mosfet as a switch to short out the dut periodically and measure the overall drift, in a similar fashion. It has the disadvantage of requiring a DC voltage / constant current source across the dut.

dannyf, please, really appreciate your efforts by helping this noob to visualize on what are you suggesting, if you don't mind.

It doesn't need to look pretty as long its readable, even a photo of a rough hand sketched drawing on paper should be more than enough. 

[oldway]

Thank you for sharing this very interesting project.
ESR meter is very useful for the repair and whe do'nt need a high precision ESR meter for this purpose.
Design is simple, low cost, reliable and well protected.

Some suggestions:
- The worst that could happen would be to measure a charged capacitor, the highest possible voltage is 400V (SMPS with PFC). Your design seems to be protected against such error.
- some people claims to use cheap and easy available components.
1) +/- 2.5V seems to be low edge power supply for most of the OP's.I would feed the OP's with half of the battery voltage. (+/- 4.5V).
2) For this reason, i would make a different power supply project, generating +/- 4.5V unregulated (half battery voltage) and +/- 2.5V regulated.
3) I would use 3 OP's of a LM324 (9V power supply) to do this.
- one OP with BC 847 + BC857 would provide a 0V center point.
- an output of another OP would feed the +2.5V power rail
- Output of the third OP would feed the -2.5V power rail.
reference votage of 2.5V would be provided by a TL431.
4) as oscillator, i would use a Cmos version of 555, (a TLC555 for example) with this very simple basic design running at 200Khz. (with 5V power supply)
http://wiki.xtronics.com/index.php/555_Delta-Sigma_Modulator
5) For 50% symmetry and inverted outputs, a would use halve of a CD4013B D type flip flop. (5V supply). (Square wave of halve the frequency of oscillator = 100Khz)
6) For switches, a CD4066B or better, a CD74HC4066 could be use in place of the CD74HC4053. (5V power supply)
7) as OP, i would use a TL081 with offset compensation and 9V power supply.

But you basic project is very good, nothing need to be changed if components are available and not too expensive.

[dannyf]

1) +/- 2.5V seems to be low edge power supply for most of the OP's.

2.5v rails are good for usb powered devices.

I would actually go down to 3.7v/2 so it can be easily powered by li-ion batteries.

[mariush]

You can always add a dc-dc converter in SEPIC configuration to get whatever voltage you want from 1.2-6v which ranges from one rechargeable aa battery to a crappy phone usb charger.

If needed, there are LDOs which can smooth out the dc output and at those low currents, they only need a few mV above the output voltage to give good output.
Adds $1-2 to the BOM.

A MC34063 in inverter mode to get -2.5v is also just about 20-40 cents added to the BOM, if voltage divider isn't "cool"

[qno]

Nice design.

I always wondered what would happen to the ESR when an Electrolytic Capacitor is biased with some voltage.


The insulation layer between the plates is formed by the voltage between the plates.

[Jay_Diddy_B]

Hi,

Here is a modified concept using some ideas from the forum. It uses a 555 for the oscillator to generate a 50% square wave. The oscillator is also used to generate a negative rail for the op-amp. The positive supply comes directly from the 9V battery. The op-amp is only working at DC in this design. You can use a OP07 with an offset pot to implement the zero adjustment.

In the original design one of the goals was to use single sided construction, so that the PCB can be the front panel.



I have attached the LTspice model

Jay_Diddy_B

[oldway]

Bipolar version of 555 do'nt work very well at 5V. (output not going to rail nor ground voltage)
Output voltage will not be 50%.
Better to use a Cmos version of 555.
For generating the negative voltage, use a pair of bipolar transitors BC847/BC857 driven bij 555 for higher current.
Collector of BC847 can be feed with 9V so it does not overload the 5V voltage regulator.
Bases from the 2 transistors connected together and with pin3 from 555.
Emitters connected together and with C8.
Collector BC857 connected to ground.

[blackdog]

Hi Jay_Diddy_B,

Can you please make some corrections to your schematic.
It is saying 4016 and 4053 as a fet switch...
Can you please put the pin numbers in the schematic for the 4016 or 4053?

Your output from the 555 wil not be RR, the components for the negatif supply rail wil load the 555 to mutch.
Use a transistor/fet buffer.
The 555 oscilator is NOT 50%/50%, it nead some extra components for that, take a look @ the data sheet for that.

Keep up the good work! :-)

Kind regarts,
Blackdog

[oldway]

4066B is far better than 4016B  (much lower ON resistance) but both can't be use here without inverting 555 output.

Output of cmos version of 555 with 5V power supply:
IOH = -1mA     VOH = 4.8V
IOL = 5mA      VOL = 0.13V
Good enough to succeed nearby 50% / 50%
If you need 50% with precision, you have to run the oscilator at 200Khz and use it as clock of a D flip flop. (1/2 4013B)

[Jay_Diddy_B]

Hi Jay_Diddy_B,

Can you please make some corrections to your schematic.
It is saying 4016 and 4053 as a fet switch...
Can you please put the pin numbers in the schematic for the 4016 or 4053?

Your output from the 555 wil not be RR, the components for the negatif supply rail wil load the 555 to mutch.
Use a transistor/fet buffer.
The 555 oscilator is NOT 50%/50%, it nead some extra components for that, take a look @ the data sheet for that.

Keep up the good work! :-)

Kind regarts,
Blackdog

The schematic is an LTspice model of the real schematic so the pin numbers are not shown. There is a real schematic in this thread with the pin numbers.

https://www.eevblog.com/forum/projects/esr-meter-adapter-design-and-construction/msg341177/#msg341177

The switch is the 74HC4053. The switches in the HC4053 are around 140 Ohms. They are in series with a resistor of 470 + 1600 + 200 ohms, the switch only make up 6% of the total resistance.

The advantage of the 74HC4053, over using 4016 or 4066 switches is that I don't need an oscillator with complementary outputs. The inverter is inside the 74HC4053.

The 74HC4053 is considerably faster than the CD4053, but is a lower voltage part.

The 555 is not configured in the normal way. The output is used to drive the RC network. In this configuration to the duty cycle is very close to 50%. It is supposed to be 50% in this configuration.

The 555 output does not need to be rail-to-rail. The analog switches in the source make it rail-to-rail. The CMOS version of the 555 would be better, but there is no LTsice model for the 555C.

@oldway

The 2F divided by 2 with a F/F will give an exact 50% duty-cycle.  I would probably use that technique if was building a bench meter. But I was building a small adpter.

The LTC6990 timer IC can also be used to provide an exact 50% duty cycle. There is a Frequency divider inside this chip. It has a single output, so an inverter is required.

Total power consumption of the circuit is less than 10mA, so there is no need to added any transistor buffers.

I did post the LTspice model if you want to play with this design.

There are many ways to do this, some is personal choice, some decisions are driven by the parts that you have. The fun is giving building your circuits and testing them.




Regards,

Jay_Diddy_B

[oldway]

Total power consumption of the circuit is less than 10mA, so there is no need to added any transistor buffers.

Output current of the Cmos version of 555 is very low (only 10mA source, 100 mA sink), this is the reason why i recomand to add a transistors buffer.
Bipolar 555 can source and sink 200 mA and buffer is not necessary.

[Jay_Diddy_B]

Hi group,
Here are some accuracy measurements made from the prototype.

The ESR Adapter and a HP 3457A in the 4-wire mode were used to measure a General Radio 1433-W decade resistor. This decade resistor can be set in 0.01 Ohm increments.

The graphs show the HP3457A on the X axis and the ESR adapter on the Y axis.





The equation for the graph is displayed in the y=mx + C

No attempt was made to adjust the ESR Adapter. You can see that the ESR Adapter is reading 4% high with 0.1 Ohm offset. I am not sure where the 0.1 Ohm offset comes from. This was after shorting the leads and using the REL feature on my Fluke 189.  Later I will measure some SMD resistors.


Jay_Diddy_B

[c4757p]

The 555 is not configured in the normal way. The output is used to drive the RC network. In this configuration to the duty cycle is very close to 50%. It is supposed to be 50% in this configuration.

I came to this conclusion about that configuration as well, but I tried it a few times and have found that to be very far from the case. The last time I used that method I had a duty cycle around 40%! Worked fine in SPICE though. Are you sure it's working properly?

[Jay_Diddy_B]

I came to this conclusion about that configuration as well, but I tried it a few times and have found that to be very far from the case. The last time I used that method I had a duty cycle around 40%! Worked fine in SPICE though. Are you sure it's working properly?

@c4757p

I have not built the 555 version of the ESR adapter. I was simulating different configurations of the circuit proposed in the forum.

Using the LTC6990 will produce a very accurate 50% 100kHz oscillator.

What I realised afterwards is that the symmetry in this configuration is a function of the loading on the output pin. If the output pin is unable to swing to the rail or ground, this will increase the time spent in the that state.
The timing capacitor is being charged and discharged between 1/3 and 2/3rds of the supply voltage.

I am very pleased with the version of the circuit using the LTC6241 dual op-amp.

The accuracy measurements speak for themselves. A trimming resistor in series with the 1600 Ohm resistor in the source can be used to adjust the gain. In my unit the gain needs to be lowered by 4%.

I think the 0.1 Offset that I measured with the General Radio Decade resistor, is probably going to be something subtle like skin effect, the different between the DC resistance (HP3457A) and the AC resistance measured with the ESR Adapter.

Later I will be exploring the source of the offset.

But since the main purpose of the ESR adapter is to find dried out caps, the performance already exceeds the goals.

Thank you for your interest.

Jay_Diddy_B

[oldway]

The 555 is not configured in the normal way. The output is used to drive the RC network. In this configuration to the duty cycle is very close to 50%. It is supposed to be 50% in this configuration.

I came to this conclusion about that configuration as well, but I tried it a few times and have found that to be very far from the case. The last time I used that method I had a duty cycle around 40%! Worked fine in SPICE though. Are you sure it's working properly?

This happen because output voltage (high) of a bipolar 555 is only 3.3 V with 5V power supply.
With Cmos version, output voltage is 4.8 V and duty cycle is then very close to 50%.

[kripton2035]

No attempt was made to adjust the ESR Adapter. You can see that the ESR Adapter is reading 4% high with 0.1 Ohm offset. I am not sure where the 0.1 Ohm offset comes from. This was after shorting the leads and using the REL feature on my Fluke 189.  Later I will measure some SMD resistors.
Jay_Diddy_B

can you do the same measurements at 10KHz ?

[grenert]

Could part of the 4% high reading be related to the fact you are feeding a square wave into the cap, rather than a sine wave?  You have high frequency harmonics accompanying your fundamental.  So when you think you're measuring ESR at one frequency, the effective measurement is actually at something higher?

Obviously, 4% is already very accurate!  This is more of a curiosity question. 
Thanks for sharing the design with us!   

[PA4TIM]

When I designed my ESR meter the biggest problem was getting a 50% dutycycle. I solved that by making an in frequency adjustable comparator oscillator (20kHz to 200kHz) followed by a 4013 devide by 2 to control the action of the 4066 ports.

I used a very easy way to zero the reading. The minus probe of the multimeter (or panel meter) is taken from a Voltage divider between 5V and ground. You measure the offset and then calculate the fixed resistor and potentiometer so that the wiper sees the offset voltage as it is set in mid position.

What is the lowest capacitance you still can measure ESR ?
 
There are a few reasons I made it adjustable.
-the first is because datasheets give ESR for frequencies between 100Hz and 10 kHz as a function of D (and D at 1 kHz gives after calculation,  ESR at 1 kHz and that is not the same at 100 kHz)
-At 100 kHz they give Impedance.
-Big caps in classic lineair supplies can score high on ESR because at 100 kHz skineffect and ESL polute the measurement and because they work around 50-100 Hz it is useless to measure them at 100 kHz
- and because almost nobody does it. It is just adding a potentiometer so it is not much work. (and it is a good test. If ESR goes sky high at 10 kHz the meter is measuring impedance instead of ESR)

[dannyf]

Later I will be exploring the source of the offset.

Depending on your set-up and capacitors used, there could be many potential reasons.

The esr meter is no different than the ones proposed here earlier: it measures the ac impedance on the dut. The difference is that a synchronous detector was used so you could measure low (ac) impedance - thus low ESR. The diode detectors used in other esr meters would not be able to do that due to the Vfwd threshold.

Another approach would be to use a precision rectifier but that requires considerably higher slew rate.

A synchronous detector in my view is a nice solution for its low/zero threshold and linearity.

[Jay_Diddy_B]

Could part of the 4% high reading be related to the fact you are feeding a square wave into the cap, rather than a sine wave?  You have high frequency harmonics accompanying your fundamental.  So when you think you're measuring ESR at one frequency, the effective measurement is actually at something higher?

Obviously, 4% is already very accurate!  This is more of a curiosity question. 
Thanks for sharing the design with us!   

In the source the following resistors add up:

470 ohm
140 ohm 74HC4053 switch
1600 ohm resistor
200 ohm resistor
=============
2410 ohms (nominal)

With +/- 2.5V supply this should put 207.4 uA pk-pk through the device under test.

with a 10 ohm resistor this becomes 2.074mV

This is multiplied by the gain of the amplifier stage:

The amplifier has a nominal gain of 1.8 MEG / 33.2K = 54

This gets us to 2.074 x 54 = 112 mV

So the design should read high.

5% resistors were used in parts of the prototype, the 5V regulator tolerance also contributes.

So some pretty simple things can explain the 4% error. Some form of adjustment is needed.

Jay_Diddy_B

[Jay_Diddy_B]

Hi,
I have done a little investigation.

The General Radio 1433-W decade box is a calibration laboratory grade decade resistance box. It is made with non-inductive resistors. I measured the resistance box on my HP 4274A LCR meter. I found that decade box a residual with the knobs set to zero is around 30 mOhms. I also discovered that the decade resistor had an inductance of 700nH.

700nH has an impedance of 0.45 ohms at 100 kHz.

So the ESR adapter has dealt with some of the reactive component.

The challenge here is that the ESR adapter uses square waves for the source. The effect of the inductance is not straight forward.

Resistance Standard







I decided to build a resistance standard using 1% surface mount resistors. I have two terminals at each end of the resistors to allow 4-wire measurements.

The measured inductance of these resistors is between 7-20nH


With this resistor I got good measurements.

The synchronous detector is helping with the accuracy, but for it to work properly it needs a sine wave source.

Jay_Diddy_B

[dannyf]

the ESR adapter uses square waves for the source.

You can run it through a filter to produce a fair good sine wave. R/C filters would be sufficient since you use opamps to amplify the signal.

[PA4TIM]

How you are gonna measure ESR with a sinewave ?

[oldway]

@Jay_Diddy_B: I think you are going in the wrong way.
This is a simple, cheap and clever project: it's not intented to compete with 5000 US$ instruments.
Your ESR meter will be very useful for repair, not for quality control and we don't need high precision.
I have made some modifications for my own use :
I will not use the four terminals option, i don't need this.
But i provided a switch for 10Khz/100Khz and also a trimpot for calibration so it is not necessary to use 1% precision resistors.
No worry about offset, i will use the relative function of my Fluke 87 IV.
Nb: schematic only for explaining my ideas, it is not been tested.

[Jay_Diddy_B]

Hi,
Here is the concept for measuring the ESR with a sine wave. I have attached the LTspice model for people who want to try the model.



The square wave source has been replaced by a sine wave generator. In addition to the sine wave you also need a square wave that is in phase with the sine wave to operate the analog switches in the detector. The AD9838 would be handy, because it has a sign output, which indicates if the output is positive or negative.

The AD9839 would require the addition of a micro to set the frequency etc..

I am going to try and do an analog design.

This modification improves the performance for small value capacitors and greatly improves the performance if there is inductance in series with the capacitor.



The design retains the protection feature develop earlier.

Again, these improvements are largely academic. The original design will sort the good caps from the bad ones.

Jay_Diddy_B

[Jay_Diddy_B]

@Jay_Diddy_B: I think you are going in the wrong way.
This is a simple, cheap and clever project: it's not intented to compete with 5000 US$ instruments.
Your ESR meter will be very useful for repair, not for quality control and we don't need high precision.
I have made some modifications for my own use :
I will not use the four terminals option, i don't need this.
But i provided a switch for 10Khz/100Khz and also a trimpot for calibration so it is not necessary to use 1% precision resistors.
No worry about offset, i will use the relative function of my Fluke 87 IV.
Nb: schematic only for explaining my ideas, it is not been tested.

I had a look at your schematic. The only concern that I have is the Vos of the op-amp in the U1-A position. The Vos is multiply the gain.

The LM324 is 2mV typical, 7mV max. Multiplied by the gain this becomes 110mV typical  385mV max.

The LM324A is better at 3mV typical, 3mV max.

Jay_Diddy_B

[Jay_Diddy_B]

You can spend countless hours and dollars trying to build a quality LCR meter. Thats why they cost several thousand dollars. Given the avalibility of low cost DAC,DDS chips and fast 32b micro's to process the signals (phase /amplitude) it would be intresting to do if you had the time.

I know the original design is good for the intended purpose of finding bad capacitors.

Is there any interest in improving the performance so the design will work with very low ESR parts?

Is 20 Ohms full scale the right value or would 5 or 10 Ohms be better?

How important is it that the board is 5x10 or 10x10 cm so that it can be made at itead?

Thank you for your interest.

Jay_Diddy_B

[oldway]

I had a look at your schematic. The only concern that I have is the Vos of the op-amp in the U1-A position. The Vos is multiply the gain.

The LM324 is 2mV typical, 7mV max. Multiplied by the gain this becomes 110mV typical  385mV max.

The LM324A is better at 3mV typical, 3mV max.

I have allready answered to this:

No worry about offset, i will use the relative function of my Fluke 87 IV.

This is not a mass product project, you can also select the best LM324 (lowest offset) if you want.

Is there any interest in improving the performance so the design will work with very low ESR parts?

I don't have interest.
20 Ohms full scale seems to be a good option.
I will do my own board.

NB: good quality 9V battery are expensive, for this reason, it's very important is to reduce power consumption.
I took great care of this:
- TLC555 (Cmos version of 555) has a very low power consumption of 1mW at 5V. C8 must be choosen of low value to minimize power dissipation in R7 and R21.
- 4013B has a low consumption and no output load.
- TL431 is working with min. current for regulation. (1mA)
- power supply is low loss
- Led is in serie without loss.
- And, of course, LM324 is a low power quad OP with very low supply current drain.

