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Error: cannot add/remove references in the sketch

HatimAbdul
1-Newbie

Error: cannot add/remove references in the sketch

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.

10 REPLIES 10

Hi

Please Upload the part or few screen shots for better understanding

Regards

K.Mahanta

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

-Greg

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

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
22-Sapphire II
(To:HatimAbdul)

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.

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

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

Hi Frank. Thanks for the contribution. I think I thought of using "replace". I believe the references dialog was completely grayed-out. The error message blocks any access to that dialog. You OK the error and the dialog closes.

I've had to deal with this error message couple of times already. Then I had to redefine the features so they became driven by sketch where I could put the symmetry condition. Just for this odd reason.

Call this tool productive.

Anyway FMX mirror feature solves this issue. The thing is that you have to know that in advance and most importantly you have to have FMX. I don't like using FMX features where I don't really have to, they add up alot to regen times.

Hi...!!!

Still this issue is not solve in Creo parametric 6.0.1.0

 

i also facing same...

 

 

please help..

 

 

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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