NX Annotation Preference Defaults

[Herbertaylor]

When preparing detail drawings I need to change annotation preferences for each new drawing. I have not yet found the method to retain a new set of default preferences. (Text size, arrow size, units, etc) See attached.

I have searched this forum, the web and a couple other learning resources. Everything points to the customer defaults. However, how to actually accomplish this still eludes me. While I'm sure the method must be in there, I have finally reached the point of asking for help with this issue.

Thanks in advance for helping a new NX user.

Herbert

NX 8.0
Win 7 Ultimate 64 bit

 

[cowski]

It depends on how you start the new file. If you use File -> new -> model/drawing -> [any option other than blank], you will need to open the template file that you are using and change the preferences in the file. If you are using File -> new -> model/drawing -> Blank, then you will need to modify the customer defaults as desired. File -> utilities -> customer defaults -> drawings -> drafting standards. It is possible for the CAD admin to lock down values at the group and/or site level so that individual users can't change things such as font, arrow style, etc. The most common options to lock down are those that deal with the drafting entities. If you get into the customer defaults and an option is greyed out and has a locked lock icon next to it, this means the option is locked and the change will need to be made by the CAD admin at the group or site level.

www.nxjournaling.com

 

[BABUGOUDA]

Hello,
Very Simple.You can do this by using a macro. when you need to set the annotation values to the required standards.
Procedure..
1. Open a new file
2.Tools-Macro-start record-Save macro at any location.
3 set the Required std annotation preferences
4. tools-Macro-stop record

Now you have macro file with all standard annotation Values.
so for each new drafting file you create, Please playback the macro you saved before you start dimensioning or writing text.(macro-Playback)
so now when you dimension, NX takes the standard dimensions,text etc.

Please let me know if you need any help.

Thx
BGD

 

[lbd7700]

Hi

In addition to what Cowsky said, if you are not familiar with the template files location, this can help you:

http://allyplm.com/knowledgebase/20...awing-template-and-add-to-nx-75-template-list

Regards

 

[Herbertaylor]

Excellent, thanks for your replies and guidance!

I made the macro to deal with existing drawings.

I updated the default model template so when I create a new file it already has the correct settings. I studied the Allyplm tutorial to get familiar with template location. At some point I might add new templates to the list but for now I just changed the default mm template for models. (model-plain-1-mm-template.prt)

I appreciate all the guidance. It is very helpful and I learned a lot this morning.

I have a follow up question related to the customer defaults.

The screen capture I attached to this message shows Customer Defaults > Drafting > Annotation > Lettering

This dialog does not show many of the letting settings available in Preferences > Annotation > Lettering

Your advice solved the issue I had. Now I am just wrapping my brain around better understanding of the differences between these letting dialog boxes.

NX 8.0
Win 7 Ultimate 64 bit

 

[cowski]

For the other options, you will have to go to the Drafting -> General tab then press the Customize Standard button. This will open a new dialog with many dimension style options.

www.nxjournaling.com

 

[JohnRBaker]

Why are you changing the MODELING templates to get control over what happens when you create a Drawing? You should be using the Master Model approach where the Model and the Drawing are TWO DIFFERENT part files. That way it makes NO difference whatsoever what the settings were when someone created the models, ONLY what the settings are in the Drawing template files that are used when creating your Drawings.

And for the record, THERE is a way to control which set of Drafting Standards are being used even if you're using a DRAWING template that was not created using the desired settings.

Actually there are two different things that you can do. If you don't want to go back and change every Drawing template but you've set-up your Customer Defaults to be correct, as suggested by cowski above, before creating your Drawings simply go to...

Preferences -> Drafting -> General

...and change the 'Drawing Settings' from 'Use Settings from Drawing Template' to 'Use Settings from Standard'.

Now if you've already created your Drawing but before you've not yet added any dimensions or notes, you can go to...

Tools -> Drafting Standard...

...and change it there on the fly. But note that changing the standard there will have no effect on any Drafting objects already created.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[Herbertaylor]

cowski; thanks for pointing me to the 'Customize Standard' button. That is one thing that I had not yet found.

John, thanks for your explanation. Being new to NX I was not familiar with the Master Model approach. (my previous years of CAD use were AutoCAD then VISI Progress).

In the few things I have done thus far I had been creating the 2D layout in the same file as the 3D model. Hence, my previous comment about making changes in the model template. I have been seeking out resources and information concerning best practices in NX for the Master Model method. Over the past couple weeks I have gotten this straightened out and now am getting my file structures and drafting templates properly set.

This question is fully resolved and I appreciate the advice from everyone. I now have a much better understanding of these topics. Every reply on this thread has provided me with critically useful information.

NX 8.0
Win 7 Ultimate 64 bit