How to handle paste on non-fitted components by variant

[Psi]

Does anyone know how to disable paste apertures for not-fitted components?

We have been looking for a while and just cant see any way to do this in Altium.

Thanks.

[mrpackethead]

You could manually adjust each pad you wanted to deal to by reducing it to zero. You could write a script to do the same thign.

[T3sl4co1l]

I haven't done this precisely so I'm not sure, but give it a try?

Under Variant Options, check "Allow Variation of Fabrication Outputs".

In the OutJob, set the Gerber/ODB item to a particular variant.  Or, use the Select One Variant for All Outputs option.

View the output files and see if a combination of these does the trick.

I don't think it makes much difference as CMs tend to do their own masks.  For example, I'll often be lazy and set a large pad without anything special, and the assembly comes back with obvious valleys in the solder, where the pad was divided into sections because the span was otherwise too wide.

If you're doing the paste yourself, nevermind that.

Tim

[Psi]

Unfortunately that didn't work, but keep ideas coming. There must be a proper way to do this in Altium.

[ajb]

Can you create a rule that sets a negative paste mask expansion for not fitted parts?  Obviously you then need to make sure that all of your expansions are from rule and not set in the pad properties.

If you're sending this to a CM, you should probably make it clear to them that you don't want DNI pads pasted, as, like Tim says, they'll probably do their own mask anyway.  Which also means you could just make it their problem and tell them to crop the paste apertures from DNI parts themselves.  Depends on how much trust you have in your CM.

[wraper]

May I ask, why would you bother with this in the first place? At least I don't see why this would be required normally, and I very rarely see this on actual PCBs. Usually paste is just applied and components not fitted. Moreover this would require separate stencil for each variant, and makes version control more difficult.

[mrpackethead]

That is a good question..    But heres a real example of why

I have created parts for my fiducals.  I have four differnet styles, for differnent purposes.   ( pcb fids, componet fids, panel fids and fids for the pnp to find for various purposes, such as detecting X-out boards ).

Those fids are created as SMT parts..   But are set up as DNP's,.,. ( you dont' put a part on a fidicual )..  And i dont' want paste on them, becuase that will impact on the machiens ablity to vision them.

I have manually adjusted my apatures in this case so that they are closed completley.

[T3sl4co1l]

That's just a matter of appropriate fab -- don't want paste on test pads or fiducials?  Then disable it!

I don't think there are design rules for variants.  But you can take a look and see.  Otherwise, yeah, you're customizing for each paste variant you want.  Huge pain, error prone.

I have seen boards made with glue variants.  Most obvious evidence: a table on silkscreen showing the options, with a little dab of glue inside each option that particular variant had.   (Was also a 2-side load, with bulky-ish inductors and BGAs -- a laptop motherboard -- so they needed glue anyway.)

They also used OSP, obvious from the now-tarnished, unplated, untinned mounting holes.  Something to think about if you need testable or solderable pads later in your product's life cycle.  Tin, ENIG or solder helps a lot.

Tim

[wraper]

That is a good question..    But heres a real example of why

I have created parts for my fiducals.  I have four differnet styles, for differnent purposes.   ( pcb fids, componet fids, panel fids and fids for the pnp to find for various purposes, such as detecting X-out boards ).

Those fids are created as SMT parts..   But are set up as DNP's,.,. ( you dont' put a part on a fidicual )..  And i dont' want paste on them, becuase that will impact on the machiens ablity to vision them.

I have manually adjusted my apatures in this case so that they are closed completley.

This is very different from fiducials. Op wants no paste on normal components, not components which were intended to be not populated from the very beginning.

[ajb]

After thinking about it, I remembered I tried to do some design rules based on variants a while ago and didn't have any luck.  That would be a good feature to request, for whatever good requesting features from Altium does.

You might be able to define component classes for your different variants and use those to drive paste expansion rules, but I don't think there's a good way to make classes visible on and driven by the schematic

The easiest and least error-prone way to do this might be to define paste expansion rules for the DNI parts explicitly by designator.  This would be tedious but relatively easy to manually synchronize with your BOM, and you can define multiple rules for different variants--though I guess you'd have to manually set the rule priority before generating outputs for a different variant.

[mrpackethead]

In version 17 there is support for User-defined variants in the Query Language.     I think this with a bit of thought could let you set up what you need/want.   Add a user-defined parameter,  that is different for each variant, and then create a rule to deal with the paste.

http://www.altium.com/documentation/17.0/display/ADES/NFS_17_0((Support+for+Parameters+in+PCB+Footprints))_AD

[julianhigginson]

I'm not sure what's even the problem with placing solder on unused footprint pads.

But I know that for one kind of pad finish I've seem (an OSP) not soldering unused pads is a very bad idea - for that finish you need to make sure that even testpoints have paste mask opened.

[Psi]

I'm not sure what's even the problem with placing solder on unused footprint pads.

It just seems untidy.

And i have seen shorts on unpopulated pads that get pasted.
Quite rare but does happen from time to time on designs that uses some really big SMT parts combined with some ULTRA fine pitch parts.

[T3sl4co1l]

Related problem: I've seen shorts between nearby vias, after wave soldering.  Lead-free solder is kind of sticky and can do that.

Often you need vias untented for testing purposes, but you should also have generous spacing between those, both for this reason, and as it makes test mfg easier.  All other vias should be tented to prevent problems -- at least to the extent that it's reasonable to do so, if you're still anticipating some prototype modding work.

Tim

[tszaboo]

I'm not sure what's even the problem with placing solder on unused footprint pads.

But I know that for one kind of pad finish I've seem (an OSP) not soldering unused pads is a very bad idea - for that finish you need to make sure that even testpoints have paste mask opened.

There is a legit reason to do this. For example you define multiple different inductors for different variants, and the footprints overlap. And the solder would lift the inductor or cause sort to the ferrite material. I've seen this happen.
I dont think this is easily supported in Altium. Variants is for BOM and pick and place, not for the gerber files. Probably you need to talk to the manufacturer to leave the pads. Or manually edit the gerber files. It is not nice in any case. Maybe you can play with the panelisation of the board... Not nice. Or for these components move the pastemask to a different layer, and do a "mechanical layer to add to all plots" with just the paste file. And carefully generate the files.