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Introduction to Model Based Definition with Creo Parametric 7.0
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Creating Hole Note Annotations from Driving Dimensions

You can create your own custom hole notes by leveraging a feature’s driving dimensions and its parameters.

  • No leading zeros.

  • Tolerances on depths and diameters. Countersink depth tolerance.

  • Counterbore diameter.

  • Driving dimensions: Syntax = &d##

  • Parameters: Syntax = &:FID_###

Figure

Figure 1 - Viewing a Custom Hole Note

Figure

Figure 2 - Viewing the Dimension Names

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Figure 3 - Viewing the Feature’s Parameters

Creating Hole Note Annotations from Driving Dimensions

Figure

Figure 1 - Viewing a Custom Hole Note

Sometimes the default hole notes that the system creates do not provide the necessary information you wish to convey in a hole note. For example, perhaps you do not want the leading zeros in the dimension callout, or you want to add tolerancing information to a dimension. While you can edit the note by adding additional content to it, you cannot remove leading zeros or add tolerancing information.

You can create your own custom hole notes by leveraging a feature’s driving dimensions and its parameters. Those dimension and parameter values can be added to your own custom created note to display the following:

  • No leading zeros.

  • Tolerances on depths and diameters. Countersink depth tolerance.

  • Counterbore diameter.

You can create a planar note with a leader to the hole (a surface reference is best practice), then add dimensions and symbols per company hole note callout policy.

Viewing and Using Driving Dimension Names

Figure

Figure 2 - Viewing the Dimension Names

You can view the driving dimension names associated with each shown dimension by clicking Switch Dimensions

Figure from the Model Intent group on the Tools ribbon tab. To reference a dimension value in a note, use the following syntax:

  • &d##, where ## is the value of the dimension name. For example, if a dimension name is d31, you would type &d31 in the field to display the value for the d31 dimension in the note.

Viewing and Using Feature Parameters

Figure

Figure 3 - Viewing the Feature’s Parameters

You can view the parameters and the values specified for any feature in the model by selecting the feature, right-clicking, and selecting Parameters

Figure . The parameters assigned to that feature, and their values, display in the Parameters dialog box.

To reference a parameter value in a note, use the following syntax:

  • &:FID_###, where is the name of the parameter as it displays in the Parameter dialog box, and ### is the feature number that the parameters are assigned to. For example, if you wish to use parameter THREAD_SERIES, and that parameter is assigned to feature 200, you would type &THREAD_SERIES:FID_200 in the field to display the value for the THREAD SERIES PARAMETER in the note.

Creating Hole Note Annotations from Driving Dimensions

Close Window

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Erase Not Displayed

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Figure

MBD\Hole-Notes

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SENSOR_MOUNT_MBD_ZZ5.PRT

Steps

  • Task 1. Display a hole note’s driven dimensions. Disable all Datum Display types.

  • Click File > Options .

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

  • Type tol_display for the Option name.

  • Select yes for the Option value.

  • Click OK > OK > No .

Figure

  • In the ribbon, select the Annotate tab.

  • Select the 7D combined state tab.

  • Click Show Annotations Figure from the Manage Annotations group and select the front hole feature. Figure

  • In the graphics window, select the .375 , .313 , .850 , .750 , .625 , and .100 dimensions. Figure

  • Click OK in the Show Annotations dialog box.

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

  • From the In Graphics toolbar, select No Hidden Figure from the Display Style types drop-down menu. Figure

  • Task 2. Edit the tolerance of a dimension. In the graphics window, select the .100 dimension.

  • In the Dimension tab, click Tolerance and select Plus-Minus Figure . Verify the Upper tolerance as +0.005 .

  • Verify the Lower tolerance as -0.005 .

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

  • Task 3. View the shown dimension IDs and hole feature parameter values. In the ribbon, select the Tools tab.

  • Click Switch Dimensions Figure from the Model Intent group.

  • Note the dimension symbol numbers for each of the hole’s dimensions. Figure

  • Select the hole feature edge from the graphics window, right-click, and select Parameters Figure .

  • In the Parameters dialog box, note that the hole feature is feature id 319 .

  • Note also the different parameter names and the corresponding values for this feature. Figure

  • Click OK .

  • Task 4. Create the note using parameters and driving dimensions. Select the Annotate tab.

  • Click LEFT Figure from the Annotation planes group. Figure

  • Select Leader Note Figure from the Note types drop-down menu in the Annotations group.

  • Select the inner counterbore surface. Figure

  • Middle-click the location shown to place the note.

  • In the Note field, type the following lines: &d98 &THREAD_SERIES:FID_319 - &CLASS:FID_319

  • &d102 DRILL &d105 TAP &d100

  • &d104 &d101

  • X2 HOLES

  • Using the symbols in the Text group, insert the depth and countersink symbols where needed.

  • Click in the background to complete text entry.

  • Click in the background to complete the note. Figure

  • Select the Tools tab.

  • Click Switch Dimensions Figure . Figure

  • Select the Annotate tab.

  • In the detail tree, select DRV_DIM_D98 , press SHIFT, and select DRV_DIM_D105 .

  • Click Remove from State Figure from the mini toolbar.

  • From the In Graphics toolbar, select Shading Figure from the Display Style types drop-down menu.

  • In the graphics window, select the note and move it approximately as shown.

  • Click in the background to de-select the note. Figure