[dannyf]

In addition to the sine wave you also need a square wave that is in phase with the sine wave

To generate a precisely in phase square wave from a sine wave, you will need a good zero-cross circuit - not easy.

It is far easier to generate a sine wave from a square wave.

The AD9838 would be ...

Check out 5932/5933 - they are meant for this type of work (true LCR meters).

fast 32b micro's to process the signals (phase /amplitude)

People have done that with 8-bit mcus (8051), 16-bit mcus (msp430) and 32-bit mcus (stm32). The ones with 8-bit / 32-bit mcus are good to 0.4% full range.

I prototyped one on PIC24F with minimum out-board hardware (fixed frequency, onboard adc) but it required some pretty fancy math - ieee 1057 3-parameter sine wave fitting.

[dannyf]

You arent for example going to be measuring phase differences down to a couple 100nS with a 4MHz PIC for example at least not accurately.

Depends on how it is implemented. Most people would get the bulk of the work done in the analog work and the mcus would be doing signal generation, adc, and display controls (and sometimes calibration). A 4Mhz PIC would be an overkill for those type of works.

If you are, however, doing some serious math - what I did with the pic24 for example, it takes some hard work to get it going.

[BravoV]

Just an academical question, what is the advantage using sine wave instead of square wave while still using this method in measuring ESR, again "ONLY" ESR, not other impedance attributes like in LCR meter.

[PA4TIM]

For impedance a sinewave will do better. I build something like that to  measure femtoFarrads

I think the meter from this topic is good as it is now. It is foolproof to build without critical components and because he made a pcb layout impossible to screw up using the wrong pcb desing (my meter is less fool proof because I do not have a pcb design. A friend builded it and he used bad sample caps that he mounted next to each other so they influenced each other and the trace holding the measured result routed all around the pcb picking up a lot of garbage. It still was usefull as an indicator but performed not even half as good)

 I measure phase difference between voltage and current in an other project with an arduino with Atmel 328 ( I only use the arduino IDE and a USBasp to program the 328 using ISP) and an analog circuit. Two LM311 comparators make a square from the AC signals. Then a 74LS86 and the output from that is feed to the 16 MHz atmel. It measures first the high and then the low time.

But for my ESR meter all is done analog
http://www.pa4tim.nl/?p=1728 the final version is at the bottom of the page. This one measures real ESR and not impedance (I can measure caps smaller as 100 nF) It has an adjustable frequency and uses 4 cheap IC's and some resistors. I use a panel volmeter module for display but you can use a DMM or microprocessor and LCD display or like I did at first an analog meter. The latter has the advantage that you see problems better. If the meterreading  is not steady it could be a shorted cap (they have the ultime low ESR  )

I spend a lot of time measuring and exploring ESR on every possible way. I also collect bad caps. I solder them on documented pcb strips for research purpose, like a sort of bad-standard caps )

I used IV-meter, VNA , LCR meters, C bridges, squarwave and scope, several homebuild meters, a few commercial ones and the result is, I allmost never measure ESR since then. In my opinion the an over rated parameter and most times measured the wrong way (but by accident often the right way because the datasheets spec impedance at 100 kHz not ESR and 90% of the meters measure impedance).

Besides that without knowing the ESR specs you still do not know anything and measuring in situ can mask a bad cap if it is has a good one parallel, and often there are more caps between a rail and ground. I have measured many caps first in situ and then desoldered them and test them again. The difference is often rather big and a complete bad cap can measure good in situ, A DC shorted cap can measure low ESR too.
The most cap failures are: DC shortage, loss of capacitance, high ESR.

When I started experimenting on ESR a few years ago I thought it was great. I used it a lot for testing. I use a scope as main trouble shooter if possible and I noticed a lot of caps that looked bad in ESR did not give problems in the circuit and that was strange. I have a rather big collection LCR bridges and other component testers so I started analysing the "bad"caps. For instance I repaired a sat tuner and it had 34 bad caps. 2 had real high ESR, most had degraded capacitance  and several leaked DC. But the good thing about an impedance "ESR" meter is that the degraded capacitance shows as high ESR.

So my ESR meter measures ESR and that makes it less usefull if you want an ESR meter to repair consumer gear in situ. Better use the impedance versions that have troubles measuring ESR under 10 uF because reactance becomes to high.

Today I sometimes use the ESR meter in situ as a first impression while restoring long not used gear (and as part of the proces of analysing caps for other people).
Then I desolder one leg, reform the cap and do a DC leakage test and after that I measure capacitance  and measure D. Most times at 1 kHz. D tells you realy if a cap is bad. If the caps do not need reforming and I can power up the instrument I use my scope to check everything and I find every  bad cap this way.

http://www.pa4tim.nl/?p=1728 measuring bad caps
http://www.pa4tim.nl/?p=3775 about ESR and several testing methods
http://www.pa4tim.nl/?p=1385 About DC leakage

[kripton2035]

in elektor esr meter (sept 2002) , they use the same principle as the one described here with a square test signal and 4 4066 gates and a lf412 as difference amplifier. but they said that they had to use a VHC 4066 to minimize at best the unwanted reactance. nowhere did they tell about sine wave.

[BravoV]

I think the meter from this topic is good as it is now.

Agree, this circuit is more than enough for it's purpose, really appreciate JDB's effort, and for sure I'm going to build it.

For impedance a sinewave will do better. I build something like that to  measure femtoFarrads .... <snip> ...

How exactly ? Any chance to explain further on how sinwave is better ?

Looking at your tools, skills and experiences above, you must be very expert and pretty sure you able to explain it to noob like me, please.

[PA4TIM]

A cap has a certain impedance at a certain frequency. In that case the signal must be a sinewave by nature of the principle and math. And impedance is tghe "resistance" for AC signals. Just like you measure a resistance while using a known current or voltage or a ratio measurement (an unknown in series with a well known resistor) you can use a siewave current or voltage to measure impedance for a resistor, coil or capacitor.

A square wave in not "1" frequency like the frequency in the reactance formula. So it will have a lower reactance for the fast components in the squarwave. Impedance |Z| is the absolute value of real R + imaginair R, and split it is Z=R+jX where jX is negative for a cap.

[oldway]

ESR schematic:
C8 = 470pF
R7 = 5K6
R21 = 56K

[codeboy2k]

since PA4TIM posted the method... I'm working on an LCR meter that calculates impedance exactly like that.. |Z| = R+jX. It uses a 4-wire measurement, putting a 600mV p-p up to 1.5V p-p peak sine wave through the DUT, measure voltage and current and determine if the phase is leading or lagging...I'm using an MSP430 and its onboard 16-bit ADC. I am not sure if I want to use another processor yet, or if I want to use an external ADC, but the MSP430 seems ok for the job right now.

I only have the front end prototyped up, but I am not sure of the opamps I've chosen, and I may change them out still, but they seem ok so far. Just I haven't finished testing all the ranges. And since I didn't want to use $11.00 450Mhz opamps, I chose the cheaper ones with GBW up to 50Mhz, these are just between $3.50 and $4.50 on digikey for duals. I also tried cheap CFB triple video amps in one device (3 for less than $3.00), and they had great bandwidth out to 200Mhz or more, but I couldn't get them to go below 100Hz, and I was shooting for 20Hz to 1 Mhz flat, which I am able to get now with the amps I am using, just with some finicky bits.

The sine wave passes though the DUT and I differentially measure both the voltage across the DUT and the current across switched sense resistors. 

The frequency response is flat from 20Hz up to 1Mhz, that took me a while to get it flat. It's literally .058 dB down at 1Mhz using those parts, but I've found it susceptible to stray capacitances causing peaking at 10Mhz or so, which causes small gain errors at 1Mhz. That may be unavoidable without moving up to a 100Mhz or higher part. I'm trying to keep this a CHEAP high-performance swept LCR meter from 20Hz to 1Mhz with reasonable performance comparable to the $4000 meters.

I have found that I can measure the voltage across the DUT and currents through the DUT to within .01% accuracy, from 20Hz to 1Mhz, but I haven't completed testing with all the ranges.  Maybe a final build will end up with 0.1% guaranteed accuracy as an LCR meter.  I am hoping for that at least.

Cheers!

[PA4TIM]

Codeboy, that sounds as an very interesting project. Almost a vna like system. Very impressive results. I know how hard it is to get such a flat responce over that range. I have not tested CFB opamps. I use LT1028 and OPA37. The GBW is OK but I want to try opamps with a faster slewrate (I used good IC feed so it is not much work to change opamps in a later stage.(I need arounsd 10 of those so that is a bit expensive. I want to try a very fast LT opamp a friend tested, but those are around 8 euro a piece so I do not know yet is the extra investment makes it so more usable as it is now (I can measure power from DC to 500 kHz and 0V to 300V and 0- 10 A. RMS AC+DC , PF, phase, current, voltage, shunt temp, Watt and VA and I will use it 90% of the time to monitor 230V and current to the instruments I'm repairing or building)

I just bought a launchpad but have not used it much yet because I only have 5V displays here and I'm rather new in digital. I now use the arduino ide and a tried energy but I am busy learning normal C.

Are you planning to make it sweeping ? A sawtooth X out to the scope and a two DAC's to make the Y signals. Or a small graphic lcd display (i'm learning C to  couple analog design with digital, not to replace it. More like 1+1=3) My first project was a 2GHz counter and RF powermeter added as readout and powercontrol to an analog project I just finnished (a 25MHz to 2000MHz sweeping signal generator)

In the powermeter I'm working on, I use a LTC2400 as ADC. Not needed it but I had a testboard in my junkbox for some time. That is the first time I use it but it works great (thanks to code I found and use as base and the SPI header)

[dannyf]

I can measure the voltage across the DUT and currents through the DUT to within .01% accuracy

That would be an impressive (almost impossible I think) result on a production unit. It is fairly doable on a one-off unit, with calibration.

[codeboy2k]

Codeboy, that sounds as an very interesting project. Almost a vna like system. Very impressive results. I know how hard it is to get such a flat responce over that range. I have not tested CFB opamps. I use LT1028 and OPA37. The GBW is OK but I want to try opamps with a faster slewrate (I used good IC feed so it is not much work to change opamps in a later stage.(I need arounsd 10 of those so that is a bit expensive. I want to try a very fast LT opamp a friend tested, but those are around 8 euro a piece so I do not know yet is the extra investment makes it so more usable as it is now (I can measure power from DC to 500 kHz and 0V to 300V and 0- 10 A. RMS AC+DC , PF, phase, current, voltage, shunt temp, Watt and VA and I will use it 90% of the time to monitor 230V and current to the instruments I'm repairing or building)

Thanks. Yes, I wanted to have a different LCR meter, that wasn't just a few fixed frequencies, but I could set any test frequency from 20Hz to 1Mhz  or sweep over the entire range and plot the output.

Yes, it's very hard to get the signal chain flat from 20Hz to 1Mhz, and in the end if I build it up on a PCB I might not be able to get it that good anyways; I will probably have to include some code to compensate; probably do a baseline sweep and use that to compensate for offset and gain errors in the signal chain.  So maybe it's trying so hard to get it flat is not worth it after all and just  a few dB down at the top and bottom end can always be compensated for in software, but I took a hardware approach and did my best to get it at flat as possible.    I'm using two OPA727 and an LT6231 in a standard instrumentation amplifier configuration.  I'm using the OPA727 (GBW=20Mhz, SR=30V/us) as gain=2 buffer, at the top and bottom of the DUT, followed by a LT6231 (GBW=215MHZ, SR=70V/us).  There are two LT6231's, one is gain=2.5 (total gain=5) and the other is gain=2, for a total gain=10).  I am probably going to have to add 2 more LT6231's in cascaded x2, x5 gains to get another gain x10, and reach a total gain of 100 (or a single LT6231-10 in gain=10, depending on price).  The LT6231 has higher input offset voltages, but at the ends of the gain stage it is less and less of the error budget.

I like the high common-mode input impedance of the LT1028, it would make a nice buffer, but I don't think it's slew rate is high enough for signals larger than 1V @ 1Mhz. 

Anything really good is $10, $15 or more.

Are you planning to make it sweeping ? A sawtooth X out to the scope and a two DAC's to make the Y signals. Or a small graphic lcd display (i'm learning C to  couple analog design with digital, not to replace it. More like 1+1=3) My first project was a 2GHz counter and RF powermeter added as readout and powercontrol to an analog project I just finished (a 25MHz to 2000MHz sweeping signal generator)

Yes, I will make it settable test frequencies and sweeping across the range.  I wasn't planning on scope output, but that sounds interesting.
Actually, I wanted to avoid a front panel at first, so I've just considered it to be USB controlled, and software on the PC. Then sweep it and graph the result on the PC like a VNA.  I'll probably start like that.

In the powermeter I'm working on, I use a LTC2400 as ADC. Not needed it but I had a testboard in my junkbox for some time. That is the first time I use it but it works great (thanks to code I found and use as base and the SPI header)

Yes, I'm also considering whether I will use an off chip ADC like the LTC2400 too.  This might improve the noise level as well, since I hear the horror stories of using a high-resolution ADC that's on the same substrate as the digitally switching micro... And with an off board ADC then I can use a (cheaper?) micro with a USB built in and no concern for it's ADC capabilities.  As it stands, it's hard to find a reasonable cost micro with 16 or 24bit ADC and USB. It's easy to find a micro with USB and a 12-bit ADC, or a micro with no USB and a 16-bit or 24bit ADC.   And I can always use one of the USB to Serial chips from FTDI, but I don't want to go that way if I can use a micro with built in USB.

Right now I'm at the early stages, and just seeing what performance I can get and where I can go with it.

That would be an impressive (almost impossible I think) result on a production unit. It is fairly doable on a one-off unit, with calibration.

Yes, I think so too.  I can get it with my hand-tweaking on the bench, but I want to be able to specify say, a 2.2pf feedback bypass cap for gain limiting to reduce the peaking, and not be way off because the tolerance of the cap actually changes the gain peak so much that I get gains errors anyways (and thus can't read the voltage across the DUT accurately anymore).

So ultimately, I think all my effort to get a flat response like this might not be worth it, and in the end I'll have to run a calibration cycle anyways to get the baseline as built, and use that baseline to compensate and flatten the signal chain.

[Jay_Diddy_B]

Hi Group,

I have been experimenting with the effects of sine versus square wave excitation and the interaction with the synchronous detector.

Here is the first LTspice mode.



I have a made a difficult circuit to analyze consisting of a 2.2uF capacitor, a 0.1 Ohm resistor and a 1uF capacitor.

I have implemented the synchronous detector with a circuit that has a gain of +1 for one half cycle and -1 for the other half cycle. This is feed to an averaging filter. This circuit gives that magnitude of the in-phase component, the ESR. The current source is implemented as relatively high voltage and a resistor, this is close enough to an ideal current source for the experiment.

One of the models has a sine wave source and the other model has a square wave source.


These are the voltage waveforms of the circuits under test:



The shapes are very different. The sine wave case results in a sine wave. The square wave case has pulse which come from V=L di/dt from the edges. and then dv/dt = I /C for the triangular portion.



These are the waveforms at the output of the phase detector, before averaging. If the timing is perfect, the components from inductance and the capacitance average to zero and you are left with the real component.

Here is the output from the filter. It is the same for both the sine wave and the square wave case.




Introduce a small delay.

Have added a small delay, only 50ns, to the synchronous detector timing in this model:



The output of the synchronous detector changes to these wave forms:



After averaging, there is little change to the sine wave circuit and a relatively large change to the square wave circuit.




This effect is only really sensitive to inductance. The effect of the capacitor is much less.

I have attached the LTspice models.

Jay_Diddy_B

[oldway]

Very intesting: it show that choosing sine or square wave does not matter if there is no or little delay in the synchronous detector.
Using a 4013B to switch the synchronous detector should reach this goal.
It proove also that the option of 2 frequencies (100Khz and 10Khz) is far better, as the changes will be 10 times reduced with 10Khz instead of 100Khz.

[Jay_Diddy_B]

Hi,

The main thing I see, if you can arrange the switches to come on for the central part of the square wave in each half cycle, the circuit will not see the effects of the caused by the inductance. I am trying to think of a simple way to generate the required signals.

Here is the model:



The switches S3 and S4 are turned on in the center of each half cycle. This is timing required for the switches:



The result:



The circuit is no longer sensitive to the inductor. The capacitive part is left, but it averages to zero.

I have attached the LTspice model.

Jay_Diddy_B

[oldway]

The main thing I see, if you can arrange the switches to come on for the central part of the square wave in each half cycle, the circuit will not see the effects of the caused by the inductance. I am trying to think of a simple way to generate the required signals.

A short delay of the on stage of the synchroneous rectifier switches would do the same and is easy to do.
But is it necessary?
Before to modificate a project, you should know if it's worth.

[Jay_Diddy_B]

Hi,
 A short delay is not sufficient. If you use a delay you will pick up the inductive pulse at the end of the half-cycle. You need to delay the start and turn the switch off before the end of the cycle.

This analysis is really academic. The design as published will find bad caps.  I works absolutely fine with capacitors 10uf and greater. A test lead inductance of 1uH causes about 0.1 Ohm the reading only if the 2-wire configuration is used.

I am conducting the analysis to reveal why some methods are better than others and what the deficiencies are. You can then use this information to predict how well other ESR meters will work.

Jay_Diddy_B

[BravoV]

My brain hurts just thinking about generating or orchestrating that pulses, a 4017 decade counter ?  Assuming ruling out using mcu, just a noob wild guess here. 

[codeboy2k]

My brain hurts just thinking about generating or orchestrating that pulses, a 4017 decade counter ?  Assuming ruling out using mcu, just a noob wild guess here. 

Those S3 S4 waveforms are similar to a synchronous buck converter top and bottom gate drives with dead time . I know it's overkill, but you could use a controller with external sync and lock it to your test frequency. The LT3838-1, for example, has an external PLL input and an internal VCO that can be phase locked to the external signal.  If you wire up the voltage and current feedback pins to reasonable values, the controller won't know any better

Unfortunately, it's not actually a viable solution. These controllers aren't designed to go much below 50KHz and the LT3838-1 in particular has an internal VCO with a lower limit of 140KHz.

But with a 50% duty cycle, the Top SW and Bottom SW would give the needed waveforms from Jay's spice run , syncronized to the source

If anything, perhaps the study of the internals of other synchronous controllers with dead time will give a (analog) solution.

[BravoV]

What I have in mind is, with the 10 counting pulses, as source by tapping output 0 and 5 is for main 50% pulse, while ouput 1 and 3 in pair with output 6 and 9 which have narrower pulse for both S3 and S4 respectively, cmiiw. 

