Creating Sections Using Alternative Methods

You can create aligned sections views, aligned section cuts, offset section views or offset section cuts.

This task shows you how to:

Before you begin:
  • Open a product containing a 3D part and a generated drawing representation.
  • Make sure the front view is active on the drawing (double-click it if needed).
  • Tile your windows vertically to see both your part and the related drawing.
See Also
About Sections
Creating an Offset Section View/Cut
Creating an Aligned Section View/Cut

Create Sections Using a Planar Surface

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

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

  1. From the View Layout section of the action bar, click Offset Section View .
  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 sheet to generate the view.


Create Sections Using a Cutting Profile Defined in 3D

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

For this scenario, you have to 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 area, click Sketch and select the xy plane as the reference plane.

    You are now in the Sketcher app.

  2. Click Profile and sketch the profile that you are going to use as cutting plane. For 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 app.
  6. In the drawing window, click Update to update the view.
  7. From the View Layout section of the action bar, click Offset Section View .
    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 View Layout section. If the 3D profile is not valid for generating the appropriate view, you are not able to select it. In this case, you have 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 in the sheet to generate the view.


    Important:
    • You can modify the section view/section cut by editing the 3D profile. After doing so, update the drawing.
    • When editing a 3D profile, 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 is not displayed (an error symbol appears).
    • If you delete the 3D profile and then update the drawing, the section view/section cut is not deleted. The profile is no longer associated with the geometry. You can subsequently edit the profile directly in the drawing by double-clicking it.
  10. To reuse this sketched profile in creating more sections for other parts, perform the following actions:
    1. Copy the defined sketch in which the profile is created.
    2. In the tree, right-click the part body, of which you want create a section view, and select Paste Special.
    3. In the Paste Special dialog box, select As Result With Link.
    4. From the View Layout section of the action bar, click Offset Section View or Aligned Section View .
    5. Select the copied sketch.
    6. Click in the sheet to generate the view.

Create Sections Through Circular and Cylindrical Elements

You can create a section through circular and cylindrical elements.

For 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. Click Offset Section View or Offset Section Cut .
  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 creation.

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



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

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



  5. Click to position the view.