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Editing Dimensions after placement problems

SOLVED
Participant

Editing Dimensions after placement problems

Hi There,

 I am having a problem with Creo 5.0. Its possibly something im doing. 

 

Lets say I have a simple part drawing, with a few dimensions created using the dimensions tool on the annotate tab. I create a hole diameter measurement and add some text through the dimension text box. All is well in the world. Close the drawing. Check in to Windchill or sometimes don't check in.

 

When I come back to the drawing later, say I want to change the text or add the basic box around the dimension/add a tolerance, when I select the dimension, Creo doesn't bring up the dimensions tab, instead it brings up a format tab. This gives me no options to make the changes I wanted to make. I have tried multiple different way of selecting the dimension, including ensuring that I am in the annotation tab and that I use the drop down selection filter. Nothing works.

 

The end result is that I have to delete the dimension and recreate it. Which is fine once or twice but when its every dimension on the drawing, then it becomes painful.

 

Any thoughts

Lee

1 ACCEPTED SOLUTION

Accepted Solutions

Re: Editing Dimensions after placement problems

Verify the .prt (or .asm) file is unlocked in windchill. Depending on your config file, created dimensions in the drawing may be actaully in the model. If the model is locked, you will not be able to edit the dimensions.


Steve Williams
Pro/E Version 15/16 (Circa 1995/1996)

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5 REPLIES 5

Re: Editing Dimensions after placement problems

Any pictures or screen shots you can share to clarify what you are asking?

Re: Editing Dimensions after placement problems

Verify the .prt (or .asm) file is unlocked in windchill. Depending on your config file, created dimensions in the drawing may be actaully in the model. If the model is locked, you will not be able to edit the dimensions.


Steve Williams
Pro/E Version 15/16 (Circa 1995/1996)

View solution in original post

Re: Editing Dimensions after placement problems

Hi,

please attach pictures of Creo UI. Show us

1.] which tabs are available when you create new dimension

2.] which tabs are available when you edit existing dimension


Martin Hanák

Re: Editing Dimensions after placement problems

Hi Steve,

 I think you are correct, I have just tried a few times and it wont let me edit a dimension in the drawing unless the model is also checked out, once its checked out it works fine. I wasn't aware of that.

 

Thanks

Highlighted

Re: Editing Dimensions after placement problems

Just for clarification, there is a config option  called create_drawing_dims_only and its default is NO which basically means that created dimensions in the drawing actually "belong" to the model and are stored in the model.

If you set the option to YES, then the created dimension is in the drawing only.

There are some drawbacks to each setting. One of which you found. I know another that affected us was if you had a created dimension, you couldn't associated model GD&T to the created dimension.

I think there are other advantages/disadvantages but I can't think of them right off hand


Steve Williams
Pro/E Version 15/16 (Circa 1995/1996)
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