[oldway]

My brain hurts just thinking about generating or orchestrating that pulses, a 4017 decade counter ?  Assuming ruling out using mcu, just a noob wild guess here. 

Very simple, have a look how i should do this using the triangular wave of the 555.
Schematic is only to explain my ideas, it has not been tested.

I modified several times the schematic, my apologies for that.

[BravoV]

oldway, thanks, learned something new here today ! 

[Jay_Diddy_B]

Hi,

I like the idea of using a 4017. I would actually use the 74Hc4017.

I would clock the part at 1MHz. The carry output, pin 12, would drive the analog switches in the source. This pin has a 100kHz 50% duty cycle.

I would use a 74HC4075 to combine outputs 1,2 & 3 for S3 and combine outputs 6,7 & 8 for S4.

I would use 74HC series because it is much faster than standard 4000 series CMOS.

Jay_Diddy_B

[BravoV]

Thanks JDB, just happy to hear the self taught and spent many days/weeks learning basic logic stuffs and Karnaugh map does mean something, even though just an idea.

Aware that your original version should be more than enough to rule out bad or good caps, its just I'm so fascinated and intrigued to build it, btw, is there an official name for such measuring technique ?

[oldway]

Offset compensation of the LM324 op-amp:
See schematic.

[Jay_Diddy_B]

Hi group,

Time for another update. My PCBs arrived today from itead.

Solder Paste Stencil

The first job was to make a solder paste stencil. I started with an aluminium pop can. I cut out the side wall with a pair of scissors and flattened it:




I taped the aluminium sheet to a scrap piece of 0.062" FR4 on the bed of my circuit board router:





I have previously made a file from the top solder paste layer.

Here you can see the stencil being cut:



After the stencil was finished, I made a simple fixture to hold the board while I applied the solder paste. The fixture was made by taping scrap pieces of copper clad board together:



Assembly

After I applied the solder paste, I manually placed all components using tweezers. I then had four boards ready for reflow in a toaster oven. I don't have a reflow controller. I use a Fluke 52 thermocouple thermometer and a watch to set the soldering profile.



Here is the finished board:



And the board mounted on the box. The box in the picture is a Hammond 1591LGY.




I did a quick check and this works like prototype.
Here is the final version of the schematic:



I have also attached a pdf version of the schematic.

Jay_Diddy_B

[BravoV]

+1 and thanks for sharing, look great. 

Edit : What is that R21 used for ?

[robrenz]

Very nice work 

[Jay_Diddy_B]

Edit : What is that R21 used for ?

R21 is a zero ohm resistor. It was used to jump over a track so that the layout doesn't have any vias and no traces on the top side of board. The top side of the board is the front panel.

I played around with the layout for a long time, but I just could not work around having the one zero ohm resistor.

Jay_Diddy_B

[BravoV]

Ahh.. got it. 

Also curious on the 2W vs 4W results from these boards, any significant differences ?

[oldway]

Simple, cheap, very well protected, it's a very nice project.
Thank you very much for sharing.

[Jay_Diddy_B]

Ahh.. got it. 

Also curious on the 2W vs 4W results from these boards, any significant differences ?

BravoV asked, so I did some tests.

I first measured some capacitors on an HP 4274A LCR (Z) meter. The ESR adapter was zeroed before each test using the relative button on the DMM.

4.7uF 50V measured ESR 1.28 Ohm


Measurement with short leads approximately 4 inch (10cm)

2W 1.25 Ohm

4W 1.22 Ohm

Measurement with medium leads approximately 18 inches (45cm)

2W 1.36 Ohm

4W 1.23 Ohm



1000uF 35V 105C  70 mOhm

Measurement with short leads approximately 4 inch (10cm)

2W 79 mOhm

4W 70 mOhm

Measurement with medium leads approximately 18 inches (45cm)

2W 87 mOhm

4W 80 mOhm


So the answer is not that much.

For trouble-shooting I would use 2W long leads.

For more accurate measurements I would use 4W short leads.

For really accurate measurements I would use my LCR meter. I would not use my LCR meter for trouble-shooting because it lacks adequate protection.

Jay_Diddy_B

[jaxbird]

It looks really great  Simple and beautiful design.

Love the diet Pepsi stencil, although, personally, I would probably have used diet Coke instead

[BravoV]

Jay_Diddy_B, thank you so much for the efforts, results look very impressive compared to that thousand dollars LCR meter ! 

[SuperHerman]

Hi,
i was following this thread with great interest and decided to build an esr meter, because i liked the idea of cutting out the inductive voltage spikes i decided to build a version similar to oldboys last design. Being only a prototype i didnt bother to make a pcb but just started building the circuit on a copper clad board. At the moment i am still testing the thing but it seems to work fine, it has a full range of only 4.2 Ohms but that is ok for an esr meter because when a cap has an esr higher than that i do not really care how high anyway. It works good to below 10µF, and a 150nF Cap still reads slightly over 1 Ohm ( the orange one in the picture ).

The resistors i measured in the pictures are:
1 Ohm 10% --> 1,018 Ohm --- i measured this Resistor to 1,014 Ohms with another meter
3,3 Ohm 10% --> 3.347 Ohm --- measured this one to 3.347 Ohm and calibrated the esr meter with it
0.062 Ohm 10% --> 0.061 Ohm
0,180 Ohm 10% --> 0,184 Ohm
0,120 Ohm  ?% --> 0,119 Ohm

The resolution and accuracy of this design could be increased by using a precision voltage reference (i rely on the ouput of the LM7810 i use)
and not using cd4066 as a switch, but i like the results and will use it in the future. Usually when repairing stuff i don't rely on esr measurement anyway but look at the voltage across the elkos with a scope to see if they are good, but for quick measurements a reliable esr meter is a good thing to have, so it will suffice for my needs.

[BravoV]

SuperHerman, thanks for sharing, the results look impressive ! 

Btw, curious on that BNC connector, what is that for ? For scope measurement point ? or external pulse generator ?

...i decided to build a version similar to oldboys last design.

You mean oldboys oldway's circuit ? -> Oldway's variant @ post #75

...and not using cd4066 as a switch...

So what are you using for the switch ? 4053 ?


Talking about the switches, I know the results so far are "more than enough", just purely academical here, will there be any significant difference when using HCT4053 vs HCT4066 ?

[SuperHerman]

Sorry for the name fail on my part oldway, ,

The BNC connector is part of the 4 wire measurement, the 2 twisted cables provide the current to the DUT and the coax cable conducts the signal back.
I do use the 4066, but i think it is not an optimal device to switch the current to the DUT due to the relative high internal resistance and its tempco. If i would do it again i would use 2 complementary fets or some other way to provide  a more precise and stable current like maybe an improved howland current source, but it is not really important for an esr meter to be highly precise, so it would be more an academic question. At the moment the offset drift is the biggest error, it changes up to 5mV at the output until everything reaches thermal equilibrium, i used 2 op177, one as a buffer and the other as a differential amp with a gain of 100 and 0.1% resistors (only around the x100 amp) with low tempco of 20ppm/°C  if i remember correctly. Offset correction is done only at the buffer amp. I don't know yet where the offset drift comes from, but part of it comes surely from the opamps.
Greetings

[Jay_Diddy_B]

SuperHerman,

You have got excellent results !!

Can you post a schematic of your amplifier configuration?

The offset and the temperature coefficient of the offset will be amplified by the gain of the amplifier. So if you are seeing a 5mV change at the output of the op-amp this would be a 50uV change when referenced back to the input. So this is inline with the op-amp specifications.

I would not worry too much. If you test a small capacitor like 4.7uF 50V and warm the capacitor with your fingers the ESR will drift a lot.

The same switches are used in the source as the detector to match the propagation delays. In my configuration I have a spare 1/3 of the 4053 which I could connect in parallel with the one in the source. I didn't do this because I wanted a single sided layout.

I explored the effects of delays in this message:

https://www.eevblog.com/forum/projects/esr-meter-adapter-design-and-construction/msg344453/#msg344453



The switch resistance is typically 80 Ohms, this in series with 470 + 1600 + 200 =2270 (assuming the pot is in the centre). So if the switch resistance changes by 40 Ohms the current will change by less than 2%. For the intended purpose, finding bad capacitors, this is academic.

Jay_Diddy_B

[jaxbird]

I am now the happy owner of one of these nice boards:




I know it was designed for a specific box, but having a 3D printer, I enjoy making small boxes for projects, so this is what I came up with:




Made a couple of short Kelvin(ish) cables for it:




It works really well, big  to Jay_Diddy_B for the nice ESR meter adapter design.

[BravoV]

Nice enclosure, love the way you made the room for that 9 V battery. 

Hmm... torque screws. 

[jaxbird]

Nice enclosure, love the way you made the room for that 9 V battery. 

Hmm... torque screws. 

Thanks .. I was thinking about how to avoid having the battery short the backside of the board and make sure the bananas wouldn't touch the battery, so I thought better make a separate compartment. Also prevents any battery leaks from ruining the device.

A cool board needs cool screws

[oldway]

My ESD tester works well.
Thank you to Jay_Diddy_B !

I made some changes: (see diagram ESR3)
- Test frequencies of 100 kHz and 10 Khz
- Only 2W...4W is not practical for such an ESD tester.
- Offset and the resistance of test cables are compensated  by setting to zero with a 20K potentiometer. It's no longer needed to use the "relative function" of the multimeter. (cheap 5 bucks multimeter can be used )
-choice of easy to buy and low cost components.
- fully protected to 100V (seems to be enough)
The PCB is single sided and the components are SMD.
Only one jumper was needed.
Consumption is about 7 mA.

I'am preparing a more sophisticated version without problem of delay and two ranges, one from 0 to 20R and a more accurate one from 0 to 2R. (see diagram)

[astra]

Thank you all of you for the time you dedicate in sharing this useful projects..!
astra.

[TorqueRanger]

How anyone used this design and whats the best design?


Thanks
Jason Sr

My ESD tester works well.
Thank you to Jay_Diddy_B !

I made some changes: (see diagram ESR3)
- Test frequencies of 100 kHz and 10 Khz
- Only 2W...4W is not practical for such an ESD tester.
- Offset and the resistance of test cables are compensated  by setting to zero with a 20K potentiometer. It's no longer needed to use the "relative function" of the multimeter. (cheap 5 bucks multimeter can be used )
-choice of easy to buy and low cost components.
- fully protected to 100V (seems to be enough)
The PCB is single sided and the components are SMD.
Only one jumper was needed.
Consumption is about 7 mA.

I'am preparing a more sophisticated version without problem of delay and two ranges, one from 0 to 20R and a more accurate one from 0 to 2R. (see diagram)

[BravoV]

My ESD tester works well.
Thank you to Jay_Diddy_B !

I made some changes: (see diagram ESR3)
- Test frequencies of 100 kHz and 10 Khz
- Only 2W...4W is not practical for such an ESD tester.
- Offset and the resistance of test cables are compensated  by setting to zero with a 20K potentiometer. It's no longer needed to use the "relative function" of the multimeter. (cheap 5 bucks multimeter can be used )
-choice of easy to buy and low cost components.
- fully protected to 100V (seems to be enough)
The PCB is single sided and the components are SMD.
Only one jumper was needed.
Consumption is about 7 mA.

I'am preparing a more sophisticated version without problem of delay and two ranges, one from 0 to 20R and a more accurate one from 0 to 2R. (see diagram)

Thanks oldway, glad to see JDB's base design is evolving into another flavours. 

Whats the difference between esr3 vs esr4 ?

Btw, the attached schematics esr3 and 4 appear to be blurry, am I the only one who experience this ?

[kripton2035]

a bit blurry for me too, must be the software that generated blurred jpegs

[BravoV]

a bit blurry for me too, must be the software that generated blurred jpegs

Ok, then I'm not alone.

To oldway, for electronic schematic, its better to save in lossles format PNG instead of lossy JPG, sometimes it will get even higher compression level than JPG with high compression setting.

JPG is suitable only for photograph real life images, for "cartoon" like image with much less color gradient and sometimes less color counts, use PNG.

[oldway]

Thank for your comments.

- I modified my previous post and replaced the JPG by PNG pics.

- I noticed a problem with the original project: voltages on the 2 capacitors C11 and C12 of my ESR3 diagram should be symetrical (one + and the other -) in reference with AGND.
This is not happening: voltages are drifting at an average value far from AGND.
I realized that the reason of this is because there is no AGND reference in that circuit and that this is a high impedance "floating" circuit.
If there is a little difference between the positive and negative synchroneous rectifiers, this generate a DC voltage and a drift .
For this reason, I added the 2 resistors R1 and R27 of 10K in parallel with the capacitors C11 and C12.
As my version must be calibrated with R32, those resistors have no influence on the precision of the reading.

- "Difference between ESR3 and ESR4 ?"

1)Delays of the analoge switches causes some lack of precision.
Jay_Diddy_B reduced this by choosing fast analog switches.
ESR4 is another approach to solve this problem by reducing (of a symetrical manner) de conducting angle of the synchroneous rectifiers to 150° instead of 180°.
This is made by the comparator LM311.
2) I added a 10x gain OP amp so we have two ranges: 0-20R (reading: 1V = 10R) and 0-2R (reading 1V = 1R). The last one seems easier to use.
3) I modified the power supply, using the original project of Jay_Diddy_B for two reasons:
- I was spilling 1mA consumption only for the TL431, this is nonsense.
- I needed to free an OP amp of the LM324 for de 10x gain amplifier.

[kripton2035]

the png are still blurried ... but it's still readable not a big problem.

[neslekkim]

the png are still blurried ... but it's still readable not a big problem.

Check your glasses, or clean your screen , the png's are not blurry at all, no compression artifacts at all.

[fpliuzzi]

To see the much clearer schematics by Oldway, I had to click on the image, then right-click on the image and select VIEW IMAGE. Finally. click again to magnify the png image to its full size. They are very sharp now... thanks.

[oldway]

You could also download the PNG pictures and open them on your computer.
They seems to be very good.

[TorqueRanger]

Does anyone have gerber files or know how to make the pics for thermal transfer ?

[Jay_Diddy_B]

Hi TorqueRanger and the group,

I have attached pdfs that should help DIY construction of the ESR meter adapter.

There is copper layer which has been mirrored for toner transfer. I have included a scale so that you can make sure the board is the correct size.
There is pdf showing the silk screen layer so you know where the components go.
I have also attached the latest version of the schematic.

Jay_Diddy_B

[TorqueRanger]

Hi TorqueRanger and the group,

I have attached pdfs that should help DIY construction of the ESR meter adapter.

There is copper layer which has been mirrored for toner transfer. I have included a scale so that you can make sure the board is the correct size.
There is pdf showing the silk screen layer so you know where the components go.
I have also attached the latest version of the schematic.

Jay_Diddy_B

Thank you so very much

Thanks Again
Jason SR

[TorqueRanger]

Does anyone have any reviews ,updates ,or problems ??

[echen1024]

Does anyone have any reviews ,updates ,or problems ??

I was sent one of these by Jay, and I haven't had the time yet for a full review, but I'll tell you what I think so far. 1st. I received a dud. I found that there was a dry joint on a 7805 regulator, fixed that, and went on my way. It is really very easy to use, outputting 100mV per ohm, and plugging directly into the DMM. I have tested it, and it is relatively accurate. I have used it in helping me to determine replacements caps in my ageing 6114A power supply, and can say that 4 wire kelvin measurements really do help. All in all, a nicely designed little adapter that does what it's supposed to without fuss. Only tip is to test each one  .

[TorqueRanger]

Does anyone have any reviews ,updates ,or problems ??

I was sent one of these by Jay, and I haven't had the time yet for a full review, but I'll tell you what I think so far. 1st. I received a dud. I found that there was a dry joint on a 7805 regulator, fixed that, and went on my way. It is really very easy to use, outputting 100mV per ohm, and plugging directly into the DMM. I have tested it, and it is relatively accurate. I have used it in helping me to determine replacements caps in my ageing 6114A power supply, and can say that 4 wire kelvin measurements really do help. All in all, a nicely designed little adapter that does what it's supposed to without fuss. Only tip is to test each one  .

No problem ...
Thanks for the information because I was going to etch a board up and see how it works out too..

[echen1024]

Sorry for the delay, but for anyone interested, I have made a short video detailing how it works and a demonstration of usage.

[zaoka]

Is there any chance that you modify schematic so that we can use it with analog meter 100uA. If so please make the scale non linear, the range of up to 50ohm and that 25% of the scale goes for the range from 0-1ohm and the rest is for up to 50ohm.

I know that most of engineers does not consider analog ESR meter, however, for troubleshooting work it is way faster and better to use than digital.

With this modification we would have final ESR tester that everybody can use and be happy.

The ideal would be to implement both, digital and analog readout at the same time 

[zaoka]

If you can do this I will create scale for the meter so that everybody can use.

[Jay_Diddy_B]

Is there any chance that you modify schematic so that we can use it with analog meter 100uA. If so please make the scale non linear, the range of up to 50ohm and that 25% of the scale goes for the range from 0-1ohm and the rest is for up to 50ohm.

I know that most of engineers does not consider analog ESR meter, however, for troubleshooting work it is way faster and better to use than digital.

With this modification we would have final ESR tester that everybody can use and be happy.

The ideal would be to implement both, digital and analog readout at the same time 

Zaoka:

If you are looking for an analog meter, have a look at this project:

https://www.eevblog.com/forum/projects/5-transistor-esr-meter-design/msg171364/#msg171364

This one does not have the protection that the ESR Meter Adapter has.


Jaxbird designed a digital version of the 5 transistor circuit, He linearized the output using a micro. You can find information in this thread:

https://www.eevblog.com/forum/projects/esr-meter-build/

You could probably build a dual display version.

Jay_Diddy_B

[Pat Pending]

I encounter this design back in 2011, not sure where from, but its basically the same as discussed here.
It defaults to the 4W measurement mode.

[BravoV]

I encounter this design back in 2011, not sure where from, but its basically the same as discussed here.
It defaults to the 4W measurement mode.

That design was posted in Silicon Chip magazine by Len Cox.

Similar maybe, but there is a tiny yet crucial difference, it has no protection against a charged cap compared to Jay's design, cmiiw.

[Jay_Diddy_B]

I encounter this design back in 2011, not sure where from, but its basically the same as discussed here.
It defaults to the 4W measurement mode.

