> > Taper a face or recognized feature (boss or pocket)

Taper a face or recognized feature (boss or pocket)
To taper a planar, cylindrical, conical face, or recognized feature to a draft plane, specify either:
The draft plane,
The draft direction, a draft point and the angle of the draft , or
The angle dimension
Taper a face
The tapering of a face means its inclination at an angle relative to a draft plane. The draft plane is an imaginary plane indicated by an arrow and its base. The draft plane sections the planes which are defined by the part's faces. It does not have to be a section of a face itself.
The axis for the inclination is the intersection of the draft plane and the face's plane.
Taper a recognized feature
System recognized features are bosses, pockets, holes, or a combination of them. The tapering of a recognized feature means the inclination of its faces relative to a draft plane. The axes for the inclination are the intersections of the draft plane and the planes defined by the feature's faces. The faces rotate around the intersections in the same way as when tapering faces.
The faces rotate around the intersection like a door swings on its hinges. A positive draft angle inclines the faces on the positive side of the draft plane to the inside of the part; a negative draft angle inclines the faces on the negative side of the draft plane to the inside of the part. The arrow indicates the positive side of the draft plane.
Change the draft plane
The figure shows the results of changing the position of the draft plane (1) while keeping the taper angle (2) constant.
If you select the Keep as Feature option, a taper feature is created and you will find its icon in the Structure Browser. You can apply or deactivate the taper feature, so you can temporarily remove the taper if needed. You can also easily change a taper feature.
 If the face or recognized feature you want to taper is referenced by a 3D Annotation angle dimension, you can use this dimension and simply specify a new angle for the referenced face or feature.
To taper a face or recognized feature (boss or pocket),
1. Click Modeling and then, in the Engineering group, click Taper. The Taper dialog box opens.
2. Select the faces or features to taper:
Click Faces and select a face to taper in the viewport. Press Shift to select multiple faces.
Click Rec.Feat and select a feature to taper in the viewport. Press Shift to select multiple features. You can select a feature type from Feat Select. Automatic selects the boss/pocket, rib, or slot with the smallest number of faces.
Click Taper Feat and select a taper feature in the Structure Browser to adjust an existing taper. You can identify a taper feature by the icons (applied) or (not applied).
3. Set the following options:
Keep Tan: Preserve the tangential transitions between neighboring faces. Click Control to fix or unfix edges and faces. If you choose not to Keep Tan, smooth tangential transitions are replaced by edges.
Redo Blend: Allow the operation to make automatic adjustments to blends. Click Control to specify the blends to redo.
Chk & Fix: Use when you suspect a part is corrupt. Chk & Fix checks for self-intersections, knife edges, and void shells and attempts to fix them. If a part fails the check and fix, it is not modified and remains in its original state.
Keep as Feature: Creates a taper feature in the Structure Browser so you can activate and deactivate the taper, or quickly adjust the taper later.
Automatic: The system defines the blend value.
Min Face Thickness: You define a minimum face thickness for the faces adjacent to the blend. The new blend radius will maintain this minimum face thickness.
5. Click Draft Plane and set the draft direction.
6. To taper faces using a draft point and direction,
a. Click Draft Dir and set the draft direction in the viewport.
b. Click Draft Point to position the draft plane. The draft plane is defined automatically by a plane through the draft point with the W direction of the plane normal being equal to the draft direction.
7. If you want to modify an existing taper, select an Angle Type:
Relative: Calculates the new taper angle in addition (relative) to the original angle.
Absolute: Calculates the new taper angle against the draft direction. To remove a draft angle, type 0 as the absolute angle.
8. Type a Draft Angle.
9. The Upd Rels option is available when the Parametrics module is active. Select this option to update relations with your changes.
 You can toggle between Realistic and Quick to see either realistic feedback or quick feedback when you taper a face or a recognized feature in the viewport. See Realistic feedback.
10. Click to complete the operation.
 If you do not have a planar face to use as a reference for the draft plane, you can create a draft plane by positioning a workplane where you want the draft plane to be located. In the Taper command, click Draft Plane and use the option W or -W in Axis 3D to define the direction of the normal for the draft plane.
Limitations
When tapering faces, you can add or remove material. You can also remove edges and faces, but you cannot add them.
When tapering recognized features, you can add and remove material. You can even add and delete faces, edges, and vertices. But if the tapering moves the feature to or beyond a face edge, it loses its characteristics and it is no longer recognized as a feature (unless you use the Undo function). Click Preview to see the impact of these changes before you accept them.
Generally, only planes, cylinders, and cones can be tapered using a draft plane. Other types of faces may be tapered with advanced tapering techniques.
You must set the Angle Type to Absolute if you create or modify a taper feature.
If you select the Redo Blend option, the system will attempt to recreate the blend with the same blending options. However, in some situations that may not be possible. If the blend was created with the RollAtSharp or RollAtSmooth options, the blend may be recreated without those options.
If you use the Taper command on multiple parts, the successful operations are displayed as a partial result and the failures are displayed as labels (error feedback). The feedback labels are attached to the faces, on which the operation has failed.