Assembly challenges for shared pad between mounting hole and resistor
Hi,
I was watching Many EMC Tips to Help You Design Better PCB Boards (with Keith Armstrong) and at 1:01:30 timestamp he talks about bonding reference plane to chassis and emphasizes that the connection has to be low-impedance and very close:
My question is the practicality of doing this, how would the assembly process look on the left side pad of the resistor? I imagine the paste would flow all over the mounting hole pad. Here is what I had in mind instead:
Please let me know what you think about these two options and any experience you have regarding this!
3 answers
Here's how I usually lay out optional grounding through a mounting hole. The connections are wide copper pours which reduces the connection inductance. Multiple vias to GND also reduce inductance.
One may have insights about the EMC, but one doesn't really know until one tests. Optional earth ground is useful in prototype boards. Furthermore, the EMI situation may change because the way your device is used may change (normal turn of events for lab equipment, for example).
The R201 and C201 footprints are 0603, and they have a finite inductance. I haven't got data up to what frequency range this connection is effective against EMC. If I needed to make an ad hoc low inductance connection there, I would solder a wide strip of braid or copper tape across R201 and C201.
p.s. Another way to create a mounting hole with a disconnectable chassis ground. If your mounting hole works with a standoff, sometimes you have a choice if the standoff is plastic or metal.
The following users marked this post as Works for me:
| User | Comment | Date |
|---|---|---|
| Elleanor Lopez | (no comment) | Mar 24, 2026 at 12:15 |
The zero ohm resistor only needs to be there in the first place if connection to chassis is optional - if it is mandatory then there's no need for the resistor to begin with.
If the resistor is there, then indeed the proposed layout is bad, since the circular copper pour will get paste on it and also soak up a lot of heat if you try to solder a resistor there, no matter if done with pick & place + reflow or if soldered by hand. Furthermore if automatic optic inspection is used, it will probably find the wetting on the pad towards the screw to be fishy.
I would guess this is a typical case where the average EE draws some layout while they don't have much clue about the soldering process in practice - it is quite common.
Your solution is better since it prevents the solder from wetting onto the screw copper pour, and it also ought to act as thermal relief.
Do note that a screw in whatever material (galvanized steel most likely), as well as the chassis connection (toothed washer? cable lug?) will likely have much higher resistance/inductance in comparison to the copper trace. For the best possible connection to chassis you would use a connector instead.
0 comment threads
As Lundin said, a 0 Ω resistor is for allowing an optional connection. By the time you are laying out the board, you really should have a good grasp on the overall grounding and RF emissions strategy. That would certainly include knowing whether the board ground plane will be connected to the chassis or not.
I would ditch the optional resistor. It's not really a very good RF connection anyway.
With nothing needing to be soldered to the pad for the mounting screw, there is no point to add thermals. Make sure to remove the screw pad from the paste layer so that it doesn't get covered with solder. The screw will be solidly connected to the pad. If the ground plane is the top layer, then the screw is connected to it directly. If one of the other layers, then the screw is connected to it with a large-diameter via. Either way should be better RF-wise than going thru a 0 Ω jumper.
If you want to disconnect the board from the chassis in testing the prototype, you can leave off the screw and put a piece of tape underneath, or use a nylon screw.
For lowest RF emissions, the board ground should be connected to the conductive chassis at one point only. That point should be as close as possible to where external connections come thru the chassis onto the board.
0 comment threads
0 comment threads