Welcome to our site! EDAboard.com is an international Electronics Discussion Forum focused on EDA software, circuits, schematics, books, theory, papers, asic, pld, 8051, DSP, Network, RF, Analog Design, PCB, Service Manuals... and a whole lot more! To participate you need to register. Registration is free. Click here to register now.
What makes you think a multi layer board with stubs on the dual ground vias makes a good ground plane?
The coplanar tracks are OK but not the stubs orthogonal to the vias so near the dielectric between the conductors.
The Dk , low loss tangent , and etch back factors are also needed as well as type of gold plating.
it is also not drawn to scale and ought to have a w/h ratio near 2 depending on Dk or Er
For ~ 10 GHz you are concerned about zagged sharp edges for conductors and you have a comb running vertically on both sides producing lots of zeros.
The posts are high impedance on their own, so making the coplanar the same dimensions with stubs below is not good. This is a rough idea how to visualize the ground plane to scale.
Good one Volker. Yes the pins and shoulder (I estimate) are about 0.5 nH/mm which is ~30 ohms per mm inductive @ 10 GHz with the gap having some capacitance in the cavity thus raising overall Z^2=L/C. It seems you chose around 3.8 for insulation.
Notice how Volker also made the coplanar distance much smaller than the inner post width. The ratios or conductor OD/ID determine the impedance in the coaxial get flattened into the rectangular wave guide . the coplanar insulation gap is not so sensitive as the vertical gap and conductor width. Since the skin effect is now about 0.6um (or about the 1/4 wavelength of UVC @ 10 GHz) the inner surface roughness in reality will also add length and inductance with scattering diffusion but not show up in your simulation.
Thank you very much for your help sir SunnySkyguy and volker@muehlhaus.
I make the modifications in the simulations and I will come back to you for the new results
thank you
With thinner substrate to gnd plane, you can achieve low impedance with thinner tracks and lower loss with less material in between.
But beware the dimensions become more critical with smaller size and electrical testing is recommended to validate Er with TDR supplier tests, while effective Er reduces with rising frequency in this range.
Z only depends on the surface ratios of the OD/ID for a given Er, and not so much the size.
However making a thin laminate makes it too flexible so a stiffener is needed underneath in some cases like bulk FR4 and surface roughness becomes more sensitive.
We used to make them in FPC this way for a flex cable to reduce flex but can be shaped.
For the strip line the Rogers substrate needs to be about half the thickness of the trace width. Compute for actual value with more gnd plane vias in the middle.
Getting a high performance launch into a micro strip with side grounds and vias often is achieved with a combination of simulation and lab testing. I have often used Hittite and Southwest Microwave connectors and demonstration boards as a guide. The details of your particular connector and small gaps all play into the launch.
Typically the RF feed is on layer one and the ground plane is on the next layer. At 10 GHz a -15 to -20 dB s11 should be relatively easy to achieve and maintain. If your stack-up really puts the reference ground several layers down, that might be the source of your issue. Alternately, you could reduce the side gap spacing if you cannot put the ground on layer two but exciting the appropriate coplanar mode would be an issue. My preference is to keep the line looking like a simple micro strip with the strongest fields between the center conductor and lower ground.
This site uses cookies to help personalise content, tailor your experience and to keep you logged in if you register.
By continuing to use this site, you are consenting to our use of cookies.
