Many features use profiles to define the shape of material to be added to the part or removed from the part. Profile-based ordered features are associative to their profiles; if you change a profile, the feature automatically updates.
You can draw the profile as part of the ordered feature construction process, or select a profile from a sketch you drew earlier. You draw a profile or sketch on a reference plane. You can use one of the default or base reference planes, or you can define a new reference plane using a face on the model.
Solid Edge provides commands to add material and to remove material. For example, you can use the extrusion commands to add material by:
extruding a profile along a linear path,
revolving a profile about an axis,
sweeping a profile along a user-defined path,
or fitting through a series of profiles.
All of the protrusion commands can be used to construct a base feature.
All profile-based ordered features are constructed with the same basic workflow. For example, when you construct a extrusion feature using an open profile, the Extrude command bar guides you through the steps described below:
Plane or Sketch Step—Define the profile plane by selecting a planar face or reference plane.
Draw Profile Step—Draw the profile in the profile view. The Draw Profile Step is automatically activated when you construct a feature.
Side Step—Define the side of the profile you want to add material to by positioning the cursor so that the directional arrow points towards where the material is to be added. The Side Step is skipped if you use a closed profile.
Extent Step—Define the extent of the material to add with the cursor (A) or by typing a value in the command bar (B). You can also use keypoints on another feature or another part in the assembly to define the extent for a feature. See the Using Keypoints to Define Extents section for more details. When working in the context of an assembly, many features also allow you to select a keypoint on another part in the assembly to define the feature extent associatively.
Treatment Step—Define the crown or draft angle treatment you want for the feature. This step is optional. See Applying Draft Angle and Crowning to Features for more details.
Finish Step—Process the input and construct the feature. The profile and dimensions are hidden automatically when you click the Finish button.
Each type of profile-based feature has a set of requirements for the type of profile geometry it can use. For example, a protrusion that is the base feature must have a closed profile, but subsequent features can have open or closed profiles. When you finish drawing a profile, or accept a profile you select from a sketch, the feature command checks to make sure the profile is valid for the feature type. If the profile or sketch used to create the feature is invalid, the Profile Error Assistant dialog displays a description of the profile error. When you move the mouse cursor over the description, the element containing the error highlights in the profile window. You can click the error description to select the invalid element and zoom to the element, delete the element, change the color of the element, change the element to construction geometry, or save the geometry as a sketch or failed feature. You can make corrections to the profile and then click the Validate button to re-validate the profile. If the profile is valid, you are returned to the next feature creation step. If the profile still contains errors, the description list is updated to display any errors. You can also save the profile as a failed feature or sketch. Construction and reference elements are ignored during profile validation.
When you construct a feature with an open-ended profile, the ends of the profile are extended toward intersections with the existing model. Lines are extended linearly (A); arcs are extended radially (B). Material is added or removed along the full length of the extended profile, in the selected direction.
When constructing a feature using more than one profile, all the profiles must be closed. The following feature commands allow you to construct features using multiple closed profiles:
Protrusion command, when constructing a base feature or adding a feature.
Revolved Protrusion command, when constructing a base feature or adding a feature. All profiles must share a common axis of revolution.
Cutout command.
Revolved Cutout command, all profiles must share a common axis of revolution.
Web network command, when constructing a base feature or adding a feature.
When you use a keypoint on another feature or another part when working in the context of an assembly, the feature extent is associative to the keypoint on the feature or part to selected. If you modify the parent feature or part, the feature extent updates.
When you select a keypoint on another part, an inter-part link is created between the current document and the other part in the assembly. For more information on inter-part links, see the Inter-Part Associativity Help topic.
The Dynamically Preview Feature Creation option on the View tab of the Options dialog box allows you to dynamically display a feature during the Extent step of feature creation. You can override this option by pressing CTRL+SHIFT+D.
When selected, this option allows you to set the result color and tool body color. The result color is the color for the resulting feature. The tool body is the color of a cutout when it is not intersecting model geometry. In the following example, notice that the area in which the extent does intersect the model is the default tool body color. Once the extent intersects the model, the portion intersecting the model changes to the default result color.
Note:
When working with an assembly, only the Tool Body is shown during feature creation.
When a feature fails during dynamic feature creation, a warning and tool tip are displayed to provide information about the failure.
