ST25RU3993-eval PCB Internal amplifier output differential traces don't look right for preferred impedance.

[DBurt.1]

ST25RU3993-eval PCB Internal amplifier output differential traces don't look right for preferred impedance. See the traces circled in red. Shouldn't these be 100 ohm differential the same as the purple mixer feedback traces? The trace width in the layout is clearly not the same as the purple marked 100 ohm diff traces.

[DBurt.1]

I see the balun chosen for the amplifier output has a 50 ohm balanced input rating. So perhaps those traces are meant to be 50 ohm differential rather than 100 ohms?

Seems like the geometry I see in the gerber file is more like 64 ohms differential though. (31.5x5.9x31.5 mils with t=9.8 mils)

[Bart Herse]

Hello DBurt.1

the differential output impedance of the internal PA is neither 100 ohm or 50 ohm.

Therefore the trace geometry is a compromise of what is required and what can be manufactured with a reasonable effort.

The matching circuit connected to the differential outputs of the internal PA mach the impedance to the single-ended 50 ohm traces via the 1:1 balun.

Cheers,

B

[DBurt.1]

Thanks for the reply. I need to compromise on those nets as well. I ran the 100 ohm diff numbers and based on the gerbers and stack up specs and those look to be about 120 ohms. Why would that be?

I'm needing to scrunch things down quite a bit more than the eval board so my routes aren't quite as nice, especially the tuning cap section. Hopefully that won't cause too much problem.

[Bart Herse]

Which tool are you using to calculate the trace impedances since I cannot confirm your results.

Cheers,

B

[DBurt.1]

I usually consult with Saturn toolkit, my cad built in calculator (Ultiboard), and some web based calculators (https://www.pcbway.com/pcb_prototype/impedance_calculator.html is one). They all match within a couple ohms. From the gerbers and manual I get 14.6x24.3x14.6 mils with h=9.8 mils and e=4.5 for the 100 ohms diff pairs. The eval board says e=4.7 for the top DE, but my builder says use 4.5 for their process. Makes little difference anyway.

[Bart Herse · Accepted solution]

Hi DBurt.1

You mentioned your calculation results to 120 Ohms using the parameters below:

W=14.57 mils

S=24.4 mils

H=9.84 mils

Er=4.5

Testing with one of the tools you have mentioned I get a trace Zdifferential of 99.4 Ohms and Z0=52 Ohms.

I suggest if you have doubts use the tool your PCB manufacturer recommends and/or let ask your PCB manufacturer cross check the impedance with the insights of the specific manufacturing process.

Cheers,

B

[DBurt.1]

I re-checked on Saturn and it does agree very closely with your answer. For this one I had used pcbway, which gave just over 118 ohms. I suppose I'll cross that one off my list of calculators to use. Thanks.