How can we add numbers to sub-assemblies in CATIA to see them in balloons and bom list automatically in drawing?

özgür kesebir

30 Jul, 2014 08:15 AM

Here is the tutorial and files. Have fun...

1. Step 1:

   Here is my assembly tree.
   

   

2. Step 2:

   First type of Advanced Bill of Material table. Type is Summarized and type result shown.
   

   

3. Step 3:

   Second type of Advanced Bill of Material table. Type is TopLevel and type result shown.
   

   

4. Step 4:

   Now how did I do. First get a front view from assembly.
   

   

5. Step 5:

   Double click on sheet (shown with 1) and turn the frame from active to inactive (means red to blue). We do that to create a bom table out side of frame. If you want to insert table into frame you can pass this step.
   

   

6. Step 6:

   Go: Insert-->Generation-->Bill of Material-->Advanced Bill of Material
   

   

7. Step 7:

   BOM Creation window will pop up. Click ok then select front view frame and then click anywhere on the sheet. (Be carefull if you click too bottom, table will be splitted to 2 sheets automaticaly. So click mid side or top side on the sheet.
   

   

8. Step 8:

   BOM table occurs. Right click on table. And go Properties.
   

   

9. Step 9:

   Check BOM format type. It is as Summarized on default CATIA. Which give you second picture results.
   

   

10. Step 10:

    We need to change it TopLevel. Which will give you third picture results.
    

    

11. Step 11:

    Now run CATIA as Admin Mode.
    

    

12. Step 12:

    Go: Tools--> Standards...
    

    

13. Step 13:

    Now change category to drafting. And select xml file which you want to change. (I used ISO)
    

    

14. Step 14:

    In Styles, find Bill of Material. And change Bill of material format from summarized to toplevel. Then save standard and close adminmode. Replace it with your original xml. (old one which located at --> C:\Program Files\Dassault Systemes\B21\intel_a\resources\standard\drafting) (new one which located at where you run admin enviroment files. Something like that--> \CATCollectionStandard\drafting)

    Now open catia as a normal user. Repeat Advaced Bill of Material and get BOM table with sub-assemblies.