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23-Emerald III
BenLoosli23-Emerald III
23-Emerald III
June 2, 2015
Solved

Merge independent part into a family table

  • June 2, 2015
  • 2 replies
  • 10634 views

One of our designers had a problem modifying a Family Table that he created so instead of asking for help, went and created 3 independent part files with the sme number scheme.

Now I want to merge them into the family as instances.

Is this possible to do with Windchill 10.0 m040? I know I could do it with Intralink 3.3.

Is there a PTC document that explains the process or has someone got a cheat sheet for the steps involved.

Thanks.

Best answer by BrianToussaint

Ben,

I took this from my directions to take a single object and rename it to make a generic and add instances.  Since you have all the objects already there, you will need just these.  Make sure that you only put your current generic and instances in the workspace to begin and not the one you want to add.

 

  1. Open the part in CREO.
  2. Create a family table.  Add instances for the original number and each number created in Step 4-5 above.

    2.jpg

  3. Return to the workspace in CREO.
  4. Remove the CAD part from the workspace.  In the “Remove from Workspace” dialog box, uncheck the box for “Erase object(s) from CAD Application”

    4.png

  5. Go back to the model in CREO.  Verify the family table and save.
  6. Go back to the workspace.  Everything should show up as new and the original part is now an instance.

    6.jpg

  7. Add all the parts into the workspace.  Verify that “Reuse modified workspace content” is selected.

    7.jpg

  8. Select Yes to Replace in Session the renaming of the objects.

    8.jpg

  9. Notice that the part has the icon for “Modifications are not eligible for upload”. Select the parts and the drawing and do a Check Out.  It is now available for Check In.

  

2 replies

B
BrianToussaint19-TanzaniteAnswer
19-Tanzanite
June 2, 2015

Ben,

I took this from my directions to take a single object and rename it to make a generic and add instances.  Since you have all the objects already there, you will need just these.  Make sure that you only put your current generic and instances in the workspace to begin and not the one you want to add.

 

  1. Open the part in CREO.
  2. Create a family table.  Add instances for the original number and each number created in Step 4-5 above.

    2.jpg

  3. Return to the workspace in CREO.
  4. Remove the CAD part from the workspace.  In the “Remove from Workspace” dialog box, uncheck the box for “Erase object(s) from CAD Application”

    4.png

  5. Go back to the model in CREO.  Verify the family table and save.
  6. Go back to the workspace.  Everything should show up as new and the original part is now an instance.

    6.jpg

  7. Add all the parts into the workspace.  Verify that “Reuse modified workspace content” is selected.

    7.jpg

  8. Select Yes to Replace in Session the renaming of the objects.

    8.jpg

  9. Notice that the part has the icon for “Modifications are not eligible for upload”. Select the parts and the drawing and do a Check Out.  It is now available for Check In.

  

    H
    hhj1-Visitor
    1-Visitor
    April 29, 2019

    Dear @BrianToussaint                              

    thank you very much.

    the imcompatible issue offen make me job very hard, I checked all PTC online help, howerver can not clearly understand the main points, up to here I see your example. there two time undertable replace, change name and keep content.

    I am in elevator industrial, there are a lot of similar part which is organized by family table, which is managed by Windchill, however, we time to timely modify some intent and forget download whole family, so imcompatible will happen, and I do NOT want redo all modification, your way is only way to keep my mofication and successfully check in.

    thank you!

    Best regards, Hongjie

    B
    23-Emerald III
    BenLoosli23-Emerald IIIAuthor
    23-Emerald III
    August 20, 2024

    This is my write up on taking a standalone part into an existing family table based on Brian's reply to my original post.

     

    Adding a standalone part to a Family Table

    1. Name the standalone part to the new FT instance name
    2. Open the generic FT in Creo
    3. Create the new instance with same name as in step 1
      1. Set all to continue
    4. Remove the generic and instances from the workspace
      1. Uncheck the Erase object from CAD application
    5. Verify the FT and save it
      1. All items should show as new
    6. Add the standalone part to the workspace
      1. Check reuse modified workspace content
    7. Select Yes to Replace in Session for renamed object
    8. Check out the generic and instances
    9. Check in the generic and instances
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