The design is similar in functionality, and probably has similar performance. As BravoV said, I have implemented better protection for charged capacitors and applied voltage.

The Silicon Chip Design has four chips plus a regulator.

My design uses only two chips plus a regulator. The reduced chip count allows the circuit to be built on the back of the lid.

Jay_Diddy_B

[oldway]

If Jay_Diddy_B did know the Silicon Chip Design of 2011, it would be fine if he had presented his project as an improvement of this earlier design.
But, anyway, this new version has a lot of features:
- using +/- 2.5V power supply instead of +/-5V, so it can be powered  by a single 9V battery.
- fully protected against charged capacitors.
- few components
- single sided board project.
But i don't agree with some ideas:
- 4W is nonsense as this project is not a high precision tool....it's intended for diagnose and repair.
Using Kelvin probes is not practical at all.
- need a zero ajust pot for compensating both offset and resistance of the test probes. With such a zeroing  pot, there is no more need of a multimeter with relative function, nor to choose a low offset op amp. You short circuits the probes and ajust the pot for 0V reading.
- I would prefer to have two frequencies: 100Khz and 10Khz as 100Khz seems a little high for big capacitors.
- Actual range is 100mV = 1R....better to have 2 ranges, also 1V = 1R for easier reading and greater accuracy.
- in my opinion, should use only very easy to buy components...TLC555 (cmos version of 555), 4013, 4066, LM324, 78L05.
I also found an error in this project: there is no ground reference for the inputs of the op amp because there is an isolating capacitor and high resistance values. Inputs are "floating" and are not symetricals compared with ground.
For solving this problem, I added two 10K resistors in parallel with the capacitors C3 and C4 of Jay_Diddy_B schematic.
- A made 2 new versions, the first is allready working very well. I have still to make the board of the second one, but it's not that easy because I want to make a single side board project.

[Jay_Diddy_B]

If Jay_Diddy_B did know the Silicon Chip Design of 2011, it would be fine if he had presented his project as an improvement of this earlier design.
But, anyway, this new version has a lot of features:
- using +/- 2.5V power supply instead of +/-5V, so it can be powered  by a single 9V battery.
- fully protected against charged capacitors.
- few components
- single sided board project.
But i don't agree with some ideas:
- 4W is nonsense as this project is not a high precision tool....it's intended for diagnose and repair.

etc.

Oldway is correct in his observations.

The is a very good collection of ESR meter designs, that have been collected by Kripton2035, here:

http://kripton2035.free.fr/esr-repository.html

I studied a lot of them. I made LTspice models for the analog portions of some of them.

I was aware of the Silicon chip design of 2011. I believe that it dates back to 2005.
I was also aware of the Elektor 2002 design. This is the earliest design that aware of that use analog switches instead of diodes.

The general design, is (incorrectly?) called a lock-in amplifier.

These circuits use either the 4016 or 4066 analog switches.

At some point I simulated the Silicon Chip Design:



I believe that mine circuit is the first one to use the 74HCT4053, for the analog switches. This removes the need for complementary drive signals.

I also took inspiration from the 1967 HP 4338A milliohm meter design:



(There is a d.c. path to ground for the capacitors C3 and C4. The path is through the analog switches)

I appreciate the changes that Oldway has made, and the reasons that he made them.


Jay_Diddy_B

[oldway]

That's the right way to develop a new design 
Looking for what already has be done, choosing the best solutions and improving them...
Again, thanks very much for sharing your work.
Few people are doing this on this forum.

(There is a d.c. path to ground for the capacitors C3 and C4. The path is through the analog switches)

I don't agree, at one side, there is no resistor to ground, only 2 diodes D4 and D3, and at the other side, only a high value resistor (R11 : 1.8MR)
In the earlier design, ground reference was done by the 1K resistor and the DUT itself....in your design, this ground reference does not exist anymore because C6 is insulating this side from the grounded DUT.

[zaoka]

We could use FLUKE 4W tweezers with this design if we knew where to get female terminals of this kind

http://us.flukecal.com/products/accessories/test-leads-probes-and-clips/tl2x4w-twz



Maybe just cut it and install 2 BNC's 

[oldway]

If i were a rich man...
Not a low cost solution for sure...
http://www.amazon.com/Fluke-TL2X4W-TWZ-Tweezers-Voltage-Current/dp/B00937VPPU
Only US§ 90   
My solution:
http://dx.com/p/multimeter-test-leads-75cm-red-black-leads-6518
Cost: US§ 1.91

[BravoV]

- A made 2 new versions, the first is allready working very well. I have still to make the board of the second one, but it's not that easy because I want to make a single side board project.

Any changes on the schematics ? Post the updated version and also share some photos once its finished, please.

[oldway]

- A made 2 new versions, the first is allready working very well. I have still to make the board of the second one, but it's not that easy because I want to make a single side board project.

Any changes on the schematics ? Post the updated version and also share some photos once its finished, please.

I already shared the schematics of the two versions, there is no update.
See my previous posts. (ESR3 schematic + board and ESR4 schematic)
I don't have any digital camera, nor webcam, that's the reason why I don't share photo's.
I have only a Praktica MTL3 and I have to make all the 24 poses of the film before I can have the prints...
Now you understand why my nickname is "OLDWAY"     

[BravoV]

Another bump, just want to thank Jay_Diddy_B for sending me the fully assembled ESR adapter kit he built, a special edition that is also hand tuned by the "Designer" himself    , and also a very cool, one of the kind in the world, a customized 3D printed box by Jaxbird made to fit in like a glove for this ESR adapter. 

Don't have enough words to explain the awesomeness when both combined, I guess I will let the photo speaks for it self.

Again, thank you very much to you both.   

I don't think I need to demonstrate it's capabilities since its proven, now purely just for the killer look.




A tiny improvement at the on/off switch so I don't forget to turn it off. 

[The Electrician]

BravoV, you are in a position to make an interesting test I have wanted to make since Jay_Diddy_B's first post in this thread.

He went to the trouble of using a phase sensitive rectifier so that his design would, as he said in post #1, "Be a true ESR meter as oppose to an impedance meter."

I'm very curious to know how well that feature works.

You have a known capacitor that can be used to test that feature.  In this post:

https://www.eevblog.com/forum/projects/reference-for-lcr-or-esr-meters/msg393364/#msg393364

The capacitor you have labeled "B" is a film cap, and its impedance is very different from its ESR at 100 kHz.  I didn't capture the exact sweep of the impedance/ESR for the capacitor I sent you, but I have 8 more of those caps, and here is a composite superposition of the sweeps of them:



They are quite consistent, and it's reasonable to assume that the cap I sent you has a characteristic near the ones shown.  That cap is over 6 uF so it should be within the meter's operating range.

Try to make the measurement with connection made as close as possible to the capacitor body.  Here are two sweeps showing the effect of making the measurement right at the capacitor body, and also with the full length leads of the capacitor:



So, if you would, what does the meter show for a measurement on this capacitor?

[dannyf]

"Be a true ESR meter as oppose to an impedance meter."

That will depend on how you define a "true ESR meter". The synchronized detector is able to integrate over the two halves and subtract them, to obtain a measure (really a proxy) of the esr. However, that differential is strictly speaking non-linear, as it varies, inversely, with the voltage across the dut - which for a small capacitor can vary significantly.

We minimize that linearity with fast switching frequencies (so that the dut doesn't get charge up too much), large current limiting resistors (more like a ccs), etc. But the effect is there.

Newer commercial units generally don't use that approach: they are mostly D/FFT driven or follows 3/4 parameter 1057 algorithms.

That's not to mention the cap's own mechanism on esr - our "serial" resistor model applied to a capacitor is idealistic to begin with.

I'm very curious to know how well that feature works.

Me too.

[The Electrician]

"Be a true ESR meter as oppose to an impedance meter."

That will depend on how you define a "true ESR meter".

I would define it to mean "a meter which displays the real part of the capacitor's impedance, as measured at a single frequency with sinusoidal excitation".  This is the desired functionality, and it is what professional grade impedance analyzers do.

Newer commercial units generally don't use that approach: they are mostly D/FFT driven or follows 3/4 parameter 1057 algorithms.

Could you please provide a link to such an instrument?  I'm unaware of them, and I'd like to have a look at the performance specs.

[dannyf]

"a meter which displays the real part of the capacitor's impedance, as measured at a single frequency with sinusoidal excitation"

I got the first part. Not sure why one would care how it is measured.

As to meters, Agilent makes a few network / impedance analyzers and I am sure others do (Hioki?)

Analog has had a few such chips that integrate signal generation, adc + dft on a single chip, with limited capabilities at both ends of the measurement range. They just announced a new chip that further integrates a cortex-m3 + associated afe together. No detailed datasheet yet but it would be interesting to see what can be done there.

[The Electrician]

"a meter which displays the real part of the capacitor's impedance, as measured at a single frequency with sinusoidal excitation"

I got the first part. Not sure why one would care how it is measured.

Because if it is measured with a square wave or pulse as most of the low cost "esr" meters do, that's not measuring impedance as it is understood in network analysis.  It's measuring some summation of "impedances" at the fundamental and harmonics of the applied excitation.

As to meters, Agilent makes a few network / impedance analyzers and I am sure others do (Hioki?)

What I see from Agilent using FFT techniques are combination VNA/impedance analyzers.  I'm aware that recent VNAs use FFT Techniques; my R&S portable VNA does.  Those instruments don't have the dynamic range a swept sine type analyzer has.  Hioki doesn't use FFT techniques in its analyzers.  The best performing impedance analyzers for frequencies in the low MHz range use swept sines and don't try to also be VNAs.

I've seen some special purpose impedance analyzers aimed at the audio business.  They use sound cards for excitation and FFT techniques to produce the results, but here wide dynamic range isn't needed.

[dannyf]

if it is measured with a square wave or pulse as most of the low cost "esr" meters do, that's not measuring impedance as it is understood in network analysis.  It's measuring some summation of "impedances" at the fundamental and harmonics of the applied excitation.

That's not necessarily true.

Synchronized detectors (typically runs off a square wave), for example, are true measurement of the real element of the impedance - with the caveats with discussed that are entirely due to implementation, not fundamental to the approach itself.

A pulse excitation can also be used to measure both real and imaginary parts of the impedance - think of it as a Dirac excitation on the system, and by analyzing how the system reacts to the excitation, you can indeed measure the impedance. Mathematically, a Dirac excitation is all you need to know to describe any linear system.

[BravoV]

@The Electrician, as requested, the measurement on the red cap at the ESR meter adapter, also results using the LCR meter MS5308.

First, the DMM was zeroed using one of the cap pin shorted across the two beefy measurement probes.




The red cap measurement result, and I didn't use 4 wires since the results were very close when using these two gold plated beefy banana connectors which conduct very good and also really near the circuit. 4 wires only needed when I use long wired alligator clips.




The red cap in series with a 100 mili Ohm resistor, to verify the resistance measurements consistency.





Results on the red cap using the LCR meter MS5308 at various frequencies.

[The Electrician]

Thank you, BravoV

That's a very good result.  6 milliohms for the Jay_Diddy_P meter, versus 9 milliohms for the MS5308.  The sweeps I show for the 8 remaining caps I have, suggest that 9 milliohms is likely a correct result.

Jay_Diddy_P's meter clearly distinguished the true ESR from the 239 milliohm impedance  He achieved his goal.

For comparison, the Atlas ESR70 reads 20 milliohms for this capacitor, and the MESR100 reads 89 milliohms

[Jay_Diddy_B]

Hi,

I have also done some testing with a film capacitor. I do not have the 'official' 6.8uF film capacitor. I used a 4.7uF 250V Metalized polypropylene film capacitor.

Here is a picture of the capacitor used for test:



This is has an extremely low ESR. I first measured the capacitor using my HP4274A LCR meter with a HP 16047A test fixture. Here are the measurements:



Note: That the device impedance is very reactive, >89.6 degrees at 100 kHz

Here a couple of sample pictures of the measurements:







When I connected the capacitor to the ESR adapter using the 4W configuration, I zeroed the meter using the relative feature on  the DMM.
I measured 5.355mV which corresponds to 53 m Ohms.



This is 0.26% of the ESR meter adapters full scale, and significantly lower than the impedance of the capacitor 340.7 m Ohms.



Regards,
Jay_Diddy_B

[The Electrician]

When looking at BravoV's results, I forgot that the output from your meter is not a one-to-one correspondence of millivolts to millohms.

His result was 61 millohms, not 6 millohms.

Still pretty good, though.  A lot better than just displaying the "impedance".

[BravoV]

Yeah, my mistake not mentioning its 61 instead of 6 miliohms, sorry.

With the full scale of ESR measurement capability max at 20 ohm, the resolution and accuracy at 100 miliohms as demonstrated in my measurement means it has 0.5% accuracy. By looking at the circuit cost and relatively simple to build, I think this performance is very good indeed.

[BravoV]

The main thing I see, if you can arrange the switches to come on for the central part of the square wave in each half cycle, the circuit will not see the effects of the caused by the inductance. I am trying to think of a simple way to generate the required signals.

Here is the model:



The switches S3 and S4 are turned on in the center of each half cycle. This is timing required for the switches:



The result:



The circuit is no longer sensitive to the inductor. The capacitive part is left, but it averages to zero.

Re-reading the fine thread, bumped on this again.

Academically, I am very-very curious and really like to build this someday just for fun. 

[AJ4OM]

Does this design to in-circuit readings?

[BravoV]

Does this design to in-circuit readings?

Yes.

[3roomlab]

hmmm so to trigger in between edges or blanking. use a 1Mhz clocking and trigger off from a decade counter? or maybe even 2Mhz with 2 decade counters?

also i got kinda lost looking at the HP readout chart vs the ESR adapter 5.3mv ... what is going on there?

[Jay_Diddy_B]

also i got kinda lost looking at the HP readout chart vs the ESR adapter 5.3mv ... what is going on there?

The impedance of a pure capacitor at frequency F can be expressed as:

Xc = 1/(2 x Pi x F x C)

So an ideal 4.7uF capacitor at 100 kHz has an impedance of:

Xc = 1/ (2 x Pi x 100,000 x 4.7E-6) = 339 mOhm

This is a vector quantity and can be written as:

Z=339 mOhm, Angle = -90 degrees

or

Z= -339m  jOhm


The capacitor has a resistive component, ESR, which is at 90 degrees to reactive component.

*** See later post. There are some maths errors. JDB ***

The total impedance


Z = 4m - 339mj Ohms

The magnitude is

|Z| = Sqrt ( R² + Xc²)

|Z|= Sqrt (4m + (339m)²) = 334.8 m Ohms

The phase angle = ArcTan -339m / 4m = -89.32 degrees

If the ESR meter was to read impedance, it would read |Z| which is 334.8 m Ohms.

If the ESR meter could read the ESR accurately it would read 2m Ohms.

The ESR adapter reads 53.55 m Ohms

Note: That is a particularly difficult ESR measurement. A 4.7uF electrolytic capacitor will typically have an ESR around 1 Ohm, which is much easier to measure.


Jay_Diddy_B

[3roomlab]

thanks for the very nice breakdown Jay

i understand the first part, ideal Z of the 4.7uF cap. straight forward equation.

i got lost again at the second equation, (R²+Xc²), the value of R comes from ... ? (but if R² = 4m, wouldnt R = 0.063? ... yep im really lost    hahaha)

i kind of understand where the equation is getting at, but i dont understand where the value 4milliohm (4m) is taken from? (as usual, its something right there that i couldnt comprehend lol)

i keep thinking there is something about the casing in bravoV pic ... OF COURSE ! its 3D printed ! wonderful arnt they? 3dprinting ... no longer would you need to hunt for a matching box ...

[Jay_Diddy_B]

thanks for the very nice breakdown Jay

i understand the first part, ideal Z of the 4.7uF cap. straight forward equation.

i got lost again at the second equation, (R²+Xc²), the value of R comes from ... ? (but if R² = 4m, wouldnt R = 0.063? ... yep im really lost    hahaha)

i kind of understand where the equation is getting at, but i dont understand where the value 4milliohm (4m) is taken from? (as usual, its something right there that i couldnt comprehend lol)

Hi,

The equation (R²+Xc²) comes from vector maths. The impedance of the capacitance is at 90 degrees to the resistance so you use Pythagoras' theorem to obtain the impedance.

The measured value of the ESR, the resistive part is 2m Ohms, (from the HP 4274A LCR meter).

I made a some mistake in the original calculations.

The impedance should be:

|Z| = sqrt ((2m x 2m) + (339m)(339m)) = 339m

This is because 2E-3 x 2E-3 = 4E-6, very small

The angle should have been:

ArcTan(-339m/2m) = 89.66^o  This agrees with the HP 4274A meter now 


This just demonstrates how hard it is to measure the ESR of the film capacitor.

Sorry for the mistakes in the math.

Jay_Diddy_B

[dannyf]

His math is messed up.

ESR=4m is presummed / measured earlier on that capacitor - it is very close to the 1-2mohm list earlier.

(serial) Impedance of the (ideal) capacitor is 339ohm, per calculation on the (presummed / measured?) capacitance. It is 90 degrees away from the ESR.

So the "combined" impedance of the ESR + ideal capacitor = squrt (4m^2 + 339m^2) = 339.0236mohm -> Xc so overwhelms the ESR.

[The Electrician]

Jay_Diddy_B, here's something you may want to try on your 4274.

I've noticed that even the best professional LCR meters begin to have trouble making an accurate measurement of the smaller part of an impedance when the ratio of the larger part to the smaller part begins to exceed 1000.  An example of this is when measuring the ESR of a very good quality polypropylene capacitor.

It would be good to have a way to test a meter, but with capacitors there's no way to be sure just how low the ESR is at low frequencies (which is where that ratio gets large (this is the Q in the case of a capacitor).

An alternative is to measure the inductance of a wirewound resistor.  A high value wirewound resistor measured at a low frequency provides a test.  Here's a picture of a suitable resistor I used.  It is a 10k ohm resistor, wound with very small diameter resistance wire.  This wire is so small that skin effect will not be noticeable up to several MHz:



Here's the result of a sweep of this resistor on the impedance analyzer.  The real part of the impedance is shown in yellow, dead flat at 10000 ohms.  The imaginary part (X) is shown in green and shows the expected behavior as we go down in frequency until we reach about 10 kHz, the frequency where Rs is 1000 times larger than X.  Below 10 kHz, the reactance curve is no longer the straight line we would expect--the meter is having trouble making the measurement.



