4 Replies Latest reply on Jan 5, 2015 8:55 PM by syhaunguyen

    Variant Manager BOM generation




      Is it possible to format the output of the Variant Manager BOM Report to be the same as Part Lister?


      In the user manual it states following:

      "Variant Manager reads the PartListerDefaults.ipl file when generating BOM. If you want to exclude parts from the BOM:"


      I have tried to change the PartListerDefaults.ipl to the same format I use with the "Part Lister" without any luck.


      I'm using DX Designer 9.5 and Variant Manager


        • 1. Re: Variant Manager BOM generation

          Hi Aboen,


          there are 4 (or 6) ways of generating the BOM:

          two out of DxD,two (or three) out of the Layout tool, and automation at last.

          I wont discuss the last two, because it involves other tools and a lot of setup.


          In DxD:

          1) You use part lister. It will generate your bom and you can use the *.ipl file to configure the output.

          If you have variants the procedure is different if you do a master BOM (with all components) or a Variant BOM (some components excluded)

          - the Master BOM just start partlister from the menu tools--> part lister.

          - The variant BOM: you have to start variant manager window and you will have to create a variant. With the variant active (variant window still opened, variant icon selected, click on the DxD schematic window that has now a yellow strip telling you the active variant and is read only) you can now start partlister from the menu and the generated BOM will now abide to the variant changes, and will be formatted with the *.ipl file.

          Remember that doing a BOM from Partlister will not include all mechanical part that are added in PCB.


          2) You use BOM reports. This BOM will be started from the variant window. Right mouse button on the list of component in the variant window will allow you to choose Reports-->BOM Reports. Now you will have the possibility to generate a BOM that will include mechanical parts from PCB, but you will not have any possibility to use *.ipl to format the outputs. Be aware that you have to manually fill the lines that are not equipped. (Even if the symbol has a part list exclude=true  property set)


          In PCB:

          3) You use Bill of Materials from the Menu output-->Bill of materials. Here you will need to have a Fablink license. The formatting is a formatting that is different than the *.ipl form the DxD. Parts that have a property Forward to PCB=False will not be included in the BOM, some mechanical parts will be missing.


          4) use BOM Report. Similar as in DxD, you have one of the most accurate BOM including mechanical parts. Some schematic parts will be missing, if the right combination of Forward do PCB and Part List Exclude = False is set.


          5) Use Report Writer. Besid being an outside tool, it will have dificulty with variants.


          6) Using automation. Not discussed.



          No one of the results is like the other. So out of this I have made a Mentor Idea: D13292 BOM generated in DxD and in PCB are different for mechanical parts, alternate cells, parts excluded,https://mentor.brightidea.com/ct/ct_a_view_idea.bix?c=FDA2FA5D-237C-48D7-A66F-5DA754706D6C&idea_id=3DCC6618-68B7-4046-B607-D1208CCED9CE

          Please vote on this idea and support it, so that Mentor can do an unified BOM generation.


          Thanks and hope this helps



          3 of 3 people found this helpful
          • 2. Re: Variant Manager BOM generation

            Hi Matija,


            Thanks for your answer. I tried to use the variant with the part lister (e.g. Lesson8.prj), but the unplaced parts in the variant is still included in the BOM generated by the part Lister.


            Do I need to include a property in my part for this to work or is this a bug in the new DX Designer 9.5?


            I agree with you Mentor should make an unified BOM generation tool!





            • 3. Re: Variant Manager BOM generation

              Hello Anders,


              If you are doing method nr 2. the BOM will be correct only if you save the variant.


              See the difference if you just open a variant (Menu: view--> other windows-->Variants), create a new variant (icon with the hammer), mark some element as unplaced (right mouse button on the white variant column and select "Unplaced"), generate the variant schematic (icon with a green IC and a small X), then use part lister (Menu: Tools-->Part Lister). The BOM will be incorrect, as shown in picture BOM_MyVariant_not_saved. (Note that the disk on the left of the variant Manger window is black, indicating that the variant is not saved)


              You have to save the variant with the disc icon (the disk must be gray), close the variant schematic with the master icon in variant window (icon with a green IC and a small M). Then regenerate the schematic (icon with a green IC and a small X), and the new schematic will open (vusually  nothing has changed). Now you can regenerate the BOM with the part lister (Menu: Tools-->Part Lister). And now your BOM is correct, as in picture BOM_MyVariant_after_save.


              Hope this helps and clarifies some.



              P.S: Please vote on the Mentor idea site, click somewhere in the description text of the indicated idea on the previous response where the idea is linked. A new page will open. Click on the promote word in the left upper side. Thanks.

              1 of 1 people found this helpful
              • 4. Re: Variant Manager BOM generation

                I have same Q for this. I'll try follow. i think it is the best way for my question. Thanks you