5. Step bend

Exercise 5: Suction hood 

Version compatibility

This exercise was carried out with version 27.0 (Vertex 2021).

In this exercise you will learn to

• Modeling a part using cross sections and lofting. Thus creating the main shape of the desired hood. 
• To create a sheet metal part with the tangential offset function.
• To create the Step bends that are required for the Unbend (Flatten sheet projection)
• To create a 3D unbend.

Functions to be used:

• Sketching + operation: Cross Section
  
• Lofting > Boss (Skinning)
  
• Tangential offset.
  
• Step Bend
• Unbend

Create a new part

• File > New > Part.
  
  • Enter the label (which is also the name of the model and by default will be the name of the drawing).
  • Enter the archive information by clicking Arc.Data.
  • Select the project where the model will be saved.
  • OK.

Create the first cross section

• New Sketch > To horizontal (XY) plane.
  

Sketch the shape

• The function: Two point rectangle.
  • Sketch a rectangle symmetrically about the vertical axis of the central cross.
• Add the Conincident constraint between the upper horizontal line and the central cross.
• Add the Symmetry constrain between the vertical lines and the center cross.
• Add the Distance constraints.
  • 800 and the formula: WIDTH.
  • 400 and the formula: DEPTH.
• Click the two points in the bottom corner.

• The function: Round.

  • 150 and the formula: R1.

• 

Operation

• Cross Section.

Create the second cross section

• Click  the first cross section.

• Right-click function: New Sketch > Parallel.

  • Enter the value: 400 and the formula: HEIGHT.

Sketch the shape

• The function: Two point rectangle.
  •  Sketch a rectangle symmetrically about the vertical axis of the central cross.
• Add the Conincident constraint between the upper horizontal line and old line, if needed.
  
• Add the Symmetry constrain between the vertical lines and the center cross.
• Add the Distance constraints.
  •  400 and the formula: WIDTH2.
  • 200 and the formula: DEPTH2.
• Click the two points in the bottom corner.

• The function: Round.

  • 30 and the formula: R2.

• 

Operation

• Cross Section.

Use cross sections to create a part

• Click both cross sections (Remember Ctrl key with later cross section).

• The function: Lofting > Boss.

  • The Loft dialog opens.
• Accept defaults.
• OK.

Create step bendings

Step bends must be created on each surface to be separately.

• Click the face, shown in the figure.
• Right-click function: Step Bend.
  
  • Number: 7 and the formula: PCS.
  • Radius: 4 and formula: RADIUS
• OK.

• Click the face, shown in the figure.
• Right-click function: Step Bend.
  • Number: 7 and the formula: PCS.
  • Radius: 4 and formula: RADIUS.
• OK.

Note the radius value

The radius of the Step Bend depends on the following factors:

• Are you adding material In, Middle or Out with the function Tangential Offset (See the next step).
  
• From the radius of the bending blade.
  

Create a sheet metal part

• Choose one of the oblique faces.
• Right-click function: Tangential Offset.
  • Value (Sheet metal thickness): 1.
  • Click: In (the direction the material is added relative to the selected surface.)
• OK.

Create a 3D unbend

• Activate the ribbon of Sheet metal part.
• The function: Unbend.
• Accept the face selected by the program or select a face.

Create rebend

• The function: Rebend.
• Note that if no features have been added to the unfolded part, the Rebend function removes the Flatten Sheet feature.

Save the model

• File > Save or click

  

  or press

  

  

Further processing of the model (These are presented in Exercise 5 "Drawing on model")

You can add a material item to the model with the right-click function Item Data.

• These will also appear in the parts list of the model drawing.

You can create a drawing for the model:

• In the feature tree, select Drawings.
• Right-click function: New Drawing.

Download the hood model (VX_SMD7.vxz) here.