Author Topic: Ground pour on RF layer  (Read 923 times)

0 Members and 1 Guest are viewing this topic.

Online T3sl4co1l

  • Super Contributor
  • ***
  • Posts: 12987
  • Country: us
  • Expert, Analog Electronics, PCB Layout, EMC
    • Seven Transistor Labs
Re: Ground pour on RF layer
« Reply #25 on: June 13, 2019, 12:03:46 am »
Your screenshot shows a negative angle compared to the diagram in the paper.

2.7GHz is like "DC", see the axes in the paper!

Actually, why are they showing transmission loss at DC?  Is this not the entire structure, are they missing something?

It's also written specifically about monolithic structures (high resistivity Si, SiO2 insulator, micron measurements), so who knows what everything they were doing was.  Maybe it's part of a planar transformer structure, and that's why the low frequency response drops off.

Tim
« Last Edit: June 13, 2019, 12:05:24 am by T3sl4co1l »
Seven Transistor Labs, LLC
Electronic design, from concept to prototype.
Bringing a project to life?  Send me a message!
 

Offline schratterulrich

  • Contributor
  • Posts: 20
  • Country: at
    • Elektronik & Layout
Re: Ground pour on RF layer
« Reply #26 on: June 13, 2019, 12:13:55 am »
I am also of the opinion that the trace width of the microstrip section must become wider than the coplanar waveguide section.
This is due to the increased capacitance of the coplanar section. So with same trace width the coplanar section would show smaller Z0 (Z0=sqrt(L/C)).

I think formula based calculations of trace width has limitations on accuracy. I would prefer TNT for example. It's a free FEM based Transmission line solver. You can find it at https://sourceforge.net/projects/mmtl/

I don't know free simulation tools capable of simulating the transition from Coplanar to Microstrip. But there are models for tapered lines, corners and pads in Ansoft Designer SV. It's a obsolete free student version of a very comprehensive RF suite.
You can find it at http://www.gunthard-kraus.de/Ansoft%20Designer%20SV/English%20Tutorial%20Version/DesignerSV050610.exe
You can find a good introduction somewhere on this homepage http://www.gunthard-kraus.de/
 

Online Nikos A.

  • Regular Contributor
  • *
  • Posts: 53
  • Country: cy
Re: Ground pour on RF layer
« Reply #27 on: June 13, 2019, 12:28:44 am »
Your screenshot shows a negative angle compared to the diagram in the paper.


Please see my calculations (attached files) for microstrip and coplanar trace width.. The coplanar is wider.. Do I have anything wrong?



Thank you for you links!!
 

Online T3sl4co1l

  • Super Contributor
  • ***
  • Posts: 12987
  • Country: us
  • Expert, Analog Electronics, PCB Layout, EMC
    • Seven Transistor Labs
Re: Ground pour on RF layer
« Reply #28 on: June 13, 2019, 08:16:32 am »
Yeah, going to guess Saturn's CPWG formula is wrong. :)

Again, while theoretically amusing, these tweaks are way, way down in the noise of practical engineering.

Tim
Seven Transistor Labs, LLC
Electronic design, from concept to prototype.
Bringing a project to life?  Send me a message!
 

Offline TheUnnamedNewbie

  • Frequent Contributor
  • **
  • Posts: 758
  • Country: 00
Re: Ground pour on RF layer
« Reply #29 on: June 13, 2019, 05:01:26 pm »
I stuffed both into HFSS real quick. Take these results with a grain of salt, as I didn't solve it the 'right' way for such low frequencies:



Modes from modesolver below. I think the problem here is that the distance to your gap is significantly larger than the thickness of the PCB. As a result you pretty much get a microstrip, with some additional metal on the side that results in more fields going through the air. This in turn results in somewhat lower capacitance. This is also seen in the simulations - the CPW has higher impedance.

(note that while the impedance are not exactly equal, they are within what you can expect from standard FR4 tolerances).





If I have time later, I might actually try and giving you the design of a quick taper from HFSS too, and compare results of what you had as well as with/without taper.
The best part about magic is when it stops being magic and becomes science instead
 

Offline schratterulrich

  • Contributor
  • Posts: 20
  • Country: at
    • Elektronik & Layout
Re: Ground pour on RF layer
« Reply #30 on: June 13, 2019, 09:23:23 pm »
Did you connect the "coplanar" planes to ground at the waveport entry in your HFSS simulation?
 

Offline TheUnnamedNewbie

  • Frequent Contributor
  • **
  • Posts: 758
  • Country: 00
Re: Ground pour on RF layer
« Reply #31 on: June 13, 2019, 09:51:04 pm »
Did you connect the "coplanar" planes to ground at the waveport entry in your HFSS simulation?

I forgot! re-did the sweep, same shape, but now around 49 ohm instead.



In other words, the two give pretty much the same impedance indeed, just with a slight offset found in the saturn pcb calculator tool. Doing a full s-parameter simulation gives me the same results within a fraction of an ohm.
« Last Edit: June 13, 2019, 09:59:12 pm by TheUnnamedNewbie »
The best part about magic is when it stops being magic and becomes science instead
 

Online Nikos A.

  • Regular Contributor
  • *
  • Posts: 53
  • Country: cy
Re: Ground pour on RF layer
« Reply #32 on: June 13, 2019, 11:09:45 pm »
Thank you guys for your help, so I am going to proceed with this design and will reconsider after testing the completed board.  :-+

 


Share me

Digg  Facebook  SlashDot  Delicious  Technorati  Twitter  Google  Yahoo
Smf