4 layer PCB design problems at Microwave frequencies

[naman.barmecha]

Hi,

I had designed a 4 layer PCB board for 13 GHz using RO4003 as substrate material. In oder to get the feel of designing boards at these frequencies, I started with a 50 Ohm microstrip. The microstrip forms the top layer, and the remaining 3 bottom layers are stitiched together as ground. For some reason, I see resonances and high insertion loss at fequencies greater than 9 GHz. But, if I peel off the bottom two layers and convert the 4 layer board to 2 layer board, it works fine. Has anyone experienced the same problem or can provide some guidance on solving and understanding this issue.

Thanks,
Naman

 

[thylacine1975]

Heya naman,

I suspect you're exciting (unwanted) parallel plate waveguide modes between the stacked layers of unused ground planes. With regular stitching vias I know it seems you *shouldn't* (couldn't) be exciting such modes, but the tenacity of those EM fields never ceases to amaze me

A recent 5 GHz design of mine required the distances between the ground-plane stitching vias (for a length of coplanar waveguide on 4003) to be made *much* smaller than I would have intuitively expected - the crosstalk and unwanted modes finally fell to an acceptable limit at around 5 mm spacing. At 13 GHz...? The two layer design sounds the best approach at any rate (and perhaps preferable from a cost/manufacturability standpoint?) but if you've got 4 layers for other reasons, you could always just not place copper on the lowest 2 layers.

Keep an eye on your substrate thickness so as not to provoke excessive radiation loss too.

Cheers!

 

[vfone]

Is just about basics of capacitor Self Resonant Frequency. Your ground planes form a capacitor which resonate at particular SRF.
As was stated, use multiple vias between grounds and the problem will disappear.

 

[FvM]

Although sufficient via fences should abandon most problems, even a single ground plane can show modes if the coaxial to microstrip transition isn't made correctly.

 

[naman.barmecha]

Thanks all for the info. I do have quite a bit of vias placed at 4 mm apart. I will try to get them as close as possible from manufacturability point of view and see if it works. I will update this thread once I do the test with more closely spaced vias.
Appreciate your help.

 

[Element_115]

Hi,

I had designed a 4 layer PCB board for 13 GHz using RO4003 as substrate material. In oder to get the feel of designing boards at these frequencies, I started with a 50 Ohm microstrip. The microstrip forms the top layer, and the remaining 3 bottom layers are stitiched together as ground. For some reason, I see resonances and high insertion loss at fequencies greater than 9 GHz. But, if I peel off the bottom two layers and convert the 4 layer board to 2 layer board, it works fine. Has anyone experienced the same problem or can provide some guidance on solving and understanding this issue.

Thanks,
Naman

It sounds like the Grounding is an issue. When you have 4 layers, I assume your SMA's ground is connected to the bottom layer. Once you use vias they can act like inductors and each ground planes can act as Caps (especially at high freqs). Also be careful when you solder the SMA center pin to the
PCB. What seems like a small gap can be a big issue at these frequencies.

 

[tony_lth]

The wavelength of 13G in air is 23mm, so in the board it's about 23/2=12mm. Quarter wavelength is about 3mm, but your via spacing is 4mm, how do you think. 1mm spacing with several lines interleaving is better.