Can anyone explain how to get a complete bom out of Creo into Excel (or similar) please?
This is a very simple task for Solidedge or Solidworks but seems to be missing from Creo.
My problem is in two parts:
1. How do I display a complete BOM table showing everything including all sub assemblies and parts, we have tried every option we can think of but some sub assemblies won't show up.
2. How do I get the BOM from creo to excel. Saving as CSV doesn't work because it only exposrts the first 665 lines of the BOM and the BOM is over 4000 long.
Thnaks in advance
You can get an indented BOM from TOOLS - MODEL - then apply on the top level radio button. This creates a text file in your working directory which will be your assembly file name .inf.1 (don't worry about displays in the embeded browser, I think that is worthless)
I usually just import that in to excel and filter it as I need. It does add some useless feature info at the bottom that I simply delete out.
You may also want to save various tree settings for quick BOM export and resetting back to default. I haven't tested this method with something as large as 4000 parts yet.
I have a similar problem but it involves the BOM on the drawing. I want "reference models" as I call them to be automatically filtered in the BOM (without having to filter the BOM table) AND have the ability in Windchill to show the BOM only - not the whole document tree.
FYI - everything we want is brain-dead simple in SolidWorks. You can RMB click on the model tree and there are settings for 'Include In BOM", "Include Children in BOM", and "Show When inserting assembly" or something like that. They have all the bases covered to my experience. With these 3 things you can
1) Show only top level assembly in BOM
2) Show only children and skip top level assembly in BOM
3) "Hide" some parts when inserted in a higher level assembly
These settings are carried on the "link" not the file, so you can change them on a "per usage" basis.
If someone can help with these problems (without having to restructure Winchill or write macros) let me know.
You might follow up with this Component Parameter in repeat Region - http://portal.ptcuser.org/p/fo/st/thread=56143
It touches on creating component level (link) parameters. You'll be most interested in http://portal.ptcuser.org/x/fo/st/imagelb?fid=27878&topic=3 which is image006.png on the above page.
Thanks - I'll look into it. Seems a lot more complicated than simply picking a checkbox on a form as in other CAD packages.
OK - that works. Here is the process if anyone else wants to know it:
1) In the assembly, open parameters form.
2) Set "Look In" selection box to "Component"
3) Select component you want to exclude from BOM
4) Add a parameter to the "Component" such as "INCLUDE_IN_BOM" as Yes/No and set to "No", then designate it.. Side note - this is called a link or relationship in other CAD tools. It puts the parameter on the relationship, not the part model. Many people use "Component" and "Model" interchangibly but they are not the same in Creo.
4) Do the same for all componenents you want to skip.
5) In the assembly drawing, add a filter rule to the BOM table with &asm.mbr.cparam.INCLUDE_IN_BOM != FALSE
That should do it. Does not answer my problem with Windchill though - how can I see the BOM list, not the document tree, in Windchill, and also export it to Excel.
Contrast that to the following for solidworks
1) RMB click on component in model tree
2) Unselect "Include in BOM"