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H
HatimAbdul1-Visitor
1-Visitor
May 16, 2012
Question

Error: cannot add/remove references in the sketch

  • May 16, 2012
  • 6 replies
  • 12204 views

I encountered this message (attached) that informs me I cannot add or remove references in the sketch and the reason is this feature has many dependents. This is the first time I see this. I used to be in control of my design intent by redefining and rerouting my features any time and resolve any subsequent failures. Have anyone seen this? Thanks.

6 replies

K
KshetrabasiMaha1-Visitor
1-Visitor
May 17, 2012

Hi

Please Upload the part or few screen shots for better understanding

Regards

K.Mahanta

G
GregFrankland1-Visitor
1-Visitor
May 17, 2012

I have seen similar messages when redefining a feature that has dependent copies. Is that maybe what you have here?

-Greg

J
John.Pryal1-Visitor
1-Visitor
May 17, 2012

Hi,

to figure out what features have become dependant upon the feature you wish to change, & try changing the references of those. Not always possible but sometimes you get lucky.

Regards

John

H
HatimAbdul1-VisitorAuthor
1-Visitor
November 15, 2012

I have to admit I didn't know that at the time I posted this but I found out this message comes up (cannot edit sketch references) if the feature is mirrored. I had to delete the mirror, rededfined and re-mirrored. It makes more sense to me to be able to redefine a feaure that is mirrored and the mirror updates.

    Patriot_1776
    Patriot_177622-Sapphire II
    22-Sapphire II
    November 19, 2012

    This is another thing PTC should fix instead of giving us the rubbish that are ribbons. Why should we have to delete mirrored or dependent copied features just to dd references. Of note, you can REPLACE references in sketcher.

      J
      JonathanHodgson13-Aquamarine
      13-Aquamarine
      November 19, 2012

      Submit an idea, Frank, and I'll vote it up.

      Or, if you don't have active maintenance, I'll put the idea up...

      I
      ICAD_Support14-Alexandrite
      14-Alexandrite
      August 9, 2019

      Hi...!!!

      Still this issue is not solve in Creo parametric 6.0.1.0

       

      i also facing same...

       

       

      please help..

       

       

      P
      Pettersson15-Moonstone
      15-Moonstone
      January 14, 2020

      I get around this by mirroring geometry instead of features. So instead of selecting the feature to mirror, select the surfaces (using Seed & Boundary, usually), copy-paste, mirror the resulting quilt (you can mirror the copy feature, but I prefer mirroring the quilt), then solidify. You get a better and more stable mirror that's easier to redefine, and you can change references in your sketches as much as you want. If it's a lot of features that you want to mirror, it results in a smaller feature count and quicker regeneration, too.

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