Continue to Site

Welcome to

Welcome to our site! is an international Electronics Discussion Forum focused on EDA software, circuits, schematics, books, theory, papers, asic, pld, 8051, DSP, Network, RF, Analog Design, PCB, Service Manuals... and a whole lot more! To participate you need to register. Registration is free. Click here to register now.

Microstrip layout - can the path be branched?

Not open for further replies.


Newbie level 6
Jul 2, 2009
Reaction score
Trophy points
Activity points
I don't have much experience with RF layout considerations regarding trace routing and anything that may affect performance (such as type of trace bends or extra pads in the output RF trace) so I am looking for suggestions on a specific question.

If I have an output 50 ohm microstrip line trace going to the chip antenna and I'd like to branch off from this trace to route to a footprint for a coax test port, can I do something like put a 0r jumper in series with the normal chip antenna trace to be able to cut that path when not in use and at the same time have another 0r jumper coming off the RF trace at 90 degrees to route to that test port, so that I populate one jumper at a time depending what RF output path I want?

I didn't know if it was an issue to have a 90 degree bend through the one jumper, and if the unused pads and small dead end (unpopulated) traces matter or not.


Hello, I think the solution is to use the Microstrip TEE or Cross or the best way to use the some thing similar to circulator...

Use any RF Simulation tool to check or verify the above such as Microwave Office (MWO) from AWR has good microstrip routing elements for layout with simulation capability...


Take a look at Murata miniature coax connector with embedded switch.

It has a low inertion loss when the coax is not inserted and it switch the signal into the coax when inserted.

Freq range, If I well remember, is in the range of few GHz.


Mazz said:
Take a look at Murata miniature coax connector with embedded switch.

That was on our last iteration of the design but we've been directed to go with u.fl this time so I need to branch off the main microstrip but I'm not sure what the do's and dont's are. Been searching all morning and I just find general info like RF doesn't like sharp corners etc, but I can't seem to find something specific to tell me how to create the alternate path and if leaving a pad for a jumper will be an issue (I saw something where there was a section of extra bulk that looked like a square pad hanging off a microstrip and it was a notch filter equivalent).

The more I read the more confused I become.

If you deviate the from the parameters of your microstrip at all, you will create an impedance mismatch at the point of deviation. This applies to bends, pads, stubs, etc. This even affects your coax connector at its solder points, likewise with the chip antenna.

That being said, these variations can frequently be pretty minor. While I'm not overly experienced with microstrip layout, I doubt that you'll have much problem as long as you're dealing with lumped element sizes (i.e. the size of the jumper, or other deviation from the microstrip is much less than λ/4) and you're not deviating much from the microstrip parameters (obviously, introducing a short, a large capacitance or a large inductance is going to change things a lot more).

I have, on occasion, seen designs with a 3-pad resistor footprint in the signal path. It acts as a build-time switch. You can either have a test unit or a production unit, depending on how the resistor is populated.

If your λ is short enough that you're not dealing with lumped elements, you might be able to use λ/4 stubs. In that case, you can connect two stubs of λ/4, and always short one (this acts as a bandpass filter). The other goes to the antenna (connector or chip). Be careful to always short one since a floating λ/4 stub is an RF short circuit!

Again, put a bit more research into this, since I'm by no means an expert.

This is an example of what I'm trying to do and don't know if there's a problem with it or how to improve it. 2.4GHz 50 ohm trace coming in from the right side normally feeds to the L3/L4 antenna matching pad directly but we want to add J3 for a U.FL test port. The antenna or test port will be used one at a time so to control this we have R2 and R4 0402 footprints. If R4 is vacant and R2 is 0r, we use the test port. If R2 is vacant and R4 is 0r we use the antenna. It's not a Tee junction that I require since I only need one path at a time. I just need to figure out the proper way to provide a jumper option on a 50 ohm RF trace.

So the single resistor pads sitting there on the 50 ohm trace, I don't know if those are an issue especially when the one is unpopulated and it's a stub, and if throwing the jumpers in series with the 50 ohm trace is an issue itself, if going at 90 degrees from 50 ohm trace into R2 jumper path down to test port is an issue, etc.

I've been trying to find design resources for 2 days and I either find hard core calculations I can't make use of, or just general theory that doesn't apply to my situation. Maybe someone out there can assess what I've drawn? I just roughed in the layout for the purpose of showing the objective.

The best think you can do is to use a single pad for R4 and R2 (you can define a 3 pin component), as you are thinking not to solder them at the same time.

With the overall dimentions used and used freq you will not have any problem to have a direct access to your RF port.


Place a test pad and use an SMA test spring needle as in the figure attached.
I used successfully this approach in production test for many years.
The test pad could be placed on the component side just before the antenna matching components, or on the other side of the board as in the figure attached.
If you don’t have a jig for this device, can be placed a miniature coaxial connector, just for lab conducted tests, and remove it during production tests.

I'll go with the 3 pin right angled jumper approach and see how it turns out. As soon as the layout is done we'll be ready to get samples made so soon enough I'll know if it works.

Your design can be simplified slightly by overlaying R2 and R4 such that there are two placement options in an L shape. This eliminates one pad from your signal trace and and simplifies the problem.

If you do that, then the only remaining question is whether a 0-ohm resistor will affect your signal. It will, but I don't think the effect will be particularly significant since the length of the 0402 resistor is much less than 2cm. (approx 1/4 wave length)

If you want a better answer than that, you only have two options: Use a microwave Finite Element Analysis package, or do loads of brutal calculations yourself.

Do you have 4 cm to spare? If so, the 1/4 wave stub suggestion I made in my previous post is totally viable.

.                <---1/4--->
Receiver--------+-----------antenna match network
.               +-----------test port
Simply short the end of the stub which you're not using, thus turning it into a 2.4GHz bandpass filter.

I won't need to go through all kinds of analysis for my application. I only wanted to know if there's a show stopper with practical considerations of doing this jumpering of multiple paths at 2.4GHz since I don't have experience with it and some info out there makes it sound as if the time of day can impact an RF circuit. If it might have "some" impact on performance that can be negligible then I'm ok, much like if I have a circuit that draws 100mA in normal use and a choice between a few parts could raise that to 105mA, some people might care but I wouldn't. Just wanted to know if I would be turning 100mA into 2.2A in that analogy!

Not open for further replies.

Part and Inventory Search

Welcome to