Functional features and feature points

Extended modules > 3D Documenation > Create GD/T datums and tolerance labels > Functional features and feature points

You may need to create your own functional features or functional feature points in cases where the required reference structure is too complex for Creo Elements/Direct Modeling to recognize automatically. Explicit functional features and feature points can be used to create more complex GD&T call structures.

If a series of elements needs to be grouped into a new structure, each face can be defined by an explicit functional feature, and grouped under a single GD&T call-out. By naming each face as an explicit functional feature, they can then be selected individually or together for inclusion as GD&T elements. You can therefore select individual features later when another GD&T call-out needs only part of the pattern.

Like datums and tolerances, functional features and functional feature points can be owned by either a single part or a single assembly. No face can belong to more than one functional feature for a given owner. The feature labels are colored like other GD&T labels: cyan for part-owned and magenta for assembly-owned features.

Defining functional features

To define a functional feature,

1. Click 3D Documentation and then, in the Annotate group, click the arrow next to More.

2. Click

Functional Feature. The Functional Feature dialog box opens.

3. The two distinct methods for defining explicit functional features are by Faces and by Features:

Faces	If you create a functional feature on a face that has not previously been used in a datum or tolerance, then the required features must be selected with the Faces option.
Features	If you create a functional feature on a face that is already a member of an existing datum or tolerance, you must use the Features option for selection.

4. Specify a name for the feature in the Name box.

5. Optionally, specify a description in the Descr box.

6. Specify an owner for the feature in the Owner box.

7. Click

to complete the operation.

Defining feature points

To define a feature point,

1. Click 3D Documentation and then, in the Annotate group, click the arrow next to More.

2. Click

Feature Point. The Feature Point dialog box opens.

3. In the Method box, choose a reference. You can define a feature point with respect to a number of references:

On Face	Defines a feature point on a specific face.
By Vertex	Defines a feature point with respect to a vertex. When you select the point's location, Creo Elements/Direct Modeling automatically selects the nearest vertex as reference, and states its X,Y,Z offsets from the selected point. You can change these offsets, if necessary.
RefPlane	Defines a feature point with respect to a reference plane. Again, you can change the U,V offset of the point, and specify the plane by its normal and U direction.
By 2 Edges	Defines a feature point with reference to two edges. Offsets from the two selected edges can be given.
CenterPt	Defines a feature point with respect to the center point of an element.
3 Surfaces	Defines a feature point at the intersection of three planes (faces or workplanes).

4. Specify an owner for the feature in the Owner box.

5. Click Ref. Face and select a reference face in the viewport.

If selecting a reference face in Creo Elements/Direct Modeling creates a feature point offset from the original edge, then the reference is not associative to the geometric changes in Creo Parametric. In this case, the datum point is referred instead of actual edge reference.

6. Specify a name for the feature point in the Name box.

7. Optionally, specify a description in the Descr box.

8. Click

to complete the operation.

Explicit functional features and functional feature points are otherwise created similarly to other custom process features.

When you export feature points to Creo Parametric,

• Feature points are exported as datum points. For more information, see Exporting feature points and references.

• Some types of feature points are not associative to geometric changes in Creo Parametric, as shown in the following table:

Type of feature point in Creo Elements/Direct Modeling	Comment	Type in Creo Parametric
On Face	Reference is not associative in Creo Parametric.	Datum Point
By Vertex	Reference is not associative in Creo Parametric.	Datum Point
Ref Plane	Reference is not associative in Creo Parametric.	Datum Point
By 2 Edges with zero offset	Dimension reference is associative to the intersection of the 2 edges.	Linear dimension reference (datum point is not referenced)
By 2 Edges with non-zero offset	Reference is not associative in Creo Parametric.	Datum Point
CenterPt	Dimensions referenced to the midpoint of any 3D edge are associative in Creo Parametric.	Linear dimension reference (datum point is not referenced)
3 Surfaces	Reference is not associative in Creo Parametric.	Datum Point

Note that feature points can be hidden from view using the Creo Elements/Direct Modeling Show menu.