Author Topic: Dynamic Electronic Load Project  (Read 69785 times)

0 Members and 1 Guest are viewing this topic.

Offline CK345

  • Newbie
  • Posts: 3
  • Country: cn
Re: Dynamic Electronic Load Project
« Reply #50 on: December 04, 2016, 05:47:22 pm »
Analysis of a great :-+
 

Offline CK345

  • Newbie
  • Posts: 3
  • Country: cn
Re: Dynamic Electronic Load Project
« Reply #51 on: December 08, 2016, 10:36:05 pm »
Hello:
    why this figure gain margin is negative, the loop is stable?According to the loop analysis gain abundant negative       loop unstable!
 

Offline henken

  • Contributor
  • Posts: 26
  • Country: se
Re: Dynamic Electronic Load Project
« Reply #52 on: February 01, 2017, 12:02:37 am »
Hello,

Very informative analysis going on here. Thanks a lot for making it all available for us to see and learn.

I have been playing around with variations of the first time domain model in this thread, and I have a few questions from the perspective of a beginner in the subject.

I am looking into different variations of supply voltages, MOSFETS, number of MOSFET stages, and current limits. The main variables affecting the current drawn from the source are (as you of course know): the reference voltage (vref), the resistance of the current sense resistors, and the number of MOSFET stages. I understand the relationships between these, how they affect the current draw, and how they put constraints on the supply rails.

My questions are all related to which of these things can be changed without significantly affecting the stability analysis (I am still not understanding the subject well enough to trust my own analysis).

How sensitive is the system with regards to changes in:

1. Number of MOSFET stages. My uneducated guess is that this is not an important factor since they are all individual control loops.

2. Current sense resistor value. Again my guess here is that I can vary this within reasonable limits to adjust the current draw.

3. The reference voltage. My guess here is that this can also be changed somewhat without seriously affecting stability. For example, can a 1.25V reference be used instead of 2.5V? This would matter if a -5 rail is available instead of a -9V rail.

4. MOSFET choice. This is of course a major factor in the stability analysis. I can't source the IRFZ20 MOSFETs for a reasonable price, so I am looking for alternatives that don't require a completely new analysis. The MOSFET model used in the initial simulation model is the IRF530. I assume that this model will work instead of the IRFZ20.

In short:
I am thinking of implementing this circuit with 4xIRF530 to spread the heat over more devices. Thus, I would need to either change the reference voltage to 1.25V, or increase the current sense resistor to 0.2? in order to keep the same 5A ranges. My hope is that this won't negatively affect the stability analysis already made.

Thanks in advance for any further advice.
 

Offline Jay_Diddy_B

  • Super Contributor
  • ***
  • Posts: 1668
  • Country: ca
Re: Dynamic Electronic Load Project
« Reply #53 on: February 01, 2017, 01:01:49 pm »
Hello,

Very informative analysis going on here. Thanks a lot for making it all available for us to see and learn.

I have been playing around with variations of the first time domain model in this thread, and I have a few questions from the perspective of a beginner in the subject.

I am looking into different variations of supply voltages, MOSFETS, number of MOSFET stages, and current limits. The main variables affecting the current drawn from the source are (as you of course know): the reference voltage (vref), the resistance of the current sense resistors, and the number of MOSFET stages. I understand the relationships between these, how they affect the current draw, and how they put constraints on the supply rails.

My questions are all related to which of these things can be changed without significantly affecting the stability analysis (I am still not understanding the subject well enough to trust my own analysis).

How sensitive is the system with regards to changes in:

1. Number of MOSFET stages. My uneducated guess is that this is not an important factor since they are all individual control loops.

2. Current sense resistor value. Again my guess here is that I can vary this within reasonable limits to adjust the current draw.

3. The reference voltage. My guess here is that this can also be changed somewhat without seriously affecting stability. For example, can a 1.25V reference be used instead of 2.5V? This would matter if a -5 rail is available instead of a -9V rail.