This resistor has no ferromagnetic core and we can be sure that the inductance does not rise by several orders of magnitude at low frequencies, so if we plot the inductance vs. frequency over a range from 100 Hz to 1 MHz, the result should be a flat line.You can see that the "measured" inductance rises drastically at low frequencies.  Notice that the inductance begins its drastic rise about the time that the ratio Rs/X reaches 1000.  At larger ratios, the meter can't make an accurate measurement.

[dannyf]

when the ratio of the larger part to the smaller part begins to exceed 1000.

When the phase angle approaches 90 degrees, the calculation becomes tricky, particularly for 24-bit floating point math, and algorithm that uses tan()/atan(): the derivative of tan() at 89.9999 for example is close to 600K. A tiny bit of rounding will kill the precision.

If the integration is done in hardware, a tiny bit of timing off from turning on / off those switches will throw off the calculation.

This is where DFT/FFT or 1057 type algorithm is powerful - they are practically immune to that.

[The Electrician]

when the ratio of the larger part to the smaller part begins to exceed 1000.

When the phase angle approaches 90 degrees, the calculation becomes tricky, particularly for 24-bit floating point math, and algorithm that uses tan()/atan(): the derivative of tan() at 89.9999 for example is close to 600K. A tiny bit of rounding will kill the precision.

If the integration is done in hardware, a tiny bit of timing off from turning on / off those switches will throw off the calculation.

This is where DFT/FFT or 1057 type algorithm is powerful - they are practically immune to that.

Current Professional meters don't just use 24 bit floating point arithmetic; they use a decent processor with IEEE floating point--56 bit double precision, 80 bit extended precision.

The derivative of the tangent at 89.9999 degrees is 3.3*10^11; the tangent itself of 89.9999 degrees is 572958 (close to 600k).  No LCR meter tries to measure a phase angle of 89.9999 degrees.

Professional LCR meters don't use gated analog switches for phase detectors.  The schematics I've looked at show double balanced mixers with very accurate zero degree and 90 degree references.

[The Electrician]

The Wayne-Kerr 6440B is described by the manufacturer as able to measure very low D capacitors.

I did a sweep of the inductance of the same wirewound resistor as in the previous thread.  One can see that the 6440B doesn't begin to have problems until the frequency is below 1 kHz, which is about 10 times lower than the Hioki.  A good measurement is obtained even when the larger part of the impedance is 10,000 times the smaller part.  Note that the vertical scale is not logarithmic, but the frequency axis is:



Not many LCR meters can do this.  However, the 6440B is a low frequency instrument only; no RF measurements with it.

[Bryan]

Hi TorqueRanger and the group,

I have attached pdfs that should help DIY construction of the ESR meter adapter.

There is copper layer which has been mirrored for toner transfer. I have included a scale so that you can make sure the board is the correct size.
There is pdf showing the silk screen layer so you know where the components go.
I have also attached the latest version of the schematic.

Jay_Diddy_B

Hi Jay_Diddy_B:

I have a couple build questions. Is this the latest schematic?

What is the purpose of the potentiometer?. Is it to zero the DMM if the meter does not have a Relative feature.?

Can the LT6241CS8 be substituted with the  LT1498CS8. The LT6241CS8 is not available from Newark.

Are you able to provide the source for the PCB board, not sure what program you used. but would like to modify the PCB board. 

Cheers and thanks.
 

[xwarp]

Has anyone built one of the two shown in the quote below?

I'm interested in bread boarding one for fun, but can't make sense of some of the things pictured.

Oldway stated in a later post that ESR4 is updated to correct some things in ESR3, but unless I am reading something wrong, the dates on the schematics show that ESR3 is a later version than ESR4.

Also, ESR4 doesn't have the 10/100 khz switch as in ESR3.

Also, where do the leads connect in for testing a cap and where is the output from the unit to the meter?

Apologies if these are dumb questions.

My ESD tester works well.
Thank you to Jay_Diddy_B !

I made some changes: (see diagram ESR3)
- Test frequencies of 100 kHz and 10 Khz
- Only 2W...4W is not practical for such an ESD tester.
- Offset and the resistance of test cables are compensated  by setting to zero with a 20K potentiometer. It's no longer needed to use the "relative function" of the multimeter. (cheap 5 bucks multimeter can be used )
-choice of easy to buy and low cost components.
- fully protected to 100V (seems to be enough)
The PCB is single sided and the components are SMD.
Only one jumper was needed.
Consumption is about 7 mA.

I'am preparing a more sophisticated version without problem of delay and two ranges, one from 0 to 20R and a more accurate one from 0 to 2R. (see diagram)

[Shock]

Anyone have a spare or populated PCB made up?

[oldway]

As nobody has reacted anymore, I thought this was a dead topic and i did not make updates anymore.

Schematic ESR4 is the good one but modifications has still been made.

As schematic and layout must be consistent, I have not placed on the schematic the components who are not mounted on the board as potentiometers, terminals, switches, ...

That's the reason why you have some difficulties to understand this schematic.

[Jay_Diddy_B]

Anyone have a spare or populated PCB made up?

I have sent you a PM.

Regards,

Jay_Diddy_B

[3roomlab]

i wanted to see if i understood the concept of the meter, and so i tried it with a 4017 as a drive for the 4066. however i am not sure if it is a simulation problem, it seem to work in a weird way.

generally what i did is 1Mhz --> 4017 --> select pins to use to trigger/sense
using 6 of the output to split 1 cycle (of 100kHz) into 3 parts of +ve/-ve trigger (cyan waveform), and then 2 of the 3 parts as a "sense" trigger (magenta/blue waveform). did i do this in the correct way? (ignore the incomplete opamp at the sense end)

[Jay_Diddy_B]

i wanted to see if i understood the concept of the meter, and so i tried it with a 4017 as a drive for the 4066. however i am not sure if it is a simulation problem, it seem to work in a weird way.

generally what i did is 1Mhz --> 4017 --> select pins to use to trigger/sense
using 6 of the output to split 1 cycle (of 100kHz) into 3 parts of +ve/-ve trigger (cyan waveform), and then 2 of the 3 parts as a "sense" trigger (magenta/blue waveform). did i do this in the correct way? (ignore the incomplete opamp at the sense end)

Hi,

The original version that was described in the beginning of this thread and is presented in this message:

https://www.eevblog.com/forum/projects/esr-meter-adapter-design-and-construction/msg391885/#msg391885

works fine. It is certainly good enough to sort out good and bad capacitors in and out of circuit.

A proposal was made to improve the performance by blanking the measurement during part of the measurement cycle. One way to implement this is with a 4017, like you have done. I have not built this circuit with the blanking, because the improvement is probably academic.

My original version uses 74HC4053 for the analog switches. The HC part is important, they are significantly faster than the non HC versions.


If you are interested I suggest building the original version.

Regards,

Jay_Diddy_B

[hugo]

Hi Jay_Diddy_B:

What is the purpose (value) of the potentiometer R22 ?

Thanks

[Jay_Diddy_B]

Hi Jay_Diddy_B:

What is the purpose (value) of the potentiometer R22 ?

Thanks

The value of R22 is 500 Ohms.

R22 is used to adjust the ESR meter adapter. I typically use a 1 Ohm resistor and adjust R22 for an output of 0.1 volts.

I made a test fixture like this:





Regards,

Jay_Diddy_B

[SeanB]

I like that test fixture, very nice. When I built my ESR meter I just used some 1R resistors to write the calibration points on the meter face using a Rotring pen, using a 0.5R, 1R, 2R 5R and 10R calibration points on the non linear scale. 3R is about half scale, and it works good enough to test capacitors.

[Edwin G. Pettis]

The problem is not your meters, per se, with the exception of low resistance, the 'Q' of a wire wound resistor rapidly drops to virtually zero at low frequencies and higher values, approximately somewhere in the range of 50 to 150 ohms, the 'Q' drops below 1 and for all intents and purposes, there is no inductance, it is totally swamped by the resistance.  At higher frequencies, it is mostly parasitics that your meters are reading because the 'Q' of a wire wound resistors varies little with freqency.  I have used several different bridges in researching the inductance of wire wound resistors, including calculations of inductance based on actual windings of equivalent copper coils vs resistor alloys.  Have you ever noticed that good inductors always have low resistance to keep the 'Q' high?  When you replace copper with resistance alloys, the 'Q' plunges even for exactly the same size of wire and turns on the same core.  No 'Q', no inductance, there has been some arguments to the contrary but the measurements are what they are, unless you're using wire wound resistors at high frequencies (the effect varies with the type and resistance a lot), you aren't going to see inductance and what you're seeing is mostly parasitics of inductance and capacitance.  I did many measurements while I was at Ultronix (and Ultrohm Plus) plotting the effect of frequency on actual 'resistance/impedance', in most cases the DC resistance was mostly unchanged until the frequency was well over 20KHz, mostly over 50KHz or even 100KHz before parasitic effects showed up.

The inductance of wire wound resistors is mostly well overstated!

[Jay_Diddy_B]

Is R21 meant to be zero?

R21 is a zero Ohm resistor. It is used as a jumper. The layout is single-sided. The circuit is built on the back of the front panel.

Jay_Diddy_B

[DJMota]

Great proyect!
Jay_Diddy_B Where i can buy the pcb of this proyect?
Thank for share it!

[cat87]

Thank you Jay_Diddy_B

Just finished building the adapter this weekend and recently I had the opportunity to  test it out against a Hameg HM8118. This baby will do 75 KHz and 100KHz measurements and I was really pleased to see that for some caps, the adapter was spot on (<5% accuracy) which is pretty satisfying. For some other no-name caps, the readings were kind of off. I don't know why, but I suspect the caps were the ones at fault here, not the ESR adapter.
So, for a quick go-no go type of measurement, it's perfect.

[Jay_Diddy_B]

Thank you Jay_Diddy_B

Just finished building the adapter this weekend and recently I had the opportunity to  test it out against a Hameg HM8118. This baby will do 75 KHz and 100KHz measurements and I was really pleased to see that for some caps, the adapter was spot on (<5% accuracy) which is pretty satisfying. For some other no-name caps, the readings were kind of off. I don't know why, but I suspect the caps were the ones at fault here, not the ESR adapter.
So, for a quick go-no go type of measurement, it's perfect.

Thank you for your kind words.

Can you post a picture of your version?

Regards,

Jay_Diddy_B

[cat87]

Sure thing. Sorry for the delay, but I'm moving house right now, and things are...well, all over the place.

This is how mine turned out:

[lpc32]

Anyone knows of a similar ESR-to-voltage adapter available on eBay?

[Jay_Diddy_B]

Hi group,

I have used up all the PCBs from the original batch that I had made by iTead.

For these I paid a premium to get black boards. You can see pictures of the boards in this message:

https://www.eevblog.com/forum/projects/esr-meter-adapter-design-and-construction/msg372155/#msg372155

Questions

1) Would there be any interest if I made the blank board available?

2) Is worth the extra money to have it black instead of green?

3) Should I remove the 4 wire feature and make it 2 wires only?

I am not promising anything this just a quick survey.

I would ship by Canada Post. You can check the shipping charges to you location here:

https://www.canadapost.ca/cpotools/apps/far/business/findARate?execution=e1s1

Regards,

Jay_Diddy_B

[quarks]

Hello Jay_Diddy_B,

Great work
I think many of us would like to have such a nice ESR adapter from you

to your questions
1) yes
2) I would prefer black
3) I would prefer 4wire

Maybe you should make a poll for this

bye
quarks

[KD0CAC John]

Yes
Yes
No

[lpc32]

Hey Jay. Thanks for the design.

1) I was thinking initially of one of those $10-15 AVR Transistor Testers/component identifiers, so I'd prefer a populated device or in kit form. But a cheap enough board might still be interesting, especially thru-hole.

But I guess being in Canada makes it more expensive, combined with the cost of small scale production, and more per-item work/overhead required on your part. On the other hand, I think there should be a market for a complete cased device if priced right. On the other other hand, someone in China might start producing clones.

2) Functionality and price are more important to me than looks.

3) 4 wire as an option is better. Even if you don't use daily it doesn't add much to the BOM.

Speaking of BOM, maybe these cheapo 4mm jacks can work. Hopefully they're not too crappy:
Black: http://www.ebay.com/itm/221637907699
Red: http://www.ebay.com/itm/221606765590

Can anyone suggest an eBay/China-available cheap opamp alternative?

[LA7SJA]

Hello Jay_Diddy_B

I have made a through-hole veroboard version that sort of work, but I would like to build/buy two of your smd design. And a big thank you for getting me interested in LT-Spice.

Back to your questions.
YES I am interested in at least two pcb's.
YES I would pay extra for Black.
4W is the best! Maybe you could leave the 4W undrilled (or just a pilot hole) so the builder can deside when building and even "upgrade" at later stage.

Johan-Fredrik

[Shock]

I reread the thread to refresh.

1. I would still like to see you offer a kitset or built option as chasing the parts here in Australia is an expensive exercise. You could still do all three (kitset/built/pcb) if you really wanted to. I'd buy another prebuilt depending on inclusions to the design.

2. The black color looks good to me. But what percentage of the PCB cost (before shipping) are we talking here? An increase in a dollar is less significant to the buyer than it is to the seller.

3. I've not tested the 4W, but if the 4W accurately cancels out the impact of the 2 wire test leads and produces enough benefit (I'd also throw in testing resistors into this basket) then I think keep it. There is also room to make custom adapter boards (zif socket etc) keeping 4 sockets may add a bit of stability to doing this kind of thing.

As for Oldways suggestions:
A compensation trim pot, and a 10/100 switch, juggling a few components. Anything that improves the design without losing features or accuracy is a positive thing (obviously within the realms of cost and simplification). So if you feel you can improve the design overall go for it. If you have to trade off accuracy, overload protection, or a feature, you have to weigh up the pros and cons after comparing them.

[dabbler]

Hello,

first thank you for sharing this project. I made a (mostly) through-hole version and when I first tested it, it seemed to work. I was getting the 100mV for a 1ohm resistor (after minor tweak of the pot), a then tried a few different caps that appeared to have somewhat reasonable vals. Before the first test I also double and triple checked that everything was correctly connected etc..

So after the test I removed the battery again and left the circuit untouched (in the same location where I tested) for a day, until I could buy a plastic box to put it in. I put it in the box, soldered the 1-pol switch and connectors for test leads to the prepared wires, the same wires to which I had clamped the test components and DMM earlier. Really nothing there that could've caused any kind of issues.

I then went ahead to try it, again with the 1ohm resistor, but now everything was dead. I wasn't getting any readings. After checking the circuit it turns out the 78L05 seems dead. It's getting the 9V in, but 0 comes out. So, first time it worked, I even measured the output during my first test, then without having done anything inbetween that in any way should be able to affect the functionality, the volt. reg. has died.

Now, I'm very amateur. If some device, typically older, breaks down I usually check for bad caps. I figured this tool could help me with that. Otherwise my usual "constructions" are in the form of a microprocessor and a few surrounding components, so my skills to determine what could've gone wrong are limited. Googling what might cause the volt. reg. to fail, the only normal thing I could find was that they don't like reverse current/voltage and typically you're suggested to add one or two diodes to prevent this.

The ua78L05 datasheet (http://www.ti.com/lit/ds/symlink/ua78l05.pdf) confirmed this, in section 8.2.2, and also mentions it can happen during startup. I'm not seeing this kind of protection in the ESR meter circuit, so I'm wondering is that reverse voltage situation not possible here? If not, does anyone have any idea what else could break the regulator? Could I add those diodes only and have everything else still working without changes?

Any hints would be greatly appreciated.

(I do have one regulator left, but it feels like simply replacing it doesn't fix the root cause and only risks breaking that as well. Then I'd have a problem because ordering new ones within forseeable future isn't in the books with the rediculous shipping costs around here.)

[Shock]

Test it out of circuit or isolated it in circuit so you can check if anything is pulling the output down. Then should should check everything else in the circuit, dozen resistors, handful of caps and diodes, easy.

Add the diode if you want. To test measure a few known resistors individually or a length of wire (something consistent). Then add the two resistors in series or parallel and see if they add up and makes sense (or double the length of wire). I think you get the idea.

Should you not know the wrath of your bench supply (overshoot and such) use a battery.

[ZeTeX]

Hello,

first thank you for sharing this project. I made a (mostly) through-hole version and when I first tested it, it seemed to work. I was getting the 100mV for a 1ohm resistor (after minor tweak of the pot), a then tried a few different caps that appeared to have somewhat reasonable vals. Before the first test I also double and triple checked that everything was correctly connected etc..

So after the test I removed the battery again and left the circuit untouched (in the same location where I tested) for a day, until I could buy a plastic box to put it in. I put it in the box, soldered the 1-pol switch and connectors for test leads to the prepared wires, the same wires to which I had clamped the test components and DMM earlier. Really nothing there that could've caused any kind of issues.

I then went ahead to try it, again with the 1ohm resistor, but now everything was dead. I wasn't getting any readings. After checking the circuit it turns out the 78L05 seems dead. It's getting the 9V in, but 0 comes out. So, first time it worked, I even measured the output during my first test, then without having done anything inbetween that in any way should be able to affect the functionality, the volt. reg. has died.

Now, I'm very amateur. If some device, typically older, breaks down I usually check for bad caps. I figured this tool could help me with that. Otherwise my usual "constructions" are in the form of a microprocessor and a few surrounding components, so my skills to determine what could've gone wrong are limited. Googling what might cause the volt. reg. to fail, the only normal thing I could find was that they don't like reverse current/voltage and typically you're suggested to add one or two diodes to prevent this.

The ua78L05 datasheet (http://www.ti.com/lit/ds/symlink/ua78l05.pdf) confirmed this, in section 8.2.2, and also mentions it can happen during startup. I'm not seeing this kind of protection in the ESR meter circuit, so I'm wondering is that reverse voltage situation not possible here? If not, does anyone have any idea what else could break the regulator? Could I add those diodes only and have everything else still working without changes?

Any hints would be greatly appreciated.

(I do have one regulator left, but it feels like simply replacing it doesn't fix the root cause and only risks breaking that as well. Then I'd have a problem because ordering new ones within forseeable future isn't in the books with the rediculous shipping costs around here.)

Have you put large output capacitance? Over 22uF? Try to put all protection requird for the regulator.

Sent from my Nexus 5X using Tapatalk

[dabbler]

Well, I feel like the biggest doofus right now... That must've been the dumbest chain of events. Please disregard my post above.   

But thanks for the replies!

