Mounting Holes & Clearance

I looked at some posts and videos about making mounting holes but it’s not clear to me what the best way is. In pcbnew I put the component MountingHole_3.2mm_M3. By default there is a narrow exclusion zone right around 3.2mm.


I am using metal posts and screws so I need quite a bit more non-conductive clearance around the hole (about 7mm diameter). Some people suggest to adjust the pad size as shown here


This will create a copper pad around the hole with a narrow area around the pad size that has no copper, i.e. the black area here:


I guess this is functional and I have seen plenty of PCBs that have copper around the mounting holes which never made much sense to me (maybe there is a reason).

As you can see, I have a copper field and some people suggested to increase the minimum distance between copper field and components/traces. However, in most cases I want to keep this distance small, i.e. much smaller than the ~2mm I am trying to create around the mounting hole.

I experimented with a few more parameters and think the “Net pad clearance” might do the trick. I set this to 1.9mm because I want 7mm diameter clearance. The hole has a radius of 1.6mm (M3, 3.2mm hole). 7mm diameter clearance = 3.5mm radius. 3.5mm - 1.6mm = 1.9mm.


This results in the following:


This looks pretty much what I was looking for, i.e. a 3.2mm hole for a M3 screw and 7mm diameter clearance without any copper. Will this work or did I miss something that might create a connection to the copper field or any components?


You have discovered the methods which implement the two most common approaches to mounting holes (a copper pad around the hole, or an area of bare PCB around the hole). The choice is actually a design decision, and you should probably chat with your production engineering, and mechanical design, people before you make a final decision.

The copper ring is said to function as a washer under the fastener. Fiberglass PCB material is rather brittle, and it is claimed that it will powder and shred under a tightened fastener, due to thermal cycling. The result is a loose fastener. Supposedly, the copper ring under the fastener head is ductile enough to absorb thermal expansions and prevent abrasion of the board material. (I never understood why the copper ring is supposedly better than a simple washer under the fastener head, except for the nuisance of small, loose, parts during assembly.)

The copper ring is also used to create a ground connection between the PCB assembly, and the enclosure or chassis. This “incidental ground” approach is often discouraged in favor of a “made ground” (i.e., a designated ground conductor passed through a connector or terminal strip).

Your choice of mounting hole styles may be influenced by the capabilities of your board fabricator. The copper ring will only be an option if the mounting hole is plated, but mounting hole dimensions are often at (or beyond) the largest available plated-through hole size.

Whichever approach you take, look carefully at the dimensions of your fasteners - which means knowing the head style of screws (round, binding, fillister, etc), and whether or not a washer will be used during assembly (and whether the washer is full O.D, or reduced O.D.). If you don’t want the fastener to touch surrounding copper, leave a generous clearance - I allow 20 mils (0.5mm) or more. The mechanical tolerances on fasteners are typically not as tight as tolerances on electronic components, and the (necessary!) practice of designing some wiggle-room around mounting holes means that the actual fasteners may be shifted from their designed center locations.



dchishom, thank you for your detailed reply. I will chat with the Production Engineer = Mechanical Design Engineer = me :wink: (this is my first person hobby project)

There will be a significant amount of stress on the board because I have more than a dozen 12 AWG wires connecting to the board. I am not sure if the copper around a mounting hole will be any beneficial, though. Maybe the mantra is that it doesn’t hurt.

It seems to me that the most important part is your comment about the maximum ‘via’ size. I set the “Pad type” to “NPTH, Mechanical” so I would assume it will not be plated. Hence, I hope this will not cause any limitations from the manufacturer’s side. Or am I missing something?

The manufacturer will tell you the ranges of hole sizes he can reliably produce. As I recall, for plated-through holes the smallest will be about 16 - 20 mils (0.4 - 0.5mm), and the largest is around 125 - 200 mils (3 - 5mm). The exact values vary among manufacturers. For unplated holes the upper limit is larger - 250 to 300 mils (6 - 7.5 mm), and even larger sizes are treated as a cutout, produced by routing the outline rather than drilling a hole.


For a mechanical view I think nylon washers may be good to distribute the stress from heavy wires on the pcb, especially combined with a steel washer between the nylon and the nut.
Be carefull with SMD, these can crack easily if a PCB is bent.

Some manufacturers charge extra for NPTH, because it is an extra production step. The wall of drilled via’s is copperized by a chemical process, and then thickened by electrolysis. NPTH’s must be made after this.

But for boards which are being routed this usually does not matter much.

This topic was automatically closed 30 days after the last reply. New replies are no longer allowed.