base features require an unconsumed sketch .
For base features, use the Distance, Distance-Distance, Angle, or Angle-Angle fixed termination methods (in the Extents drop-down list). To Next, Between, To, and All termination methods are only available for parts with more than one feature.
Features created after the base feature can use either an unconsumed sketch or the boundary of another feature as a profile. To use an existing feature, set the sketch plane on a feature, then click to select the boundary as the profile to use for the new feature.
To select multiple profiles, click all the profiles you want to include. To remove profiles from the selection set, press and hold Ctrl and click. A profile can be a single loop, multiple loops, intersecting loops, nested loops, or islands.

When you create a feature by adding volume to a profile, you can define the feature extent (termination) in several ways. Termination options are available for Extrude, Revolve, Sweep, and Loft features.

To update features correctly, avoid using faces and edges that can change or be removed because of a design change. Where possible, use inclusive termination options, such as Through All rather than Between, to ensure that the feature persists, even if its termination geometry is removed.

How do termination options differ?

Not all the following options are available for all features, but the following table provides information about choosing the best termination option.

All	Cuts through all faces. If some faces are removed from the feature, All remains a valid termination method because it does not rely on a specific distance or face.
Distance	Do not use a greater distance than necessary to extend through the entire part. If the part changes, the distance can be inappropriate because the feature continues at the distance specified, regardless of the part size. Use All to make sure that the feature is always the correct distance.
Distance - Distance	Use the Distance - Distance option when you wish to extrude in two directions. Unlike creating a symmetric midplane extrusion with the Distance option, Distance - Distance lets you create an asymmetric extrusion with different positive and negative values.
To Next	If possible, use instead of To because To Next does not specify a specific termination element. Use To Next to terminate a feature on a planar or curved face, a line or a curve, while To is a planar termination only.
Between	Use only if you are sure the beginning and ending faces remain intact throughout design changes. If one of the two faces disappears, the feature fails. When creating in-place parts in assemblies, use this method to terminate on the face of a component.
To	Restricted to planar terminations. If possible, use To Next or All. When creating in-place parts in assemblies, use this method to terminate on the face of a component.
Angle	Specifies an angle of revolution for a Revolve feature.
Angle - Angle	Use the Angle - Angle option when you wish to revolve a profile in two directions. Unlike creating a symmetric midplane revolution with the Angle option, Angle - Angle lets you create an asymmetric revolution with different positive and negative values.
Full	Specifies 360 degrees revolution for a Revolve feature.

What geometry can be used for termination planes?

In most cases, you can terminate a sketched feature on the following types of geometry:

A construction surface can be selected as a termination plane. Profiles can be extruded, revolved, lofted, or swept to form construction surfaces.
Features and surfaces can be terminated on any combination of solid and surface features.
Extrusions can be terminated on extended faces with analytic geometry other than planes.

What surface types can be used for extended faces?

In addition to flat faces, you can terminate features on the faces of cylinders, elliptical cylinders (with no draft), cones, spheres, and toroids.

Procedures

Use Extrude or Revolve to model open profiles

Shape propagation applies to open profiles. The result of the operation contextually depends on the extension of the ends of the profile and the shape of extant extrusions. Use the Extrude or Revolve command to propagate a Match Contour or Match Shape, as described in the following sections.

Overview

Note the difference between Match Contour and Match Shape using Extrude. The open profile enables one of two solutions. The side you select to keep determines the result. The Match Shape option is available upon selection of an open profile sketch, such as the sketch on the following part.

Match Contour

With Match Shape unselected in Extrude, the profile is completed by the face which it intersects, and the extrusion is generated from that profile.

Match Shape

With Match Shape selected, the profile is completed by the face which it intersects, and the extrusion flood fills to that face (or faces) as it extrudes, like a To Next termination.

Match Shape

The Match Shape option is available in the Revolve and Extrude dialog box upon selection of an open profile sketch, such as the sketch on the following part.

Revolve

When the Match Shape option is selected, a flood-fill type solution is also created. The open ends of the profile are extended to the axis of revolution, if possible, or to the bounding box of the body.

Extrude

When the Match Shape option is selected in the Extrude dialog box, a flood-fill type solution is created. The open ends of the profile are extended to a co-edge or face, and the required faces are quilted together to form a complete intersection with the extruded body.

The side you select to keep determines the result.

