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More drawing format questions

More drawing format questions

More drawing format questions



I am a ProE user, and am using UG to do a small project for a client.  I am pretty clueless on some of the basics, but can't find answers in CAST.  Currently, I am stuck on what should be a fairly simple problem.  

I have the client's drawing format as a part file (all the line and text entities are in the part model, there are no drawings in the file).  I am trying to get that format into my part file drawings.

I can't find a way to copy and paste, or to import into the drawing.  What is the best way to do this?  Might it involve creating a drawing template?

Dan Blaugrund

RE: More drawing format questions

One way is to import the drawing format to your part file; use File->Import->Part... then browse to the file containing the drawing format.

RE: More drawing format questions


How do I get the line entities to import into the drawing, rather than the model?

Thanks, Dan

RE: More drawing format questions

A better way is to save the format file as a pattern and then use Format-Pattern and bring it in that way. This will bring in the format as a single entity instead of multiple lines and text notes. Like a Pro/E format, but without the predefined views.

If you do the File import, be sure that you are in drafting when doing the import. This should bring the format into the drafting view.

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

Ben Loosli
CAD/CAM System Analyst

RE: More drawing format questions


Sorry to be clueless, but I still can not figure out how to get the clients format(title block), which exists in the model application, into the drawing.

Also, how do you save it as a pattern?


RE: More drawing format questions

What version of UG are you using?

If you want, zip the drawing format file and e-mail it to me and I will prepare it to be a pattern for you and then send it back. Me e-mail address is in my profile.

I haven't saved a format in years since they hardly ever change. I know there used to be (V16) a button to save pattern files. It might be under File-Options-Save.

You will need a GRIP program to conevrt model entities to drafting entities. There might be an interactive option, but I am not aware of one. It is like saving a format, I don't do it much since ours are all set.

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

Ben Loosli
CAD/CAM System Analyst

RE: More drawing format questions

Hi Dan,

The best way to do is to save the file as pattern and retrive it .
procedure for it :

1.Open the prt file which has drawing format.
( make sure WCS is in Absolute coordinate system)
2.go to file/Options/SaveOptions
3.Save option dialog box appears ,in it select Pattern data only.
4.give apply and ok.
5.Save the part file.
6.Now open a new prt file
7.In it open format/pattern
8.pattern dialog box appears,in it select retrieve pattern
9.retrieve pattern dialog box appears ,select ok
10.select the prt file select ok ,ok
11.point constr dialog box appears ,press reset ok
12.Now the drawing format will be in your new prt file .

Thats all ,


RE: More drawing format questions


Thanks for the help!


RE: More drawing format questions

I know it does seem ridiculous to create a drawing format in modeling and import to Drawings but lots of UG users do that.

As long as you make sure that the CSYS of the Format has the XY plane oriented along with the format lines and is at the lower left corner then you should have no problem placing it on the drawing by choosing the Drafting Application and do a File Import Part and choose your part and 0,0,0 as the placement location.

If you have time to do the Pattern then that may be helpful if the format gets changed or updated.
If you would like to know more about patterns you can use the link below.


RE: More drawing format questions

I just wanted to clarify something about patterns that was not explained.  Patterns are Ok especially for reasons of easily propagating updates etc, but what was not explained to the originator of this thread was that he will need to ensure his Part File containing the use of the Pattern will need to always know the path to the actual Pattern file, which is set in his environment file.  He is a new UG User and the use of a pattern was not a good suggestion for him in this instance because the caveates of using Patterns was not fully explained.  He even stated he was not upto speed on the basics.  Helping him import a Format onto a Drawing would have been simpler.

RE: More drawing format questions


I indicated both how to import the Format into the Drawing
and that Patterns were good if he wanted to look into that option.

To solve the problem of path to the pattern file it can be assembled into the partfile using the pattern and hidden in a layer and then it will always be opened with the file. I've used Pro/E for many years and I'm pretty sure that Dan was looking for a way to use the format as on Pro/E where Format files .frm are used like a pattern on UG.

I'm sure if he had problems with the pattern not being found he would post a question on that.


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