Advanced iFeature placement

As you become proficient at creating and using iFeatures, your features can become more complex. You can decide what geometry to include in the Position Geometry list of the Extract iFeatures dialog box.

In the Position Geometry list, you can add reference edges that position the base feature sketch of the iFeature. Including reference edges captures more design intent, but it requires that the iFeature be positioned in the same way it was originally placed.

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, the geometry is shown in the following way:

• 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 is shown once (Profile Plane2).
• Selecting the face in the Position Geometry list highlights both faces in the Selected Features tree.

In the Position Geometry list, you can right-click the plane and select Make Independent to list the planes separately. 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 additional 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.

iFeatures created from multiple-sketch features (such as lofts and sweeps) can be 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 additional 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.

Optionally, 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 is shown 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, you can 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, you want to 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.