How to manage board Mounting holes in your PCB designs.

Recently I have seen comments on the web recently from people asking "how do I do mounting holes in CADSTAR?".

There are a few methods that you can use to implement mounting holes in CADSTAR.

Which one you choose is dependant upon the type of hole you want and how you want to use it.

First what is a mounting hole for ?

They are not always simply for putting a screw through to mount the PCB onto a chassis or similar, as they can also be used for molding pegs or other mountings that can align or affix the board such as pem studs, earthing screws, plastic standoffs etc. They will generally need to be placed in specific locations.

Each type of mounting may need a different type of hole, be it non plated with no lands through to fully plated through with plenty of pad/land surrounding it.

Simple board cutouts:

The simplest way to add mounting holes into your board is to add them as a cutout to the board outline.

This is made in the Design Editor by choosing the "Add Circle" tool, changing the shape type to "Cutout", selecting the board outline and drawing a circle within it. No need to worry about drawing it exactly where it needs to go, just draw the circle near and then select and move it later.

To be specific about the hole diameter - simply use the working grid I.E. for a 3mm hole, set the grid to 1.5mm (1/2 the radius).

If you want your hole to be 5mm in from each side of the corner, draw a 5mm temporary square, snap it to the corner then move the circle to snap to the corner of that (then delete the square).

Cutout holes are they are easy to do and are not removed by an ECO, however are harder to change as they need to be deleted first, they do not appear in drill files and you have to add them to your drill drawing manually, cannot be plated through nor have any pad lands around them unless you manually add a copper circle there yourself.

Mounting holes using Components:

So this leads us onto creating mounting holes using components, by making a component that has a single pad with a drilled hole of the required size and pad lands/plating etc as required. They can simply be added in position (using the square mentioned above or) by entering coordinates directly in their properties.

So we add a component out of the library as our mounting hole, the only problem is come the next ECO update it will be removed and then we have to enter the component names into an ignore file. Simple enough except I tend to forget the file when I return to the design after 12 months and I'm on issue F. At which point the ECO removes it again.

(You might think that is a bad thing, but it's not really - it is just CADSTAR ensuring that the PCB is a match to the schematic.)

Mounting holes using Parts:

So the answer is simple, make a part and add it to the schematic.

Make the part with a plain circle or a screw head shape etc for the schematic symbol, a hole component for the PCB and add the part to an additional sheet for "PCB only stuff". This way we do not get them appearing on printed schematics and someone says "whats this for?".

So now you have added parts to your schematic, they appear in the rats nest and can be connected to a net (or not) they can be updated and changed with an ECO but are not removed because they are always in the schematic.

In my libraries I have a range of parts called "Mounting Hole NPTH 3.0mm" , "Mounting Hole NPTH 4.0mm" (which are simple pads with a drill size bigger than the pad), "Mounting Hole PTH 3.0mm/6mm Pad" etc which is a 6mm pad with a 3mm hole - this gives me land for the screw head etc.

They all have the symbol "screw" and call the component "Mounting Hole" however I have alternatives which enable me to change the hole on the fly if needs be (as can often be the case as mech design change their minds).

Because I add them as a part on a separate sheet they are not printed out or included in any BOM (unless I want them to) and are all included in any ECO.

Simples really.