Testing the effects of releaving ground plane beneth a component

[G0HZU]

You definitely need lots of ports for classic coplanar waveguide but I think a run of grounded coplanar waveguide can be modelled just fine with 1 port at each end of the run. It is important to make sure the coplanar shapes touch the sidewalls of the box.

I'd be interested to know how (and why) you modelled it with 3 ports at each end. That number of ports would be fine for classic CPW but not required for GCPW?

[Marsupilami]

Hey @joeqsmith

Sorry, I only read about half of this thread, but simulating from that cap s2p is problematic. If you have access to any tools that can approximate sNp networks with a spice circuit that would be a good step. Maybe even you could do it manually just putting extra reactive elements to get the resonances visible on the s-par plot.

I have a fairly usable 3D EM simulator but it can only deal with simple lumped components or a SPICE subcircuit. This one is using simply the ESL, ESR and Ceff of the cap. This won't show the weird parasitic effects.

[eb4fbz]

One thing to watch out for is that the ATC s-parameter models are taken over a PCB substrate so I'm not sure it is a good idea to use them anyway. These capacitors behave differently when mounted vertically or horizontally and this is because the metal structure within the cap body acts a bit like a transmission line when mounted over a given substrate. This is part of the reason these caps have sharp resonances and they often aren't suitable for wideband design work.
 
For your EM simulations you can try playing with (free) Sonnet Lite but I think it only allows a perfect capacitor model in the Lite version. It probably will let you play with the groundplane but I've not really used the Lite version very much.

One thing worth noting is that it can sometimes be a good idea to deliberately use fatter pads (compared to the ideal microstrip width) for the component if it has a tiny amount of series inductance. The fatter pads and the series inductance form a pi network and this can help improve the s11 response up at UHF.

At work I use Genesys and Sonnet combined together for stuff like this. I've used various EM simulators and Sonnet always comes out top for the most critical tasks. It can do multi layer simulation and can allow custom groundplane shapes with gaps. When used with Genesys it allows s-parameter models allowing very good simulation of LNAs and lumped+ distributed filters. It is a very powerful combination in my opinion.

I'm not really sure what you are trying to do but I suspect there will be cases where removing part of the groundplane will actually make things worse and sometimes it will help. A lot depends on the component and the pad shape it requires. Also, a lot depends on the chosen PCB material in terms of dielectric constant and substrate thickness.

https://www.modelithics.com/Model/SubstrateScaling

[MartinL]

You definitely need lots of ports for classic coplanar waveguide but I think a run of grounded coplanar waveguide can be modelled just fine with 1 port at each end of the run. It is important to make sure the coplanar shapes touch the sidewalls of the box.

I'd be interested to know how (and why) you modelled it with 3 ports at each end. That number of ports would be fine for classic CPW but not required for GCPW?

Ah, you're quite right - I've just looked into it again and what I said is true for CPW but not for GCPW. That makes the Lite version quite a lot more useful actually - I'll need to have a proper play with it. Thanks!

[Marsupilami]

I was playing around a bit more with this.

1.5mm thick FR4. Trace is 2.5mm wide with 1.5mm gaps. I made a giant-ass 3x4mm cutout under the cap and it still has very little effect.
I'm guessing the contribution from the bottom ground is relatively low in this configuration plus even at 6GHz a 3mm gap is about 10th of the wavelength so it can find its way around easy.


I used a SPICE model for the cap from Murata because that's what my simulator likes. Apparently they have the parallel resonances modelled in it. (2.7 and 4.5GHz)
I found this article that describes how the capacitor orientation effect the parallel resonances. This was new to me, quite interesting.
https://www.johansontechnology.com/srf-prf-for-rf-capacitors
It explains the missing resonances from the AVX s2p as they take those in the vertical orientation so the odd parallel resonances are out. PPI has a matching cap for the AVX 100B series (1111P) and they actually provide S-Parameters for both horizontal and vertical orientation.

[joeqsmith]

I see no reason why a capacitor would be required other than this is what the OP had asked about.   They haven't chimed in, so I doubt have any interest in it. 

