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Introduction to Model Based Definition with Creo Parametric 7.0
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Creating Geometric Tolerance Annotations

The feature control frame is displayed on the model and automatically updates as you configure the tolerance.

  • Combined states 5_Datums, 7A, 7B, 7C, and so on

  • Semantic referencing to datum feature symbols.

  • Syntax checking.

  • Various editing and symbol options.

Figure

Figure 1 - Geometric Tolerances with Leaders

Figure

Figure 2 - Geometric Tolerance in a Dimension

Creating Geometric Tolerance Annotations

Figure

Figure 1 - Geometric Tolerances with Leaders

Figure

Figure 2 - Geometric Tolerance in a Dimension Geometric tolerances can be created in the 5_Datums combination state or any of the 7-series combined states. When creating geometric tolerances, the feature control frame is displayed on the model and automatically updates as you configure the tolerance. This enables you to check the configuration as you make adjustments, if necessary. The steps involved in creating geometric tolerances include:

  • Specifying the type of geometric tolerance to insert; for example, Position.

  • Using the Geometric Tolerance tab to configure the following elements: Specify the dimension or reference entity to which you add the geometric tolerance, as well as place the geometric tolerance on the model.

  • Specify the datum references and material conditions for the datum references.

  • Specify the tolerance value and the material condition.

  • Specify the geometric tolerance’s symbols and modifiers, as well as the projected tolerance zone.

  • Specify additional text that you want associated with a geometric tolerance while creating or editing it.

Editing a Geometric Tolerance

You can easily edit a geometric tolerance by selecting it. A context-sensitive ribbon tab opens on selection, enabling you to edit the geometric tolerance. The ribbon tab closes on de-selection of the geometric tolerance.

You can always edit the geometric tolerance reference location by selecting the gtol, right-clicking, and then selecting Change Reference. You can then select a different reference to re-place the feature control frame leader line and arrow.

Using Semantic References

When creating a geometric tolerance, if you reference an existing datum feature symbol for the primary, secondary, or tertiary datums, the system establishes a semantic reference between the two, and the label turns green in the field. If you change the datum feature symbol label, the datum label automatically updates in the feature control frame when the model is regenerated.

Syntax Checking

As you fill out the geometric tolerance’s feature control frame, the system automatically checks the syntax to conform to the ASME Y14.5 standard. If you enter a character or symbol in a location that violates the standard, the system displays a caption to let you know, and also displays a red —spell checker — line underneath the incorrectly specified character or symbol.

Additional Editing Options

The following editing options are available for a geometric tolerance:

  • Composite frame — Add multiple rows to the base geometric tolerance.

  • Indicators frames — Add additional Indicators frames to the geometric tolerance, including: Direction Feature, Collection Plane, Intersection Plane, and Orientation Plane.

  • Modifiers — Add additional modifiers to the geometric tolerance, including All Over, All Around, Unilateral, and Boundary.

  • Additional Text — Add additional text to any of four areas around the outside of the feature control frame.

  • Arrow Style

  • Symbols — Add symbols to many areas of the feature control frame by placing the cursor in the desired location and clicking from the context-sensitive tab in the ribbon. A comprehensive set of both ASME and ISO symbols displays. You can then select the desired symbol, and it is added to the field where your cursor is placed. The system dynamically checks the syntax to verify that it meets the standards.

Creating Geometric Tolerance Annotations

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Erase Not Displayed

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Figure

MBD\Geom-Tol

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SENSOR-MOUNT_GEOM-TOL.PRT

Steps

  • Task 1. Create a standalone geometric tolerance for angularity. Disable all Datum Display types.

  • In the ribbon, select the Annotate tab.

  • Select the 5_Datums combined state tab. Figure

  • Click LEFT Figure from the Annotation Planes group.

  • Click Geometric Tolerance Figure from the Annotations group. Select the angled surface shown.

  • Drag the cursor up and middle-click to place the geometric tolerance.

Figure

  • In the ribbon, click Geometric Characteristic and select Angularity Figure . Notice that datum A is already specified in the primary datum field.

Figure

Notice that a semantic reference has been established between the geometric tolerance and the datum feature symbol.

  • In the Tolerance & Datum group, edit the tolerance value to 0.05 , if necessary, and press ENTER.

  • Click in the background to de-select the completed geometric tolerance. Figure

  • Task 2. Create a standalone geometric tolerance for perpendicularity. Click Geometric Tolerance Figure . Select a location on the top surface for the leader.

  • Drag the cursor up and middle-click to place the geometric tolerance.

Figure

  • Click Geometric Characteristic and select Perpendicularity Figure In the Tolerance & Datum group, edit the tolerance value to 0.02 and press ENTER.

  • Click in the primary datum field, delete any existing datum reference, and press ENTER.

  • Click Select Datum Reference Figure next to the primary datum field, select datum feature symbol C , and click OK .

  • Click in the secondary datum field, type B , and press ENTER.

Figure

  • Place the cursor at the end of the specified tolerance value.

  • Click Symbols Figure from the Symbols group. Select the Statistical tolerance symbol.

Figure

  • Click Additional Text Figure from the ribbon.

  • Click in the field above the feature control frame and type 2 SURFACES .

  • Click in the background to de-select the completed geometric tolerance. Figure

  • Task 3. Create a geometric tolerance within a dimension. Select the 7B combined state tab. Figure

  • Click TOP Figure from the Annotation Planes group.

  • Click Geometric Tolerance Figure . Select the .50 diameter dimension.

Figure

  • The geometric tolerance is automatically added to the dimension.

  • Click Additional Text Figure and delete the text from the field above the feature control frame. Figure

  • Click Additional Text Figure again to collapse it in the ribbon.

  • Click Geometric Characteristic and select Position Figure . In the Tolerance & Datum group, edit the tolerance value to 0.001 and press ENTER, making sure to also delete the statistical tolerance symbol.

  • Click in the primary datum field, type A , and press ENTER.

  • Click in the secondary datum field, type B , and press ENTER.

  • Click in the tertiary datum field, type C , and press ENTER.

Figure

  • Place the cursor at the end of the specified tolerance value.

  • Click Symbols Figure from the Symbols group. Select the Maximum Material Clearance symbol.

  • Place the cursor at the beginning of the specified tolerance value.

  • Select the Diameter symbol.

Figure

  • Click References Figure from the References group.

  • Reorient the model, press CTRL, and select the three cylindrical surfaces shown. Figure

  • Click OK from the References dialog box.

  • Click in the background to de-select the completed geometric tolerance.