4. MOSFET choice. This is of course a major factor in the stability analysis. I can't source the IRFZ20 MOSFETs for a reasonable price, so I am looking for alternatives that don't require a completely new analysis. The MOSFET model used in the initial simulation model is the IRF530. I assume that this model will work instead of the IRFZ20.

In short:
I am thinking of implementing this circuit with 4xIRF530 to spread the heat over more devices. Thus, I would need to either change the reference voltage to 1.25V, or increase the current sense resistor to 0.2? in order to keep the same 5A ranges. My hope is that this won't negatively affect the stability analysis already made.

Thanks in advance for any further advice.

Thank you for your kind words.

Let me answer your questions in the same order:

1) You are correct, each MOSFET has its own control loop, so the number of stages used in parallel does not impact the control loop stability.

2) If you examine the voltage gain of the MOSFET stage from the gate of the MOSFET to the source of the MOSFET as shown in this LTspice model:



The results are:



So the maximum gain is 0dB if the Source resistance is high and the transconductance of the MOSFET is high. The gain is reduced if the transconductance is lowered or the source resistance is lowered.


3) The reference voltage does not directly impact the gain.

4) Choice of MOSFET

The Vishay datasheets show that the IRFZ20 and the IRF530 are similar. The gm for both MOSFETs changes with the operating point. They do not show gm directly but a graph like this:



The transconductance is the change in Id versus the change in Vgs.
 
These MOSFETs are close enough to be considered equivalent.

When the control loops are designed there should be a least 6dB of gain margin. 6dB is factor of 2. so this allows for some significant changes while maintain stability.

Do not forget the RC damping network. This is critical in making a good load.

Good luck with your project, please share your results.


Regards,

Jay_Diddy_B



 

Offline henken

  • Contributor
  • Posts: 26
  • Country: se
Re: Dynamic Electronic Load Project
« Reply #54 on: February 02, 2017, 08:38:50 am »
Thanks for your response!

The reference voltage and MOSFET answers are clearly understood, and make great sense (just turning the potentiometers will affect the set voltage anyhow). The source resistor answer is a bit more difficult to understand.

2) If you examine the voltage gain of the MOSFET stage from the gate of the MOSFET to the source of the MOSFET as shown in this LTspice model:

[pic]

The results are:

[pic]

So the maximum gain is 0dB if the Source resistance is high and the transconductance of the MOSFET is high. The gain is reduced if the transconductance is lowered or the source resistance is lowered.

...

When the control loops are designed there should be a least 6dB of gain margin. 6dB is factor of 2. so this allows for some significant changes while maintain stability.

Clearly the gain increases when the resistance is increased. I'm not entirely clear how much this affects the actual stability in the end, and how it ties together with the actual gain margin. I need to read more about this subject. I will keep the same 0.1 milliohm source resistance anyway, and choose a different reference.

Do not forget the RC damping network. This is critical in making a good load.

I picked up on that from your earlier posts.  :-+

After some further testing with the time domain model, I found that the current slew rate seems severely limited. I actually don't have a clear idea about how large current slew rate is actually needed for some basic transient testing, but I looked around and found some application notes on the subject:

http://cds.linear.com/docs/en/application-note/an104f.pdf
http://www.ti.com/lit/an/snoa507/snoa507.pdf

They mention current slew rates at least in the tens of A/us (TI mentions 50A/us, and the rise times in LT's figures are much faster than what I can achieve in the simulation).

One limitation in the model seems to be the LT1013 op-amp, which only has a slew rate of 0.4 V/us. I tried changing the op-amps to ideal ones with the same slew rate as the TL074. This gave me much faster edges on the stages before the actual MOSFET driver. Doing that didn't speed up the final current rise times significantly, which seems to be due to the 220pF capacitors at the output stage.

I tried to measure the slope of the drawn current in LTspice. The current seems to peak at less than 1 A/us in the model you provided. Removing the 220p caps yielded a peak slope of 45 A/us, when the op-amps were interchanged with 13 V/us op-amps. Of course the lead inductance plays into all this, and I had to reduce it to get these figures.