Match Contour

Match Contour closes the open profile, through profile extension, to the body, and the operation takes place as if you have specified a closed profile. If the sketch plane of the profile lies on a planar face, the loops of the face are used to close the profile. In all other cases, the edges defined by the intersection of the profile plane with the body are used to close the profile.

Revolve

When the Match Shape option is disabled, the open profile is closed by extending the open ends of the profile until they intersect the solid body. If the sketch plane of the profile lies on a planar face, the loops of the face are used to close the profile. Otherwise, the edges defined by the intersection of the profile plane with the body are used to close the profile.

Extrude

With Match Shape unselected, the profile is completed by the face that it intersects, and the extrusion is generated from that profile.

Here are the extension rules for closing the profile:

The initial sketch plane is offset from the top surface of the base of this part.
The original profile lines (green) are extended (red-dashed) to the face elements.
The loop is closed by utilizing the intersection lines of the sketch plane and the solid body (purple)
Side to Keep must be specified.
Extrude is performed and a normal closed loop extrusion results.

Edit a feature

Modify the feature sketch

You can change a feature sketch by editing its dimensions or by adding, changing, or deleting constraints to change geometric relationships.

In the browser, find the feature to change.
Right-click the feature and select Edit Sketch from the menu. The feature is temporarily hidden and the sketch is displayed.
Make edits:
- To change an existing dimension, double-click the dimension, and then enter a new value. Click the green check mark to accept the new dimension.
- To add a new dimension, click the General Dimension command, and then click to select the geometry and place the dimension. Click the dimension and set its value.
- To delete a constraint, click the Show Constraints command, and then click to select the geometry. Right-click the constraint on the active constraint box and select Delete.
- To add a constraint, click the appropriate constraint command, and then click the geometry to constrain.
Click Update to update the feature with the new values.

NotePlaced features such as holes, face drafts, and chamfers do not have sketches. To resize a placed feature, redefine it as explained in the following section.

Redefine a feature by changing values used to create it

You can change a feature by selecting a different profile, changing the size or angle of geometry, choosing a different method to terminate the feature, or choosing whether it joins, cuts, or intersects another feature.

Select the feature to edit in the graphics window or the browser.
Right-click and select Edit Feature from the menu. The feature sketch (if applicable) and the feature dialog box are displayed.
Change values as needed. If you click Profile, other values are not selectable until you select a valid profile .
Click Update to update the feature with the new values.

NoteYou cannot change the feature type from solid to surface, for example. Right-click the feature in the browser and select Delete, but retain the feature sketch geometry. Use the sketch geometry to recreate a feature, and select a different feature type.

Tip

You can quickly edit or move a feature by dragging it to a new size or position. In the part browser, right-click the feature to edit, and then select 3D Grips or Move Feature from the pop-up context menu.
To change a legacy loft feature to a loft type such as Point or Centerline, first delete it while preserving the sections, and recreate the loft using the sections.

Move a feature

Use Move Feature to drag an extrude, revolve, or sweep feature to a new location, or use the 3D Move/Rotate command to enter precise coordinates relative to selected geometry.

TipWhen using Move Feature, right-click and select Commit And Move from the pop-up context menu to accept the current changes and switch to 3D Grips.

Show Me how to use 3D Grips to move a feature

What are some uses for Move Feature?

You can drag a feature belonging to a part file deep in the assembly hierarchy, without having to in-place activate any subassemblies or the part containing the feature.

Drag to "cruise move" a feature to a new planar face. The feature sketch reattaches to the new plane, breaking its link with the original face. If the new position is not a planar face, a fixed work plane is automatically created on which to place the feature.

TipWhen moving a feature, you can right-click and select 3D Grips from the pop-up context menu. Use grips to drag a feature or face or snap to other geometry to resize a feature.

How does Move Feature position a feature?

Move Feature approximately positions a feature on a face of a solid model. Add sketch constraints, by editing the feature's sketch, to accurately and persistently position the feature relative to model edges.

TipClick Tools tab

Options panel

Document Settings to access the Document Settings dialog box and then click the Modeling tab to set snap precision. In the 3D Snap Spacing box, set the Distance Snap and Angle Snap increments.

