Problem with drawing files

[ptc-5182908]

I am having a problem where I create drawing A, then save a copy of A and rename it B. I then go into drawing B and delete dimensions and save the changes. Now when I go into the original drawing A, the dimensions are gone. I gave the drawing copy a new name so why is it affecting the orignal?

Thanks for your help.

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[TomD.inPDX]

The only way this should happened is if the dimensions were model dimensions (driving) that were truly deleted instead of drawing dimensions (driven). But if you simply changed them on the drawing, this should not affect the model.

It really is difficult to know exactly what is happening without knowing more about your process... but if you can duplicate this to the extent that it really is unexplainable, customer service can certainly help define a true bug. Somehow I must assume there is something amiss with your process, and if not, definitely open a support case.

If you want, you can post files using the advanced editor if you want us to look at them to see if this easily resolvable.

Welcome to the forum, Joe.

[ptc-5182908]

Ok, I found a work-around. I still don't fully understand why, but if I right click on the dimension in drawing B and choose 'erase' instead of 'delete' then it will only drop the dimension on drawing B and not effect drawing A.

[TomD.inPDX]

This is wierd. Can you submit this as a support case to understand why this is happening? This seems like something PTC should know about.

[MartinHanak]

Joe,

it looks like drawings A and B use the same drawing model. Is it your intention to have two drawings for one model ?

Martin Hanak

[SylvainA.]

It is probably because the dimensions are saved in the same part.

Then, if you delete a dimension, it will be deleted from the part, and cannot be "called" by another drawing.

See the descritpion of the Config.pro option create_drawing_dims_only :

Default and Available Settings

• yes—Save all new dimensions created in the drawing inside the drawing as associative draft dimensions.
• no*—Save all dimensions created in drawing mode in the part.

[TomD.inPDX]

That doesn't sound right. Deleting a dimension in a view should only remove it from that view and nothing else. You can show it again in a different view with the Show Annotation dialog.

I am certain there is a good reason for the apparant issue, but it is not clear how to reproduce the problem. I've never had a model dimension deleted by deleting a previously shown annotation.

[SylvainA.]

I'm not talking about driving dimensions. Drawing's dimensions (shown as draft entities in the drawing tree) are stored in the model, thus deleting it from one drawing will delete it from other drawings too (assuming that the same dimension is used twice).

[TomD.inPDX]

Interesting. That is a very scary option for any copied drawing.

[SylvainA.]

Yes, and I learned it the hard way

[dgschaefer]

As mentioned by Sylvain, dimensions created in the drawing are, by default, stored in the part or assembly model, not in the drawing. This allows for using model dimensional and parameter information inside created dimensions.

For example, if you wanted to report the model 'material' parameter in a dimension denoting the thickness, you might create a dim for the thickness and change the dimension text to:

@d THICK &material

Which might look like this on the drawing:

0.125 THICK 6061 ALUMINUM

You can set the config option mentioned above (create_drawing_dims_only) to yes and newly created dims will be stored then in the drawing, but it limits or prevents the use of model dimensions and parameters inside created drawing dimensions.

So deleting a dimension deletes it from the model and it then cannot be displayed on any other drawings that use that model Using the 'erase; command, as the original poster discovered, leaves the dim in the model but removes the display from the drawing.