20dB 'RF' attenuator - seeking feedback to improve

[enut11]

@duak
Should the input, output and center pads for the resistors just be islands on an otherwise continuous ground plane? This seems to go against what I have seen so far in this thread??

I will try an upper ground plane later but I do not have the means to test it properly until my NanoVNA adapters and leads arrive.

Cables? Currently cheap Chinese BNC on RG58 along with in-line 50 ohm BNC loads.
enut11

@joeqsmiith
I was not very clear in my reply about testing the latest attenuator.
I set up my Wavetek Model 80 to output 50MHz at 1V and compared the output of my 2 attenuators on my DST1102B DSO.
There is not enough evidence at this time to draw any conclusions.
enut11

[joeqsmith]

@joeqsmiith
I was not very clear in my reply about testing the latest attenuator.
I set up my Wavetek Model 80 to output 50MHz at 1V and compared the output of my 2 attenuators on my DST1102B DSO.
There is not enough evidence at this time to draw any conclusions.
enut11

I think we have an answer to your problem. That attenuator is meant to drive into 50 ohms where your scope appears to not support it.  You would need to add and external 50 ohm terminator.   Something like these:


https://www.amazon.com/Copper-Adapter-38-5mm-Through-Terminator/dp/B07G566JC7/ref=pd_sbs_23_t_1/131-1485153-0357844?_encoding=UTF8&pd_rd_i=B07G566JC7&pd_rd_r=d6af2da5-ac8f-46c0-b283-2f19c2d95aad&pd_rd_w=h3Kiw&pd_rd_wg=Cdwgs&pf_rd_p=5cfcfe89-300f-47d2-b1ad-a4e27203a02a&pf_rd_r=JA7B155VSYWS2A3KXGYC&psc=1&refRID=JA7B155VSYWS2A3KXGYC

After you get the termination correct, you should see your 10:1 divider.   

I repeated your test.  I ran the RF generator into a splitter.  One port goes to directly to the scope, the other through the attenuator then to the scope.  Even with the three resistor T, you can see at 50MHz, I am very close to 10:1.   One thing to keep in mind is your want to make sure your scope is working in a linear region. 

With the Nano, you are already working with a 50 ohm system so you can just measure it directly.   

Hope this helps.

[joeqsmith]

Same setup, at 300MHz. 

[duak]

Enut11 - yes, a mostly solid ground plane tying all the signal common points together is best.  There can be cutouts for circuit nodes but otherwise it should be solid.

The way I visualize it, the ground plane does at least two things: it ties all the signal common points together with the shortest, lowest impedance path possible.  Secondly, it modifies the way electric fields are formed around components.  eg., if you take a resistor in free space and apply a voltage to it, electric lines of force are formed connecting its terminals together.  This is not good as at high frequencies, the resistor is bypassed by a capacitance.  Placing the resistor close to a ground plane causes the electric lines of force to connect to the ground plane instead of to the other terminal.  In essence, it converts a capacitance across a resistor into two capacitances to the ground plane and the resistor is bypassed with a much smaller capacitance.  This is why I suggested a ground plane on top of the circuit too and for ultimate rejection, having the resistors pass through the ground plane.

Things are actually more complicated than this as there is also the magnetic field that becomes important at high frequencies but I think my mental model is good enough up to VHF.

[RCinFLA]

Think about stray capacitance and inductance everywhere.  Components and PCB layout.

Primary stray for chip resistors is shunt capacitance.  RF chip resistors are thin film on low dielectric substrate with single sided solder pads.  Normal thick film ceramic (high-k substrate) chip resistors with full end cap terminations are good for a couple tenths of pF shunt capacitance.  PCB solder pads for chip resistor are worth a couple of more tenth of pF.  Ground plane to component solder pad are worth a couple more tenths of pF.

PCB strays can hurt.  Avoid ground plane behind chip solder pads. 

Metal film leaded resistor are disaster for series inductance.  They are often trimmed to value with a barber pole spiral laser cut which makes a lossy inductor.

[enut11]

Enut11 - yes, a mostly solid ground plane tying all the signal common points together is best.  There can be cutouts for circuit nodes but otherwise it should be solid.

