Mounting holes questions?

[josr]

I am absolutely new to Eagle or PCB in general and I have some questions about mounting holes:

- Do I create them via the "hole" command?
- How do I ensure I get enough insulation around it for the screw or nut? So I do not want any copper around it (eg trace or pour).
- If I aim for M3 should I make the hole 3.5 mm or what are the general rules of thumb around this?
- I can make those holes via Hole (or another command if that is not the right one) but how do I nicely align them in the 4 corners (so same space from each side)?

Thanks.

[jfiresto]

... I have some questions about mounting holes:

- Do I create them via the "hole" command?

Yes, that, or you can create a via if you wish to electrically connect the screw to the board copper.

- How do I ensure I get enough insulation around it for the screw or nut? So I do not want any copper around it (eg trace or pour).

You can set a general Drill/Hole value on the DRC / Distance tab. If that is not enough, you can add more insulation by adding circles on the bStop and tStop layers.

If I aim for M3 should I make the hole 3.5 mm or what are the general rules of thumb around this?

It depends on how tightly you can or want to put things together. A plain DIN 125 washer for an M3 screw has a 3.2mm inner diameter – that is a good suggestion.

I can make those holes via Hole (or another command if that is not the right one) but how do I nicely align them in the 4 corners (so same space from each side)?

One way is to get information about each hole (with the i button) and enter its x- and y-coordinates.

[jpanhalt]

Placing a few holes using the properties tool is relatively easy to do and is what I do for simple geometric designs of the board or component packages.  It helps enormously to have the package or board centered on the coordinates.

For more complex designs, I use a conventional CAD package, export as DXF, and then import that into an appropriate Eagle layer, such as outline.  I then center the imported design, trace and change layers as needed.

Note, you can make the board a package and use that for other designs too.

[Jeroen3]

There is a library with mounting holes.
It's called "holes.lbr". (who would have thought)

A M3 mechanical hole would be a 3.2mm hole with 7mm silkscreen keepout.

[westfw]

or you can create a via if you wish to electrically connect the screw to the board copper.

You can also use a via that is isolated - copper around the hold, but not connected to anything else.
Drilling non-plated-through holes requires an extra fabrication step (drill vias, plate, mask, etch, DRILL NON-VIAS, strip, soldermask, silkscreen...)The inexpensive prototype PCB places may not want to do this.

[Sylvi]

Hi
I've been using Eagle fora long time but there are many features of it I do not use - one is the solder restriction layers. Instead, I make a circle in the reference layer to show the clearance I want around a hole or other pad. For mounting holes, I use 0.125", which is 3.175mm. I'm using 4-40 hardware which is about the size of M3 but with coarser threads - it is what's available here.

I drop the hole, then move the reference circle over top of it. The circle has to allow for the bolt head diameter, spacer diameter, nut diameter, PLUS some isolation space to the nearest trace.

I am often designing tube stuff, so voltage clearance is important. I use a conservative guide of 0.12mil/V. if you take the mils (0.001") and divide by 0.12 you get the voltage spacing. For example, a 25mil space between a bolt head and a trace provides 25/0.12=208V of isolation. There are way more aggressive (less conservative) guides than this and I've seen those boards burn.

It used to be that PCBs began as copper-clad fibreglass sheets. These had to be etched and drilled in two steps. Drilling accommodates holes that will be vias AND mounting holes, then the holes needing plating are done as a separate step.. These days, the boards are blank fibreglass, holes are drilled and copper is sprayed on with plated holes plated at that time. I believe drilling of through-holes and plated holes (vias) is one step, but in any case, no board house charges extra for mounting holes.

When you select the Holes icon on the left-hand menu, a drip-down list of hole sizes appears. Scroll down to the size you want. if you do not see the size, choose one anyway and drop it on the board, then go to the Change icon (wrench) and select drill, then scroll to the bottom of that list and type in the diameter you want. Then cursor over the hole on the board and click on it - it will change to the new size. The next holes you drop will be this size, too, unless you select a different size. Alternatively, you can do the Change drill size before dropping any holes, then select the Holes icon and they will be the new size.

With my reference circle, I make one to the side of the board, then move it over the first hole. Then I use the Copy icon to makes copies of it to drop over the other holes. When you drop the holes, use the largest grid possible that positions the holes where you want them to be. My holes are usually on a 0.1" grid where traces may be on a 0.0125" grid. You can move back and forth between different grid sizes as you draw the board outline, drop holes, drop components, and then add traces. The traces will need the finer grid to allow for odd pin centres of components, especially if you mix metric and inch footprints.

Note also, that the "i" (information) icon allows you to click on any hole, component, line, trace or via and see the information about that item. You do not have to enter x-y data to see this info. The information window opens when you click on the item, then you click it off by pressing the "okay" button inside the window. Then cursor to other items and see their info. Select STOP to exit the information mode.

Remember to SAVE  frequently - every few steps of whatever you are doing. It is easy to lose hours of work if Eagle crashes.