In the part browser, right-click the feature, and select Move Feature from the pop-up context menu.
In the graphics window, click the feature and drag to a new position.
When dragging, you can quickly and precisely move by snapping center points to other center points of circles, edges to other edges, and so on.
Use 3D Move/Rotate to position the feature precisely. Do one to display the triad:
- Click Tab.
- Right-click and select Triad Move.
Click the triad to redefine alignment or position:
- Click a triad axis and drag to rotate around the selected axis.
- Click a triad arrowhead and drag to move in the direction of the arrow.
- Click a triad plane and drag to move in the selected plane.
- Click the triad sphere and drag freely in any direction.
If appropriate, right-click and choose an option:
- After dragging the feature to a new face, click Redefine. You can no longer drag the feature.
- Click Tentative drag to reposition the feature temporarily.
- Click Move Triad Only to leave the feature in position but move the triad.
- Click Cruise Move to switch off the 3D Move/Rotate dialog box. Click Tab to reopen it.
In the 3D Move/Rotate dialog box, enter values to correspond with the selection on the triad.
Click Apply and then continue to refine the position as needed. Click OK to quit.

If a feature is confined to a work plane, you cannot use Cruise Move. When the feature is selected, the 3D Move/Rotate dialog box opens automatically.

Note3D Move/Rotate moves a feature a precise distance, but doing so can break the association of the feature to a face of the solid model.

Using 3D grips

Using grips, drag a feature or face, or snap to other geometry to resize a feature. Arrows indicate the drag direction. The feature preview shows the expected results before you commit to the change.

NoteSet 3D Grips preferences in the parts tab in the Application Options dialog box.

Access:
- Right-click the face of an editable face or feature, and then select 3D Grips from the pop-up context menu.
In the graphics window, move the cursor over a grip point on the feature to highlight direction arrows.
Click a direction arrow and use one of these methods:
- Drag to see a preview of the new size.
- Click a face, edge, vertex, or work feature to snap to the selected item.
Continue to click and drag arrows to resize the face or feature. When dragging, the distance moved from the previous position is displayed.
After you drag to a new size, if appropriate, right-click an arrow and enter values:
- Click the arrow indicating length and choose Edit Offset or Edit Extent. Enter a value in the edit box.
- Click an arrow indicating width or radius and choose Edit Offset or Edit Radius. Enter a value in the edit box.
Right-click and select Done to quit.

Drag to reverse the direction of a feature

This example shows how to reverse the direction of a dragged feature.

1. Right-click the feature you want to drag and select 3D Grips from the pop-up context menu.

2. Click an arrow and drag toward the opposite face of the base feature.

3. Drag to the appropriate length.

4. Right-click and select Done to quit.

The sketch plane and profile sketch of the dragged feature is moved to the opposite face.

NoteYou cannot change the extent type of a feature using 3D grips. For example, you cannot change an extrusion from a join to a cut, or from a cut or join.

Infer constraints with 3D Grips

Constraint behavior depends on settings on the Part tab of the Application Options dialog box. For more information, see Application Options - Parts tab.

Constraints are added when you click a 3D Grip handle, and then click the face of the feature to which you want it constrained. Four handles (Sketch Line, Sketch Point, Sketch Circle, and Sketch Arc) are visible when grip-editing, and the inferred constraint (Tangent, Concentric, Coincident, or collinear) depends on the selected handle and the geometry to which it is snapped. This example shows the handles:

Sketch Line
Sketch Point
Feature
Sketch Circle
Sketch Arc

If an inferred constraint placement is possible between selected geometry, the cursor changes to preview the constraint before placement. You can infer constraints from a static handle (one that has not been dragged) or a dragged handle.

Click the handle, and then click the geometry to which the feature is constrained.
Inferred constraints are previewed on the cursor based on the projected geometry that would result from the selected geometry.
Right-click and select Done to quit or Commit And Move to enter precise coordinates for one or more axes.

NoteTo prevent constraints from being inferred between a static handle and reference geometry, hold down the CTRL key before selection. To prevent constraints from being inferred between a dragged handle and reference geometry, hold down the CTRL key while dragging the 3D Grip handle.

Show Me how to create 2D sketch constraints while using 3D Grips

Tip

Select a face, right-click and select 3D Grips from the pop-up context menu. Drag any grip to resize the feature sketch.
When using the 3D Grips command, right-click and select Commit And Move from the pop-up context menu to accept the current changes and switch to the Move command. You can enter precise coordinates for one or more axes or redefine the orientation of the axes.
Set application options on the Parts tab to specify how dimensional and geometric constraints respond when feature changes caused by 3D Grip editing are inconsistent with existing constraints.
Edit the sketch of the feature to add constraints or dimensions or edit inferred constraints.

