Bill Of Material

[DonSA]

Is it possible to save a bill of material format in Assembly Design? Also is it possible to insert user parameters to a BOM, as in material size, type etc.?

 

[0328500091]

Yes you can do this macro :

Sub CATMain()
Set productDocument1 = CATIA.ActiveDocument
Set product1 = productDocument1.Product
Set assemblyConvertor1 = product1.GetItem("BillOfMaterial")
Dim arrayOfVariantOfBSTR1(6)
arrayOfVariantOfBSTR1(0) = "Name"
arrayOfVariantOfBSTR1(1) = "Number"
arrayOfVariantOfBSTR1(2) = "Lenght"
arrayOfVariantOfBSTR1(3) = "Quantity"
arrayOfVariantOfBSTR1(4) = "Material"
arrayOfVariantOfBSTR1(5) = "MaterialNorm"
arrayOfVariantOfBSTR1(6) = "Mass"

assemblyConvertor1.SetCurrentFormat(arrayOfVariantOfBSTR1)

Dim arrayOfVariantOfBSTR2(3)
arrayOfVariantOfBSTR1(0) = "Name"
arrayOfVariantOfBSTR1(1) = "Number"
arrayOfVariantOfBSTR1(2) = "Lenght"

assemblyConvertor1.SetSecondaryFormat(arrayOfVariantOfBSTR2)

End Sub


Dominique

 

[KooKoo]

Yes you can add user parameters to the BOM.
First you should have parameters already defined in you parts.
Go to the Properties of one Part, pick the Product tab, scroll to the bottom and pick define other properties...
Create a new parameter (can be the same name as the one in your part), (no need to enter a value) pick OK then pick Apply.
Right-Click in the field beside your parameter name select Edit Formula and pick the parameter in your part that you want to insert in the BOM.
Back in the Assembly go to Analyze, Bill of Material, pick Define Formats and add the new parameter.
Hope that helps.