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.

Thermal Relief on RF PCBs

Not open for further replies.


Newbie level 5
Jan 31, 2013
Reaction score
Trophy points
Canberra, Australia
Activity points
Are there any rules of thumb for thermal relief on RF PCBs running at 2.4GHz?

I have taken over the design of a system that the previous engineer had refused to do any thermal relief on in the belief that this was a no-no for RF PCBs. However no thermal relief is creating a lot of manufacturing problems (tombstoning of SMD parts, difficult rework). Hence I would like to put in thermal relief.

Is thermal relief really a problem at these frequencies, or is my predecessor over-cautious? The size of the relief is such a small fraction of the wavelength that I struggle to see why it should create a problem.

I'm thinking that I will put relief on:
All SMD component pads
All power-plane connections to vias that are under or near components pads - the PCB uses filled vias (vias-in-pad) technology.
elsewhere the planes will remain stitched with direct connect vias.

Does anyone know any rules or thumb or techniques that I should be using? Does the above approach seem reasonable?


SMPS's are regurarly designed without thermal relief on SMD pads these days. I have seen numerous designs with no thermals on the SMD pads and I know that thousands of boards have been made. What I have not seen is tombstoning (in fact I have only ever seen it 3 times in my career as a PCB designer). It worries me that you are getting tombstoning, I would look at the thermal profile for the boards, solder paste deposits etc.
  • Like
Reactions: FvM


    Points: 2
    Helpful Answer Positive Rating
Thanks Marce.

Our contract manufacturer has done what they can and have indicated that only PCB changes will improve it (and hence reduce the rework).
The PCB is about as bad as it can get with multiple layers of ground planes. The thermal in-balance between a ground pad and a signal path on the likes of a 0402 component means that solder flows differently on these pads and pull the component up. The manufacturing process uses vapour phase soldering and lead free solder - both of which I believe make things worse.

Rework of the PCB is the other issue - they currently need a lot of pre-heating to be able to work on them due to the large ground copper area.

So thermal relief is required in this case - I just want to see if it is going to bite me with RF performance problems. So anyone's experience with placing thermal relief on a PCB with 2.4G RF would be helpful.


I don't see how missing thermal relief would promote thumbstoning, presuming correct SMD processing. Thermal relief is strongly unwanted for RF circuit, bypass capacitors in digital and fast analog circuits that are planned to be low-inductive, all kinds of power circuits, any via with thermal functionality, dedicated thermal vias as well as regular vias connecting pins of power components to planes.

Thermal reliefs are often required for through-plated component pins to allow correct wave soldering. This can create a conflict of objectives in case of power or ground pins. As a compromise, we e.g. connect only one of multiple ground planes.

I see the rework problem. Rework stations providing preheating of SMD boards are an industry standard however and should be used at least for sensitive boards.

On the other hand, thermal relief might be acceptable for components with moderate ground inductance requirements, e.g. small capacitor values. You can also estimate ground inductance numbers and put them into your design calculation.

Thanks for your comments. Although it is understood that some level of preheat is normal for rework, our PCB seems to be at the extreme.

I have plenty of references citing thermal imbalance being a common cause of tombstones, and the fix being thermal relief. What I'm trying to understand is the effect of this relief on the RF circuitry. I'd like to be able to put some real numbers to it. For example, what would be the impedance of the component to plane connection with and without thermal relief? How could I estimate this? From here I can judge if this is significant at 2.4GHz. I'm still researching this, so any ideas on where I can find some real impedance numbers would be helpful.

- - - Updated - - -

Found some more references:

This looks like a good resource on RF design. It says not to use thermal relief for RF design, and that RF/Microwave is >500MHz, although >100MHz is considered to be RF.

Based on this I will minimise my thermal relief to only the non-RF parts of the circuit that need it.

I have plenty of references citing thermal imbalance being a common cause of tombstones, and the fix being thermal relief.

It's probably a question of applied soldering technique. Modern solder methods achieve an almost uniform heating of components and board, thus there's no problem with vias or asymmetrical heating of component pads.

Not open for further replies.

Part and Inventory Search

Welcome to