So, I have a couple more questions:

1. Would it be desirable to have faster rise times, or are they already fast enough for basic load transient testing?

2. How could the circuit be modified to get faster rise times, while maintaining stability?


Good luck with your project, please share your results.

Thanks. it's going to take a while until I have anything to show. I must finalize the design, source parts, and get enough free time to put it together.

Cheers
 

Offline Jay_Diddy_B

  • Super Contributor
  • ***
  • Posts: 1668
  • Country: ca
Re: Dynamic Electronic Load Project
« Reply #55 on: February 04, 2017, 10:55:29 am »
Thanks for your response!

snip ...


So, I have a couple more questions:

1. Would it be desirable to have faster rise times, or are they already fast enough for basic load transient testing?

2. How could the circuit be modified to get faster rise times, while maintaining stability?


There are some faster loads out there. I have done a quick survey:

HP 6060A or 6060B:



The HP6060B has two ranges 0-30A high range and 0-3A on the low range. The slew rate is adjustable.

The BK Precision manual shows:






So the BK is not as fast as the HP/Agilent.

How fast is good enough?

We can explore this in LTspice. Here is a model with a dynamic load. The transition time is being stepped between 1us to 50us in a 1-2-5 sequence.



Here are the results:



You can see that the transition time has little effect until the transition time is similar to the response time of the power supply.

V=Ldi/dt constraints

Inductance between the load and the power supply will constrain how fast the load current can be stepped.

Jim Williams in Linear Technology AN133
Link: http://cds.linear.com/docs/en/application-note/an133f.pdf

describes a very fast load, suitable for testing low voltage high current power supplies. But, you can see how just 20nH of inductance wrecks the performance:



This is a special load for testing core supplies for FPGAs. It would not be a very good general purpose load.

You have the right idea, small MOSFETs, faster op-amps. But you have to follow the procedure outlined in this thread.

I do not want a load that is marginally stable when testing power supplies.

Regards,

Jay_Diddy_B

« Last Edit: February 04, 2017, 11:00:43 am by Jay_Diddy_B »
 
The following users thanked this post: BravoV

Offline henken

  • Contributor
  • Posts: 26
  • Country: se
Re: Dynamic Electronic Load Project
« Reply #56 on: February 04, 2017, 12:38:29 pm »
Thanks for the reply, and for the effort you put into them. Much appreciated.

I also found AN133. Good read.

Now I am diving into learning more about AC analysis (there's a huge amount to learn here :)). Meanwhile, I have been playing around with the AC analysis in LTspice, using your model as a starting point.

By random testing, I think I have found a configuration with much higher bandwidth that appears to be stable (from my unexperienced read of the Bode plots). This is probably all obvious to someone in the know, but I'll put it out anyhow.

1. Use a higher bandwidth op-amp
2. Reduce feedback capacitor (what is the proper name here?) from 220pF to 20pF.
3. Remove, or reduce the base resistor to the MOSFET (Downsides?)
4. The changes above cause instability -> Change the compensation by removing the resistor, and reducing the compensation capacitor to 1uF. (This makes the configuration look just like a regular bypass capacitor, which does fill the same role. I am not sure if that's improper in some way in the context of an electronic load. Seems fine.)

With these changes, I can get very clean waveforms, with a bandwidth of ~500kHz, and ~7A/us peak (4 source MOSFETS), even with plenty of lead inductance. Undoubtedly, things may turn out differently when I build this thing. The nice thing is that the architecture seems general enough to allow lots of experimentation with different component values, so if things turn out unstable, there is no need to start over with a new board (as long as the layout is good enough).

One issue I found with the circuit in this thread, is that the square wave reference voltage for pulsed loads has large spikes. The spikes are not present at the oscillator itself, but only after the transistor switching the reference voltage. Some kind of parasitic of the transistor must be to blame here. The spikes cause over/undershoot at the sourced current, which go away when clean pulses are used. Changing transistor has an effect, but I have not been able to get rid of the spikes that way. Ideas?

More questions:

1. What is the point of manually setting up the frequency stepping, and accessing the Bode plots through the error log vs. using a regular .ac command for sweeping the frequency?
2. Any advice on cleaning up the input pulses without overly impacting the rise-times?

