Can I use variants to do this ?

[snoopy]

I've been playing around with variants on Altium but I am not sure if it can do exactly what I want.

What I need to do is to have one schematic that represents similar boards that differ in a type of connector used. It is an RCA connector but from different manufacturers and therefore has essentially the same pin-out on the schematic but a different footprint on the pcb.

I've created a variant with a different footprint but according to the online doco it appears that Altium wants to populate the board with both footprints instead of creating another board with the alternative footprint. Have I missed something here. Is there some other option to create different boards from the one schematic ? Also with these connectors it is not possible to overlap footprints on the same board because the footprints conflict with each other.

http://techdocs.altium.com/display/ADOH/True+Variants

cheers

[ajb]

I don't believe there's a way to do that with variants.  You might be able to do something ridiculous like put the connector on its own sheet and insert that as a sheet symbol, then create a second project that links the same schematic files but with a different internally-saved schematic doc for the connector sheet.  Not sure if that would actually work, and even if it did you'd still wind up with two fully-independent PCB files.

[snoopy]

Yep I think I just have to create two different projects.

cheers

[c4757p]

Any way you could create a footprint that can fit either part? Not always possible, but clever and useful when it is.

[snoopy]

Any way you could create a footprint that can fit either part? Not always possible, but clever and useful when it is.

Unfortunately I can't do it with these parts but is a great solution when it fits

cheers

[T3sl4co1l]

Assembly variants are just that: assembly only.  The schematic and PCB must be coherent, and support all options you intend to populate.

So what can happen with different parts is, you can make one single footprint (don't make two and try to overlap them -- that counts as shorts and clearance problems, even if all the holes are in the same place -- after all, two holes in the same place means zero point zero clearance between them!), providing all the holes and pads necessary for the two parts.  Then use variants (in the variants dialog, check the "allow variations" box, and change the MFGPN/supplier link/etc. as needed), and assemble them accordingly.

[snoopy]

Assembly variants are just that: assembly only.  The schematic and PCB must be coherent, and support all options you intend to populate.

So what can happen with different parts is, you can make one single footprint (don't make two and try to overlap them -- that counts as shorts and clearance problems, even if all the holes are in the same place -- after all, two holes in the same place means zero point zero clearance between them!), providing all the holes and pads necessary for the two parts.  Then use variants (in the variants dialog, check the "allow variations" box, and change the MFGPN/supplier link/etc. as needed), and assemble them accordingly.

Because I can't physically overlap the two parts what I really need is a PCB variant and not an assembly variant so I can make two different PCB's from the same schematic.

cheers

[armandas]

Because I can't physically overlap the two parts what I really need is a PCB variant and not an assembly variant so I can make two different PCB's from the same schematic.

cheers

You can have two different PCB documents in your project. They will both reference the same schematic design, so you can put both footprints in your schematic, push the changes onto the PCB and just delete the unneeded footprint. The only catch is that you'll have to delete the unwanted footprint after every update from schematic. Still, it maybe a better option than having two separate projects.

[tautech]

Because I can't physically overlap the two parts what I really need is a PCB variant and not an assembly variant so I can make two different PCB's from the same schematic.

cheers

You can have two different PCB documents in your project. They will both reference the same schematic design, so you can put both footprints in your schematic, push the changes onto the PCB and just delete the unneeded footprint. The only catch is that you'll have to delete the unwanted footprint after every update from schematic. Still, it maybe a better option than having two separate projects.

Isn't it easier than that. 

2 PCB documents with a different footprint in each, with a title name so you can tell them apart.
You can change the footprint from the within PCB file.
Just don't update to the schematic from either PCB file.

[armandas]

Isn't it easier than that. 

2 PCB documents with a different footprint in each, with a title name so you can tell them apart.
You can change the footprint from the within PCB file.
Just don't update to the schematic from either PCB file.

You can if you create a component that has both footprints. But Altium will still want to change the footprint on the PCB whenever you update from schematic.

[T3sl4co1l]

Ew, no.  Keep SCH and PCB in sync.  To do otherwise is madness.  Sooner or later you'll forget what you did, and things get screwed up...

One way you could do this is to put everything that *doesn't* change into separate schematic(s), and the one thing that does change, into a separate schematic (one for each version).  Start two projects, each with all the common schematics, and one with the first schematic variant, and the other with the other.  Now you have two PCB projects, which means all the schematics that generate the PCB, and the PCB, and the project settings for them.  By using common schematics, you avoid the madness of having to sync two PCBs.

By far the best is to use a single project, one common footprint (assuming they don't conflict), or two footprints (in different locations, again to avoid conflict).  If neither of these is possible, and you really need two separate PCBs, then you're better off using two separate PCBs.

It's noteworthy that variants can be selected in the OutJob for fabrication outputs too, but I don't know if that's useful here or not.  If so, it again seems like a good way to generate confusing outputs (are these files, in the same folder and with the same file names, from variant A or B?).

Tim

[laseralex]

I just solved this problem myself, and I'm posting here in case anyone else happens to find this thread when searching as I did.

I needed to make 3 versions of a board with 3 different, overlapping footprints which would have interfered with each other.  Even with "Allow variation of fabrication outputs" selected in the Edit Project Variant dialog box, I wasn't getting correct outputs.

I kept the 3 variants of the design to allow generation of unique output files.  (In my outjob I use the VariantName parameter to create a subfolder and to label the files.)  However, I put all three components on my schematic at once, with the same reference designator.  I then covered each of the 3 components with Altium's "Compile Mask" feature.

For each output, I use the compile mask to mask out 2 of the 3 footprints, and recompile the project.  I then set the outjob variant to reference the component I'm keeping (to enable the corrct VariantName), and generate my outputs.  The files are all generated with the correct footprint and file names.