The way I visualize it, the ground plane does at least two things: it ties all the signal common points together with the shortest, lowest impedance path possible.  Secondly, it modifies the way electric fields are formed around components.  eg., if you take a resistor in free space and apply a voltage to it, electric lines of force are formed connecting its terminals together.  This is not good as at high frequencies, the resistor is bypassed by a capacitance.  Placing the resistor close to a ground plane causes the electric lines of force to connect to the ground plane instead of to the other terminal.  In essence, it converts a capacitance across a resistor into two capacitances to the ground plane and the resistor is bypassed with a much smaller capacitance.  This is why I suggested a ground plane on top of the circuit too and for ultimate rejection, having the resistors pass through the ground plane.

Things are actually more complicated than this as there is also the magnetic field that becomes important at high frequencies but I think my mental model is good enough up to VHF.

Hi @duak
Good stuff on how ground planes work! Thanks for that.
Could you please elaborate on "for ultimate rejection, having the resistors pass through the ground plane", with a diagram if possible?

Hi @joeqsmith. About the 50ohm in-line load to the DSO, yes you are right. I discovered this also by accident but thanks for your reply.
enut11

[T3sl4co1l]

For a verbal description -- consider two boxes sharing a common wall.  There's one connector entering each box, and a hole through the common wall.  The shunt resistors shall be placed by the hole, as close as possible on either side; the series resistor goes through.

Or for a tee rather than pi arrangement, the shunt resistor is in the hole*, and the series resistors are placed close to it.

*I've heard of PCBs actually being made this way, with a resistive layer that can be connected between pads and ground anywhere a termination resistor is needed.  Like for ECL and LVDS circuits.  You can have a resistor to ground, literally in the hole the connection is routed through.

Note that the paths between connectors and hole must still be 50 ohm transmission line -- this is the key step missing from an earlier example:



If the connections are simply routed down from the connectors, along the ground plane, then up to and through the hole, the lumpy response will straighten out.   (Well, nearly -- this assumes the hole is plated-through, making a coaxial connection say.  It looks like drilled copper clad, so there will be a gap between the two faces, not a direct connection.  This can be solved by shortening the walls, so the connection can wrap over and around a contiguous ground, without interruptions.)

Regarding paired resistors, probably better to have them closer together, but it depends on the transmission line impedance of that geometry.  You could evaluate this, for example, using a field solver (full 3D preferably, but even a 2D prismatic solution like ATLC2 gives useful insight for much less time and money spent), using the approximate dimensions of the resistor bodies, spacing and ground plane.  (Note that the resistor's conductive body is under the enamel; this might not have an obvious way to measure, so I hereby grant full permission to burn a resistor, utterly destroy, completely turn it to ash, and measure the film/foil/ceramic core dimensions. )

Tim

[enut11]

Hi @T3sl4co1l
I like your sense of humour.
Heavy stuff indeed. I will have to read it several times to let it sink in

[enut11]

Think about stray capacitance and inductance everywhere.  Components and PCB layout.

Primary stray for chip resistors is shunt capacitance.  RF chip resistors are thin film on low dielectric substrate with single sided solder pads.  Normal thick film ceramic (high-k substrate) chip resistors with full end cap terminations are good for a couple tenths of pF shunt capacitance.  PCB solder pads for chip resistor are worth a couple of more tenth of pF.  Ground plane to component solder pad are worth a couple more tenths of pF.

PCB strays can hurt.  Avoid ground plane behind chip solder pads. 

Metal film leaded resistor are disaster for series inductance.  They are often trimmed to value with a barber pole spiral laser cut which makes a lossy inductor.

@RCinFLA
OK, I get that leaded resistors are history for VH frequencies and that metal film resistors may the the worst of the pick.

"PCB strays can hurt.  Avoid ground plane behind chip solder pads" I think this means I cannot have a continuous ground plane under a solder pad. Seems to rule out using double sided PCB for VHF attenuators?
enut11

[T3sl4co1l]

Think about stray capacitance and inductance everywhere.  Components and PCB layout.