I am of course looking into these things myself as well, but any pointers are appreciated.

Best regards

Edit: Ehm. Too quick to celebrate perhaps. Measuring I(R5) as you do, there is ringing with my modified configuration. The current waveform through the load is clean though. I'm not sure how to approach this from a power supply test perspective. Need to do more research..
« Last Edit: February 04, 2017, 12:51:22 pm by henken »
 

Offline Aroogz

  • Contributor
  • Posts: 5
  • Country: za
Re: Dynamic Electronic Load Project
« Reply #57 on: July 31, 2017, 10:06:49 pm »
Hi ,

Nice and Interesting work Jay_Diddy_B. well Done.

However, I am trying to build a dynamic electronic load with the following specs:
  • frequency: 0.1Hz - 10kHz
  • Voltage range: 0 - 40V
  • current range of 0 - 30A

Please what's your advice and could this be modified to accommodate the requirements?

Thankyou.

Aroogz.
 

Offline fcb

  • Super Contributor
  • ***
  • Posts: 1246
  • Country: gb
Re: Dynamic Electronic Load Project
« Reply #58 on: July 31, 2017, 11:45:40 pm »
Quite ambitious.

Probably start with building a 1A 40v load and getting that working at 10KHz. Then build up from there.

Also, what is your 10KHz - a squarewave? sine?  will make quite a difference to your acceptance criteria.
 
The following users thanked this post: Aroogz

Offline Jay_Diddy_B

  • Super Contributor
  • ***
  • Posts: 1668
  • Country: ca
Re: Dynamic Electronic Load Project
« Reply #59 on: August 01, 2017, 01:56:14 am »
Hi ,

Nice and Interesting work Jay_Diddy_B. well Done.

However, I am trying to build a dynamic electronic load with the following specs:
  • frequency: 0.1Hz - 10kHz
  • Voltage range: 0 - 40V
  • current range of 0 - 30A

Please what's your advice and could this be modified to accommodate the requirements?

Thankyou.

Aroogz.

Thank you for the kind words.

You indicate that you need 0-40V and 0-30A, do you need 1200W?

Because the MOSFETs are being used in the Linear region, 40W per MOSFET is a sensible target. The HP 6060A/B uses 8 MOSFETs for 300W.

Each MOSFET needs it own op-amp to control the current.


Quite ambitious.

Probably start with building a 1A 40v load and getting that working at 10KHz. Then build up from there.

Also, what is your 10KHz - a squarewave? sine?  will make quite a difference to your acceptance criteria.

This is great advice!!

My original circuits has two MOSFETs, but it can be extended to many.


The oscillator in the circuit shown is set to run at 330Hz. This is a good frequency for testing most power supplies. There is no reason why it can't be set higher.
To get high bandwidth in the load you need to use small MOSFETs and lots of them.



Good luck !!

Regards,

Jay_Diddy_B


« Last Edit: August 01, 2017, 02:36:17 am by Jay_Diddy_B »
 
The following users thanked this post: Aroogz

Offline Aroogz

  • Contributor
  • Posts: 5
  • Country: za
Re: Dynamic Electronic Load Project
« Reply #60 on: August 02, 2017, 08:19:47 pm »
Quite ambitious.

Probably start with building a 1A 40v load and getting that working at 10KHz. Then build up from there.

Also, what is your 10KHz - a squarewave? sine?  will make quite a difference to your acceptance criteria.

Thanks very much for your reply.

The 10kHz is a sine wave signal (of about 250mAp-p) which will ride ontop of a set DC current of the load.

Regards,
Aroogz.
The goal is to use this to perform a frequency sweep (0.1Hz - 10KHz) at set DC load point.
« Last Edit: August 02, 2017, 09:21:45 pm by Aroogz »
 

Offline Aroogz

  • Contributor
  • Posts: 5
  • Country: za
Re: Dynamic Electronic Load Project
« Reply #61 on: August 02, 2017, 08:36:41 pm »
Hi ,

Nice and Interesting work Jay_Diddy_B. well Done.