[dabbler]

I also wanted to note that some resistors in the BOM from "Construction Notes 2.pdf" in this post have conflicting values with their counterparts in the schematics of the same post.

R3: 6.8k in BOM - 6.2k in schematic
R6: 1.6k in BOM - 1.3k in schematic
R8, R17: 475 in BOM - 470 in schematic

I don't know what impact that would have if any, but it could be a bit confusing to someone like me and even causing the purchase of the wrong components (again for someone like me ).

[Jay_Diddy_B]

I also wanted to note that some resistors in the BOM from "Construction Notes 2.pdf" in this post have conflicting values with their counterparts in the schematics of the same post.

R3: 6.8k in BOM - 6.2k in schematic
R6: 1.6k in BOM - 1.3k in schematic
R8, R17: 475 in BOM - 470 in schematic

I don't know what impact that would have if any, but it could be a bit confusing to someone like me and even causing the purchase of the wrong components (again for someone like me ).

R3 sets the operating frequency. Traditionally 100kHz is used for ESR measurements. A small difference in frequency does not change the ESR reading.

R6 is used to centre the calibration pot. You need to change R6 if you are unable to calibrate the adapter.

475 versus 470  The small change in value comes from 1% resistors come in E96 values (475) and 5% resistor in E12 and E24 values (470)
Either value will work.

Regards,

Jay_Diddy_B

[Shock]

Well, I feel like the biggest doofus right now... That must've been the dumbest chain of events. Please disregard my post above.   
But thanks for the replies!

What happened?

[dabbler]

Turned out the (brand new) on/off slide switch is junk. Despite having checked it with a DMM prior to use, just to double check the pin config, once it was connected and mounted its function is glitchy. Sometimes it turns on more often not, when wiggling it slighty on on-position it goes on and off.

What must have happend was that I connected the DMM leads, turned it on and measured the 9V on the regulator input. Fine. So I turned it off again, moved the test lead to the regulator output while off, to avoid accidental short circuitnig, turned on the switch again and got 0V output. Having already tested the switch prior to use it didn't for one second occur to me that there could be a problem there.

[Lassivv]

Hi all

Interested to build this ESR meter. Just thinking is there any place where i find part list to this? Shematic i see most components, but not get right package sizes and is there example some very accurate tolerance resistors etc?

I think i use Farnell.com to order parts what i need and think if i do that circuit board on china because not have devices to do circuit board my home or work

I am very happy every tips and big thanks To Jay_Diddy on whole project.

edit: Can this meter use circuit directly without remove caps out of circuit?

[Jay_Diddy_B]

Hi all

Interested to build this ESR meter. Just thinking is there any place where i find part list to this? Shematic i see most components, but not get right package sizes and is there example some very accurate tolerance resistors etc?

I think i use Farnell.com to order parts what i need and think if i do that circuit board on china because not have devices to do circuit board my home or work

I am very happy every tips and big thanks To Jay_Diddy on whole project.

edit: Can this meter use circuit directly without remove caps out of circuit?

Look at the zipfile attached to this message:

https://www.eevblog.com/forum/projects/esr-meter-adapter-design-and-construction/msg342045/#msg342045

Most of the information you need is in this file.

Yes, it will work in-circuit, with the usual limitations.

Ask again if you need any clarifications.

Regards,

Jay_Diddy_B

[Lassivv]

Ok thanks for fast response. I think is there protection charged caps or do i need to empty capacitors with resistor before plug this meter there? Of course thats always normal way to empty capacitors before, but is this goes brokenif not remember do that? (i mostly talking low voltage secondary side caps).

Any specifield needs multimeter what to use with this meter. I now use Fluke 79 III is that good enought to this?

edit: Can i use some low voltage caps, resitors etc on normal part list. (C1, C3, C4, C7, C8, C9) Example 50v caps X7R 10%? And resistors i think can use normal resistors (tolerance 1%)?

R21 need to be some resistor close to 0R? Example 0.13ohm?

Anyone use some low voltage drop regulator there easier use with batteries? (I think use two lion cells (about 6.4-8.4v), this regulator  stop working correctly 7volts? Example this one: http://uk.farnell.com/richtek/rt9058-50gx/ldo-fixed-5v-0-1a-sot-89-3/dp/2377642

Lions are protected undervoltage situations. Just think if this LDO regulators are not that accurate that normal linears, if that so i keep that linear regulator what is default part.

[Jay_Diddy_B]

Ok thanks for fast response. I think is there protection charged caps or do i need to empty capacitors with resistor before plug this meter there? Of course thats always normal way to empty capacitors before, but is this goes brokenif not remember do that? (i mostly talking low voltage secondary side caps).

This ESR meter adapter is fairly unique, the meter adapter was designed to read the ESR of the capacitors without having to discharge them. This is achieved by using ac coupling for the measurement. C5 and C6 are the coupling capacitors. For safety it is better to discharge the capacitors been tested.

Any specific needs multi-meter what to use with this meter. I now use Fluke 79 III is that good enough to this?

The Fluke 79 III will be fine. Meters that have a relative feature, make it a little easier to use. Without the relative feature you will have to subtract the offset. This isn't a big issue, because bad capacitors are normally so high that there is no need to worry about the small offset.

edit: Can i use some low voltage caps, resistors etc on normal part list. (C1, C3, C4, C7, C8, C9) Example 50v caps X7R 10%? And resistors i think can use normal resistors (tolerance 1%)?

R21 need to be some resistor close to 0R? Example 0.13ohm?

I have attached a spreadsheet with more details on the parts.
R21 is used as jumper. You can buy a zero ohm resistor for this. It is only needed because the layout is single-sided without vias. You can use a low value resistor, 10 Ohms or less should be o.k.

Anyone use some low voltage drop regulator there easier use with batteries? (I think use two lion cells (about 6.4-8.4v), this regulator  stop working correctly 7volts? Example this one: http://uk.farnell.com/richtek/rt9058-50gx/ldo-fixed-5v-0-1a-sot-89-3/dp/2377642

Lions are protected undervoltage situations. Just think if this LDO regulators are not that accurate that normal linears, if that so i keep that linear regulator what is default part.

It should be o.k. to use a different LDO. There are more modern parts than the uA78L05 that was used on the prototype. Check that the pinout is compatible and the input and output capacitor requirements.

Typically an ESR meter is  only used occasionally, so there is little benefit to using rechargeable batteries.

Regards,

Jay_Diddy_B

[panoss]

Jay_Diddy_B thank you so much for publishing this project!
I' m going to build it but I don't know which is the 'suggested' version of PCB.
Is it the one at this post? (4053_ESR HAMMOND 1591L DIY.pdf)

(it 's different from the PCB in your 1st post)

[Jay_Diddy_B]

Jay_Diddy_B thank you so much for publishing this project!
I' m going to build it but I don't know which is the 'suggested' version of PCB.
Is it the one at this post? (4053_ESR HAMMOND 1591L DIY.pdf)

(it 's different from the PCB in your 1st post)

There are several versions of the PCB. All the layouts are essentially the same. They have different outside dimensions, to fit various boxes.
The Hammond 1591L box will take a board that around 50mm wide. Many of the low cost PCB manufacturers have special rates for boards that are 50mm x 100mm.
The original board was wider than 50mm and did include the calibration potentiometer. This is shown in this message:

https://www.eevblog.com/forum/projects/esr-meter-adapter-design-and-construction/msg341771/#msg341771

The version included in this message, does not include the adjustment potentiometer:

https://www.eevblog.com/forum/projects/esr-meter-adapter-design-and-construction/msg342045/#msg342045


After the first board was made on the an LPKF Protomat c60, I had some boards made by iTead. These were designed to fit a smaller box. This board can be seen in this message. This board contains the adjustment pot:

https://www.eevblog.com/forum/projects/esr-meter-adapter-design-and-construction/75/



This message contains the artwork for a DIY version. It has the artwork mirrored so it is ready for toner transfer:

https://www.eevblog.com/forum/projects/esr-meter-adapter-design-and-construction/msg391885/#msg391885


I have attached a zipfile to this message with the latest version of the Gerber files for the Hammond 1591L box.



Let me know if you have any questions.

Regards,

Jay_Diddy_B

[pgs]

Hi everybody.
Jay_Diddy_B
Yoy 're writing: 'If I plot Vout versus ESR, I get:'.
This is what I 'm trying to do with the LT SPice file, the '4053 esr meter.asc' you have uploaded.
How can I do this simulation, Vout versus ESR?
Thank you in advance.

[Jay_Diddy_B]

Hi everybody.
Jay_Diddy_B
Yoy 're writing: 'If I plot Vout versus ESR, I get:'.
This is what I 'm trying to do with the LT SPice file, the '4053 esr meter.asc' you have uploaded.
How can I do this simulation, Vout versus ESR?
Thank you in advance.

pgs and the group,


First, let me welcome pgs to the Forum.

When the thread was started the forum would not allow LTspice files as attachment. So the simulation that you are writing about is included in the zipfile attached to the first message in this thread.

Since the forum rules have changed and now allow .asc files as attachments I have attached the file below.


The LTspice file includes:



.step param ...

This causes LTspice to run the simulation multiple times with different values of the specified parameter. In this case ESR.

.meas ...

This statement causes LTspice to save the average output voltage with a variable name output for each of the steps defined above.

When the simulation is Run, you run the simulation in the normal way, the simulation will run as many times as there are parameter steps. In this case 9 steps.

When all the simulations are finished.

Click View -> SPICE Error Log.

Right Click anywhere in the new window.

Click 'Plot Step'ed .meas data'

And the result will be shown.


Let me know if this helps.

Regards,

Jay_Diddy_B

[pgs]

It worked fine! Thank you!

[pgs]

You also wrote:
'I wanted to make sure that the adapter is not damaged if it is connected to a charged capacitor. To demonstrate this a switch is used to connect the adapter to a charged capacitor, the charged capacitor is connected at t=2ms'.

1. Why did you use a switch (S5, MySwitch) to connect the adapter to a charged capacitor and you didn't connect it directly without a switch?
2. The charged capacitor is illustrated by V3, right? But the voltage of V3 goes to the two pins of S3.
That is: to GND (logical) and to the bottom of R4 (non logical for me)!
I would connect V3 at GND and top of C1.
Could you explain a bit?
3. V3 is a pulse which begins with -2V and after 2milliseconds goes to 2V. Stays at 2V for 5milliseconds and then falls.
So, where do the 400V, that we see accross the terminals, come from? Why did you put 2V and not 400V?

[Jay_Diddy_B]

You also wrote:
'I wanted to make sure that the adapter is not damaged if it is connected to a charged capacitor. To demonstrate this a switch is used to connect the adapter to a charged capacitor, the charged capacitor is connected at t=2ms'.

1. Why did you use a switch (S5, MySwitch) to connect the adapter to a charged capacitor and you didn't connect it directly without a switch?
2. The charged capacitor is illustrated by V3, right? But the voltage of V3 goes to the two pins of S3.
That is: to GND (logical) and to the bottom of R4 (non logical for me)!
I would connect V3 at GND and top of C1.
Could you explain a bit?
3. V3 is a pulse which begins with -2V and after 2milliseconds goes to 2V. Stays at 2V for 5milliseconds and then falls.
So, where do the 400V, that we see accross the terminals, come from? Why did you put 2V and not 400V?

S5 is used as a switch to simulate connecting the leads to a charged capacitor. If the capacitor was connected at the start of the simulation we would not be able to see the transient caused by connecting the capacitor.

The charged capacitor is not modelled by V3. The charged capacitor is modelled by the capacitor C1. The capacitor is charged to 400V by the statement:

IC=400

initial conditions equals 400V.

Think of the switch S5 as being similar to a relay or a solid state relay. The main terminals are on the top and bottom. The terminals on the side are the controlling terminals, (think relay coil).

The V3 is used to control the timing of the switch.

This model statement describes the behaviour of the switch:

.model MySwitch SW(Ron=0.01 Roff=100Meg Vt=0 Vh=-.5 )

The resistance when on is 10m and resistance off is 100meg 
The threshold is 0V
The hysteresis is negative 0.5V. This means the switch will switch smoothly from 100MEG to 10m when the input is between -0.25V and +0.25V. This means the switch doesn't 'snap'.

Regards,

Jay_Diddy_B

[lisafig]

The original board was wider than 50mm and did include the calibration potentiometer. This is shown in this message:

https://www.eevblog.com/forum/projects/esr-meter-adapter-design-and-construction/msg341771/#msg341771

The version included in this message, does not include the adjustment potentiometer:

https://www.eevblog.com/forum/projects/esr-meter-adapter-design-and-construction/msg342045/#msg342045

Does it means that the new version doesn't need a potentiometer?

[Jay_Diddy_B]

Hi,
Sorry about delay in replying, I didn't see the question.

The prototype:



This is the first unit I made. This does not have a potentiometer. I calibrated the unit by selecting one of the resistors.

The later units I made, using boards from iTead, all had a potentiometer, R22, as shown here:



Regards,

Jay_Diddy_B

[lisafig]

Thanks Jay_Diddy_B! By the way, I read in the forum that you were making prebuilt esr meter adapter. Are you still making them or do you have, by chance, an unsold one liying somewhere begging for some action in its life?

[Tek Tech]

Very clever. Thanks for generous sharing of your intellectual property!

BTW, if you sold this as a kit, I would be a buyer.

[Jay_Diddy_B]

Hi group,

Somebody asked me:

I want to know if C1 C5 C6 must choose the exact capacitance value and withstand voltage value?
(500V withstand voltage chip resistor is difficult to find)

I assume that an error capacitor is used, does it affect the results?


The BOM was supplied in this message:

https://www.eevblog.com/forum/projects/esr-meter-adapter-design-and-construction/msg1399602/#msg1399602

The voltage rating of C1 is not important.

The voltage rating of C5 and C6 impacts the maximum voltage that can be applied to the ESR meter adapter without damage. I used 500V parts. These are available from Digikey.

If you use lower voltage capacitors the maximum voltage is limited by the rating of the capacitors.



Regards,
Jay_Diddy_B

[daisizhou]

Does anyone know how to determine the resistance of R6 and r22?I can also use R6=1.2k ohms.

I hope to get the correct calibration method

[Shock]

Does anyone know how to determine the resistance of R6 and r22?I can also use R6=1.2k ohms.
I hope to get the correct calibration method

R6 in that last schematic posted was 1.3k which means if you have a 500 ohm pot you will have 100 less ohms in calibration range. If you ran into problems you could just add 100 ohms more in series it's not a big deal from what I see.

[mixiom]

Hello, I too build this nice meter and it seems to work. But the output voltage looks not very smooth - is that normal? My multimeter shows valid DC values when I use it with the esr-meter, but my Arduino does not get correct values from it, thats why I "investigated" the output waveform with an oscilloscope.
I expected the output waveform to look a bit more "straight"/rectified. Does anybody know what is going on, is that normal or perhaps do you straight on see that I somewhere made an error in the build process? Thank you!

[Jay_Diddy_B]

Hello, I too build this nice meter and it seems to work. But the output voltage looks not very smooth - is that normal? My multimeter shows valid DC values when I use it with the esr-meter, but my Arduino does not get correct values from it, thats why I "investigated" the output waveform with an oscilloscope.
I expected the output waveform to look a bit more "straight"/rectified. Does anybody know what is going on, is that normal or perhaps do you straight on see that I somewhere made an error in the build process? Thank you!

Hi Mixiom and the group,

The original design of the ESR Meter Adapter uses a 5V regulator and a rail splitter to generate +/-2.5V supply rails. This is fine because the DMM used to read the output of the adapter is floating.

How are you connecting the power supplies to the adapter and the Arduino? Can you post a schematic?

Regards,

Jay_Diddy_B

[mixiom]

Hi!

I may have explained my problem in a wrong way. That weird waveform is always at the measurement points (where your multimeter probes connect) when I have a device-under-test connected to the 2W connectors. But my multimeter displays a plausible, rock solid value none the less. It is when I try to replace the multimeter with my Arduino that I have problems, because the Arduino receives no smooth, but very fluctuating values. I totally assumed that the esr-meter has for example 100mV flat DC on the output when a device-under-test has an ESR of 1 Ohm. Perhaps the esr-meter requires an output device that does big voltage averaging, which i guess a multimeter does behind the scenes! If that is correct I would have to implement some averaging in software for the Arduino to display valid results.
The last picture above shows the Vrms and Vavg conforming to my multimeter values (plus some offsets).
But I am curious what the waveform on a know-good esr-meter looks like (at the output/voltagetestprobe connectors); if they are similar to mine or smooth DC.

You asked for my setup: The esr-meter is powered by 9V battery and Arduino by USB from Laptop, but that waveform is present with only multimeter connected too. (The DMM averages the stuff I guess, my Arduino software doesnt yet.)

Ciao



Edit: I included a painting that maybe explains the situation

[Jay_Diddy_B]

Mixiom,

I just measured one of my units. Here is the 1 waveform:




It looks very similar to yours.

Regards,
Jay_Diddy_B

[Jay_Diddy_B]

Mixiom,

Here is the waveform with 10 :





I am not sure what is causing this. It could be the transient response of the LDO.

In any case a simple RC filter should take care of this. Set the frequency to be 1.6kHz 1k and 0.1uF capacitor.

Regards,

Jay_Diddy_B

[mixiom]

Thank you, the filter works nicely! Now I can add one of those ebay OLEDs to the unit and Arduino takes care of removing offset etc.  Wonderful project of yours JayDiddy!

[daisizhou]

I also made a similar resistance calibrator.During the calibration process, I found a problem.Whether the measured value is accurate?
I tried to adjust the 500 ohm variable resistor, but the effect is not obvious.Is it my installation failure or is the circuit originally like this?

[tmf]

Has anyone created a PCB for this??

Thanks!

[Jay_Diddy_B]

I also made a similar resistance calibrator.During the calibration process, I found a problem.Whether the measured value is accurate?
I tried to adjust the 500 ohm variable resistor, but the effect is not obvious.Is it my installation failure or is the circuit originally like this?

Hi,

I just measured one my ESR meter adapters.

I first use a zero  standard like this:




With the short in place, I pressed the relative button on the DMM.


I used a resistance 'standard' like this one:



and



I measured the actual values of the resistors with a Keithley 2001 in the 4W mode.


I then use the ESR meter adapter to measure some of the resistors.



There is good agreement with the actual values.

Regards,

Jay_Diddy_B

[Jay_Diddy_B]

Hi group,

Here are few more pictures:

The zero Ohm standard




You use this so you are measuring a very short, very wide, pcb trace.





