Copy the same part into assembly, then edit, then save derived parts??

Yes, this shouldn't be a problem. Save one of the parts under a new name, then make the cut that parts needs. You need to be sure that you are editing the part, not making an assembly cut.

Jerry Steiger Tripod Data Systems "take the garbage out, dear"

thanks for the help,

that happens to be exactly what I was trying to do though. I stacked multiples of the same piece and then used the extrude cut (in the assembly) to remove the required shape to maintain the proper stacked configuration.

I was able to 'edit part' in the assembly by clicking on the specific copied part (eg. brick) and then save that part as a copy. I was hoping for a more efficient way to extrude cut around 10 bricks at the same time with one shape and then save the resulting parts.

Maybe I have to 'save as copy' the original part 50 times and bring them into the assembly individually?

thanks again,

john

An assembly cut will not show up in the individual parts. Here is how you might create the necessary cuts.

1. In the part to be cut (target part or TP) create a design table.
2. In the design table create however many versions of the part you are going to need.
3. Insert the part into the assembly in the proper relationship the other TPs.
4. Create another part to do the cutting. Call this the cutter part (CP). It represents the "hole"
5. Locate the CP in relation to the TPs. Make sure the CP goes through all the TPs.
6. In each instance of a TP RMB to get the properties dialog and choose a unique config name previously created with the design table.
7. Insert a cavity feature in each TP using the CP repeatedly.

This will create in-context features in each TP. Once they are created you can lock them to prevent the assembly from changing them.

On a scale of one to tedious this is a ten. And AFAIK you can't automate selecting the config of each TP which means it is always going to be manual.

Hello, thanks TOP for the input. I'm not too familiar with design tables but I was able to find a work around;

instead of bringing in mulitples of the same part into the assembly, I used Insert>Pattern/Mirror>Linear Patter to multiply the part while in the part document.

Then I brought the part into the assembly where I went to edit part and did the necessary changes (extrude cuts)

While editing the part, I was able to go to the feature manager tree, opened up the tab for 'solid bodies', then right clicked on a specific solidbody of choice, and finally clicked 'insert into new part' which allowed for me to be able to save all of the various parts seperately.

thanks again, john

Cool! Nice way to use multi-body parts.

Jerry Steiger Tripod Data Systems "take the garbage out, dear"