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

You can create new dimensions as annotations that are driven by geometry.

  • Orientation Model

  • Annotation plane

  • Annotation type icon

  • Attachment type

  • Place annotation

  • Display options

  • Cleanup Move to Plane

  • Update

Figure

Figure 1 - Selecting References

Figure

Figure 2 - Placing Dimension

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Figure 3 - Dimensions Moved to Planes

Creating Driven Dimension Annotations

Figure

Figure 1 - Selecting References

Figure

Figure 2 - Placing Dimension

Figure

Figure 3 - Dimensions Moved to Planes Create new dimensions as annotations that are driven by the geometry, specifically the selected geometric entities that define the ends of the dimension.

Typically, the dimension annotation elements are grouped together within the various combined states. The system displays the created annotation features in the detail tree and in the model tree Annotations node (annotations must be enabled in the model tree filters). Once they are 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.

The following process is used to create driven dimension annotation elements:

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

  • Similar to a 2-D drawing, plan which views should contain the appropriate dimensions and how you want the dimensions to appear as the model is oriented or —posed.—

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

  • Annotation type Select the appropriate annotation type from the icons in the Annotations group. For example, click Dimension Figure . You can also click the Annotations group drop-down menu and select Reference Dimension Figure . These dimensions are typically not to be inspected.

  • Attachment type Select the appropriate attachment type for the geometry to be selected to create the dimension. You can mix and match options for each end of a dimension. The following options are available: Select Entity Figure

  • Select Surface Figure

  • Select Reference Figure

  • Select Tangent Figure

  • Select Midpoint Figure

  • Select Intersection Figure

  • Best practices recommend that surface references are the most robust and are not likely to vanish if the model changes; thus the dimension will always remain. Furthermore, surface references can be consumed by metrology programs to streamline the inspection process and reduce duplication of work.

  • The first reference selected defines the Z depth of the dimension. The dimension will lie in an X-Y plane defined by the currently selected Annotation Orientation plane from the gallery.

  • Place annotation Once references are selected, locate the cursor in the desired location and middle-click to place the dimension text.

  • The dimension text, leaders, and extension lines are created on the plane of the first selection. A dashed offset line is created to display the extent of the Z depth from the end of the extension line to the second geometric reference.

  • Once the dimensions are placed, the Dimension tab displays in the ribbon with all the available display options, based on the reference specified. The orientations refer to the current annotation orientation, with the horizontal matching the blue arrow direction for the annotation plane. To change orientation, click Orientation from the Display group and select one of the following: Horizontal Figure

  • Vertical Figure

  • Slanted Figure

  • Parallel To Figure

  • Perpendicular To Figure

If you specified an arc reference, you can choose any of the following arc attachment options in the Display group:

  • Min Figure

  • Max Figure

  • Center Figure

  • Cleanup Once all the dimensions have been added to a combined state, reorient/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 enter 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.

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

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

Creating Driven Dimension Annotations

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MBD\Dimensions_Driven

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SENSOR_MOUNT_DRIVEN.PRT

Steps

  • Task 1. Create driven dimensions using On Surface references. Disable all Datum Display types.

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

  • Click OK .

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

  • Orient the model as shown. Figure

  • Click LEFT Figure from the Annotation Planes group. Click Dimension Figure from the Annotations group.

  • In the Select Reference dialog box, select Select Surface Figure from the Select types drop-down menu.

  • Press CTRL and select the surface locations as shown.

Figure

  • Locate the cursor where shown and middle-click to place the dimension. Figure

  • Click in the background to de-select the dimension.

  • Click TOP Figure from the Annotation Planes group. Press CTRL and select the surface locations as shown.

Figure

  • Locate the cursor where shown and middle-click to place the dimension. Figure

  • Click in the background to de-select the dimension.

  • Click LEFT Figure from the Annotation Planes group. Press CTRL and select the surface locations as shown.

Figure

  • Locate the cursor where shown and middle-click to place the dimension. Drag the dimension as necessary.

