Frame Generator, Parts list sorted by both Part Number and Length.

Originally Published 5/31/2013


At the company where I work, we build a lot of welded steel frames.  Tube steel, angles, channels etc.  Nearly every piece of equipment we build has some sort of welded frame either large or small.

To make it easier on our welding shop, we try to format our drawings so that the parts lists show the cut length of each piece of steel.  Our purchasing system gives a distinct part number, not to each cut piece of steel, but to the steel profile and size.  For example: L1.5″ x 1.5″ x 1/4″ steel has a part number, regardless of the length it is cut to.

In order to avoid a parts list that takes up an entire sheet in our drawing set, especially for large frames, we decided long ago to sort our parts lists by both Part Number and Length parameters.  Unfortunately, the Inventor BOM editor only allows grouping parts based on the Part Number parameter.  The result is that if you have multiple pieces of steel, with the same part number but cut to different lengths, the Length column shows the value as “Varies”.  Well, that’s not very helpful, so whattya gonna do?

It was actually some discussions on the Autodesk ® Discussion Forums that led me to this solution (workaround).  First, a little background fact from Frame Generator.  Every frame member generated by Frame Generator contains a parameter called “G_L”, which is the final overall length after all end treatments have been applied.  Knowing that, I was able to put this formula into the “Part Number” field in all of my frame BOMs: =<Cost Center>-<G_L>.

“Cost Center” is a standard iproperty on all parts in Inventor, I chose that simply because we were not using it for anything else.  So, I put the formula into the Part Number field, and put our Part Number into the Cost Center field.  I do this ONLY on Frame Generator members, everything else I leave as is.  What I get as a result, then, is a combination of the two values separated by a dash, as in: 123-45678-001-36.000 in.  With these values combined, I can now group by part number and have them roll up common lengths into one row in my BOM.

So, that takes care of the BOM, now I need to make the Parts List in my .idw show this in such a way that each Part Number length combination has a row complete with a quantity of the number of pieces cut to this length.

For the columns I use “Item Qty” as Qty and simply change the heading of the Column in the Column Chooser screen of the Parts List editor.  For Part Number, I actually use the Cost Center property, and again, change the column header to Part Number.  For the Length column, I create a new property called “G_L” so it will pick up the value of that pat parameter.

I change the column header on that to Length, and the result is what you see above.  To ensure that this is done for every frame drawing we create, I built all of this into a template file which is used for all frame detail drawings.  I also added the formula to the Part Number column of all of my Frame Generator parts in the Content Center, so that it is automatically generated into each new component as it is created.


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CAD Department Supervisor at Powell Fabrication & Manufacturing, Inc. CAD Designer & Detailer specializing in Inventor Tube & Pipe, Frame Generator, Content Center, Vault Professional. Autodesk Expert Elite member. Blogger. Autodesk University Speaker 2014-2018. Husband and father. Photographer.

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7 comments on “Frame Generator, Parts list sorted by both Part Number and Length.
  1. Thank you. This is very similar to something I am dealing with. My question is: when adding the formula to the BOM, is that something you have to do for each line item in the BOM, or is there some template for the BOM itself?


    • cgbenner says:

      Hello! Thanks for the question. I’m afraid there is no template for the BOM itself. What I generally do is type the expression into the first row, an then copy and paste to the rest. You can also place the expression in the Part Number column of your content center parts. If you use an unusual iproperty as I do (cost center), you may have to add that to your content center family table as well. Populate that column with your actual part numbers and map it to the Cost Center iproperty in Inventor. Put the expression in your Part Number column properties and map to Part Number. When a frame member is generated, it should automatically have this information on it. If you can wait a day or two, I may have time to make a video of this, and post a link.


  2. cgbenner says:

    A question was posted in another thread related to this topic, so I am addressing it here. The question was: Do the iproperties of each frame member need to be individually modified?

    The quick answer is yes. But if you look at the previous reply, you will see a description of how to do that quickly while editing your BOM, as well as how to add it to the Content Center so you won’t have to manually do this from now on.


  3. S. says:

    Hi there,

    I am looking to increment the part number numerically, eg 485-0073-010-01 for the first instance, 485-0073-010-02 for the second instance and so on. Is this possible?



    • cgbenner says:

      As far as I know this is not possible at this time. The part numbers are generated automatically. I’m not very knowledgeable in iLogic, but it may be possible to create a solution using that. I would suggest postin in the Autodesk Inventor forum, there are a lot of iLogic gurus there who may have a clue. Thanks for rading and good luck!


  4. Michael Peterson says:

    I’m running into the issue of the “size” drop down within the FG dialog showing my expression rather than size. I authored an iPart, so there are multiple sizes within that family. I assume it’s happening because it’s pulling the information from the part number column in CC. Have you seen this issue by chance?


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