I am using a student version of Inventor 2012 to design the FSAE Chassis for our University team this year. I was not able to find suitable geometry for the required tubing to make the chassis. So I found a guide on setting up a Custom Content Center and publishing parts. I have followed that. The Chassis has turned out great but now I am trying to draw it up and the BOM is not populating as desired.
-Custom Project file with Read / Write Library added.
-Custom tubing geometry created and published to the Library.
-Chassis constructed using standard Frame Generator techniques.
Previously I had the chassis modelled using standard Content Center parts and the BOM would populate with the individual tubes in the drawing environment. Now with the custom tubes the BOM calls up each of the individual tubing sizes, ONCE only and has large quantities. The automatic "Measure" Column is also populated with "*Varies*".
I am out of my depth here but have a few ideas. In the Frame Generator wizard each tubing size has come up as it's own "Family".
I believe this is because I have published the different part sizes individually. I am guessing I should have published only the one active part but with variable geometry selectable in the "Size" drop down? I am unsure how to achieve this if that is the problem.
I have tried forcing the assembly into the "All Levels" view with the Bill of Materials pop-up in the Assembly environment, but even this is not populating correctly.
Something else I have notcied is the individual tubes are using a different naming convention in the model tree.
See the attached pics.
Can somebody help me populate the BOM correctly?
With Frame generator, because there are an almost infinite number of ways that companies set up their BOMS, you have to play some games. For example:
We like to sort our Parts Lists by Part number and cut length. Out of the box, this does not work for us, since the part number only refers (in our system) to the profile. So we get all 3" angle iron (for example) lumped together with the cut lengths showing as "Varies". Like what you are seeing.
We decided to:
1. Put the Part Number into the Cost Center field (because it was open... pick an open field).
2. In Part number we put the equation: =<Cost Center>-<G_L>
(g_l is the parameter used in all Frame Generator parts for cut length, after any trimming and notching is done.)
3. In our Parts List we mapped the column labeled Part Number to the Cost Center property since that has the actual part number for that profile in it. Under our Length (your measure, I assume) we mapped to G_L.
4. In the BOM, we still sort by Part Number, but since we have the equation in there, it will sort by the part number AND length, and list each separately. So, if you have (6) pcs of 2" tube cut to 2' long, and (3) cut to 1' long, they will list separately, but show up with the same part number.
This is a lot to follow, but it may get you at least close to what you want. Play around with those equations, using the format I posted... and maybe you can get what you are looking for.
Hope this helped!
Hi Chris, There are two work flows which may assist you with your problem.
The first, is part number merging, the second is unique part numbers. The part number merging behaviour seen in your IDW Parts List can be turned off via the assembly Bill Of Materials; the option that you’re looking for is “Part Number Row Merge Settings” , simply disable it. Once disabled, any parts that have the same part name will no longer merge.
The second alternate work flow would be to edit your custom tubes Family table, and program your parts so that when generated they all generate with a unique file name. For example, I see one duplicate part number is “1_0.095Tube”, and every time you generate a similar part the same name will be used over and over. One relatively easy way of creating a unique name would be to add the cut length to the part name, so that the final part number reads as “1_0.095Tube 10x1050mm” or something similar. Let me know if this makes sense. I can show you via a remote session if needed.
Karl Hosking | Technical
Cadgroup Australia Pty Ltd
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sounds great - exactly what I need - but how do you do it?
One relatively easy way of creating a unique name would be to add the cut length to the part name, so that the final part number reads as “1_0.095Tube 10x1050mm” or something similar.
Would be very grateful for a tip!
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