You could try removing the capacitor from the equation.  Maybe just plot the before and after the slit are added.   Will your simlator support Smithcharts?       What about exporting to Touchstone?   

If you stay with the dimensions/material I show,  I could attempt to replicate it in hardware. 

[joeqsmith]

Something like this? 

Shown sweeping the gap in 5 mil increments, exporting to Touchstone and importing to METAS.  The dimensions are still a swag. 

[Marsupilami]

That looks good. Is that Sonnet?
What dimensions did you use? Er of the dielectric?
I can do that too without the cap and export touchstone. That'd be a good comparison.

[joeqsmith]

Basically what I had shown in AppCAD, Er 4.6, 62 mil, 1oz copper, FR-4.   Using about a 200 mil width for the slit.

[Marsupilami]

Here's mine. It's with no slit and a 1x5mm slit.
I did a parameter sweep to but only with reduced grid resolution as I didn't have the patience for that. (Time domain simulation has it's downsides.) How things move around is similar.
Do you have s2ps for your matching results?

[joeqsmith]

Thanks for taking the time to run it.   It's good to have some sort of sanity check.

I have continued to play with the various free simulators available.    Not using any of these tools on a professional basis and having virtually no experience with any of them, take my post accordingly.

The free version of Sonnet (15.53) is from 2014.  They are up to version 17 now.  Note how they promote faster sims with 17 vs 16.  For just trying to simulate a trace, 15 is very slow. 

https://www.sonnetsoftware.com/products/sonnet-suites/new-features.html
https://www.sonnetsoftware.com/products/sonnet-suites/suite-prices.html

Sonnet has created Touchstone files with the frequencies out of order.  The tool should never do this as the standard doesn't allow it.   I've also seen where it would append data to the Touchstone files rather than create them clean.  The memory provided is very limited and prevents trying different approaches.   Many of the features are also disabled.   Sure it's free but if their goal of making a free package was to sell products, I would think they would want to showcase what they have to offer today, not where they were seven years ago.

I am not sure Looking at the data it produces, what to make of it.   Something really strange happens at 3GHz.    I've played a bit with the various settings to try and tame it. 

[joeqsmith]

The BLACK trace in the following data was collected using the same mechanical dimensions, materials and settings, except the range was increased to 6GHz. 

I then tried various combinations of coarse no edge detection, symmetry, fine edge, and cell sizes.    While they appear have some effect, none play into the overall wave shape.

What is really interesting is I swept one of the unmolested test boards which again is roughly represented by the AppCAD screen shot I posted.  Marsupilami's data is the BLACK trace.  The PNA is BROWN.   I think we got lucky they would match this close.   The PNA's s2p Touchstone file is attached. 

I manually adjusted the boards thickness, Er and loss to try and achieve the same shape.  The numbers I am using are not even in the ballpark.   

I also removed the vias, then removed the floating ground plane.  This also had no effect.   There is a note in the manual:

Please note that when the value of the S-parameters is close to 1 (0 dB) over the entire band you may have small ripples or oscillations in the S-parameter values. This is due to the rational fitting model having too many degrees of freedom when trying to fit a straight line. If this is a problem, it is recommended that you analyze the frequency band in which this occurs with another type of sweep.


I had been using linear sweeps as well as exponential.  Both have no effect on the shape.    Another part in the manual talks about the box resonance.  Running the tests, it shows there are none.   Changing the distance to the box and using free space also have no effect on the shape.   

[joeqsmith]

As much as I like that METAS software,  it doesn't appear to support Smithcharts.  Attached is AppCAD plotting data from the PNA, Marsupilami and Sonnet. 

The Sonnet data is using the settings from the AppCAD coplanar drawing.   
   

