How to Use the Modify Dimension Dialog Box in Pro/ENGINEER Wildfire 3.0
Pro/ENGINEER allows for many aspects of a dimension to be modified at once. This tip explores how to how you can use the Modify Dimension Dialog Box to achieve this.
- To begin the modification of a dimension, select the dimension, and then click Edit > Properties.
- The DIMENSION PROPERTIES dialog box will appear (Figure 1a). From this dialog box, the tolerance limits, dimension format, number of digits, dual dimensioning, geometric tolerances, and additional dimension text can be modified for the selected dimension(s) at one time.
- The tolerance mode and dual dimensioning options will only be made available after setting the drawing setup file options "tol_display" to "yes" and "dual_dimensioning" to a valid option other than "no"
- Cancel can be clicked at any time to exit the dialog box without saving the modifications
- Click Restore Values to undo modifications which have changed the value of the dimension
- To change the Tolerance Mode for all the selected dimensions at once, simply select one of the options from the Tolerance Mode pull-down menu, as in the example shown in Figure 1b. The Tolerance Mode set to (As Is) will keep the dimension(s) in the original format prior to performing the modifications.
- If the dimension is an angular dimension (Figure 2a), its angular format may be modified independently of other angular dimensions
Note: Prior to Release 2000i2, the drawing setup file option "draw_ang_units" controlled the format of every angular dimension on the drawing.
The Dimension Text
tab can be clicked to allow for adding additional lines of text as well as adding Prefixes
to all of the selected dimensions (Figure 3a
). This can be performed here instead of modifying the text of each individual dimension separately (Figure 3b
- When modifying a single dimension, the options Move..., Move Text..., and Edit Attach... become available for operations on that dimension (Figure 4a)
- At any time during the dimension modification, the Symbol Palette window can be utilized by clicking Text Symbol.... The graphical interface for the palette window is shown in Figure 4b
- The Text Style tab of the MODIFY DIMENSION dialog box is used to modify the appearance of the dimension text (Figure 5a)
- Properties such as font, text height and color may be modified (Figure 5b)
- After editing any of the options in the MODIFY DIMENSION dialog box, the dimension(s) will concurrently update in the drawing. This allows for further dimension modification without having to leave the dialog box and then start a new dimension modification process on the same dimension(s).
- To complete the dimension modification process, click OK
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