I did not see a mention of the characteristic impedance used in the PCB layout for the evaluation board (600-00435). I used a calculator based on the stack layout and found it to be 75 ohms. Is that correct? I thought the norm is use 50 ohms. Is there a reason why it was chosen to be 75 ohms. Do you offer gerber files with 50 ohm characteristic impedance?
Regarding the HMC374SC70E evaluation board PCB # 600-00435-00-2, the Z0 target for the RF traces is 50 ohms. Using a gerber reader to view the gerber files posted on the product page...
...I measured the following dimensions:
The fab drawing (the .pdf file in the gerber package) shows the topside metal as 1/2 oz copper, which has 0.7 mil thickness (which is standard for 1/2 oz copper). The fab drawing also calls out a plating thickness of 0.002"=2 mils for the topside metal, making the total thickness of the topside metal T~=3 mils. The fab drawing also calls out the RF dielectric layer as 0.01"=10 mils (=H) of Rogers 4350B or Arlon 25FR, both of which have an approximate epsilon of 3.48.
This transmission line would be best modeled as Coplanar Waveguide with Groundplane (i.e. GCPW). Entering the technical details from above into a calculator such as AppCAD, I obtain Z0=60.6 Ohms...a bit high, but not 75 Ohms. Our PCB designers have told me that, even though the impedance calculates out a bit high, the PCBs we receive are pretty much dead-on at 50 ohms. Perhaps more sophisticated modeling techniques such as EM sim would return a value closer to 50 ohms.
See attached fab details and calculation results. The gerber files linked above are the ones to use for Z0=50 ohms.