Position geometry for iFeatures

Position geometry, usually a sketch plane, describes the interface that is joined to a feature when the iFeature is placed.

Position geometry for iFeatures with shared geometry

When you create an iFeature from multiple features that share geometry, by default the shared geometry appears only once in the Position Geometry list. For example, you create an iFeature from an extruded feature that terminates on an offset work plane. The work plane is offset from the same face that the extrusion is sketched on.

In the Extract iFeature dialog box:

• In the Selected Features tree, the face is listed under both the work plane feature (Plane1 [Plane]) and the extrusion feature (Profile Plane2 [Sketch Plane]).
• In the Position Geometry list, the face displays once (Profile Plane2).
• Selecting the face in the Position Geometry list highlights both faces in the Selected Features tree.

To list the planes separately, in the Position Geometry list, you can right-click the plane and select Make Independent. When the iFeature is used, you select and position each plane separately. You have greater flexibility in how the iFeature is used, but are required to select more position geometry during placement.

In the Position Geometry list, you can rename the planes to make them easier to understand when the iFeature is placed. Rename Plane1 to Work Plane Offset Face and Profile Plane2 to Sketch Plane.

Position geometry for iFeatures with multiple sketches

iFeatures created from multiple-sketch features (such as lofts and sweeps) are more useful when you add geometric elements to the Position Geometry list.

Lofts

Lofts contain two or more sketches on separate sketch planes. By default, the first profile selected in the loft feature is shown in the Position Geometry list. The position of remaining sketch planes is defined relative to the first profile. By including more sketch planes in the Position Geometry list, the location of the included planes is selected when the iFeature is placed.

In the Selected Features tree, select the profile, right-click, and then select Make Independent. Individual sketch planes are listed in the Position Geometry list and can be positioned separately when the iFeature is placed.

You can combine two or more sketch planes in the Position Geometry list so that their positions are relative to one of them. When selecting sketch planes to combine in the list, the first selected sketch plane remains in the list. The position of the other plane is relative to the first. Right-click the sketch plane, and then select Combine Geometry.

Sweeps

If no dependency exists between the profile and path sketches, by default the profile sketch displays in the Position Geometry list. In this case, the path sketch position is defined relative to the profile.

To make placement of the path sketch independent of the profile sketch, add it to the Position Geometry list. In the Selected Features tree, right-click the path sketch, and then select Make Independent.

For some iFeatures, such as an O-ring groove created with a sweep, define the position relative to the path sketch. In the Position Geometry list, right-click the path sketch, select Combine Geometry, and then click the profile sketch. Because the path sketch was selected first, it is listed.