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

Discussion in 'SolidWorks' started by unicornhorn2, Mar 4, 2006.

  1. unicornhorn2

    unicornhorn2 Guest


    I was wondering if you can bring multiples of the same part into an
    assembly (lets say they are lego pieces being stacked) , extrude cut
    various shapes out of the assembly, and finally, save the altered parts
    as different files; in order to create a detailed part drawing?

    I have had a difficult time finding a solution for this and I'm using
    sw2006. The assembly ends up having about 400 similar pieces with
    slight modifications in relation to one another,

    Thanking you in advance,

    John (newbie to the group)
    unicornhorn2, Mar 4, 2006

  2. 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"
    Jerry Steiger, Mar 5, 2006
  3. unicornhorn2

    unicornhorn2 Guest

    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

    I was able to 'edit part' in the assembly by clicking on the specific
    copied part (eg. brick<13>) 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,

    unicornhorn2, Mar 6, 2006
  4. unicornhorn2

    TOP Guest

    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.
    TOP, Mar 6, 2006
  5. unicornhorn2

    unicornhorn2 Guest

    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
    unicornhorn2, Mar 8, 2006
  6. Cool! Nice way to use multi-body parts.

    Jerry Steiger
    Tripod Data Systems
    "take the garbage out, dear"
    Jerry Steiger, Mar 8, 2006
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