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Introduction to Model Based Definition with Creo Parametric 7.0
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Manipulating Dimension Annotations

You can manipulate dimensions in annotation elements and features.

  • Manipulations include: Move/Drag dimensions Alignment guides

  • Text style

  • Edit dimension value Driving dimensions only

  • Show/Edit tolerance values

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Figure 1 - Viewing Alignment Guides

Figure

Figure 2 - Viewing Modified Text Style

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Figure 3 - Viewing Tolerance Values

Manipulating Dimension Annotations

Figure

Figure 1 - Viewing Alignment Guides

Figure

Figure 2 - Viewing Modified Text Style

Figure

Figure 3 - Viewing Tolerance Values You can manipulate dimensions in annotation elements and features.

  • Move or drag dimensions: Select a dimension and move it to a different location. When you cursor over various parts of the selected dimension, the cursor updates to display the type of movements you can make. Cursor over the dimension text and drag to move both the dimension and dimension text. Cursor over the dimension leader line and drag to move just the dimension.

  • You can snap dimension text to be centered around its arrows. The system displays alignment guides for centered dimensions.

  • You can also snap dimensions to other dimensions. When a dimension line intersects with another dimension line, the system also displays alignment guides.

  • Text style: You can change how the dimension text displays in the graphics window. To edit the text display, select a dimension or dimensions and select the Format tab in the ribbon. You can also right-click and select Text Style Figure . The Text Style dialog box displays, enabling you to edit various aspects of the dimension text, including: Height — Clear the Default check box and specify a different height value to increase or decrease the dimension text height.

  • Thickness — Clear the Default check box and specify a different text thickness value.

  • Slant Angle — Specify a slant angle value in degrees.

  • Color — Specify a different color from the default.

  • Edit dimension values: Select a driving dimension and edit its value in the Value group of the Dimension tabClick Regenerate Figure to update the model geometry based on the new value. You can only edit the dimension values of driving dimensions.

  • Show and edit tolerance values: You can display dimension tolerances in the graphics window by editing the Tolerance mode from Nominal to Limits , Plus-Minus , or +- Symmetric .

  • Edit tolerance values either by editing the Upper Tolerance and Lower Tolerance values in the Tolerance group of the Dimension tab or by selecting a driving dimension, right-clicking, and selecting Parameters Figure . Edit the upper and lower bound values as desired.

Manipulating Dimension Annotations

Close Window

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Erase Not Displayed

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Figure

MBD\Dimensions_Manipulate

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SENSOR-MOUNT_MOD-DIMS3.PRT

Steps

  • Task 1. Drag a dimension. Disable all Datum Display types.

  • In the ribbon, select the Annotate tab. Select the 7A combined state tab.

  • Select the 4.650 dimension. Cursor over the dimension leader line and drag to move both the dimension and text, left or right only.

Figure

  • Cursor over the dimension text and drag to move both the dimension and text. Drag the dimension up until it aligns to the center.

  • Notice the phantom alignment guides that display when text is centered between the extension lines.

Figure

  • Select the 2.210 dimension. Cursor over the dimension text and drag to move the dimension up until it aligns to the center.

  • Drag the dimension to the right slightly.

  • Select the 1.250 dimension. Drag the dimension up and to the right until it aligns with the 2.210 dimension and is centered.

  • Again, notice the alignment guides.

Figure

  • Click in the background to de-select all dimensions.

  • Task 2. Modify the text style of a dimension. Select the 4.650 dimension. Right-click and select Text Style Figure .

  • In the Text Style dialog box, clear the Height Default check box. Edit the Height to 0.4 .

  • Click Apply .

Figure

  • Edit the Slant Angle to 15 . Select the Underline check box.

  • Click OK .

  • Click in the background to de-select all dimensions. Figure

  • Task 3. Edit a dimension value. Select the 2.210 dimension. Notice the Format and Dimension tabs appear in the ribbon.

The 2.210 value is grayed out in the Value group because it is a driven dimension, so its value cannot be modified.

  • Select the 4.650 dimension.

  • Edit its value to 4.75 and click Regenerate Figure from the Quick Access toolbar. Figure

  • Click Undo Figure from the Quick Access toolbar.

  • Task 4. Display tolerance values and edit their limits. Click File > Options .

  • In the Creo Parametric Options dialog box, select the Configuration Editor category and click Add .

  • In the Options dialog box, type tol_display as the Option name. Edit the Option value to yes .

  • Click OK > OK .

  • Click No , if necessary.

  • Select the 4.650 dimension. In the Tolerance group, select Limits Figure from the Tolerance types drop-down menu.

  • Notice the dimension updates in the graphics window to display limits instead of nominal.

Figure

  • Select Plus-Minus Figure from the Tolerance types drop-down menu. Figure

  • With the dimension still selected, right-click and select Parameters Figure . In the Parameters dialog box, edit the PTC_DIM_UPPER_TOL_VALUE to 0.005 .

  • Edit the PTC_DIM_LOWER_TOL_VALUE to 0.003 .

  • Click OK . Notice the tolerance value limits update in the graphics window.

Figure