SheetMetal Examples

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Introduction

The SheetMetal workbench has grown quite powerful now and it demands an appropriate documentation.

To avoid the overcrowding of the tool pages with examples this page was added to collect parts showing and explaining special SheetMetal features.

Planned phases to generate content:

  1. Collecting pictures
  2. Adding workflow descriptions
  3. Adding more detailed tutorials

Hinge



Workflow Hinge: Make Base Wall, PartDesign Pocket, PartDesign Hole, Unfold.

Hinge Step by Step

  1. Create a profile, preferably using the Sketcher Workbench. (A line and a tangent arc)
  2. Activate the Make Base Wall command to create a BaseBend object.
  3. Edit the BaseBend object's parameters:
    • Set DataMid Plane to trueto let the profile extend symmetrically to both sides of the sketch plane.
    • Set Dataradius and Datathickness to values of your choice.
  4. Create a cut-out contour, preferably using the Sketcher Workbench.
  5. Use the PartDesign Pocket command to cut off one half of the Round bit.
  6. Create a hole pattern, preferably using the Sketcher Workbench.
  7. Use the PartDesign Hole command. Avoid the countersink and counterbore options to keep the body unfoldable.
  8. Activate the Unfold command to get an Unfold object.
Done!

Paper Clip



Workflow Paper Clip: Make Base Wall, Sketch on Sheet, clone, flip and fuse, Unfold.

Paper Clip Step by Step

  1. Create a profile, preferably using the Sketcher Workbench on the XZ plane.
    Profile sketch
  2. Activate the Make Base Wall command to create a BaseBend object.
  3. Edit the BaseBend object's parameters in the properties panel:
    • Set DataMid Plane to trueto let the profile extend symmetrically to both sides of the sketch plane.
    • Set Datalength to 32 mm.
    • Set Dataradius to 2 mm.
    • Set Datathickness to 0.3 mm.
      BaseBend object and highlighted sketch
  4. Select the face between the round sections and activate the Sketcher Workbench.
    Face to support the sketch
  5. To hide the curled part use the Sketche View section command.
  6. Create the cut-out contour.
    Cut-out contour
    Cut-out contour slightly touching the selected face
  7. Finish the sketch using the Sketcher Leave sketch command.
  8. Select the face again and add the Cut-out sketch to the selection.
    Face and sketch selected
  9. Use the Sketch on Sheet command to cut around the curled bit.
    Finished first half

Now one side is finished and we need to find a way to mirror the body.

  • The PartDesign Mirrored command fails, because it can mirror features but not bodies and SheetMetal features seem to be not valid in this case.
  • The Part Mirror command creates a mirrored part, but this is no longer unfoldable.
  • One way is to use clone. This still can't be mirrored, but it can use axial symmetry (turn it 180°).
  • Another way is to use link objects.

The flip a clone way:

  1. Select the body from the tree view
  2. Use the Create a clone command. It adds a new body containing a clone object.
    To apply a 180° turn set the DataAngle under the Placement property of either the body or the clone to 180°. (Z axis is default and should be fine if you started on the XZ plane as described)
    Cloned half Flipped cloned half
  3. With the body still active, use the PartDesign Boolean operation command to add the body of the clone and finally to fuse both halves.
    Fused halves
  4. Activate the Unfold command to get an Unfold object.
    Clip and Unfold object Unfold object
Done!

The link objects way:

  1. Select the body from the tree view.
  2. Use the Make link command. This adds a new link object.
  3. Duplicate the link object by setting the property DataElement Count to 2.
  4. To apply a 180° turn set the DataAngle under the Placement property of either of the sub-linked objects to 180°. (Z axis is default and should be fine if you started on the XZ plane as described)
  5. Select both sub-linked objects in the tree view.
  6. Activate the Part Fuse command to fuse both halves.
    Fused halves
  7. Activate the Unfold command to get an Unfold object.
    Clip and Unfold object Unfold object
Done!

Omega Clamp



Workflow Omega Clip: Make Base Wall, PartDesign Hole, PartDesign Fillet, Unfold.

Hex Bowl



Workflow Hex Bowl: Make Base Wall, Make Wall, 6x Add Corner Relief, Unfold.

When a Corner Relief is added (right side) it can be necessary to adjust the value of the Size property.

Pen Clip



Workflow Pen Clip: Make Base Wall, PartDesign Pocket, 3x Make Wall, Unfold.

Extend Face Example



Workflow Extend Face Example: Make Base Wall, Make Wall, Extend Face, Extend Face, Unfold.

For the second use of Extend Face a Sketch with two contours is used for shape of the extension(s); and with the value of "use subtraction" set to true it provides the shape for the cut-outs, as well

USB shield contact



Workflow USB shield contact: Make Base Wall, Extend Face, PartDesign Pocket, Extend Face, Make Wall, Unfold.

(The pull relief is just an artistic expression of what could be hidden inside a real plug)