You use the short like this.

Jay_Diddy_B

[BravoV]

Love the idea & implementation of that simple resistance standard. 

Going to make one as all I need is just bunch of resistors, the test point inserts and a piece of single sided blank PCB and sharp cutter. 

[daisizhou]

This is what I made.I will short the 4 clips (as shown).Is this wrong?

[daisizhou]

I adjusted R22 and R6, the effect is not obvious, I don't know why?Need me to get an oscilloscope waveform?

[daisizhou]

[ Specified attachment is not available ]More than 100 milliohms

[Jay_Diddy_B]

daisizhou.

With the connections that you have in the picture, press the REL on the Fluke meter.

Now connect a 10 1% resistor to the adapter. Adjust the potentiometer for a reading on the meter of 1.000V (corresponding to 10 ).

The adapter is now adjusted and ready to use.

You need to the zero adjustment in the future. Short the leads and press REL on the Fluke DMM.

You are not just zeroing the leads, but the offset from the opamp in the adapter.

Regards,

Jay_Diddy_B

[daisizhou]

Yes, I am also adjusting this way.But I adjusted the R22 potentiometer and the multimeter value did not change much.
I don't know where the fault is?Actual measured values are too large

[Jay_Diddy_B]

daisizhou,

Try this procedure:

1) set R22 in the middle of range. It is a 500 pot so this is about 250

2) Short all the inputs together. Press REL on the DMM to remove the offset.

3) connect a 10 resistor to the test terminals.

4) Measure the voltage on the DMM

5) The DMM should read around 1.00V

The total resistance in the circuit is:

R4 + U2B(on) + R6 + R22 + R7 + R18

470 + 80 + 1.3K + 250 + 100 +100 = 2300

This is the total resistance in the path.

So if you are 5% high, say 1.05V, you need to increase the path by 5% or 115

so change R6 from 1.3K to 1.5K

Regards,

Jay_Diddy_B

[daisizhou]

nice i succeeded .
Very good effect.
Is there an upgrade plan for the circuit? Such as measurement accuracy, and so on...

[Jay_Diddy_B]

nice i succeeded .
Very good effect.
Is there an upgrade plan for the circuit? Such as measurement accuracy, and so on...

I have no plans to make any improvements. For the following reasons:

1) This adapter is intended for troubleshooting and repair. A bad capacitor will have an ESR several times larger than a good one.
2) ESR is generally specified by manufacturers as a maximum value. A new capacitor is typically 1/3 or 1/2 of the maximum value.
3) ESR is temperature dependent.
4) The ESR meter adapter, presented here, has a lot of protections against damage from charged capacitors and applied voltage. A typical LCR meter will not have these protections.

If I need better accuracy I use an HP4274A LCR meter.

The DER-5000 is a reasonably priced LCR meter widely available on eBay.

What level of performance do you desire?
Why do you need these accuracy?

Regards,
Jay_Diddy_B

[daisizhou]

I am going to measure the internal resistance of a lithium battery, such as the 18650 battery that is now widely used.
In amateur conditions, I often repair these batteries.Such as sweeping robots, remote control aircraft
In practice, these batteries are all connected in series.As long as one section of the link is damaged, the whole system will not work.
I hope to use this tool to identify the batteries that can be used and the damaged batteries.
(Battery internal resistance is generally 30 milliohms)

[daisizhou]

Hello, have you measured the internal resistance of the 18650 battery?
I found that measuring the internal resistance of the 18650 battery with this tester is very inaccurate.
I am checking, I don't know where the problem is.
I use a 1 milliohm resistor and a 10 milliohm resistor and a 2.2 milliohm resistor as a standard.
Using these resistance measurements, multiple tests, the effect is very good,The data is accurate
But measuring the 18650 battery is not accurate.

[Jay_Diddy_B]

Hello, have you measured the internal resistance of the 18650 battery?
I found that measuring the internal resistance of the 18650 battery with this tester is very inaccurate.
I am checking, I don't know where the problem is.
I use a 1 milliohm resistor and a 10 milliohm resistor and a 2.2 milliohm resistor as a standard.
Using these resistance measurements, multiple tests, the effect is very good,The data is accurate
But measuring the 18650 battery is not accurate.

Hi,

Battery impedance is different than capacitor ESR. It is frequency dependant. It is explained here:

Link: https://batteryuniversity.com/learn/article/how_to_measure_internal_resistance

Much better than I can explain it.

It includes the comment:

For example, Li-ion in an 18650 cell produces about 36mOhm with a 1,000Hz AC signal and roughly 110mOhm with a DC load. Since both readings are valid, yet far apart, the user must consider the application.



I don't think the ESR adapter described in this thread is directly suitable for the measurement.

Thinking ….

Regards,
Jay_Diddy_B

[Jay_Diddy_B]

Hi,

I am going to show a few quick measurements that I made on a Li-ion cell. This is the cell that I tested:





This a PKCELL 2200mAh ICR18650 cell. It is a few years old. I gave it a quick charge at 4.2V before I did the testing. The battery was probably around 20% depth of discharge (80% full).

HP4328A Milliohmmeter

This an old school meter that use 1kHz sinewave excitation. The meter was set on the 100m scale. This conforms to the 1kHz test method described in the Battery University webpage.
The measured ESR was 79m   Corrected, see messages below, 69m .








Electronic load and oscilloscope


The battery was connected to an electronic load. A Tektronix current probe was used to monitor the current. This is the green trace.
The battery terminal voltage was measured, ac coupled, cyan trace.
The load was set to go between 0.25A and 1.25A, 1A pk-pk.


1 kHz




The peak to peak voltage is 76mV. A resistance of about 75m


10 Hz






The peak to amplitude increased to 98mV. The indicated ESR = 98m


LTspice Model

A quick LTspice model with similar behavior:





And the modeling results:





This set of test shows that measuring battery ESR different ways, you get different answers.

Regards,
Jay_Diddy_B

[Shock]

My impression of ESR internal resistance testing of batteries was only for comparative testing anyway to determine the approximate aging effects, of new vs old. Like capacitors (or any component really if you consider it's variable testing conditions) the results if reproducible on single instrument aren't guaranteed to line up between instruments. But if the measurement is reproducible on the one instrument and varies between different DUTs enough to characterize good vs bad or somewhere in the middle, as far as I'm concerned job done. Otherwise if you want like for like testing then use the same testing method that defined the specification.

Btw Jay_Diddy_B that HP meter looks to be reading 69 milliohms not 79.

[kripton2035]

Btw Jay_Diddy_B that HP meter looks to be reading 69 milliohms not 79.

+1

[kripton2035]

But if the measurement is reproducible on the one instrument and varies between different DUTs enough to characterize good vs bad or somewhere in the middle, as far as I'm concerned job done.

+1

[Jay_Diddy_B]

Hi,

It is a correct observation that the ESR of cells can only be compared if the test method is the same. If the measurement is being used for selecting or matching cells  stick to one method.

The popular methods are:

1) a dc measurement. You step the load current between two values and measure the change in terminal voltage with a DMM. From change in voltage divided by the change in current you can arrive at the ESR.

This method is probably the best method because it is similar to the intended application.

2) You can measure the  ESR using 1 kHz sinewave, with an instrument like HP 4328A. You can use other 4-wire LCR meters if use blocking capacitors.
Keysight suggests:



3) Battery Chemists will use electrochemical impedance spectroscopy and measure the real and imaginary parts of the battery impedance. This gives them insight into what is happening inside the cell.



The impedance changes with:

• temperature
  state of charge
  operating point
  aging

etc.


They would use a frequency response analyzer, FRA, to do these measurements.

4) if you have an electronic load like the one I describe in this thread:

link: https://www.eevblog.com/forum/projects/dynamic-electronic-load-project/

and oscilloscope or even a DMM you can compare cells. You can do static dc tests or AC 1 kHz comparison tests.


Regards,
Jay_Diddy_B

[kripton2035]

Damit ! the 74hc4053 model in kicad is wrong ! pins 14 and 15 are inverted.
my pcb just arrived from china and is wrong too ...

[Jay_Diddy_B]

Damit ! the 74hc4053 model in kicad is wrong ! pins 14 and 15 are inverted.
my pcb just arrived from china and is wrong too ...

That is unfortunate ..

here is the bad code:

Code: [Select]

1 EESchema-LIBRARY Version 2.3
2 #encoding utf-8
3 #
4 # 74HC4053
5 #
6 DEF 74HC4053 U 0 40 Y Y 1 F N
7 F0 "U" -50 750 60 H V C CNN
8 F1 "74HC4053" -50 -550 60 H V C CNN
9 F2 "" 0 0 60 H V C CNN
10 F3 "" 0 0 60 H V C CNN
11 DRAW
12 S -350 600 450 -300 0 1 0 N
13 X 2Y1 1 650 150 200 L 50 50 1 1 B
14 X 2Y0 2 650 250 200 L 50 50 1 1 B
15 X 3Y1 3 650 -150 200 L 50 50 1 1 B
16 X 3Z 4 650 -250 200 L 50 50 1 1 B
17 X 3Y0 5 650 -50 200 L 50 50 1 1 B
18 X E# 6 -550 -250 200 R 50 50 1 1 I
19 X VEE 7 -550 100 200 R 50 50 1 1 W
20 X GND 8 -550 0 200 R 50 50 1 1 W
21 X S3 9 -550 350 200 R 50 50 1 1 I
22 X S2 10 -550 450 200 R 50 50 1 1 I
23 X S1 11 -550 550 200 R 50 50 1 1 I
24 X 1Y0 12 650 550 200 L 50 50 1 1 B
25 X 1Y1 13 650 450 200 L 50 50 1 1 B
26 X 1Z 14 650 350 200 L 50 50 1 1 B  [color=red]… this wrong J_D_B
[/color]27 X 2Z 15 650 50 200 L 50 50 1 1 B    [color=red]… this wrong J_D_B
[/color]28 X 16 VCC -550 200 200 R 50 50 1 1 W
29 ENDDRAW
30 ENDDEF
31 #
32 #End Library

This may have been fixed, see this link:

https://github.com/alexisvl/kicad-schlib/commit/d514c0f8439e177c63e06c8c35dd6111535f07aa

Hopefully you can fix the board with a jumper.

Regards,
Jay_Diddy_B

[kripton2035]

yeah I fixed it with some cutting and jumper. but this brand new pcb is already a mess !
this was also to warn other users that may use kicad to make their own esr meter.

[kripton2035]

well, I finally made my own jay_diddy_b's esr meter. wanted a digital one so I made this :


the inside mess :


measuring a capacitor, directly in ohms :


and comparing with a deree de5000 :

[Shock]

Nice, had the same idea aside from the tweezers. There is a few broken image links in your post by the way.

How stable did the display turn out, would love to see a video of it.

[kripton2035]

well if you measure a resistor, and your hands are steady, so is the last digit !
if you measure a capacitor, often bad ones, the last two digits can change a little.
I have added a small potentiometer to trim the output voltage, to take into account the probes resistance.
with it I can set the short probes to a fixed zero on the display.
but the amplify factor I would like also to trim it. it is ok from 0 to 1.5 ohm, but after that it degrades a little
a 10 ohms resistor is read ad 13 ohms. it is not important, but it would be so much better !
I can almost distinguish between a 0.01 and a 0.02 ohm resistor I have ! very nice.

I can see all the 4 pictures in my post. which one don't you see ?

[kripton2035]

this is the mod I made to the output opamp :
it let me setup a zero to cancel the probes resistance, with a very nice range using a multi-turn pot.
I would like to modify it to also handle the gain of the opamp, so that I can calibrate it, together with still zeroing it.
is it possible or must I add another opamp ?

[AE7OO]

I'm working on building the original meter with slight modification, I'm routing it today.
The modifications are different output and OSC, the blocking caps and going to 4 BNC connectors(So I can use the Kelvin clips I already have, I also have converters for regular probes). 

While the LT6241 is nice, I don't have any.  What I do have are a couple of ADA4807-1, which I used for the output.  For the OSC I went with a couple of inverters at about 200Khz, which I fed in to a string of SN74LVC1G80(single D FF) to get a 50% duty cycle.  I'll have the option to add a switch to control the frequency(i.e. I'll do the board to allow easy modification).

 The only high voltage caps I could find in the pulls drawer(I was not going order new) were 630V 3uF film caps.  Huge...  And so while the original called for .1u and .01u, what it got was 3u.  If nothing else this should allow me to add a much lower frequency if I need to.

*******
At the same time I'm looking into doing one that will use a sine wave.

I was thinking to use a biased non-inverting schmitt buffer to generate the in-phase square wave.  The specific chip I was going to use was the dual buffer NL27WZ17(LVC compatiable).   With a 3.1 ns typical delay, it should be transparent and placing it within millimeters of the switch input should allow me to ignore the signal edges.

I also have single inverting and non-inverting schmitt buffers available(these are actually multi-function gates, but same speeds) if need be.

Does anyone see any problems doing it this way? 
LTSpice generates the same waveform at the output(using the generic schmitt buffer) so I think that I'm in at least the same ballpark.

[hugo]

well, I finally made my own jay_diddy_b's esr meter. wanted a digital one so I made this :

What is the current drawn by the digital voltmeter?

Thanks

[Jay_Diddy_B]

While the LT6241 is nice, I don't have any.  What I do have are a couple of ADA4807-1, which I used for the output.  For the OSC I went with a couple of inverters at about 200Khz, which I fed in to a string of SN74LVC1G80(single D FF) to get a 50% duty cycle.  I'll have the option to add a switch to control the frequency(i.e. I'll do the board to allow easy modification).

 

The ADA4807-1 will work fine as the output amplifier.

The circuit will work, unmodified with the LTC6241 replaced by the ADA4807-2 (dual version)

The use of a logic oscillator at 2x frequency followed by a flip-flop will be fine.

The only high voltage caps I could find in the pulls drawer(I was not going order new) were 630V 3uF film caps.  Huge...  And so while the original called for .1u and .01u, what it got was 3u.  If nothing else this should allow me to add a much lower frequency if I need to.

This is a bad idea. The resistor in series with the capacitors will be damaged by the surge if you connect the ESR meter adapter to a high voltage (or a capacitor charged with a high voltage).

Look for old switch mode power supplies. use the X-cap (Line to Neutral) for the 0.1uF position. Use the y-cap  (Lines to GND) for the 0.01uF capacitor. The circuit will work with 4700pF (or 2x 2200pf in parallel) in this position.

Looking forward to seeing your version.

Best regards,

Jay_Diddy_B

[kripton2035]

Quote from: hugo on Yesterday at 23:39:51

What is the current drawn by the digital voltmeter?

8mA @ 5V and 6mA @ 3.3V
it is this one :
https://www.ebay.com/itm/Red-Blue-Yellow-5-Digit-LED-DC-0-4-3000-33-000V-Digital-Voltage-Panel-Voltmeter/272882019550

[MiroS]

Do you know if anyone created Kicad schematics and PCB ?

I just started to test Kicad and created one,  no footprint assigned, only raw schematics.

[AE7OO]

Thanks for the reply.

This is a bad idea. The resistor in series with the capacitors will be damaged by the surge if you connect the ESR meter adapter to a high voltage (or a capacitor charged with a high voltage).

Are you talking about R15 and R16?  If so, would going to a power resistor for those help? 

What is the largest value  that I can get away with for C5 and C6?  I would love to be able to test something at ~1.5Khz if I wished.  Since I'm already using a FF to get my 100Khz, I was going to go ahead and lay down a string of 4 or 5 of them.  So in the future it would be easy to add a switch and test at the divide freqs.(i.e. 50, 25, etc).   Or just 100/1.

Look for old switch mode power supplies. use the X-cap (Line to Neutral) for the 0.1uF position. Use the y-cap  (Lines to GND) for the 0.01uF capacitor. The circuit will work with 4700pF (or 2x 2200pf in parallel) in this position.

Would 2 caps in series or parallel at the C5 or C6 position cause a problem for the circuit?

Looking forward to seeing your version.

I'm not sure I'll let a schematic out(they work for me, but some may not like the style), but I'll post some pictures of the boards no problem.

And thank you for both the reply and posting the project to begin with.

GB

Oh, afterthought.  Would you mind commenting on my linked square wave generation method?
Thanks!

[trobbins]

I just found I had a small stash of HEF4053B, so am going to set up a diy adaptor too.  The HEF4053 allows a higher supply voltage from 2x 9V batteries to get say +/- 6V supply, but I may initially just aim for 10kHz and then check if 100kHz performs ok.

I also have a spare AD521 and 524 so will see how a vintage IA goes for trimmable offset and gain (and perhaps use its x10, x100 and x1000 programmed gains and an output level trimpot for different ESR ranges).

[Jay_Diddy_B]

I just found I had a small stash of HEF4053B, so am going to set up a diy adaptor too.  The HEF4053 allows a higher supply voltage from 2x 9V batteries to get say +/- 6V supply, but I may initially just aim for 10kHz and then check if 100kHz performs ok.

I also have a spare AD521 and 524 so will see how a vintage IA goes for trimmable offset and gain (and perhaps use its x10, x100 and x1000 programmed gains and an output level trimpot for different ESR ranges).

Hi,

Check this message regarding the selection of the 4053 mux.

https://www.eevblog.com/forum/projects/esr-meter-adapter-design-and-construction/msg341346/#msg341346

Regards,

Jay_Diddy_B

[trobbins]

Ta thanks - yes I had read the thread and noted the likely issue of speed, so will initially go for 10kHz and see how influential the type of 4053 is (I am getting some possibly slower CD4053 in at some time, but not a 74HC4053).  It is a little difficult comparing timing specs for address changes, as output loading conditions seem to be a bit different between the datasheets, and the application appears to have substantially different loading conditions (much higher load capacitance).

Was the S2 switch in the 4053 connected to toggle with the oscillator for convenience in routing, as compared to being configured to be idle?

Apart from being cheaper parts, the HEF and CD4053 allow a higher working voltage (which needs to be used to reduce the delay/transition times), and could therefore have some benefits for stand-alone testing of caps (compared to in-situ pcb testing where there may be semiconductor junctions imposing themselves on a measurement). 

I aim to construct the 4053 end on a DIP-to-soic header board (for convenience), and use a pre-existing measurement board with the IA, so hope to make the 4053 end and the gain end swappable to do some comparisons.

Ciao, Tim

[Jay_Diddy_B]

Tim,



If you mean the part of the 4053 that is on the left side of the circuit, it is there to match the delays with the switch on the right side of the circuit.

