To Create an Annotation Feature
This topic describes the general procedure of creating an Annotation feature.
1. Define the active annotation orientation before creating the first annotation in any session.
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If you skip step 1, then Creo Parametric uses the default active annotation orientation. However, if you have previously created annotations then Creo Parametric uses the same annotation orientation as the previously created annotation.
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2. Click > 
Annotation Feature. The ANNOTATION FEATURE dialog box opens with the Definition tab active.
Annotation Feature. The ANNOTATION FEATURE dialog box opens with the Definition tab active.3. Select one of the following annotation types:
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— Create a driven dimension with tolerance to include in the Annotation Element.
— Create a driven dimension with tolerance to include in the Annotation Element.◦ 
— Create a reference dimension to include in the Annotation Element.
— Create a reference dimension to include in the Annotation Element.◦ 
— Create an ordinate baseline dimension.
— Create an ordinate baseline dimension.◦ 
— Create one or more ordinate driven dimensions to include in the Annotation Element.
— Create one or more ordinate driven dimensions to include in the Annotation Element.◦ 
— Create one or more ordinate reference dimensions to include in the Annotation Element.
— Create one or more ordinate reference dimensions to include in the Annotation Element.◦ 
— Create a geometric tolerance to include in the Annotation Element.
— Create a geometric tolerance to include in the Annotation Element.◦ 
— Create a Datum Feature symbol to include in the Annotation Element.
— Create a Datum Feature symbol to include in the Annotation Element.◦ 
— Create a surface finish to include in the Annotation Element.
— Create a surface finish to include in the Annotation Element.◦ 
—Set manufacturing information for the part to include in the Annotation Element. For more information, refer to documentation on Sheetmetal Forms.
—Set manufacturing information for the part to include in the Annotation Element. For more information, refer to documentation on Sheetmetal Forms.◦ 
— Select a previously saved manufacturing template to include in the Annotation Element. For more information, refer to documentation on NC Manufacturing.
— Select a previously saved manufacturing template to include in the Annotation Element. For more information, refer to documentation on NC Manufacturing.◦ 
— Create a note to include in the Annotation Element. You can create an unattached note, on item note, tangent leader note, normal leader note, and leader note.
— Create a note to include in the Annotation Element. You can create an unattached note, on item note, tangent leader note, normal leader note, and leader note.◦ 
— Create a symbol to include in the Annotation Element.
— Create a symbol to include in the Annotation Element.◦ 
— The Annotation Element does not contain an annotation.
— The Annotation Element does not contain an annotation.◦ 
— Select an existing annotation item (such as a note, symbol, and so on) to include in the Annotation Element. You can also select an existing Annotation Element to include a copy of its annotation item in the current Annotation Element.
— Select an existing annotation item (such as a note, symbol, and so on) to include in the Annotation Element. You can also select an existing Annotation Element to include a copy of its annotation item in the current Annotation Element.Creo Parametric invokes the user interface for creating or selecting the annotation item. For more information on creating an annotation of a particular type, follow the See Also links.
| | • If you want to change the active annotation orientation for the annotation you are about to create then click > or click Active Orientation on the shortcut menu that opens when you right-click in the user interface for creating the annotation item. • After you place the annotation you can change the current annotation orientation by clicking Current Orientation on the shortcut menu that opens when you right-click in the user interface for creating the annotation item. |
After you create or select the annotation item, Creo Parametric creates the Annotation Element, adds its name, type, orientation, and copy flag to the elements list in the ANNOTATION FEATURE dialog box, and adds the references, along with the reference type and default reference description, to the References collector.
4. Click Parameters to specify the Annotation Element parameters.
5. You can click Edit to edit the definition of the annotation item included in the selected Annotation Element, or click Remove to delete the selected Annotation Element from the Annotation feature.
6. You can click Columns to customize the columns in the Annotation Elements list and the References list. In the Annotation Columns dialog box that opens when you click Columns, select the list that you want to customize from the Type list and move the names of the columns that you want to view in the list to the Displayed box. You can also specify the width of the column.
7. You can change the orientation of the annotation by clicking Current Orientation on the shortcut menu that appears when you right-click the annotation in the Annotation Elements list.
| | The Current Orientation command is not available for non-graphical Annotation Elements. |
8. To add additional references to the Annotation Element, click References, Surface, or Chain to activate the respective collector and select the valid entities for the specified collector.
9. In the Strong column, if the check box next to the reference name is not selected, then the reference type is Weak. If you want to change the reference type to Strong, select the check box.
| | If you have selected datum points as references, then a check box in the Auto-Propag column is also available for the datum points in the References collector. Select the check box to enable automatic propagation of datum points. If you propagate the Annotation Element to data sharing features, then those datum point references for which you have selected the check box in the Auto-Propag column are also automatically propagated. |
10. In the Reference Description column, if you want to edit the default description of the reference or add a new description, select the description corresponding to the reference name and type the new description.
| | The description should not exceed 32 characters. |
11. You can replace an annotation reference by clicking Replace on the shortcut menu that appears when you right-click the annotation reference in the References list and selecting a new reference entity of a similar type.
| | You cannot replace references that are added after the annotation is created. However, you can remove the unwanted references and add new references. |
12. To add more Annotation Elements to the Annotation feature, repeat Steps 3 through 11.
13. Click OK or click middle-mouse button to close the ANNOTATION FEATURE dialog box and create the Annotation feature.