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Introduction to Model Based Definition with Creo Parametric 7.0
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Creating Driving Dimension Annotations

You can display existing dimensions that are driving geometry as annotations.

  • Orientation Model

  • Annotation plane

  • Show Annotations From model

  • From tree

  • Cleanup Reorient

  • Move to Plane

  • Update

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Figure 1 - Showing Dimensions

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Figure 2 - Selecting Dimensions

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Figure 3 - Dimensions Cleaned

Creating Driving Dimension Annotations

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Figure 1 - Showing Dimensions

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Figure 2 - Selecting Dimensions

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Figure 3 - Dimensions Cleaned You can display existing dimensions that are driving geometry, which creates Annotation elements. The following process is used to create driving dimension annotation elements:

  • Orientation Orient the model and select, edit, or create an annotation plane.

  • Driving dimensions are created from the 3-D model dimensions. Plan how you want the dimensions to appear as the model is oriented or —posed.— The system will try to display as many dimensions as possible, given the current view orientation and model position.

Driving dimension annotation elements will not be created for dimensions that are normal to the active annotation orientation direction.

  • Show Annotations You can click Show Annotations Figure and then select features from the model or model tree. You can also select features from the model tree first, then right-click and select Show Annotations Figure .

  • Once the system displays the driving dimensions in dark red, you can select desired dimensions from the graphics window or from the dialog box. Once selected, they will change color to blue. Remember to select those items you want displayed in the current combined state.

  • Cleanup Once all of the dimensions have been added to a combined state, re-orient/pan/zoom the model to display as many dimensions as clearly as possible. This is often referred to as —posing — the model.

  • Annotations can be edited to other orientations and reading directions. Select the dimensions to edit, then right-click and select Current Orientation to open the Annotation Plane dialog box.

  • Use the option Select Existing Annotation to quickly align with other annotations in the same view. (This is the fastest way to set many items in the same orientation.) View the topic Modifying Dimension Annotation Display for more detailed information.

  • You can also select a dimension or dimensions, then right-click and select Move to Plane Figure to place it on a different plane.

  • Update Once dimensions are cleaned up, and the model is placed into an ideal pose or orientation, click Update Figure to save the changes to the current combined state.

Dimensions that are shown and created as annotations appear in the detail tree, and in the model tree beneath the feature they originated from. Enable the Annotation model tree filter to view the created annotations. Once created, you can select the dimension annotations from the detail tree, model tree, or graphics window. You can then right-click and perform editing or display operations.

Creating Chamfer Driving Dimensions

Chamfers may require special attention to dimension as desired. When using driving dimension annotation elements, the chamfer dimension may appear as a single value with a leader, depending on which dimension scheme was chosen when the chamfer was modeled. The displayed value defines the offset from the previous corner. To display two dimensions, you may need to create driven dimensions for each offset edge.

Creating Driving Dimension Annotations

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Erase Not Displayed

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MBD\Dimensions_Driving

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SENSOR-MOUNT_DRIVING.PRT

Steps

  • Task 1. Create driving dimension annotations. Disable all Datum Display types.

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

  • Orient the model as shown.

  • In the Annotation Planes group, cursor over TOP Figure . Right-click and select Edit .

  • Select 180 from the Text Rotation drop-down list.

  • Click OK .

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The annotation plane orientation is used for newly created annotations. Displayed annotations appear in the orientation in which they were originally created, but can be reoriented to match the current annotation plane direction.

  • Click Show Annotations Figure from the Manage Annotations group. Select Extrude 6 from the model.

  • Notice the dimensions that appear on the model.

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  • Select SENSOR-MOUNT_DRIVING.PRT from the model tree. Notice the dimensions that appear.

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  • Select Extrude 1 from the model tree. Select the 3.000 dimension from the model.

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  • Select the d3 Show check box from the Show Annotations dialog box. Click OK .

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  • Reorient the model as shown. Select and drag the dimensions as necessary.

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  • Click Show Annotations Figure . Select Extrude 4 from the model tree.

  • Select the d15 Show check box.

  • Click OK .

  • Reorient the model as shown. Notice that all of the dimensions are not easily readable from the same orientation.

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  • Expand feature Extrude 1 in the model tree.

  • At the top of the model tree, click Settings Figure and select Tree Filters Figure . Select the Annotations check box.

  • Click OK .

  • Notice the annotations appear in the detail tree and under Extrude 1.

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  • Task 2. Reorient dimensions. Reorient the model and drag the dimensions as shown. Figure

  • Select the 4.592 dimension. Right-click and select Move to Plane Figure .

  • Select datum plane G from the model tree.

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  • Cursor over TOP Figure to recall the preferred viewing direction. Select the 3.000 dimension.

  • Right-click and select Current Orientation .

  • Select 180 from the Text Rotation drop-down list.

  • Click OK .

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  • Select the R2.500 dimension. Right-click and select Current Orientation .

  • Click Select Existing Annotation from the Annotation Plane dialog box.

  • Select the 3.000 dimension.

  • Click OK .

  • Reposition the radius dimension as shown.

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

  • Click Update Figure from the Combination States group.

  • Task 3. Create a driving dimension for a chamfer. Select the 7B combined state tab. Click TOP Figure .

  • Orient the model as shown.

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  • Click Show Annotations Figure .

  • Select the chamfer shown. Figure

  • Select the .200 dimension. Click OK .

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  • Select the .200 dimension. Right-click and select Move to Plane Figure .

  • Select the bottom model surface.

  • Click Update Figure .

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  • Task 4. Review the updated combined states. Select the 7A combined state tab. Figure

  • Select the 7B combined state tab. Figure