Primary stray for chip resistors is shunt capacitance.  RF chip resistors are thin film on low dielectric substrate with single sided solder pads.  Normal thick film ceramic (high-k substrate) chip resistors with full end cap terminations are good for a couple tenths of pF shunt capacitance.  PCB solder pads for chip resistor are worth a couple of more tenth of pF.  Ground plane to component solder pad are worth a couple more tenths of pF.

PCB strays can hurt.  Avoid ground plane behind chip solder pads. 

Metal film leaded resistor are disaster for series inductance.  They are often trimmed to value with a barber pole spiral laser cut which makes a lossy inductor.

@RCinFLA
OK, I get that leaded resistors are history for VH frequencies and that metal film resistors may the the worst of the pick.

"PCB strays can hurt.  Avoid ground plane behind chip solder pads" I think this means I cannot have a continuous ground plane under a solder pad. Seems to rule out using double sided PCB for VHF attenuators?
enut11

To bring some subtlety to this -- the spiral cut isn't a problem, in and of itself.  Consider the spiral itself: it can be analyzed as a helical waveguide.  I don't pretend to know the inner workings of this myself, but the consequences are, it's a structure with impedance, velocity, all that -- just like any other transmission line.  It's not an ordinary, well-behaved transmission line -- the impedance and velocity aren't constant with respect to frequency, it's dispersive.  But we can still use a transmission line model over a modest range, or for that matter, reduce it to a low-frequency equivalent all the same!

Of note, helical waveguides and resonators typically have quite high impedances.  While typical TL geometries are 50-150 ohms, helices can be 100s, even a few kohms.

So what does it mean for the transmission line to have resistance and impedance?  If they're equal, it'll be very much a resistive element.

Therefore: spiral-cut resistors, of values close to their transmission line impedance, have the widest bandwidth (largest resistive range, from DC to cutoff).  Lower values are inductance-dominant, and higher values are capacitance-dominant.  And the drop in bandwidth is approximately the same ratio as the ratio of resistance to Zo.

Typical spiral-cut resistors have a sweet spot around maybe 50-300 ohms.  That's partly driven by the size of the body over the ground plane, as well (assuming the PCB has one).  Don't forget that the resistor's leads are usually welded to larger metal end caps, so an equivalent circuit (lowpass CLC) may be useful.  (Fitting values to the equivalent is an exercise for the student..)

So, relating back to attenuators -- you'll find the best results come using resistors in this range.  If you need to use other values, you may find it's worthwhile staging it instead.

As for SMT pads, be very cautious about cutting grounds.  Consider: pads are just more metal on the signal path.  It's a transmission line segment, likely very much shorter than the wavelength of interest, so manifests as a stray capacitance or inductance as the case may be.  The chip's body does the same, too.  If your Zo trace width is thinner than the component/pad width, that component will have a lower impedance, or manifest as capacitance; else, inductance.  The further off they are, the less flat bandwidth you will have, etc.

And the component forms a transmission line segment of known length.  Is that enough to matter to your application?  A few mm won't be sensible until GHz, don't worry about it.  Or if you are up there, well, do worry about it -- and consider using 0402s or smaller, or perhaps an integrated module that can offer better characteristics than board-level components can.

Removing ground under a trace or pad, increases the ground impedance, obviously; it acts as a series inductor.  Be very careful about putting anything near that opening, whether trace or component: it's a radiating source, a slot antenna (even if an electrically short one).

Or if you're on multilayer board, you can pour ground on bottom and cut it out in the middle, to give a higher substrate thickness.  Do use a via fence along this, to keep the planes from forming patch or slot antennas.

Tim

[duak]

enut11,
I've attached an image of what I mean by passing the series resistors through the groundplane.  I used some junkbox resistors and a piece of paper (instead of copper sheet).  The theory here is that the electric field surrounding the series resistors has the greatest chance of terminating on the ground plane than on the opposite terminal.

Ultimate Rejection is a term I borrowed from filters that describes the signal leaked around the filter outside of the passband.  Since any real world attenuator has a passband where it meets its specs, it seemed a reasonable way to describe what's happening here.

[joeqsmith]

You may find that at 40MHz where you are interested in working at, that you may be able to get away with a lot.

Let's start with a nice axial part.  I have cut away the insulation to show you how these particular parts are constructed. 