However, I am trying to build a dynamic electronic load with the following specs:
  • frequency: 0.1Hz - 10kHz
  • Voltage range: 0 - 40V
  • current range of 0 - 30A

Please what's your advice and could this be modified to accommodate the requirements?

Thankyou.

Aroogz.

Thank you for the kind words.

You indicate that you need 0-40V and 0-30A, do you need 1200W?

Because the MOSFETs are being used in the Linear region, 40W per MOSFET is a sensible target. The HP 6060A/B uses 8 MOSFETs for 300W.

Each MOSFET needs it own op-amp to control the current.


Quite ambitious.

Probably start with building a 1A 40v load and getting that working at 10KHz. Then build up from there.

Also, what is your 10KHz - a squarewave? sine?  will make quite a difference to your acceptance criteria.

This is great advice!!

My original circuits has two MOSFETs, but it can be extended to many.


The oscillator in the circuit shown is set to run at 330Hz. This is a good frequency for testing most power supplies. There is no reason why it can't be set higher.
To get high bandwidth in the load you need to use small MOSFETs and lots of them.



Good luck !!

Regards,

Jay_Diddy_B

Jay_Diddy_B,

Thank for your advice.

The requirement is just about 200W.

Regards,
Aroogz.
 

Offline fcb

  • Super Contributor
  • ***
  • Posts: 1246
  • Country: gb
Re: Dynamic Electronic Load Project
« Reply #62 on: August 02, 2017, 08:55:24 pm »
Quite ambitious.

Probably start with building a 1A 40v load and getting that working at 10KHz. Then build up from there.

Also, what is your 10KHz - a squarewave? sine?  will make quite a difference to your acceptance criteria.

Thanks very much for your reply.

The 10kHz is a sine wave signal (of about 250mVp-p) which will ride ontop of a set DC current of the load.

Regards,
Aroogz.
The goal is to use this to perform a frequency sweep (0.1Hz - 10KHz) at set DC load point.

250mVpk-pk..  this is a DC load - that doesn't make sense as an 'output' of the load.

Do you mean that you will adjust the load till you get 250mVpk-pk ripple?
 

Offline Rbastler

  • Frequent Contributor
  • **
  • Posts: 281
  • Country: it
  • Wörk Wörk
    • Rbastlers Blog
Re: Dynamic Electronic Load Project
« Reply #63 on: August 02, 2017, 08:57:27 pm »
Quite ambitious.

Probably start with building a 1A 40v load and getting that working at 10KHz. Then build up from there.

Also, what is your 10KHz - a squarewave? sine?  will make quite a difference to your acceptance criteria.

Thanks very much for your reply.

The 10kHz is a sine wave signal (of about 250mVp-p) which will ride ontop of a set DC current of the load.

Regards,
Aroogz.
The goal is to use this to perform a frequency sweep (0.1Hz - 10KHz) at set DC load point.

250mVpk-pk..  this is a DC load - that doesn't make sense as an 'output' of the load.

Do you mean that you will adjust the load till you get 250mVpk-pk ripple?
Maybe he wants a pulsed load ?

Sent from my A0001 using Tapatalk

http://rbastlerblog.jimdo.com/
Gamma spectrometer works. Now some yellow crystals need regenerating and testing.
 

Offline Aroogz

  • Contributor
  • Posts: 5
  • Country: za
Re: Dynamic Electronic Load Project
« Reply #64 on: August 02, 2017, 09:17:08 pm »
Quite ambitious.

Probably start with building a 1A 40v load and getting that working at 10KHz. Then build up from there.

Also, what is your 10KHz - a squarewave? sine?  will make quite a difference to your acceptance criteria.

Thanks very much for your reply.

The 10kHz is a sine wave signal (of about 250mVp-p) which will ride ontop of a set DC current of the load.

Regards,
Aroogz.
The goal is to use this to perform a frequency sweep (0.1Hz - 10KHz) at set DC load point.

250mVpk-pk..  this is a DC load - that doesn't make sense as an 'output' of the load.

