1
\$\begingroup\$

I'm working on designing a board with the RFM22B-S2 SMD Wireless Transceiver - 915MHz. The board module requires a 50 ohm feed line to the antenna. I've been looking at trace impedance calculators and I'm confused. So far every calculator I've found has a micro strip, a single trance on top with a ground plane on the bottom.

Why is there not a ground plane on top as well?

Is there a calculator that accounts for the top ground plane or is there some minimum amount I have to pull the top plane back from the feed line?

\$\endgroup\$
  • \$\begingroup\$ Either pull the ground for more than 3h,where h is the dielectric thickness. Or use a coplanner waveguide calculator \$\endgroup\$ – Mike Nov 14 '15 at 0:36
  • \$\begingroup\$ @Mike Could you post your comment for the coplanner waveguide calculator as an answer. It was the best solution. I will accept it as an answer. \$\endgroup\$ – vini_i Jan 9 '16 at 0:52
1
\$\begingroup\$

There are a number of pcb transmission line typologies. Some of them include Microstrip, Stripline and Coplanar Waveguide.

Microstrip is a single trace on the top layer, with no ground close to it on the same layer. There should be a solid ground in the layer underneath the trace. As seen here:

microstrip

In this case, close refers to at least 3 times the substrate/dielectric thickness.

In case you have ground on the top layer, which is close enough to the trace (3h, as mentioned), you have a topology called Coplanar Waveguide. You can either have a coplanar waveguide with a ground on the 2nd layer or without.

Coplanar

You have to find the appropriate calculator, in your case (coplanar waveguide) you can try this calculator, or use one of the many found in google.

\$\endgroup\$
1
\$\begingroup\$

The term you're looking for is stripline, which consists of a pc trace sandwiched between ground planes. Microstrip has gained popularity because of the widespread use of high-speed digital lines, which have a certain tolerance for things like crosstalk. Stripline is a better-controlled technique, but it requires rather more in the way of design and pcb resources (3 layers instead of 2).

\$\endgroup\$
0
\$\begingroup\$

I believe your question is about a 50 Ω trace on the top layer and its spacing from ground planes on that top layer. This can be answered by considering the edge coupled microstrip: -

enter image description here

At first this may seem nonsence but, if you imagine a vertical line halfway between the two microstrip traces, then this line will be at zero volts AC potential i.e. halfway between the differential pair of microstrips could be regarded as 0V.

A small leap of mathematics takes you to realize that you can actually use this type of calculator to do what you want....

At half "s" maybe you can imagine an extended groundplane on the top layer and the impedance seen from one microstrip to "ground" is half that calculated. Thru symmetry this extended ground plane exists on either side of the single trace.

\$\endgroup\$
  • \$\begingroup\$ If i'm understanding you correctly, the addition of a second ground plane on the other side would cut the impedance in half. What impedance should I be looking at odd, even, common or differential? \$\endgroup\$ – vini_i Nov 14 '15 at 2:24
  • \$\begingroup\$ A groundplane beginning at half s halves the differential impedance I believe. I'll take another look properly later to confirm. I'm on android at mo so impractical to give more info. \$\endgroup\$ – Andy aka Nov 14 '15 at 9:44

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

Not the answer you're looking for? Browse other questions tagged or ask your own question.