Ok, I was giving an assembly with a lot of piping in it, but the piping wasn't done using the Tube & Pipe.
I need to make a drawing of the piping with a BOM. I made an ISO view and turn off the visiblity of the parts I didn't need.
My question is if there is way for the BOM to only show the visible parts in my drawings. I know in iAssemblies I can exclude the parts I don't need, but that would take awhile considering there are over a hundred parts in my assembly. I really don't want to redo the piping mainly because of my inexperience with Tube & Pipe.
Solved! Go to Solution.
If you set up a view rep in the assembly model you should be able to select the view rep in the part list in the drawing to show only parts included in the view rep.
The BOM will still show all the parts.
I don't have tube and pipe but I assume the view reps work the same as a normal assembly.
Ok I tried that but the Part List still shows all the parts.
The only way it doesn't is if I change the BOM Structure to Reference, but then it changes it in all the view reps.
Ok, I didn't realize this until now. But the BOM still shows the qty for the entire assembly.
For example in the piping assembly I only have 7 elbows, but the BOM say I have 22, which is the qty for the entire assembly.
Is there anyway to filter that out too.
Sorry, no, that's the one drawback with this method.
Lots of folk have complained about this.
Quantity stays true to the BOM not the view.
Only way is to highlight Qty beside balloon with text or a leader, or override balloon Qty (this is possible but a bit convoluted http://forums.autodesk.com/t5/Autodesk-Inventor/Ba
If you override the part list Qty it will affect the related Qtys in all part lists in that idw file.
It may be easier to split up the large assembly and demote to assemblies you require then views and Qtys will line up.
Sorry can't be of more help.
In a way yes, but you shouldn't have to recreate them.
In the top level, if you select all the parts which you want to be in a sub, you can right click, then demote them and create a new sub assembly.
If you do this as one step most of the constraints should hold.
I sometimes do this for hydraulic hose assemblies.
Place and constrain the ends in the top level,
Create the hose and line up with the ends,
Once I'm happy, demote the ends and the hose together to a hose assembly.