Figure

  • Click Cancel from the Select Reference dialog box.

  • Task 2. Clean up dimensions and pose the model. Select the 2.21 dimension. Right-click and select Move to Plane Figure .

  • Select the planar surface shown.

Figure

  • Select the 1.25 dimension. Right-click and select Move to Plane Figure .

  • Select the planar surface shown.

Figure

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

  • Click Update Figure from the Combination States group.

Figure

  • Select the 2.21 dimension.

  • Click References Figure from the References group.

  • In the References dialog box, click in the First Dimension Reference collector to activate it.

  • Press CTRL and select the other surface shown. Figure

  • Select the Second Dimension Reference Origin check box.

  • Click OK .

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

  • Task 3. Create driven dimensions using Center references. Select the 7B combined state tab. Orient the model as shown.

Figure

  • Click TOP Figure . Click Dimension Figure .

  • In the Select Reference dialog box, click Select Entity Figure .

  • Press CTRL and select the edges of the holes shown.

Figure

  • Locate the cursor where shown and middle-click to place the dimension. In the Display group, verify the arc attachments are Center Figure for both references.

Figure

  • Click in the background to de-select the dimension.

  • Task 4. Create driven dimensions using On Entity references. Verify TOP Figure is still selected. Press CTRL and select the edge and vertex of the hole shown.

Figure

  • Locate the cursor where shown and middle-click to place the dimension. In the Display group, click Orientation and select Vertical Figure .

  • Edit the arc attachment to Min Figure .

  • Drag the .25 dimension where shown.

Figure

  • Click Cancel from the Select Reference dialog box.

  • Select the .25 dimension and then click Flip Arrows Figure from the mini toolbar.

  • Move and clean up the dimensions as necessary. Figure

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

  • Task 5. Create driven dimensions using Offset references. Verify TOP Figure is still selected. Reorient the model as shown.

  • Click Dimension Figure . Select the top edge shown.

  • Press CTRL and select the edge of the hole shown.

Figure

  • Locate the cursor where shown and middle-click to place the dimension. Figure

  • In the Display group, verify the arc attachment reference is Center Figure .

  • Reorient the model as shown.

  • Press CTRL and select the edges of the holes shown. Figure

  • Locate the cursor where shown and middle-click to place the dimension. Click Orientation and select Vertical Figure .

  • In the Display group, verify the arc attachment references are Center Figure .

  • Click Cancel from the Select Reference dialog box.

Figure

  • Reorient the model as shown. Select the 1.89 dimension.

  • Right-click and select Move to Plane Figure .

  • Select the planar surface shown.

  • Notice the dashed Z-extension lines.

Figure

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

  • Click Update Figure .

Figure

  • Task 6. Create driven dimensions for holes. Select the 7D combined state tab. Orient the model as shown.

  • Click ANGLE Figure from the Annotation Planes group.

Figure

  • Click Dimension Figure . Select Select Surface Figure .

  • Select the upper hole surface once to generate a radius dimension.

Figure

  • Locate the cursor where shown and middle-click to place the dimension. Figure

  • Select the lower hole surface twice to generate a diameter dimension. Figure

  • Locate the cursor where shown and middle-click to place the dimension. Click Cancel .

Figure

  • Press CTRL and select both dimensions. Right-click and select Move to Plane Figure .

  • Select the surface shown.

  • Click Update Figure .

Figure

  • Task 7. Create driven dimensions for chamfers. Select the 7C combined state tab. Orient the model as shown.

  • Click TOP Figure .

Figure

  • Click Dimension Figure . In the Select Reference dialog box, click Select Intersection Figure .

  • Press CTRL and select the edge of the chamfer and the edge of the wall.

Figure

  • Select Select Entity Figure . Press CTRL and select the other edge of the wall.

Figure

  • Locate the cursor where shown and middle-click to place the dimension. Figure

  • Repeat the previous steps for the other side of the chamfer. Click Cancel .

  • Drag the dimensions as necessary.

  • Click Update Figure .

Figure