Creating Sections Using Alternative Methods

You can create a section using a planar surface as cutting plane.

For the purpose of this scenario, you will create an offset section view, but this capability is also available for other types of sections.

1. Click Offset Section View in the Views toolbar (Sections sub-toolbar).

2. Select a planar surface on the 3D part. This planar surface needs to be perpendicular to the projection plane of the active view.
   
   

   Note: You can also select a wireframe plane on the 3D part.

   The section plane appears on the 3D part and moves dynamically on the part.

   The cutting profile is automatically displayed on the front view as well as a preview of the view to be generated.

3. Click in the drawing to generate the view.

   
   
   

You can create a section using a cutting profile defined in 3D as cutting plane.

For the purpose of this scenario, you will create an offset section view, but this capability is also available for other types of sections.

Sections are usually created using a cutting profile as the cutting plane; such a profile is typically driven using concentricity or parallelism constraints. Defining a profile in 3D to create a section enables you to make the profile associative with the geometry, and therefore to drive this profile using dimensional constraints, for example.

1. In the 3D window, click Sketch and select the xy plane as the reference plane.

   You are now in the Sketcher workbench.

2. Click Profile and sketch the profile you will use as cutting plane. For the purpose of this scenario, make sure you sketch your profile using orthogonal lines.

   
   
   

3. Click Constraint to create dimensional constraints between your profile and other elements.

   
   
   

4. Now, click a vertical line and the edge of the part to create a dimensional constraint between them.

5. Exit the Sketcher workbench.

6. In the drawing window, click Update to update the view.

7. Click Offset Section View in the Views toolbar (Sections sub-toolbar).

   Important: Depending on the type of profile you sketched and on the type of section (offset or aligned) you want, you can select another icon in the Sections sub-toolbar. If the 3D profile is not valid for generating the appropriate view, you will not be able to select it. In this case, you will need to select another icon.

8. Select the profile on the 3D part.

   The cutting profile is automatically displayed on the front view as well as a preview of the view to be generated. Positioning the section view amounts to defining the section view or the section cut direction.

   
   
   

9. Click to generate the view.

   
   
   

   Important: You can modify the section view/section cut by editing the 3D profile. After doing so, don't forget to update the drawing. When editing a 3D profile, make sure that you modify it in accordance with the type of section (offset or aligned) you created: if an edited profile is invalid when you update a drawing, the associated section view/section cut will not be displayed (an error symbol will appear instead). If you delete the 3D profile and then update the drawing, the section view/section cut will not be deleted. The profile will no longer be associated with the geometry. You can subsequently edit the profile directly in the drawing by double-clicking it.

You can create a section through circular and cylindrical elements.

For the purpose of this scenario, you will create an offset section view, but this capability is also available for other types of sections.

In creating an offset section view or offset section cut through circular and cylindrical elements, the first point is automatically computed if the selected element is:

• a circular generated item or a centerline,
• a generated item corresponding to a revolution surface or an axis line.

1. In the drawing window, click Offset Section View or Offset Section Cut in the Views toolbar (Sections sub-toolbar).

2. Select the circle representing the hole (or a centerline), to define a profile going through a hole.

   The first extremity of the segment is positioned automatically outside the geometry.

3. Double-click to end the profile.

   In this case you can see that the top position has been fixed.

   
   
   

4. Drag the blue manipulator to define the cutting length.

   In this case the second extremity is placed inside the geometry.

   
   
   

5. Click to position the view.