Actions
Forum Thread Details
  • State Verified Answer
  • Locked Locked
  • Replies 19 replies
  • Subscribers 87 subscribers
  • Views 9047 views
  • Users 0 members are here
Related
This discussion has been locked.
You can no longer post new replies to this discussion. If you have a question you can start a new discussion

Variant changes not shown in schematics nor BOM

ohyva

Hi,

 

I tried to make my first variant in CS. My need was to remove 3 components from my base design to make the specification for production PCB.

Making a variant seems to be quite straightforward. Marking the components "not fitted" is simple. But these seem to have no effect on the schematic nor the output files.

 

Is there something I need to do besides creating the variant? I am using the default Drawing Style options as given when the first variant was created. I have understood it should draw a red cross over the "not fitted" components (just like the example shows when in the drawing style dialog you toggle this option on and off and on again). Additionally all the components are still listed in BOM.

 

I would very much like to get the variants to work. I can of course do this in the old style editing manually the BOM and writing notes to our PCB manufacturer, but the variants seem to be the better way - if it works.

 

Are there anywhere else some settings I need to adjust to get variants to work? Now I have just made sure the Current Variant on Project-> Project Actions show the right variant I want to use.

 

BR Olli

  • 0

    Hi, assuming you have set up variants correctly and marked the 3 components as not fitted you should be able to view the red cross through the components in the schematic editor. If you open the schematic sheet at the bottom of the document window there should be two tabs, "Editor" and "Sheet1" (assuming your sheet was named Sheet1). Selecting Editor views the schematic as normal, selecting Sheet1 puts the schematic into variant view. Use the Project > Current Variant drop down to select between your base design and variants, this will show not-fitted components with a big red cross.

     

    For the BOM you will need to select the variant from the Generate Outputs dialog, this will then generate for that specific board variant.

  • 0 in reply to e14softwareuk

    Thanks.

    I guess this now works as supposed.

    But I am a bit disappointed because the implementation is not complete. The schematic editor and BOM is now OK, but I would have liked to see the variant information also in the PCB PDF document (at least in schematics but preferably also in 3D print) and in Pick and Place file. So manual editing still needed.

     

    BR Olli

  • 0 in reply to ohyva

    You should be able to get the variants on printouts. In the PCB editor select the variant using Project > Current Variant (just as in the schematic) and then the Outputs > Assembly Drawings will print or omit the variant components, same with Print > Print Preview. Hope this helps.

  • 0 in reply to e14softwareuk

    Why has Altium chosen not to allow variants in schematic prints using "Generate Outputs"?

     

    When I generate assembly drawings for internal use I always generate them with the schematics as well, as there's often extra information on the schematics a tech may use for troubleshooting. 

     

    It's a real shame that a single generate command will result in a BoM, Assembly Drawings, P&P files and 3D PCB using the variant, then Schematics and PCB Layout in the same document completely ignoring them.  Creates confusion where there really is no need.

     

    Further, I can't see how there's any way to label every generated page with what variant has be generated.  Is there a way that I'm missing?  Seems like an obvious documentation requirement.

     

    Thanks

  • 0 in reply to harvie256

    Variant printing is supported for schematics, you just need to select the variant using Project > Current Variant. Using print preview will then prepare a print for the currently selected variant. You can label the schematic sheets with the variant name, add a text string and then edit its properties, from the dropdown box select =VariantName.

  • 0 in reply to e14softwareuk

    No it is not, you are talking about something completely different.

     

    Try it, go to Generate Outputs, select the variant, check PCB and Schematics.  You will not get the variant.

  • 0 in reply to e14softwareuk

    Yes this work, but I would still like to see this "variant print" as part of the PDF created with Generate outputs action.

    Is there a way to prevent all the wires and texts not part of the components not to be shaded out? I.e. to get quite normal looking schematics print with just the not fitted components crossed out.

  • 0 in reply to harvie256

    This does work but you need to set it up correctly. In the Generate Output Files dialog, select Schematic (for example), configure... and select the Physical Document option. This will then generate a schematic to match the physical variation of the board (i.e. the selected variant).

  • 0 in reply to ohyva

    Hi Olli, as mentioned above the generate outputs action does work provided you select "physical" document options. I don't think there is any way to adjust the shading of nets attached to a variant component.

  • 0 in reply to e14softwareuk

    Thanks again. This works.

    And it actually does just what I wanted i.e. quite normal looking schematics print with just the not fitted components crossed out. The wires etc are not shaded out like they were when I did the PDF generation using the Print action.