Hole Table functionality without the Mold Wizard license

Here's one reason to consider upgrading to NX6.0.3.

You can now insert a hole table just like the mold-wizard-people do by setting the following environment variable :

UGII_DRAFTING_HOLE_TABLE = 1

Change sketch dimensions in Drafting

NX methodology normally suggests that your drafting, toolpaths, CAE model etc all depend on your 3D model, so the changes should propogate from 3D model to the rest. (thus the name master and non-master parts)

What it means, is that if you change a drafting dimension of a line from 50 to 55 mm in drafting , you'll only get a warning that the associativity between the dimension and the geometry will be lost, and your line length will remain unchanged.

Normally this really is not a problem in NX, as switching between applications like modeling and drafting is quite easy. But if you are switching to NX from another CAD application, you might want to try this approach :

• set UGII_DRAFT_EXPRESSIONS_OK = 1
• create a sketch
• create a view of the model in drafting
• select Insert -> Feature Parameters command, and place the sketch dimensions into your view
• Hit CTRL + E (expressions) and select a dimension of the sketch. You'll be able to modify and update without having to go back to modeling.

Duplicating a drawing sheet

It amazes me how flexible import and export part commands can sometimes be. Here's a way to duplicate your drawing sheet within your work part.

• Save your part
• Launch `File - Export - Part`.
  
• Select Part Specification : Existing
• Select "Specify Part" and choose your workpart from your list.

Your current sheet should be duplicated quickly.

Ignore some components in a Parts List

In order to prevent a component or a subassembly from appearing in a Parts List, there are two poorly documented attributes:

• PLIST_IGNORE_MEMBER
• PLIST_IGNORE_SUBASSEMBLY

I guess the names tell which is which. Defining one of these in the component properties - attributes window is just enough.

Parametric Sheet Templates

For a smarter sheet template solution, a tabular note cell can be populated with the following data in NX5: (You must add "<" and ">" around the variables)

1. Number of the current sheet: W@$SH_SHEET_NUMBER
2. Total number of sheets: W@$SH_NUMBER_OF_SHEETS
3. Numerator of the sheet scale: W@$SH_SHEET_SCALE_NUMERATOR
4. Denominator of the sheet scale: W@$SH_SHEET_SCALE_DENOMINATOR
5. Size of the current sheet: W@$SH_SHEET_SIZE
6. Units of the current sheet: W@$SH_SHEET_UNITS
7. Projection angle of the current sheet: W@$SH_SHEET_PROJECTION_ANGLE
8. Master Model drawing sheet part name: W@$SH_MASTER_PART_NAME
9. Sheet part name: W@$SH_PART_NAME

These items are from a post in BBSNotes by John Baker. If you'd like make an addition to the list, you're more than welcome to do so thru comments.

Truetype fonts in NX Drafting

Got bored with the old drafting fonts like latin_extended ?

Here are some ready-to-use .fnx drafting fonts, converted from

• Verdana
• Tahoma
• Times New Roman
• Segoe UI
• Trebuchet MS

Download them here, and copy the .fnx files to the UGII\ugfonts folder.

Out of the box drafting standards

An NX5 standard installation includes out of the box drafting settings for ASME, DIN, ISO and JIS standards. To activate these settings,

1. Open your Customer Settings by Tools - Utilities - Customer Defaults (be sure that your active user role includes this command. If not, you can always set one of the 'advanced' roles)
2. Go to Drafting - General
   
3. Select the Standard tab
   
4. Choose the standard of your choosing. You can also customize the existing standards.
   
5. As with all customer defaults changes, restart your NX session.