Re: Choosing the right substrate thickness for RF PCBs

Robin Szemeti - G1YFG

Nope, it depends which stackup.

7628 is a 0.2mm outer stack with Er=4.6, the 3313 stackup is a 0.1mm stackup with Er=4.05

Both have the same Er for the solder resist of 3.80 .. it is of course up to you is you place solder resist on the RF bits.

and full details of the stackup are here:


On Mon, 18 Jul 2022 at 21:53, KENT BRITAIN <WA5VJB@...> wrote:
Do some 50 Ohm lines in their program, then try another program..

VERY high probability they are using Er = 4.4

On Monday, July 18, 2022 at 03:49:45 PM CDT, Robin Szemeti - G1YFG via <> wrote:

If ordering 4 layer from JLCPCB note they have two different "stackups" with different material for the 0.2 layer ... you can specify which stackup in the "impedance control" option.

They have an impedance calculator for the two stackups as well ...

On Mon, 18 Jul 2022 at 18:35, KENT BRITAIN <WA5VJB@...> wrote:
Also the materials change Er with frequency.

Er's of 3.5-3.7 are more typical in the 5-10 GHz range.

The typical Er 4.4 is measured at 1 kHz.

On Monday, July 18, 2022 at 12:17:47 PM CDT, KENT BRITAIN <wa5vjb@...> wrote:

The fiberglass materials can be used at 10 GHz and even higher.
The important part is to keep traces a short as practical.
If you make a 10 GHz MMIC amp, try to have the whole board
only 20 or 30 mm long.  And use thinner material.  We would say 20 or 30 mil material.

For the MMIC ground tabs, us 3 or 4 ground vias on each pad.  One via usually has too much inductance at 10 GHz.   And the extra vias help conduct heat away from the device.

I love how the term FR4 continues on and on and on .........
FR4 had a Bromide anti-flammability compound in that was banned by RoHS.
It has not been manufactured in many years.   Yes, similar materials are available, but not actually FR4.

Good luck with your project   Kent WA5VJB/G8EMY

On Monday, July 18, 2022 at 11:48:45 AM CDT, Arved M0KDS <arved95@...> wrote:

Hi all,

I think similar questions may have been asked in the past but here we go again.

I am planning to use some MMICs up to 10GHz and I am still deciding on which PCB material to use. 

I have done some experiments in the past with old GaAs-Fets I had laying around on FR4 with either 0.6mm or 0.8mm thickness.
The only issue I've always had were self oscillations. I think part of the reason (including ground loops most likely)
for that might be the additional inductance created by the vias due to the "thicker" substrate.

I am aware FR4 is not ideal for this purpose but it's nice and cheap for experiments and can be made professionally for little money. 
I read through some old threads here on this reflector and in one of them I saw someone mentioning the use of 4 layer PCBs to get down to 0.2mm thickness (if you use the first two layers).

I do understand how it's meant to work. The only I am wondering is whether the remaining two bottom layers should also be connected to Ground or whether they should just be left unconnected (inductance?).
Maybe if someone has done some experiments on this I would be very interested to know. 

Many thanks and 73,

Arved M0KDS / DK5AV 

Robin Szemeti - G1YFG

Robin Szemeti - G1YFG

Join to automatically receive all group messages.