The Section command bar is used to define or modify a 3D section view of an assembly, part, or sheet metal model.
Options
Opens the Section Options dialog box for you to edit default properties for the cutting plane annotation, dimension style, and caption. You also can specify whether hardware parts, such as bolts, nuts, and washers, are cut or not.
Main Steps
Plane Step
Specify the reference plane or face where you want to draw the cutting plane profile. Use the Create-From Options List on the command bar to select the reference plane option you want.
Draw Profile Step
This step is active when you select an existing cutting plane profile to edit.
Side Step
Defines the side of the profile from which material should be cut away.
The side step is not required when the profile is closed.
Extent Step
Defines the distance to extend the profile for the cutaway view. The extent options are: Through All and Finite Extent.
Select Parts Step
Specifies the parts to be cut. You can use the Cut List options to specify which parts are cut.
Preview/Finish/Cancel
This button changes function as you move through the cutting plane profile construction process. The Finish button constructs the profile using input provided in the other steps. Once you construct it, you can edit it by re-selecting the appropriate step on the command bar. The Cancel button discards any input and exits the command.
Selecting a Plane
Create-From Options
Sets the method of defining the cutting plane profile.
Coincident Plane—Specifies that you want to define a plane that is coincident to an existing reference plane or a planar face on the part. When you set this option, a default X-axis and direction is applied to the new reference plane. You can use keyboard accelerators to define a different X-axis and direction for the new reference plane.
Parallel Plane—Specifies that you want to define a plane that is parallel to an existing reference plane or a planar face on the part. When you set this option, you can specify the parallel offset distance. When you set this option, a default X-axis and direction is applied to the new reference plane. You can use keyboard accelerators to define a different X-axis and direction for the new reference plane.
Angled Plane—Specifies that you want to define a plane that is at an angle to an existing reference plane or planar face on the part. When you set this option, you can specify the angle value you want.
Perpendicular Plane—Specifies that you want to define a plane that is perpendicular to an existing reference plane or planar face on the part.
Coincident Plane By Axis—Specifies that you want to define a plane that is coincident to an existing reference plane or a planar face on the part. When you set this option, you define the X-axis and direction for the new reference plane using a linear edge, a planar face, or another reference plane.
Plane Normal to Curve—Specifies that you want to define a plane that is perpendicular to a curve you select. This is the default option when constructing a helix using the Perpendicular option.
Plane By 3 Points—Specifies that you want to define a plane by three keypoints you select.
Feature's Plane—Specifies that you want to define a plane that is coincident to a reference plane used to define an earlier feature. You can select the feature you want using Feature PathFinder or in the graphic window. This option is not available when constructing the base feature.
Last Plane—Automatically selects the reference plane used for the previous feature. This option is not available if the last feature was a pattern or when constructing the base feature.
Deselect (x)
Clears the selection.
Accept (check mark)
Accepts the selection.
Drawing a Profile
Draw Profile Step
Defines the cutting plane profile geometry. A 2D drawing window and drawing tools are displayed. You can draw an open or closed profile. For example, you can click to define the start/end points of a single line segment or the start and end points of two connected line segments. Click the Return button on the ribbon to close the profile drawing window. This option is available only during profile editing.
Defining the Extent
Through All
Sets the cutting plane extent so that it is cuts through all faces of the part, starting at the profile plane. You can extend the profile to either side of the profile plane.
Tip:
If you use the Through All extent option here to define how much of the model is cut, you also can control the length of the cutting plane annotation displayed in the view by changing the value in the Through All field on the Section Display Options dialog box.
Finite Extent
Sets the cutting plane extent so that it is projected a finite distance to either side of the profile plane. Type the distance into the Distance box on the command bar.
Distance
Sets the distance to extend the cutting plane profile when the Finite Extent option is set.
Step
Sets the distance value to increase or decrease in set increments when you move the cursor. For example, typing a step value of 0.25 and moving the cursor away from the from point would increment the distance from 0.25 to 0.5, then to 0.75, and so forth.
Selecting Parts
Cut List
Defines which parts are cut. The cut options are:
Cut All
Cut Only Selected
Cut Only Unselected
Tip:
Parts defined as hardware parts on the Project page of the File Properties dialog box can be set to be cut or not cut using the Cut Hardware check box on the Section Display Options dialog box. For more information about cutting hardware parts in 3D section views, see the Help topic, 3D section views of a model.