Thanks. I was able to get the .iam assemblies to show up in a 'parts only' list by setting them to inseparable as suggested, but the total qty's still did not calculate for 'all levels' - maybe I am missing something?
I have attached a diagram of what I am trying to create parametrically through inventor..
What version of Inventor are you using?
Also I should explain that if you set any iam file to 'Insperable' that contains iam files you need totaled you will lose the nested iam files which show in your example pdf file. I am not sure if you did that or not?
There is no quick and easy way to answer your problem without knowing exactly what you need to accomplish. If you need the iam files listed as a 'Parts Only' in addition to what you described in the OP then you will have to consider how you do both when you change the iam files to 'Inseperable'. You might be able to accomplish what you need by creating a derived part of each iam file. Then use another iam file with the derived parts to create the 'Parts Only' option.
Actually I think you might have overlooked a workable solution that should be possible. Using the following post:
"Not as fast and easy as the "Parts"Only" BOM level, but if you ask for a "Structured - All Levels" BOM, then export it to Excel, you can use the Excel sort features to get the data you need. Just make sure you have the columns in the BOM you will be sorting by after the export."
Instead of exporting to Excel try using the 'Group' option when you edit the Parts List format or try the 'Part Number Merge' setting in the BOM Editor.
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My last attachment ASSY-ONLY-LIST.pdf is exactly what I'm trying to achieve, no more, no less - ie: total merged assembly calculation of all structure levels.
This can be tested by creating three empty assemblies and replicating the structure per the hierarchy on my previous attachment, then creating a parts list from the assembly.
Forget about parts, they can be easily isolated filtered away, I am only interested in calculating total assemblies.
- I found Inventor does not group, calculate or merge assemblies as suggested, regardless if set to inseperable, because Inventor always tries to honor the structure.
The way it is, if a user has 100's of drawings which detail an assembly that is used repeatedly at various levels, if they need to purchase total assemblies for the complete job ie; a fabricated bracket system commonly used, they have to go through each BOM assembly list on 100's of drawings and manually calculate the total quantity for order - this is a non parametric method subject to error.
I have seen similar requests on this forum dating back years ago, but still no action from Autodesk to date.
This is frustrating coming from Mechanical Desktop which could perfom this function easily.
Does anyone know a formal way to request Autodesk to add a 'all assemblies' BOM list option?
Does anyone know how to modify the existing 'parts only' BOM parts list function to 'assembly only' using VBA editor?
Thank you all for you input, in the mean time I will try playing around with excel to try and merge the assembly numbers and then perform a second function by calculating the quantities as well.. my brain is starting to hurt already.. Maybe I should just learn VBA editor when I get the time!
I have the same problem.
It has been plaguing me for years, I still don't have a solution, nor does Autodesk?
Has someone written some code for it yet? If you have found something over the past few months, please share.
I create an IPT file that has matching iProperties for each subassembly. The IPT file has no geometry. I insert that matching IPT file into its corresponding sub-assembly IAM file. In the IDW parts list for the sub-assembly I turn off the visibility of that extra IPT. This extra part file is just a placeholder for the subassembly BOM data.
On the top level assembly I create a parts-only Parts list. It will show the total quantity for each and every subassembly just like it does each part.
No need to manual expand each assembly in a structured listing
No manual calculation
Creates a line item in the parts listing for each assembly just like each part
Ability to assign a material to an assembly
Only needs to be done once for each subassembly
Must remember to create this part file for each subassembly
Must remember to copy and rename this part file when doing a copy design.
Instead of an empty IPT file you could create a virtual component in the subassembly IAM file with matching iProperties and accomplish the same thing. I prefer to use an empty part file as I have a macro that fills out the iProperty data based upon file name and file location. The empty part file has the same filename as the subassembly so the data generated by the macro is identical.
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