Sheet Metal Loft

Create a sheet metal part that transitions between two profiles.

Sheet metal loft: Desktop

Steps

To create a sheet metal loft:

While in a Part Studio, click the Sheet metal loft button ().
Select New to create a new sheet metal part, or select Add to add the loft to an existing one.
With focus in the Profile 1 field, select the starting profile (region, face, edge, or point).
With focus in the Profile 2 field, select the ending profile. Onshape creates a sheet metal model between the two profiles.
Click the Connections checkbox for more control on the twist of the resulting model. Onshape estimates the proximity within the existing vertices/edges if no matches are specified.
1. Select a vertex or edge from the loft and drag the manipulator(s) to adjust the connection.
2. To divide the model into separate parts at the connection, select Rip.
Use the Chordal tolerance field to set the maximum distance the tessellated geometry can vary from the underlying surface.
When creating new sheet metal models, you can also expand the following sections to further refine the model:
- General:
  - Thickness - Thickness of the sheet metal. Click the arrow to reverse the direction.
  - Bend radius - Inside radius of the bends created.
  - Flip direction up - Select to reverse the orientation of the sheet metal model and flat view. This is useful when defining whether bends are up or down relative to the model.
- Material (options in this section are identical to those provided in the Sheet metal model feature):
  - Bend calculation - Determines how the bends are calculated. Options are:
    - K Factor (default) - Uses the ratio of the neutral axis to the material thickness.
    - Bend allowance - Uses the length of the neutral line arc between the tangent points of a bend.
    - Bend deduction - Uses the difference between the sum of the flange lengths (from the edge to the apex) and the initial flat length.
      
      The Bend calculation selected here is used as a column in the sheet metal table. Each bend may be customized and directly edited from the table. See Sheet metal table and flat view for more information.
  - Default bend K Factor - The fraction of material thickness on which the neutral axis lies on a bend. (Default is 0.45.)
  - Rolled K Factor - The fraction of material thickness on which the neutral axis lies on a section of rolled wall. (Default is 0.5.)
- Relief (options in this section are identical to those provided in the Sheet metal model feature):
  - Minimal gap - The smallest gap between the sheet metal edges defining a rip.
  - Corner relief type -
    - Square - Sized
      Flat view: 3D view:
    - Rectangle - Scaled
      Flat view: 3D view:
    - Round - Sized
      Flat view: 3D view:
    - Round - Scaled
      Flat view: 3D view:
    - Closed
      Flat view: 3D view:
    - Simple
      Flat view: 3D view:
  - Corner relief scale - The scale of the corner opening (for Scaled openings), a value between 1.00 and 2.00.
  - Bend relief type - The shape of the bend relief:
    - Rectangle - Scaled
    - Obround - Scaled
    - Tear
  - Bend relief depth scale - A value between 1.00 and 5.00. Once you enter a value it becomes the default across all documents.
    - A value of 1 results in an obround bend relief perfectly touching the bend and a rectangular bend relief matches the depth of the obround.
    - Any value past 1 adds depth via the formula:
      (depth scale -1) * bendRadius
  - Bend relief width scale - A value between 0.0625 and 2.00. Once you enter a value, it becomes the default across all documents. The width of the bend relief is calculated via the formula:
    thickness * width scale.
When adding to an existing sheet metal model, click the Merge scope field, then select the part to add to. The merge scope can only accept bodies of a single active sheet metal model.