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JLG2-Explorer
2-Explorer
July 25, 2016
Solved

show merged pattern dimension on drawing

  • July 25, 2016
  • 2 replies
  • 5319 views

I'm currently working with Creo Parametric 2.0 M200.  In the past I know I was able to show a pattern dimension from a merged part on the drawing but I can't seem to remember how to do it. For example, I have a merged part like this:

On the drawing I can show the dimensions for the first hole in the pattern, but I can't show the pattern dimension of the angle between the holes (60° pink, created dimension below):

Does anybody know how to do it?

Thanks!


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    Best answer by manjunathrv

    Yes. You are right. I use Creo 2.0 M180 and i have the same issue.

    But there is a simple workaround. Follow these steps:

    Change the external merge feature to Inheritance feature where you inherit all the features to the merge.

    Then from the drawing model tree expand the External inheritance feature, select the pattern, RMB show dimensions by view:

    You will now be able to show the 60 degree dimension. Once this is done you can revert back the Inheritance to External merge (toggle inheritance). You will be able to retain the dimension.

    I tried this and it works

    2 replies

    M
    manjunathrv17-Peridot
    17-Peridot
    July 26, 2016

    With the Show/Erase command highlight on the view, RMB -->Pick from List and then you will be able to select the features in the merge and show their dimensions.

    J
    JLG2-ExplorerAuthor
    2-Explorer
    July 26, 2016

    Thanks for your suggestion.  Unfortunately, I can only get the hole dimensions, not the pattern dimensions by picking from the list.  We recently upgraded to M200 from M130 and I could swear I was able to do it under M130.  I simply do not see the pattern in the list.

    Anybody have any other suggestions?

    Thanks!

    M
    manjunathrv17-PeridotAnswer
    17-Peridot
    July 27, 2016

    Yes. You are right. I use Creo 2.0 M180 and i have the same issue.

    But there is a simple workaround. Follow these steps:

    Change the external merge feature to Inheritance feature where you inherit all the features to the merge.

    Then from the drawing model tree expand the External inheritance feature, select the pattern, RMB show dimensions by view:

    You will now be able to show the 60 degree dimension. Once this is done you can revert back the Inheritance to External merge (toggle inheritance). You will be able to retain the dimension.

    I tried this and it works

      R
      rohit_rajan15-Moonstone
      15-Moonstone
      July 27, 2016

      I think even if you right click on any other pattern feature other than the original feature and select show model annotations it will give you the pattern dimensions.

      Which has already been mentioned by Manjunath.

      J
      JLG2-ExplorerAuthor
      2-Explorer
      July 27, 2016

      Thanks for the suggestion!  I tried selecting a hole other than the lead, but it didn't work for me -- I still couldn't display the pattern dimension.  If you are seeing different behavior, maybe it varies between builds, or maybe there's a config option that affects this.

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