[Marsupilami]

Interesting.
What's easy to figure out first I think is the S21 phase response. On your PNA measurement is the extra length for the connectors compensated for or is it still in? Or did I screw up the length of the board. I think I did 28mm. (1.1" ?)
It's 62 vs 88 degrees per GHz. (The Sonnet result being around 50/GHz maybe?)
This thing: https://chemandy.com/calculators/coplanar-waveguide-with-ground-calculator.htm tells me that the effective Er is about 3.4
Than this: https://www.microwaves101.com/calculators/873-wavelength-calculator says that 1GHz wavelength is 162.7mm
Based on that:
Mine: 28.02mm
PNA: 39.77mm (assuming a uniform Er=3.4 line, see below)
Sonnet: ~23mm ?

If your board is indeed 1.1in and the SMA connectors are on it, which I assume have a teflon dielectric with Er ~ 2 then  7.5mm@Er=2 + 28mm@Er=3.4 + 7.5mm@Er=2 actually gets us 88degrees @ 1GHz would explain the PNA S21 phase slope perfectly.

I would try to figure out if this is correct so far and the look into why Sonnet thinks the section is shorter.

[Marsupilami]

On a related note it's ridiculous how inaccessible these software are. I started looking for one about a year ago and went through the 7 stages of grief realizing what my options were.
At some point I even considered making a project out of writing my own using an open source library or code my own front end for OpenEMS. I wasn't looking at Sonnet as I wanted a full 3D solver but I tried like a dozen and talked to a bunch of sales people. It's one thing that stuff is expensive but the big names don't even do perpetual licenses anymore so you have to be actively making a lot of money with it in order to keep up with the license costs. I ended up with XFdtd which might not be the most optimal for some problems (time domain solvers struggle with high Q stuff) but at least it "only" costs as much as a car not as much a house and they offered a reasonable lease to own plan. I really wanted to learn something at home at my own pace, the return on investment is questionable and I'm not going on vacation for a while.

[MartinL]

I was just having another look at the state of interfaces to OpenEMS, and found an example in pyopenems for simulating a ground cutout under a capacitor:

https://github.com/dlharmon/pyopenems/blob/main/examples/capacitor_ground_cutout.py

I haven't set things up to run this yet but it might be worth trying.

[joeqsmith]

Interesting.
What's easy to figure out first I think is the S21 phase response. On your PNA measurement is the extra length for the connectors compensated for or is it still in? Or did I screw up the length of the board. I think I did 28mm. (1.1" ?)
It's 62 vs 88 degrees per GHz. (The Sonnet result being around 50/GHz maybe?)
This thing: https://chemandy.com/calculators/coplanar-waveguide-with-ground-calculator.htm tells me that the effective Er is about 3.4
Than this: https://www.microwaves101.com/calculators/873-wavelength-calculator says that 1GHz wavelength is 162.7mm
Based on that:
Mine: 28.02mm
PNA: 39.77mm (assuming a uniform Er=3.4 line, see below)
Sonnet: ~23mm ?

If your board is indeed 1.1in and the SMA connectors are on it, which I assume have a teflon dielectric with Er ~ 2 then  7.5mm@Er=2 + 28mm@Er=3.4 + 7.5mm@Er=2 actually gets us 88degrees @ 1GHz would explain the PNA S21 phase slope perfectly.

I would try to figure out if this is correct so far and the look into why Sonnet thinks the section is shorter.

I would have expected the two simulators, being fed the same data would have yielded roughly the same results.  I had assumed you had used the data from the AppCAD drawing  but it sounds like you had not used these values.    This make much more sense now why there is such a difference between the two.   

Yes, all the dimensions were in inches.  Yes, 1.1" or 27.94mm.   

https://www.eevblog.com/forum/rf-microwave/experiment-testing-the-effects-of-releaving-ground-plane-beneth-a-component/msg3609708/#msg3609708

I wasn't too concerned with the data from the PNA beyond seeing if any of the data was even in the ballpark.  Eventually I will go back an measure everything but for now I am just trying to understand why the results from the simulators are so different.

You could provide details about your simulation and I would change my model or you can use the data from AppCAD and see what you come up with.   Maybe we could do both as it would not hurt to run more than one test case.   

[Marsupilami]

No no I totally used those values from your screenshot. I just rounded stuff to near metric units as my European brain can't process imperial properly.

