Siemens NX – Suppress, Unsuppress Drafting Objects

Application: Drafting.

Command: Suppress Drafting Object.

With the help of command ‘Suppress Drafting Object’, you can control the visibility of the following drafting objects.

  1. Dimensions
  2. Drafting aids
  3. Geometric Dimension and Tolerancing (GD&T) objects
  4. Tabular notes, Parts List etc.

First, define the ‘Control Expression’ with type ‘Number’ which is used to control the visibility of the selected drafting objects.

Control expression can have zero or a nonzero value.

If Control Expression = 0 (Zero value) – Selected Drafting objects becomes invisible.

If Control Expression = 1 (Any nonzero value) – Selected Drafting objects remains visible.

By default, Expression editor (Menu > Tools > Expressions ) is not available in Drafting application.

To change the value of the control expression, either you have to switch to the modeling application to access expressions dialog/editor or you can enable it in the drafting application by setting the ‘Allow Expressions’ option in the Customer Defaults.

File > Utilities > Customer Defaults > Drafting > General/Setup > Miscellaneous tab > Toggle on ‘Allow Expressions’

Enable ‘Allow Expressions’.

Define an expression with type as a number.Example: DRAFT_OBJ_DISPLAY = 1

In drafting application, Go to Menu > Edit > Suppress Drafting Object

Click on ‘Expression’ > Select the expression ‘DRAFT_OBJ_DISPLAY’ > OK

Select the required drafting objects (Dimensions/Balloons/Parts List etc.) whose visibility need to control by the expression and click on OK button of the dialog ‘Suppress Drafting Object’. This will link the drafting objects with the selected expression.

Now, Open the expressions editor – ‘Menu > Tools > Expressions’ or ‘Ctrl+E’. Change value of the expression ‘DRAFT_OBJ_DISPLAY’ to ‘0’ (zero). Selected drafting objects become invisible within that particular drawing sheet.

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