When an output profile is created, its geometry is automatically removed from the sketch feature 3D result. In other words, output profiles are made available and updated independently from the sketch within the 3D area.

You can use profile features for creating Part Design or Generative Shape Design features.

1. Click Profile Feature .
   From V5R17 onwards, as soon as Profile Feature is selected, the Profile Definition dialog box is displayed even if no geometry is selected. The name of the profile you are creating is displayed in the Name field.
   

2. Select the circle as shown:

The geometry you selected is displayed in the Input Geometry field, the resulting geometry, that is all geometrical elements that eventually are exposed in the 3D area, in the Output Geometry field.

4. Select the second circle as shown.

Whenever you wish to remove elements from the selection, just right-click the element of interest and select Delete. Alternatively, just select the element in the geometry area again.

A warning message is displayed in the dialog box because the application detects an ambiguity you need to solve: the two selected circles are not connex and the Check connexity option is selected.

5. Clear Check connexity.

6. Use the Color combo list to assign the cyan color to the profile feature you are defining.

8. Click OK to confirm the creation.
   The parameters and options you defined for this profile are kept as default values for the next profile you will create later on.
   The output feature is displayed as Profile.2 in the Outputs node in the specification tree.

9. Go into the Part Design workbench and use the profile to create a pad.

Note that the profile does not appear under Pad.2.

Profile Definition Dialog Box

Color

The color helps you distinguish the elements that are part of the selection. Once in the 3D area, that color is kept. Indeed, unlike in the Sketcher, the profile feature is visualized in the 3D area with the color you assigned to it in the Sketcher. For the purpose of our scenario, set the blue color. The selected line as well as an additional line are now displayed in blue. Note that line thickness is also increased to help you view the selected elements that will be exposed in the 3D area.

Mode

Output profiles can be defined only from geometrical elements belonging to the same sketch.
Three modes of selection are available:

• Point (Explicit Definition): you need to select all the points of interest. In that case the Input Geometry field and the Output Geometry field show the same elements.

• Wire (Automatic Propagation): after you selected a geometrical element, the application detects and selects all connex elements.

• Wire (Explicit Definition): you need to select all the geometrical elements of interest. In that case the Input Geometry field and the Output Geometry field show the same elements.

Options

Four options let you validate the profile definition. Note that the connexity and the manifold property of the profile are checked by default.

Once checks are performed, warning messages may be displayed to help you decide whether you keep your definition as such or if you need to modify it. Moreover, update errors appear for features causing trouble once you have left the Sketcher workbench. Several checks can be performed, you just need to select the appropriate option:

• Check tangency

• Check connexity

• Check manifold

• Check curvature

Reusing Input Geometry

The geometry already used to define a profile feature can be reused for the definition of another profile. Using the sketch of our scenario, for example you can create a new profile feature as shown in magenta, and create a new pad:

Cutting, Copying and Pasting Output Profiles

In the Sketcher, you are not allowed to cut or copy then paste output profiles. Conversely, in the 3D area, you can use the Cut or Copy commands. In that case, you obtain datum features.

Deleting Output Profiles

You can delete output profiles in the Sketcher only. Deleting an output profile does not affect the geometry used to define that profile.

Hiding or Showing Output Profiles

If outside the Sketcher you apply the Hide/Show capability on a sketch node, the capability applies to all elements except for output profiles.