Data Exchange > AutobuildZ > Creating Features in the Current Part > To Specify Feature Type and Define the Section Profile and Sketch Plane
To Specify Feature Type and Define the Section Profile and Sketch Plane
1. On the Feature tab of AutobuildZ, select one of the following feature types:
Protrusion
Revolve
Straight Hole
Datum Plane
Datum Curve
Datum Point
The feature creation wizard specific to the feature type opens. The wizard indicates the number of steps required for the creation of the feature.
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If you have not defined a view, a warning appears stating that no views are defined for the drawing. It prompts you to use the View Setup dialog box to define a view for the drawing. A warning also states that parts are not defined when you have not set up a part model as the active part on which to create features.
2. Type a name for the feature in the Name box. If you do not specify a name for the feature, the default feature name is used.
3. Under Type, click to switch to Cut. Protrusion is the default. Click to switch between Side1 and Side2 to indicate the direction of the cut. is available only on the Extrude Feature and the Revolve Feature wizards. It is enabled only when the active 3D part has at least one protrusion feature.
4. Click to move to the next screen of the feature creation wizard.
5. Under Section Profile, click . The Selection dialog box opens.
6. Use one of the selection methods to select entities to define the section profile. The chain method of multiple selection of entities is the default.
7. Click Close to close the Selection dialog box. The box next to displays the ID and the drawing view of the selected entities.
8. Click if you want to clear the selection and select entities again.
The section profile is automatically validated.
The result of the validation is displayed under Section Profile Validation as Successful or Failed.
If the result of the validation is displayed as Failed under Section Profile Validation, view the list of the validation checks and their results in the Section Profile Validation dialog box, and fix the section profile appropriately.
You are automatically guided to the next screen of the feature creation wizard if you have selected Automatic forward in the Preferences dialog box and if the validation of the section profile is successful. The feature creation wizard indicates that you are in the next step of the feature creation process.
9. Click to move to the next screen of the feature creation wizard if you did not select Automatic forward in the Preferences dialog box.
10. Under Sketch Plane, click to select a line entity to define the sketching plane.
The box next to displays the ID of the line entity on the drawing.
The 3D Info box displays the name of the datum plane or surface that the selected line entity represents if the datum plane or surface exists in the 3D model. If the datum plane does not exist, a new datum plane is created and its name displayed in the 3D Info box.
11. Click Flip if you want to change the sketch view direction. The section profile and the feature that are created in the Creo Parametric secondary window for preview are updated.
12. Click Preview to preview the active 3D model any time during feature creation or highlight the feature elements in a secondary window. You can preview the following feature elements in the Creo Parametric window during the relevant step of the feature creation process:
A reference surface or datum plane that represents the sketching plane is highlighted in cyan after you have defined the sketching plane.
A reference surface or datum plane that represents the "Through Until" depth is highlighted in cyan after you have defined the extent of depth for an extruded feature.
The section profile on the sketching plane is highlighted in blue after you have defined the section profile and the sketching plane.
The 3D feature is highlighted in red when all feature elements are defined.
13. Click Preview again to close the secondary window.
14. Click either of the following:
OK—Completes the feature creation process and is available only when you have defined all the relevant feature elements.
Cancel—Cancels the feature creation process. Click Yes in the CONFIRMATION window to confirm the termination of the feature creation process.