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associativity from drafting to modeling

associativity from drafting to modeling

associativity from drafting to modeling

(OP)
Hi all,
If we change the dimensions in modelling it automatically changes in drafting file.
Is it possible that if i change a dimension in drafting file will it change the models dimension.
Is there any way to achieve it.

Regards,
Karthikeyan.J

RE: associativity from drafting to modeling

I don't think so. I will have to try it. I hope that it doesn't work. This is one of the problems with Pro/E, the drafter can change the engineers model.

"Wildfires are dangerous, hard to control, and economically catastrophic."

Ben Loosli
CAD/CAM System Analyst
Ingersoll-Rand

RE: associativity from drafting to modeling

I checked some more in UG NX. UG doesn't allow you to select the dimension on the drawing face and change it. this is good. There is a switch in the default files that will allow you while in the Drafting module to have access to the expression editor. From here you can change the values that drive your shape.

"Wildfires are dangerous, hard to control, and economically catastrophic."

Ben Loosli
CAD/CAM System Analyst
Ingersoll-Rand

RE: associativity from drafting to modeling

Which "default" file would itthe switch lies in. Guess it would be in the UGII directory.

By the way, is there no way to change the dimensions manually in drafting mode?

RE: associativity from drafting to modeling

While it isn't a generally accepted practice, dimensions may be manually changed in the text editor.  To determine which dimensions on a drawing have been manually edited, go to "info, other, object specific, dimensions with manual text" and the edited dimensions will highlight.

RE: associativity from drafting to modeling

The access to the expression editor in drafting is set in the ug_metric.def or ug_english.def file. The initial default is in the UGII dir, the syslog will tell you which file you are running. (I move mine to a network drive, so all seats use a common file.)

Dimensions can be editted to manual values by selecting them in the annotation editor and then entering your value. Like ewh said, you can info the part to see which dimensions have been edited. It is a one way edit, once made manual the only way to get an automatic dimension back is to delete and re-create. Making manual edits and getting caught, gets an e-mail sent to the person responsible and the engineering manager.

"Wildfires are dangerous, hard to control, and economically catastrophic."

Ben Loosli
CAD/CAM System Analyst
Ingersoll-Rand

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