Next, lets use some BNCs with no board and just wire the thing up.  Some nice long leads.   

Now, lets toss it across the $50 Nano and sweep from a 1MHz to 40MHz.   

If you don't trust the Nano, here it is on my old HP3589A sweeping up to 150MHz.   

It's not quite an A/B compare as I am using different cables and I moved the unit and I'm sure I bent it a little.  But I think you get the point.   When I was a child I played with amateur radio for a while.  All of my equipment was very old and if you looked inside, you would see a lot of construction you may think is suspect but at these low frequencies it's far less important.    Of course, if you wanted to try and use this mess at 1.5GHz...  It seems we have designed a 550MHz notch filter.   

[T3sl4co1l]

Wouldn't surprise me if the notch varies with cable length, because of DM-CM conversion.

Although, that's kind of silly if the cable isn't one or two feet long (depending on mode), isn't it.

Tim

[enut11]

Hi @T3sl4co1l
Your words on component behaviour and PCB layout are most welcome even if my absorption rate is a little slow.

Given a choice, for a 20dB VHF attenuator, what type of ground plane material would you choose?
1) Single sided fiberglass/copper PCB?
2) Double sided fiberglass/copper PCB?
3) Solid copper sheet?
4) Something else?

Does ground plane metal thickness matter?
enut11

[enut11]

enut11,
I've attached an image of what I mean by passing the series resistors through the groundplane.  I used some junkbox resistors and a piece of paper (instead of copper sheet).  The theory here is that the electric field surrounding the series resistors has the greatest chance of terminating on the ground plane than on the opposite terminal.

Ultimate Rejection is a term I borrowed from filters that describes the signal leaked around the filter outside of the passband.  Since any real world attenuator has a passband where it meets its specs, it seemed a reasonable way to describe what's happening here.

@duak. Your illustration is perfect. I see that this type of construction would need to be planned and done in a certain order but will be worth it
enut11

[enut11]

@joeqsmith
Thanks. It is interesting to see what is under the paint on the metal film resistors. Are the miniature 1/8w carbon resistors trimmed in the same way?

WRT the VNA shots, seeing is believing!

I am still without proper cables, SMA connectors and adapters for my NanoVNA so cannot experiment any further here.

Everyone's feedback is most welcome as it greatly accelerates learning. Answers to specific questions are timely - something you cannot necessarily get out of a textbook!
enut11

[T3sl4co1l]

Hi @T3sl4co1l
Your words on component behaviour and PCB layout are most welcome even if my absorption rate is a little slow.

Given a choice, for a 20dB VHF attenuator, what type of ground plane material would you choose?
1) Single sided fiberglass/copper PCB?
2) Double sided fiberglass/copper PCB?
3) Solid copper sheet?
4) Something else?

Does ground plane metal thickness matter?
enut11

To a first order, no, thickness and material don't matter much.  Only height between signal and ground, and dielectric constant.

I assume you mean for 1., a single sided board with THT components placed on top of it (either flying wherever, or secured on islands glued/soldered on top ala "Manhattan construction").

Practically speaking, I prefer 2 sided copper clad, as it can be carved up to make traces and pads, and vias can be added (drill a hole, stuff wire in it, solder over both sides) to keep the ground pours in sync.  I prototype SMT parts this way; here's a good example: https://www.seventransistorlabs.com/Images/GD9.jpg


For best results (i.e., including higher order effects), the foil should be thicker than several skin depths at the frequencies of interest, if possible; the dielectric should be low loss; the dielectric should be solid as well (compare stripline to microstrip: stripline uses one dielectric only, while microstrip has some field running through air, which propagates at a higher velocity, thus introducing dispersion); uhh, the foil surfaces should be smooth and free of corrosion (this is harder to do, as smooth/polished copper has poor bonding, especially with high-Q laminates like Teflon), etc.


For example, this 20dB power attenuator I made -- which I think I only have a poor picture of here,
https://www.seventransistorlabs.com/Images/DistAmp2.jpg
oh, here's its backside,
https://www.seventransistorlabs.com/Images/STF6N60M2_Amp.jpg
uses a TO-220 resistor for the brunt of it (the first shunt branch, I think it's pi type), and a few axial resistors for the series branch and to tweak the exact resistances.  I think it's 75R 20W in parallel, 330R 1W (carbon film) in series, 75R 1/2W in parallel, plus whatever corrections.

