Is anyone able to help with a problem we're having?
We have recently created or own drawing border and would like it to be selectable from the list of templates available in the open drawing screen. I have followed online tutorials and have succeded in populating the list with our borders but when you open up the drawing and change the scale to fit the model within the drawing space, the drawing border changes in size too.
Solved! Go to Solution.
Are you working in Master Model mode where the Drawing is an Assembly with the part to be drafted as a Component in the Assembly file, which contains the Drawing border?
It sounds like you used the File/Import/AutoCAD DXF/DWG command into an existing part. With this method you don't get all the options for the import. Use File/Open and change the type to DWG then open the part. On the import wizard you will have more options on the options tab for where the objects show up in the new drawing template.
The important option will be "Send Model Data to" and you should select "Drawing Sheet" and not drawing view. This will make the objects show up on the Drawing sheet itself and not in a view on the sheet that will get resized with the scale. You should not see any Drawing views in the navigator while looking at your template drawing sheet.
By the way if you are in NX8 or later you can turn on the "Drawing Format" toolbar while in drafting and replace your old zones with new more robust zones. See documentation for all that it offers.
The improvements to the DXF/DWG open started in NX7.5.2. What update are you running? Go to help/About NX/System information. You should be at 188.8.131.52 to be totally up to date. You could have maintenance patches on top of that update as well
I tested in NX184.108.40.206 and on the open dialog when you click options you would get "Send Model Data to" and "Send layouts to settings". When I set to Drawing sheet it did not work but when I set both to Drawing view it did. I had to switch to drafting and double click on my Sheet to make it active. You are correct you will see your original line colors. You can make sure your format layer is selectable and then you can select all and edit the object display color to black if you want. Or you could just right click select the Drawing node in the Part navigator and set to Monochrome so that colors don't exist in the drawing.
For the background color you have to set as follows.
If working with Monochrome set:
In the Preferences --> Visualization --> Color
tab --> toggle Monochrome Display on --> set Background color by selecting gray box.
If working without Monochrome set:
Preferences --> Color Palette --> press the Edit Background icon in the
Selected Color section --> set/select the desired color/shade.
I was able to make all my lines black, turn on monochrome, and change the background to white.
I changed the scale of Sheet 1 from 1:1 to 1:5 and nothing happened.