Questions about RF board layout

[alard]

rf layout

Hello,

Need you guys' help again! I finished the design of a microstrip filter working at several Giga hertz. I wonder if I need to put GND plane through vias at the blank area on the top layer?

If so, how much is the clearance between ground and signal line? And what about the radius of vias and the distance between two vias? How can I arrange these via holes? Shall I put them periodically along my signal line?

So many question. Thank you in advance!!

Warmly,
kevin

 

[ahmad_abdulghany]

I recommend to let your RF circuit swim in a sea of ground!!

 

[Lance_RFdude.com]

Hello,

Need you guys' help again! I finished the design of a microstrip filter working at several Giga hertz. I wonder if I need to put GND plane through vias at the blank area on the top layer?

If so, how much is the clearance between ground and signal line? And what about the radius of vias and the distance between two vias? How can I arrange these via holes? Shall I put them periodically along my signal line?

So many question. Thank you in advance!!

Warmly,
kevin

I would be careful of adding ground haphazardly. You'll hear several schools of thought on this but I typically try to avoid any ground there without a good reason. You may need to keep some patches of ground there to keep the board more balanced (avoid warpage), but as much as ground can do good, it can also make some things worse. If you do put ground down make sure you've got enough vias spaced <<<wavelength to keep the patch from becoming a resonator.

If you've got a good EM simulator you might want to experiment with the effects of topside ground... if you do place it there, just make sure you do it right...

Lance

 

[normaldist]

If you have ground planes above each other, they absolutely need to be "stitched" together with vias. I typically place a 10mil via every 250 mils on a grid across my entire board. I do this after I finished laying out all of my components and omit any vias that would interfere with any thing.

I have heard several schools of thought about ground plane clearance for microstrip, typically > 2*W microstrip. When designing GHz filters on PCB, you will have alot of difficulty with "schools of thought" thats why I use a EM simulator to determine the effects of a ground plane. You should break the circuiit up to do a EM simulation to save time.

C

 

[alard]

Thank you guys. Any references on this topic are welcomed.

 

[DDavid]

Hi,

Like you said you are doing Microstrip and not CPW!!!!!

You said that you designed filter if you did it with simulation so you can check it there, just add GP around M lines and EM sim.

If you not using simulation I suggested to put GP but with distance at least w (if H>W) but the best is 2w gap from Microstrip to GP.

David

 

[alard]

Yes, I am going to simulate it in ADS momentum. But I would like to have a good start since my computer has only 1G memery. Even doing the simulation without upper GND, it may take me half hour

 

[DDavid]

Hi,

Like I understand if you will make without GP (on top) and will run Momentum you will get good results!

David

 

[alard]

Yes I got a quite good result when simulating without GND on top. But I am not sure about what it woud be after manufacturing and how the GND would affect the result.

 

[DDavid]

Like I said before ifyou will put gnd on top you have to go atleast w (2w the best)
What this mean?
This mean that gnd don't have influence...

This is my thought.

But if you will put a gnd with gap 2w I believe you will have the same results more or less.

David

P.S. If you are using connectors you must close gnd.

 

[normaldist]

Alard,

You have asked what the results would be when this PCB is manufactured. There are a number of issues.

It may be helpful at this point to know what kind of filter topology you are developing, is it a coupled edges? If so, you have to make sure that the widths and gaps are realizeable. When they are les than 8 mils you will start to have significant tolerance issues. Also, you will need to control things like the surface finish and solder mask. MOM simulators do not model thickness, 1 oz copper is 1.4 mil thick and HASL finish can add a mil. if gaps are small, you will have deviation from MOM results. Also, are there any shunting vias in the filter? You will have to have a good model for them at GHz. Assume the via is a cylindrical shell and calculate it L is a decent model.

When you get into GHz, your model better have good simulation of the parasitics. With that I have developed excellent filters past 6GHz on R4003.

Good luck

C

 

[madengr]

The 2*W rule of thumb has been mentioned a few times. Isn't it really 2*H? A circuit with a Z0=10 ohm line should still be spaced at 2*W? Probably not. 2*H makes sense since the closest ground is always at 1*H.

I have had this issue too. The customer wanted ground fills on top and it does help with warping. My philosphy is 1*H spacing until you approach lengths of 1/4*walength, then space it farther. This is for plain old microstrip txlines, not stubs or resonantors. As suggested us an EM simulator. You can use a coarse grid so it's fast.

Another philosophy is don't ground components to the ground flood (unless it's really CPW). The via inductance will turn that top-side ground flood into a patch antenna. Each SMT component should have it's own via(s) to the ground plane.

Anyway this is an intersting topic. RF philosohpy is ALWAYS argued about in design reviews. The funny thing is that everyone just waves their hands instead of whipping out a notebook with example calculation to show their point.

That thick metal can be approximated in 2.5D EM by stacking layers. Sonnet has a "thick metal" option which does this automatically:

**broken link removed**

 

[Lance_RFdude.com]

Another philosophy is don't ground components to the ground flood (unless it's really CPW). The via inductance will turn that top-side ground flood into a patch antenna. Each SMT component should have it's own via(s) to the ground plane.

Anyway this is an intersting topic. RF philosohpy is ALWAYS argued about in design reviews. The funny thing is that everyone just waves their hands instead of whipping out a notebook with example calculation to show their point.

I go with the "don't ground to the flood" philosophy as I've seen things go awry. It can become too easy to get sloppy and let the DRC convince you that everything is perfectly connected to ground...

there's a good example of this (albeit a simplistic one) in crawford's synthesizer design handbook (a little out of place in a very early chapter) but it illustrates the point I've seen before. It shows a lowpass filter where the shunt caps are all tied to a "bus" bar on the topside with periodic vias. it shows coupling through the floating ground bus in the stopband ... versus different via spacings in that ground bus bar. interesting stuff.

I would prefer higher inductance in series with each part (i.e. individual vias for each component) over "less predictable random paths through topside ground patches". For matching or bypass caps you can always compensate by adjusting the value (at least over some bandwidth).

the consistent message is of course that one can obsolete the rules of thumb quickly by analysis

Lance

 

[Azulykit]

This is a question that should be addressed with a good simulator. I am unsure if your filter is using discrete components or a coupled transmission line architecture. I also saw mention of CPW and microstrip in the discussion. If it is microstrip it is not clear where you would place via's.

In this frequency band I would not want to depend on rules of thumb. Analysis is really necessary unless you have the time and energy for lots of experimentation and tuning in the lab.

I have recently been working with another engineer on a interdigital filter several GHz higher than your application and we have been using Eagleware and Ansoft's HFSS to evaluate the design. Our first set of measurements came reasonably close to the simulations.