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RA_99096711-Visitor
1-Visitor
July 26, 2021
Solved

Component not showing up in drawing BOM and not selectable for Balloon either

  • July 26, 2021
  • 2 replies
  • 9987 views

I can add a note and dimensions in the component, and at first it was showing up in the BOM, but now it disappeared. I can't add a balloon either, but the component it's still showing up in the drawing.

 

I really don't know what to do to fix it.

 

Thank you.

Best answer by rzukowski

Check the representation of the assembly that is driving the BOM table.  Could the component have been unintentionally removed from the representation.

2 replies

S
23-Emerald III
StephenW23-Emerald III
23-Emerald III
July 26, 2021

It's difficult to tell exactly where the problem is. Can you attach a screen shot maybe? Not sure it'll help either.

Do you have multiple assembly models in your drawing? Or multiple simplified reps in your drawing? Or multiple bom tables in your drawing? Do you have filters in your BOM table? Any of these can cause issues.

You may also want to use the Regen sheets in the view tab in the drawing to update the drawing to refresh the drawing views.

 

 

    R
    RA_99096711-VisitorAuthor
    1-Visitor
    August 2, 2021

    Hi Stephen. I've already applied the "regen" option, but it didn't work. The problem is: the assembly was already in the drawing and in the BOM table, but all of sudden it disappeared (I'm not sure how this happened). The assembly it's still in the model tree and in the drawing, but not in the BOM table. This drawing has multiple assemblies, but just one BOM table.

    K
    KenFarley21-Topaz II
    21-Topaz II
    July 26, 2021

    First, it would help to know what version of Creo you are using. Is this a multibody part?

    When I've had this problem in the past, the causes I found were usually a result of the parameters in the component being wrong. The bill of materials (for our company, at least) uses parameters in the model to fill out the columns of the table. Things like the part number, description, etc. On different occasions, the problems I had were because:

    (1) The component model didn't have any of the parameters needed, so it was ignored by the bill of materials.

    (2) The component had been copied from another model and the needed parameters were not changed, so the bill of materials saw two of the components as being the same and was reporting them in the same row (the quantity was wrong, it was the sum of both).

    (3) The part number was supposed to be different for two family table parts but the relations or family table entries for two parts were resulting in the same values for the bill of materials parameters.

    Maybe one of these is causing your trouble, or maybe if you are using multibody parts there is something not set up right for you. We don't use multibody stuff in our parts, so I'm not familiar with what happens with them as far as parameters go.

      R
      RA_99096711-VisitorAuthor
      1-Visitor
      August 2, 2021

      Hello Ken!
      I'm using CREO Parametric 4.0. The problem is: the assembly was already in the drawing and in the BOM table, but all of sudden it disappeared (I'm not sure how this happened). The assembly it's still in the model tree and in the drawing, but not in the BOM table. So I guess it doesn't apply in the first situation you described because it was there but now it's not anymore, but nothing in the BOM Table filters has changed.

      R
      rzukowski13-AquamarineAnswer
      13-Aquamarine
      August 2, 2021

      Check the representation of the assembly that is driving the BOM table.  Could the component have been unintentionally removed from the representation.

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