Heh, also the 330 ohm resistor(s) have taken a bit of brown color, as they aren't quite properly rated for operation at 20W it seems.  Design mistake.

Anyways -- as far as I can tell, this is flat out beyond 300MHz (give or take a dB), based on my measurements with a bad noise generator and HP 8590A spec (I don't have a TG, unfortunately).  The layout is crude, more or less over ground plane, and seems fine for VHF work.

With respect to the above mentioned impedance theory, it's convenient that the TO-220 device has a very average resistance, and the axial resistors are somewhat higher values as fits their spiral-cut design.

Lead lengths and stray capacitances will take over at higher frequencies, sooner or later and give or take how flat you need it to be.  The component leads are all relatively thin, and some distance above ground, so will have higher TL impedances, 100-150 ohms say.  The TO-220 tab to heatsink acts as a wide pad, low-Z trace or capacitance, and the resistor end caps act similarly.  Overall, the various components will have a CLC lowpass filter response, probably somewhere a bit below 1GHz, plus zeroes as the resonances couple into each other.

Response probably looks much like joeqsmith's lashup, just with all the crud shifted to a bit higher frequencies due to the improved grounding, and perhaps not as exaggerated in magnitude because the RLC equivalents aren't so far out of whack.

Tim

[joeqsmith]

Staying with the same components previously shown I trimmed them and added a metal plate.   Similar construction to OP's first approach.   

These are the same cables and adapters previously used but notice we no longer have our 550MHz notch and the overall flatness is greatly improved.  According to our cheap VNA, even at 300MHz, we are within a half dB.   

As a reference, I have included a Coline PN# 120085 20dB attenuator.   This part is rated DC to 1GHz with a +/-0.2dB tolerance.   The Nano of course paints a completely different story, but again, it's $50.  Don't expect much from it above 300MHz.   What you can see is that up to 400MHz, the Coline part is basically flat and we can safely say that the half dB we measured with the home made part is real.   

[enut11]

Hi @joeqsmith
Excellent way to demonstrate the difference between components floating in space vs a ground-plane construction with trimmed leads for VHF applications.

Supplies from China seem to be taking longer to arrive - may be due to the current health crisis?

[enut11]

@T3sl4co1l
"For example, this 20dB power attenuator I made -- which I think I only have a poor picture of here,
https://www.seventransistorlabs.com/Images/DistAmp2.jpg"

Thanks for showing and explaining your VHF construction methods. Now, what is that very complicated setup supposed to do?
enut11

[T3sl4co1l]

Huh, odd, thought I made a post about it, doesn't seem to exist anymore?  Anyway, it's testing a 20W, 30MHz distributed amplifier, with a switching supply (because why not?) powered from a LISN for extra filtering, a white noise generator, preamp, and more amp, depending on which configuration I was testing.  Pictured was one preamp and an attenuator, so, checking small-signal response, return loss, etc.  The 4W 50MHz amp I made specifically to test this thing at full power, actually.  Since it has, what was it, 17dB gain I think, so it needs a good few watts to get going.

Oh, heh, so the 6dB attenuator is built on copper clad, using 0805 chips.  On topic content.

Tim

[joeqsmith]

Supplies from China seem to be taking longer to arrive - may be due to the current health crisis?

I suspect so.  A little over a week ago, I ordered a few things from China including those low cost attenuators.  One order has yet to ship.  One shows mid next month, the other the following month. 

[enut11]

What's wrong with my NanoVNA. This is what I see with nothing connected.
Also, cannot calibrate it?? Is there a way to reset it to factory defaults?
enut11

[joeqsmith]

I understand that there is now a manual for the nano.   It may be time for you to join the group, if just to gain access to their secrete repository. 

You may be interested in the following:
https://www.edn.com/pcb-fixtures-improve-component-measurements/

He sells these boards along with a few others that may be helpful.   
https://www.sv1afn.com/en/other/

[joeqsmith]

The plating is a bit off and note a resistor kicked up and solder to the backside.