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Can't access 'dimension properties' on shown dimensions (Creo2)

ptc-5468142
1-Newbie

Can't access 'dimension properties' on shown dimensions (Creo2)

Do you guys have any idea why I can't access "Dimension properties" of shown model dimensions in drawing? It works with dims created in drawing but not with shown dimensions. Double-click does nothing and when I right-click there is not even "Properites" option in that menu

1 ACCEPTED SOLUTION

Accepted Solutions

I had it set to cosmetic_only, and that was the problem.

Thank you guys, you helped me a lot!

View solution in original post

16 REPLIES 16

Are you in the Annotate tab?

Could it be that the model is locked (either file system or windchill)? That could explain being able to modify created but not shown dimensions.

Stephen, if you mean this (see picture), then no it's not locked.

1.jpg

Graham, yes, I am in the Anotate tab.

Is that the lock on the drawing or the lock on the model (.prt or .asm) file?

Can you modify the properties of the dimension in question in the model (not through the drawing)?

it's on the model.

Yes, I can modify it on the model.

I hate this option but it does sometimes solve "glitches". Have you tried restarting Creo? It sounds like a glitch.

well, honestly I'm struggling with it for more than one year. First I though it is "normal" for Creo (came from W2), but 2 days ago I saw one guy and it worked for him, so there must be way how to solve it for me too.

EDIT: I've got his config, but it still doesn't work...

Is the part 'In Work' and checked out to you?

yes, it's checked out, but it also doesn't work when I'm outside of windchill. Even if I create new part and make drawing out of it.

Have you been able to modify shown dimensions before and now you can't? I'm trying to remember if there are any .dtl or configuration settings that interfere, but the ones that come to mind prevent adding created dimensions to models.

I'm guessing you can select the dimension on the drawing and just not change it.

Can you make the change you want in the model and it shows on the drawing?

The most common things I've had, from the top:

1) Model is locked

2) No permissions

3) Generic is locked/no permissions

4) There's more than one model in the drawing and I need to repeat 1,2, or 3 on the correct model.

5) I accidently select the stupid view and the dimension, so no Properties are available

6) I left a select filter set to Symbol and can't select the dimension

7) The config option Gabriel Zaha mentions.

Check your config.pro for the "draw_models_read_only" option. If this option is set to yes then you are not able to modify model dimensions from the drawing.

I had it set to cosmetic_only, and that was the problem.

Thank you guys, you helped me a lot!

View solution in original post

Well that's an interesting option. It would come in handy if you wanted to make sure someone unqualified wouldn't/couldn't change anything.

An excellent addition to the config.sup file for Next April Fool's day.

Can't access 'dimension properties' on shown dimensions (Creo4) (dimension text)

what is it the problem with it

StephenWilliams
22-Sapphire III
(To:T_CAV)

The model is locked (non-modifiable).

 

or

 

There are no dimension properties in Creo 4. When you select the dimension, the ribbon automagically displays everything that used to be in the "properties" dialog box. 

 

no-properties.jpg

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