I have the following problem,
I have made a part copy that I added the the assembly but in the partlist of the assembly I need the original from which the partcopy was made. Because of the PDF I am using the 2 parts have different drawing numbers so I have no chance of making them identical.
I would have expected that in the list control I can select the original as I can select components from an assembly but apparently that is not the case.
Solved! Go to Solution.
@NorbertS, I, for one, am not understanding your issue. Perhaps you could include at least a picture of the part(s) you are talking about and what you want in the parts list.
The only way to get 2 instances of different parts into a parts list is to insert two different part files into the assembly. Whether or not the geometry created in the parts files is through a part copy or through features makes no difference.
If you are using the part copy as a "make from" and expect to see an indented parts list, you won't get that via .par files. For that to work, you would have to insert the starting part into an assembly, convert it to a weldment so you can use assembly features, then insert that .asm file into the next level assembly. Then you'll get an indented parts list.
@swertel, True, but I disagree with the convert to weldment step as being necessary. Unless you happen to need weldment features or need additive features.
Converting to weldment opens up the additive features: extrude, revolve, etc. As a non-weldment, you're limited to subtractive features: radius, chamfer, holes, and cuts.
Thanks for the reply.
I have also thought about the weld assembly but that isn't really the case.
let me exmplain a bit the situation.
Image 1 shows the part in the raw stats and that is the part that will have a drawing
Image 2 shows the part as it will be on the assembly, it is riveted on a plate with a hole in it. So I have to remove material as well as add some to simulate the rivet head. If I do it with a weld assembly I can remove the material and the added part would look like a weld bead and that is not really acceptable.
Part copy is the only way I knew how to simulate this process but now I have the partlist problem. I need to refer to the number of the part from image 1.
Just been experimenting with Adjustable Parts and Suppression Variable, and there might be a way of having both states - with and without the 'mushroom head' using a single file.
This only works in ordered mode.
In your part model create the head as a single feature using a revlove.
Right click on the feature in the tree and select 'Add Suppression Variable'.
In the variable table you should then see something like RevolvedProtrusion_2_Suppress with a value of 0.
Make the part an adjustable part (Tools > Assistants > Adjustable Part)
Identify the suppression variable and the length of the spigot as the adjustable variables.
Also, still in the part file change the suppression variable to 1 - this will suppress the head feature.
Save the part file.
Place the part into an assembly as an adjustable part.
Set the length for the spigot, and the suppression variable to 0
You should now see the correct form in the assembly.