Suppress features

Temporarily suppresses display of one or more features, but does not delete them. Features remain suppressed until you unsuppress them. In the browser, suppressed features are dimmed.

In the browser, locate the feature you want to suppress.
Select the top level of the feature to suppress all occurrences of the feature and dependent features. Or, expand the feature and select only the dependent features or occurrences.
Right-click and select Suppress from the pop-up context menu.

NoteTo unsuppress a feature, locate it in the browser and select it. Right-click and select Unsuppress from the pop-up context menu.

Change a feature appearance

To enhance a feature, you can change its appearance. This technique can be useful to help make a feature such as a fillet more visible.

Create a feature.
Right-click the feature in the browser and select Properties.
TipTo set appearance for multiple features in one step, select the features in the browser, right-click, and select Properties.
On the Feature Properties dialog box, click the down arrow on Feature Appearance. Click to select an appearance, then click OK.

Copy and paste features

Copying and pasting features is like creating and placing iFeatures, except that all pasted features are parametrically independent. You can use these methods to copy and paste features:

Select a single feature, copy it, and then paste it (default setting).
Select a single feature, copy it, and then paste the feature and its dependent features.
Select multiple features, copy them, and paste the features. You can include their dependent features.

To copy a feature

Open the part file that contains the feature to copy.
Select one or more features in the browser.
From the Edit menu, select Copy or press Ctrl + C.
TipTo copy a feature and its dependents, right-click the parent feature and then select Copy.

To paste a feature

Open the file with the feature you want to copy and open the file in which to paste the feature.
Click the window with the feature to copy. Copy the feature you want to paste.
Click the window in which you want to paste the feature.
Right-click the graphics window, and then select Paste.
As you move the cursor over a part face, a feature preview appears.
Click to paste the feature on the selected face.
In the Paste Features dialog box:
- Select how to paste the feature (Selected, Dependent, or Independent)
- Select the method to paste parameters (Independent or Dependent).
- In the parameter list, specify a value for each named parameter.
  For example, if a parameter specifies the angle of the feature with respect to the face on which it is placed, enter a value or move the mouse to rotate the feature dynamically. The angle value changes in the dialog as you move the mouse. Click to select a value.
- Click Finish when all parameters are assigned a value.

NoteClick the X symbol under the feature and move the mouse to a new location to position the feature on the face. Click the circular arrow symbol to rotate the feature dynamically or by entered value.

References

Copy and paste features

You can copy and paste features within a part file or between open part files using the Windows Clipboard. You can paste only in the part modeling environment. Copying and pasting is like creating and placing an iFeature with these differences:

By default, dependent features are not copied. Only features that are explicitly selected are copied.
The paste command allows dependent features to be copied as well.
Autodesk Inventor uses unresolved plane references to position the features.
Newly copied features are fully independent, unlike iFeatures.
If pattern features are copied and pasted, then the parent feature is also pasted.

Example: Paste a copied boss feature

Figure 1.	In the boss part file, select the top-most extrusion in the boss feature in the graphics window or the browser (Figures 1 and 2). The top-most extrusion is the parent feature for the fillet, through-hole, and cotter-pin hole features. Right-click the feature in the browser and select Copy.
Figure 2.	Activate the part on which you want to paste the feature. Right-click and select Paste. Click the face on which you want the feature placed.
Figure 3.	In the dialog, for each independent parameter, enter a value or select a value with the mouse by dragging and clicking. Click the X symbol to position the feature on the face (Figure 3) or click the circular arrow to rotate the feature. Click OK when finished.

Feature Properties

Access:

Right-click a feature in the browser, and select Properties.

Select several features in the browser, right-click, and select Properties.

The current selection in the browser determines available options.
Name	Specifies the feature name.
Suppress	Always implicitly suppresses the feature in the browser and the graphics window. If defines a condition determining feature suppression.
Adaptive	Sets adaptive status for the feature sketch or individual feature parameters. TipTo set the adaptive status of all feature parameters at once, select the feature in the browser, right-click, and select Adaptive.
Feature Appearance	Sets appearance of the selected feature or features. If appropriate, click the current appearance, and select new appearance from the list.

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