How to deal with unused components?

[cristi_m90]

Hello! I intend to send a board to a PCB manufacturer and I am wondering how to mark unused components.

I saw that EAGLE includes all components in the BOM and pick-and-place files, but I do not want all of them to be mounted.

How is it better to proceed? Should I set those component's values to DNP (Do not place) so the manufacturer knows they shouldn't be mounted, and remove them from the BOM? Or should I manually remove the unused components from the pick-and-place file and BOM? Does EAGLE offer support in this regard? Is assembly variants the only solution?

[C.Nicks · Accepted solution]

There isn't really a set way to do this. It really is up to you and any of the methods you mention would work. As long as the manufacturer has the information required to build it.

Personally I use the assembly variants feature to keep track of build versions, but I ONLY use it to print schematics and export the bill of materials. If you export the gerbers and there are parts set to not populate, Eagle will remove the silkscreen and solder paste from them, which makes it difficult to build them a different way later on. I made that mistake and had to buy a whole set of stencils ($500) because it removed the paste openings.
When I make a variant, I switch to it, print and export BOM, then switch it back to export gerbers.
In my opinion the variants should only affect the schematic and not touch anything physical in the board design or gerbers. Until they fix that, use carefully.

There are also other bill of materials export scripts that can use attributes to ignore parts. That way you don't have frames and test points showing up at the pick and place.

I use a modified version of Robert Starr's bom-ex.ulp
https://github.com/robertstarr/ulp_user/blob/master/bom-ex.ulp

[PeterA4L]

Hi Cameron,

what ulp do you use for the pick and place file? and can you share that modified ulp?

[C.Nicks]

I've attached the modified versions of the ULPs I use for manufacturing output. They are XY files are separated for surface mount and through hole.

For information on the changes I've made, see the changelog in each of the files.

[PeterA4L]

Thanks Cameron,

It is nice that the DO NOT PLACE components are not showing up anymore in the pick and place file.

Regards

[Anonymous]

I agree with Cameron.  The assembly variant's should NOT effect the board whatsoever.. and the "populate" checkbox should be editable from the layout side as well.  That makes things simple.

The chances that a user would want to actually remove a component's silkscreen and pad openings from the board is much less likely than the more common case of a user just wanting to specify a component as unpopulated.  Why would eagle design for the less common circumstance, and make it effectively impossible to do the simple one?

[charlie_didear]

I agree with @C.Nicks  and @Anonymous .  I only want to be able to select whether a part is populated or not in an assembly variant, so that it does not get exported to the pick and place (mnt and mnb) files.  Having EAGLE delete the silkscreen and cream layers for that part is certainly not desirable.

If I do not want to populate C4, C8, C9, C34, C36, C39 etc...I do not want the reference designators and part outlines to all disappear and now I have a bunch of unidentified pads on the board.  I also now don't have any solder stencil openings for that board, should I choose to add parts in later.  Usually having solder stencil openings for a part that is not populated is harmless because most applications do not care if a little bit of solder gets left on.  However, not having a stencil opening when you ARE populating the board is certainly not good.

The workaround that @C.Nicks suggested certainly seems feasible, but seems inefficient and especially prone to user error.  If the developers can add the ability to independently toggle the schematic "X," whether a part should be populated, and whether its silk and cream layers should be removed, that would be much appreciated.