Trace width: 2.8mm
Gap width: 2.1mm
Dielectric thickness: 1.5mm
Copper thickness: 0.09mm
Er of dielectric: 4.6
Length of the section: 28mm

[joeqsmith]

No no I totally used those values from your screenshot. I just rounded stuff to near metric units as my European brain can't process imperial properly.

Trace width: 2.8mm
Gap width: 2.1mm
Dielectric thickness: 1.5mm
Copper thickness: 0.09mm
Er of dielectric: 4.6
Length of the section: 28mm

Rechecking your work,
The copper is 0.00135" or 0.03429mm.    0.09mm - 0.0035", I suspect that was a typo in the conversion.
The dielectric is 0.062" or 1.5748mm.  I would round to the nearest, or 1.6mm.

If you don't mind changing it, then run a few different test cases (without the gap).  Post your Touchstone files.  I will then repeat your conditions and post the results as well.  I will change to metric to make it easier for you.   

[Marsupilami]

If you don't mind changing it, then run a few different test cases (without the gap).  Post your Touchstone files.  I will then repeat your conditions and post the results as well.  I will change to metric to make it easier for you.

I will but I doubt any of those differences would get us significantly different results.
I'll set up fixed grid points too to get better aligned with the ideal geometry.

[Marsupilami]

I haven't set things up to run this yet but it might be worth trying.

Have you done anything else with it? I feel it's too late for me to dig into it but I'm still curious to hear about some first hand experience with OpenEMS.

[joeqsmith]

For the length wise, I am using a cell size of 0.005".  For the width, I was using 0.001". 

I too am interested in seeing results from OpenEMS.  I stayed away from it due to it being script driven.  Similar to creating SPICE netlists by hand rather than being schematic based.   Maybe there is a front end for it.   

[MartinL]

There isn't any polished frontend as exists for the commercial packages. There's Qucs-RFLayout which allows you to put together a schematic in Qucs and then export to openEMS script. It currently only supports microstrip structures though, not GCPW.

And there's a FreeCAD plugin that can export geometry to openEMS.

The MATLAB scripting interface is actually already a "frontend". the actual interface to the OpenEMS solver is a C++ API.

There's also two python libraries, pyems and pyopenems, which provide a higher-level API than the built-in bindings.

I've always thought there's a real opportunity for someone to build a nice GUI on top of openEMS - it could be a game changer in making these sorts of capabilities more accessible. But it would be a big project with a fairly small potential userbase, many of whom either already have access to commercial tools, or can get by with the existing interfaces.

I'll see if I can get something running that corresponds to the test case you have.

[Marsupilami]

Here are the results of another run.
I changed the dielectric thickness to 1.57mm and the copper thickness to 0.035mm.
I also aligned the grid points to the trace features.




The return loss looks significantly different on a magnitude plot but I think below 25dB I'm hitting some numerical limits. I'd have to play around more with meshing and waveguide port settings.
The transmission changed very little.

[joeqsmith]

I had thickened the Cu layers as well, no difference.   I removed the vias to speed the tests but saw no major change.   I noticed you are using 4.  I could add them back in if you want to provide details about them.     

The width of each top side plane is 351mils or a total width of 981mils 
Cu conductivity is set to 5.8e7 S/m
FR-4, 62 mils thick, Er 4.6, Loss Tan 0.02, Conductivity 0.0 S/m, Mrel 1.0,  Mag Loss Tan 0.0
Ports resistance is set to 50 ohms (license prevents any changes)
I'm using an inch from the top of the CPW to the box, air dielectric
I'm not using the de-embed feature, symmetry

The attached Touchstone is with the above setting and matching the AppCAD drawing.   I doubt any of this will matter and suspect there is some difference in the simulators that causes this error.   

If  you want to see if the two simulators will show somewhat of a trend, I reduced the width of of the signal trace from 113 mils to 16 mils. No other changes were made.   

****
Using the baseline from AppCAD, I then changed the dielectrics thickness to 10mils.