Do you mean that you will adjust the load till you get 250mVpk-pk ripple?

Yes you are right....it's a DC load with the sinusoid (ripple on top). So this could be an analog signal that modulates the load.

It's sort of a transient load with a dc offset. For instance, I have a load of 1A with a sinusoid (to be swept over the frequency range) of amplitude of about 100mA. This will be the current drawn from the supply.

I am sorry if this isn't clear, but I will be willing to make any necessary further clarifications.
 

Offline Aroogz

  • Contributor
  • Posts: 5
  • Country: za
Re: Dynamic Electronic Load Project
« Reply #65 on: August 02, 2017, 09:19:46 pm »
Quite ambitious.

Probably start with building a 1A 40v load and getting that working at 10KHz. Then build up from there.

Also, what is your 10KHz - a squarewave? sine?  will make quite a difference to your acceptance criteria.

Thanks very much for your reply.

The 10kHz is a sine wave signal (of about 250mVp-p) which will ride ontop of a set DC current of the load.

Regards,
Aroogz.
The goal is to use this to perform a frequency sweep (0.1Hz - 10KHz) at set DC load point.

250mVpk-pk..  this is a DC load - that doesn't make sense as an 'output' of the load.

Do you mean that you will adjust the load till you get 250mVpk-pk ripple?

I am sorry, I meant to say 250mA.
 

Online edzyj

  • Newbie
  • Posts: 1
  • Country: cn
Re: Dynamic Electronic Load Project
« Reply #66 on: August 21, 2017, 05:17:05 pm »
Nice and Interesting work ! :-+
 

Offline capt bullshot

  • Super Contributor
  • ***
  • Posts: 1196
  • Country: de
    • Mostly useless stuff, but nice to have: wunderkis.de
Re: Dynamic Electronic Load Project
« Reply #67 on: May 29, 2018, 05:01:47 pm »
Great job, Jay_Diddy_B!
Safety devices hinder evolution
 

Offline dardosordi

  • Regular Contributor
  • *
  • Posts: 74
  • Country: ar
Re: Dynamic Electronic Load Project
« Reply #68 on: August 13, 2018, 10:36:23 pm »
Hi,

first I want to thank Jay_Diddy_B for your effort on this project, Im looking into building a 2nd load since my first DIY one melted its plastic case...  :-BROKE :palm:

Im considering ways to get away with a single supply. I see why you did this as a non-inverting amp in order to easily add up the voltages, but it makes you to use symmetric supply.

Could buffering the oscillator help with this and keep it single supply ?

Im using this crude simulator since I have no idea where to start with LT Spice (definitively on my list of to-do things). Using a BJT since I couldn't get the mosfet won't behave linear in it.



Here's the rather big url:

https://www.falstad.com/circuit/circuitjs.html?...



 

Offline Jay_Diddy_B

  • Super Contributor
  • ***
  • Posts: 1668
  • Country: ca
Re: Dynamic Electronic Load Project
« Reply #69 on: August 14, 2018, 11:50:38 pm »
Hi,

first I want to thank Jay_Diddy_B for your effort on this project, Im looking into building a 2nd load since my first DIY one melted its plastic case...  :-BROKE :palm:

Im considering ways to get away with a single supply. I see why you did this as a non-inverting amp in order to easily add up the voltages, but it makes you to use symmetric supply.

Could buffering the oscillator help with this and keep it single supply ?

Snip ..


Hi,

Thank you for your kind words.
Yes, the inverting configuration was used to make the summing easier. It also allows a wide selection of op-amps because they don't need to be rail-to-rail input and output.

Having said that here is an idea for you:




*** There is a mistake in the formula - I will fix later ***


Corrected Version:




The circuit combines the pulsating signal, Transient, with the non-inverting signal Vref.

The whole circuit becomes:



I have not built this circuit, so I do not know how well it will work.

I have attached the LTspice models.