Regards,

Jay_Diddy_B

[Jay_Diddy_B]

Do you know if anyone created Kicad schematics and PCB ?

I just started to test Kicad and created one,  no footprint assigned, only raw schematics.

MiroS,

I have had a look at your KiCAD schematic. I have found a few issues:



In this section there is a missing connection between the two 3.32k resistors and the capacitor.
The capacitors should be ceramic. They need to be low ESR.



In this section C6 should be 0.01uF or 10nF

R16 should be 10

Just so you know, R21 was in the original design as a jumper. It allow the circuit to be constructed single-sided with no vias.

Regards,

Jay_Diddy_B

[trobbins]

If you mean the part of the 4053 that is on the left side of the circuit, it is there to match the delays with the switch on the right side of the circuit.

Soz, I was referring to all the circuitry to the left of the gain stage.  As you have identified, analog switch operation within the same IC package should have close switch time matching, and so aligned synchronous detection.

I just found I also had 2 samples of TS5A22362, which appears to be pretty similar to the 74HC4053, and with only two spdt switches - so likely well suited to this application.

Nearly two decades ago we used a similar scheme to extract the real part of battery impedance by injecting a sine current in to large lead-acids, and used an AD630 for the demod to extract a valid signal out of a lot of noise.  The AD630 isn't a cheap IC, and unfortunately I don't have any lying around.

Tim

[MiroS]

Thanks Jay_Diddy_B, corrections and footprints included.

[kripton2035]

@MiroS: you should provide the libraries you used for the schematic because when I open your file, I get this :

[MiroS]

I am using Kicad Version: (5.1.5)-3, release build
No custom parts, all from standard libraries

My local project folder is
C:\Users\M\Documents\ESR_Tester_SMD\ESR_Tester_SMD.pro

I am attaching complete folder content, including  main archive  file  created  by Kicad itself - menu File -> Archive Project.
ESR_Tester_SMD_v0.zip.

[kripton2035]

it's ok now, even though I have an older kicad version.

[X.G.]

the ESR Meter Adapter Design which come from China,and only use one IC.

it can display the value of resistor,the ESR of cap,and the value of inductance.the  IC  is TDA1308,NE5532 or TL082.TDA1308 can work at 3~5V,NE5532 can work at 5~9V.

http://www.crystalradio.cn/forum.php?mod=viewthread&tid=683954

http://www.crystalradio.cn/forum.php?mod=viewthread&tid=683954&extra=&page=1

[Jay_Diddy_B]

Hi X.G. and the group,

This is an interesting circuit that has been shared by X.G.

I am particularly interested in the oscillator portion of the circuit built around Q1 and Q2. There are some comments in crystalradio forum (Thanks to Google Translate) that talk about this oscillator. The crystalradio forum talks about using different values of resistors in the oscillator.

For the circuit to work the oscillator has to generated a fixed amplitude sinewave at around 100kHz.

I first ran a simulation:



And I get the result:



Which is great!!

A little board was designed for a hardware test:





I built the board:



Using this inductor:



And I measured this output:



The waveform amplitude is much lower than the LTspice model.

To be continued …

Jay_Diddy_B

[Jay_Diddy_B]

Hi,

I modified the LTspice model to include the resistance of the inductor:




The results of this are:




This shows how the amplitude of the oscillation changes as a function of AC resistance in the inductor.

Improvement

Change the inductor to 100uH and the capacitor to 22nF:



The results are:



There is much reduced sensitivity to the resistance of the inductor.

Hardware Test:

Here is a picture of the 100uH board:



This is the inductor, from Wurth:



And the test results:




The amplitude is 1.4V (2x Vbe) as predicted by LTspice.

The 100uH and 22nF are much better choices for this circuit.

Regards,

Jay_Diddy_B

[X.G.]

I experimented  the style circuit of OSC in my analogue ESR meter  in July 2016.

http://www.crystalradio.cn/forum.php?mod=viewthread&tid=1623736&extra=



my notebook show the simple test  before 3 years:

1.my final selects  are  R1=51 ohms, L1=40uH(6 turns)，in the circuit work at 1.0V~1.5V.

2.when R1=22 ohms, the sine shape change,trending  to be a square(THD is higher).

3.when R1=68 ohms,the sine shape is better(THD is lower),the amplitude  reduced ,and the amplitude  reduced much than R1=51 with  lower Vcc.

4.when L1=160uH(12 turns),the wave of OSC  is likely  square.

5.I think that the open-loop gain of OSC=AC resistance of inductor/R1,so I tried to add a resistor less than 100 ohms ,paralleling with L1, for lowering the the open-loop gain,and  the OSC wave shape became better,just like highering R1.

[trobbins]

Just starting to gather parts and prepare circuitry sections now for a variant of Jay_Diddy_B's ESR meter.

I have plenty of HEF4053BT, so am going to see how this fairs up to 100kHz, given a higher supply rail of 10V to improve switching speed and on-resistance.

I also have a few vintage instrumentation opamps on pcbs, so will re-purpose an AD521 and hopefully achieve 1V/ohm scaling with zero offset, and maybe allow a 10:1 gain switch for higher ESR levels.

Aiming to see if the spare 4053 switch can operate in parallel for the voltage signal switch, to minimise the switch resistance a bit more (and hopefully not experience any switching glitches).

As this will be more of a bench speciality module, I don't mind using two 9V batteries and each 5V reg will compensate for its own battery and not need any loading for mid-point management.

I have a batch of 47milliohm 1% SMD, and 1 ohm 1% leaded, to make up a set of calibration resistors (which is timely, as my next activity it to restore a Pontavi Th2 milliohmeter).

[Johnny10]

Great Thread !

[trobbins]

I have powered up my variant of Jay_Diddy_B's ESR meter, and it is performing very nicely indeed.

The IA certainly allows easy setup up for 0 milliohm (+/- less than 0.1 milliohm) and 1.000V for 1 ohm 1%, and appears to be dead accurate down to the 47 milliohm 1% reference I have, when using a nice 30cm long Kelvin clip lead set with 4mm plugs.

I haven't yet played with the 555 oscillator, which is running at 18kHz, to see if the setup can support similar results at 100kHz.

Aiming to set up the IA gain for 1V/ohm and 0.1V/ohm to allow up to about 16 ohm max range (open circuit reads about 1.65V at the moment), and use switched fixed resistors and a trimpot for gain setup with sufficient offset trim range (which I aim to change to fixed and trimpot to reduce the present trimpot sensitivity when setting 0 ohm end).

I found a practical 'zero ohm' link to keep the Kelvin clip contact faces flat over their entire length, in the form of an 8mm wide, 0.9mm thick flat bar that had a previous life as a contact link bar in a high current contactor.  There are a few parts that show some temperature sensitivity (a few milliohm change when squirted), so packaging the circuitry to minimise local temperature changes seems worthwhile.

PS. it does work with capacitors, even the bigger ones with readings down around 10 milliohm, although ESR of a cap may be quite temp sensitive and so absolute ESR should really note the temp, and comparisons should use caps at the same ambient temp.

[ogden]

As ESR Meter Adapter is safe to measure charged capacitors, most likely it can be used to measure ESR of the batteries too. I would love universal battery/capacitor ESR meter. Hint: LTC6900 as configurable by resistor(s), clock. Please do not hesitate to post if you are interested in measuring ESR of the batteries.

[Jay_Diddy_B]

Hi group,

I have looked at measuring the ESR of cells before. You can find the message in this thread:

Link: https://www.eevblog.com/forum/projects/esr-meter-adapter-design-and-construction/msg2798498/#msg2798498

ESR Meter Adapter - Modification for 1 kHz (nominal)

Now I am going to share modifications that can be made to the ESR Meter Adapter to lower the frequency from the 100kHz, normally used for electrolytic capacitors, to 1 kHz for batteries and cells.

LTspice Model




I have indicated the changes and addition on the LTspice schematic.

The LTspice model shows an output of 100mV / 




This is nice and linear just like the 100kHz version.

Modified Circuit Board




All of the parts will fit the original except for the 100uF electrolytic capacitor.

Testing




Here I am using the test resistors described here:

Link: https://www.eevblog.com/forum/projects/esr-meter-adapter-design-and-construction/msg343855/#msg343855

to confirm the operation.

Attachments

I have attached a pdf of the modified schematic and the LTspice model.

Regards,
Jay_Diddy_B

 Modified sch 1kHz.pdf (150 kB - downloaded 262 times.)
 4053 esr meter 1KHz.asc (7.24 kB - downloaded 182 times.)

[ogden]

ESR Meter Adapter - Modification for 1 kHz (nominal)

Now I am going to share modifications that can be made to the ESR Meter Adapter to lower the frequency from the 100kHz, normally used for electrolytic capacitors, to 1 kHz for batteries and cells.

Wow, you are so fast! Thanx. Any chances to have 200 mOhm or at least 1 Ohm range? 20 Ohm is good for CR2032 and similar low capacity cells.

[hugo]

It looks like the output voltage is not quite linear below 2 ohm ...

[floobydust]

I've often wondered why this meter intentionally has such high output impedance with R3 
Usually you want to pump some current, several mA's or more through the DUT to swamp out wet effects. In the case of lead-acid battery ESR I would think the measurement is corrupted. Car battery ESR measurements are several amp pulses for this reason I think.

[Jay_Diddy_B]

Hi group,

Here are some test results using Li-ion cells.

Laptop Battery Pack




I broke apart an old Asus battery pack and separated four of the cells.




I have numbered the cells 1 to 4.

HP 4328A Measurement

This is a 1 kHz (+/- 100 Hz) sinewave ac coupled milli-ohmmeter.

Sample reading:




1 kHz ESR Meter Adapter




The adapter was read with a Fluke 289. The Fluke 289 has been set relative to remove the offset.




Results

The two methods gave very similar results. The difference are probably from the connections made with the 4328A.


[ Specified attachment is not available ]


Regards,
Jay_Diddy_B

[ogden]

I broke apart an old Asus battery pack and separated four of the cells.

Wow, very promising results. Difference between instruments below 10% and battery impedance spread below 10% as well - cell pack looks like well-balanced. Any chance for you to discharge one cell and measure ESR with both tools again? Asking to disassemble all the battery packs around until you find one with bad cell would be asking too much

[kripton2035]

@Jay
is it possible to use the schematic for the 1KHz version (bigger capacitors)
and using a switch to change the oscillator frequency, still be able to use the 100KHz ?
this would allow us to have one device to measure both batteries internal resistance and capacitors esr.
thanks.

[Jay_Diddy_B]

@Jay
is it possible to use the schematic for the 1KHz version (bigger capacitors)
and using a switch to change the oscillator frequency, still be able to use the 100KHz ?
this would allow us to have one device to measure both batteries internal resistance and capacitors esr.
thanks.

Hi,

You can add a switch in the oscillator so that it can do 1kHz and 100kHz. It will work fine.
The larger values of capacitors in the coupling network, will reduce the protection from applied voltage or charged capacitors. The coupling capacitors had a 500V rating in the original design.

Does this help?

Jay_Diddy_B

[kripton2035]

yes it helps ! thanks.
I assume it is only for the first protection capacitor 10uF/500v would be pretty big. the second 100nF is already available @ 500v for the 100khz version.
may be a DPDT switch to change the protection capacitor, and the oscillator at the same time.

[zoltanh]

Hi,

Do you have a STL of case for this ESR Meter Adapter? I would really appreciate if you share it to me. Thank you.

[kripton2035]

as I just made the pcb for my shorty-with-display project, I also made a pcb for my jay_diddy_b esr meter variation
more to come in a few weeks months.

[m3vuv]

any chance someone can do a thru hole version of this for decrepid dinosoars like me?,my eyes aint what they used to be at 54yrs old!!

[kripton2035]

I'm planning on making either a pcb with all smd components already soldered (via jlcpcb) and sell them
or once the prototype pcb is fully working another pcb with thru holes.
but be aware that the adc is in sot323 only (can use a prebuild breakboard at least)
and the aop is only soic8. so the thru-holes will have still some smd parts.

[m3vuv]

Unfortunatly not a lot of help as to the question i asked,i hate smd stuff!!

[Gyro]

any chance someone can do a thru hole version of this for decrepid dinosoars like me?,my eyes aint what they used to be at 54yrs old!!

At 54 years old, I would seriously recommend a visit to a decent optician to check whether you have any medical issues that need to be referred. They shouldn't be that bad.

Either that or you're not using any visual aids, a magnifier, even a pair of cheap reading glasses would help.

[Jay_Diddy_B]

Hi,

The board that I designed uses 1206 and bigger components. The smallest parts are SOD123 diodes. Here is photograph of the board:



These should be relatively easy to solder. You need a good pair of tweezers. I put solder on one pad. Position the part, solder that end and then solder the other end.

The op-amp used, LTC6241 is not available in thru-hole.

Regards,
Jay_Diddy_B

[sarbog]

For  Jay_Diddy_B,


Just completed   construction  of  your   original  design   and   compared  to  my   measurements  using  a  function  gen   and  oscilloscope ......   very  good    agreement...   

[sarbog]

I   am   68  years old ... used  5x  magnifier to  solder   the surface mount  components    for  the board made by  JLCPCB... The   two  signal  diodes  1N4148  in  surface  mount  are in    back   order  from  DigiKey..........      about   6 months...

[Jay_Diddy_B]

sarbog,

The 1N4148 diode is a very common small-signal switching diode. I did a quick check on Digikey.

Try this part number: 1N4148WQ-7-F   or 1N4148W-G RHG

What you need is a small-signal diode, in a SOD-123 package.

It is great to see people building the project that I posted. Thank you for sharing.

Regards,

Jay_Diddy_B

[sarbog]

Thanks,  I  will add a few of the diodes to my next Digital-Key order.

[kripton2035]

@Jay_Diddy,
I have a question about the schematic @1KHz (https://www.eevblog.com/forum/projects/esr-meter-adapter-design-and-construction/msg3296986/#msg3296986)
Why did you add the 100µF capacitor C1 ?
thanks.

[Jay_Diddy_B]

@Jay_Diddy,
I have a question about the schematic @1KHz (https://www.eevblog.com/forum/projects/esr-meter-adapter-design-and-construction/msg3296986/#msg3296986)
Why did you add the 100µF capacitor C1 ?
thanks.

Hi Kripton2035,

The resistors R13 and R14 form a mid-point between +5V and 0V. The capacitor lowers the impedance for ac currents. A higher value capacitor is needed, to get the same impedance when the circuit was modified for 1kHz.

If you want to make a dual frequency version, you can leave the 100uF capacitor in place when operating at 100kHz.

Jay_Diddy_B

[kripton2035]

I initially forgot to put the capacitor in my dual frequency version, and when I install it afterwards, I don't notice any change in the measured values, at 1 or 100KHz.
that's why i asked for the purpose of C1.
thanks for your answer.

[aleksejsm]

I initially forgot to put the capacitor in my dual frequency version, and when I install it afterwards, I don't notice any change in the measured values, at 1 or 100KHz.
that's why i asked for the purpose of C1.
thanks for your answer.

Can you share your version of dual band ESR Meter please?

[kripton2035]

it is sort of working, but I made big mistakes for the first pcb, and the working prototype is really messy
lots of cutted tracks, jumpers...
I have to clean all of this, still some more programming to clean too
and make a new clean pcb for it.
please be patient a little more...
ps: the schematic will be free and published on my web site (and here too) , but the gerbers for the pcb will be for sale as it is a lot of work.

[Texmisure]

@Jay_Diddy_B,

Can i change R13, R14 with 10k resistor? Thank you for your help and con division.

Texmisure

[Bror Ek]

Well, even after 10 years, it's still possible to simplify a design 

As there's a spare ⅓ 4053 switch pair,  it can be repurposed as
an oscillator, thus freeing one op-amp (or for other use).
One resistor less is needed as well.

I put the osc-part demo schematics and info.txt here:
https://groups.io/g/LTspice/files/Temp/Hysteres%2020_70%25%20Virtual%20External%20Input%20Port%20Buffer+Test-Demos.zip

The simulation model is aimed for the classic CD4053,
so the frequency should be adjusted with a real chip.

/Bror Ek

[Jay_Diddy_B]

Snip ...

I put the osc-part demo schematics and info.txt here:
https://groups.io/g/LTspice/files/Temp/Hysteres%2020_70%25%20Virtual%20External%20Input%20Port%20Buffer+Test-Demos.zip

Snip ...


/Bror Ek

Bror,

Please attach a screenshot of the schematic modification and attach the .asc file to your post. I can't see the schematic on the groups.io website without signing up.

If your simulation uses models that are not included in the standard LTspice installation, please create a zipfile with everything that is required.

Thanks!!

Jay_Diddy_B

[Bror Ek]

Jay,
Hope this helps -

(The RC   'C' should perhaps be increased a few times as long as
a smaller  'R'  won't load to much)

/Bror

[Jay_Diddy_B]

Bror,

I checked the Nexperia and the TI datasheets for the 74HCT4053. I do not see any hysteresis on the inputs. If there is no hysteresis this oscillator will not work reliably.

Jay_Diddy_B

[Bror Ek]

Yes Jaj, I can not see any specific Schmitt spec,
though in this application the signal edges are distinct and
the switch families gap point levels are well separated,
so in practice there should not be any problem -
see some chip spec. examples further below.

I have no sample in stock to verify yet as the only local over the desk
professional supplier for 2M people closed and I will only mail-order
for some min. items collection.

But I plan to build your design in any working version later as this
is what every household needs 


MC74LVXT4053-
Minimum High−Level Input Voltage, Channel−Select or Enable Inputs: 2.0v (stable at all temperatures)
Maximum Low−Level Input Voltage, Channel−Select or Enable Inputs:  0.8v (stable at all temperatures)
Results in a switch gap of min. 1.2v


TI CD74HC(T)4053 - at Vcc 5v
Min. High-level control input voltage: ~ 3.5V
Max.  Low-level control input voltage: ~ 1.5V
Results in a switch gap of min.  2.0v
(the simulation is closest to this family)

TI New version spec release 03 Mar 2023, TMUX4053 single supply (5 V to 24 V) or
dual supplies (up to ±12 V), or asymmetric supplies.
Min. High-level control input voltage:  1.35V
Max.  Low-level control input voltage:  0.8 V
Results in a switch gap of min.         0.55v
(this might result in close to 4 times higher frequency for the same RC?)
- This chip is also very fast.

/Bror

[hbozyq]

After all these years, which version is the "final" version? I still have interest in build one.