Regards,

Jay_Diddy_B

« Last Edit: August 17, 2018, 12:52:57 pm by Jay_Diddy_B »
 

Offline dardosordi

  • Regular Contributor
  • *
  • Posts: 74
  • Country: ar
Re: Dynamic Electronic Load Project
« Reply #70 on: August 17, 2018, 12:31:29 pm »
Thank you very much! I will build it on the weekend. Is LM324 fine for this? I also have TL082/072.

Thanks again!
 

Offline Jay_Diddy_B

  • Super Contributor
  • ***
  • Posts: 1668
  • Country: ca
Re: Dynamic Electronic Load Project
« Reply #71 on: August 17, 2018, 01:00:32 pm »
Thank you very much! I will build it on the weekend. Is LM324 fine for this? I also have TL082/072.

Thanks again!

Dardosordi,

Use the LM324 op-amps. The LM324 common range includes the negative rail. this essential in the single supply version. The TL072/82 common mode range does not include the negative rail, so these will not work with a single supply.

With the LM324 you may need to reduce the bandwidth replace C1 and C3 with 1nF or 2.2nF to prevent oscillation.


Let us know how it works.


Regards,

Jay_Diddy_B
 

Offline t1d

  • Frequent Contributor
  • **
  • Posts: 442
  • Country: us
Re: Dynamic Electronic Load Project
« Reply #72 on: August 19, 2018, 03:50:14 pm »
Hi, JDB, Thanks for referring me to this load project. Your work, on this, is wonderful, impressive and gracious.

You are helping me, on another thread, to troubleshoot a load. But, its design is not your favorite. So, I am considering your design, to replace it, once I have used the present fault, as a learning opportunity.

Firstly, I looked up the difference between a Constant Current and a Dynamic load. Okay, I get it... The dynamic load allows the current draw to be varied (at a known frequency), so that the characteristics of the supply can be observed.

Here is my first Noob question. Can this circuit be modified, to turn off the oscillation? In other words, have a Constant Current/Dynamic Current option? If it is not too much to ask, what would be that design? Is it as easy as adding a switch, to by pass the oscillator portion, of the circuit?

Thanks!
 

Offline Jay_Diddy_B

  • Super Contributor
  • ***
  • Posts: 1668
  • Country: ca
Re: Dynamic Electronic Load Project
« Reply #73 on: August 20, 2018, 12:33:31 am »
Hi, JDB, Thanks for referring me to this load project. Your work, on this, is wonderful, impressive and gracious.

You are helping me, on another thread, to troubleshoot a load. But, its design is not your favorite. So, I am considering your design, to replace it, once I have used the present fault, as a learning opportunity.

Firstly, I looked up the difference between a Constant Current and a Dynamic load. Okay, I get it... The dynamic load allows the current draw to be varied (at a known frequency), so that the characteristics of the supply can be observed.

Here is my first Noob question. Can this circuit be modified, to turn off the oscillation? In other words, have a Constant Current/Dynamic Current option? If it is not too much to ask, what would be that design? Is it as easy as adding a switch, to by pass the oscillator portion, of the circuit?

Thanks!


T1D,

There are two controls, one sets the constant level, the other sets the pulsed level. To get constant current, you simply turn the pulsed control fully counter clockwise:




Using a pulsed load is used to look how a power supply responds to step changes in current.

It would be like test driving a car, without going round corners, if you tested a power supply without stepping the load current.

Regards,

Jay_Diddy_B

« Last Edit: August 20, 2018, 12:38:50 am by Jay_Diddy_B »
 

Offline t1d

  • Frequent Contributor
  • **
  • Posts: 442
  • Country: us
Re: Dynamic Electronic Load Project
« Reply #74 on: August 20, 2018, 07:16:07 am »
There are two controls, one sets the constant level, the other sets the pulsed level. To get constant current, you simply turn the pulsed control fully counter clockwise:
Doh! Too simple...
Using a pulsed load is used to look how a power supply responds to step changes in current.
Yes, I am understanding, that part...Though I may not have said that, clearly.

As always, thank you very much.
 


Share me

Digg  Facebook  SlashDot  Delicious  Technorati  Twitter  Google  Yahoo
Smf