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 (a line and a tangent arc), preferably using the Sketcher Workbench.
  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 with the Sketcher Workbench.
  5. Use the PartDesign Pocket command to cut off one half of the Round bit.
  6. Create a hole pattern with 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.
  9. 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:
    BaseBend object and highlighted sketch
    • 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.
  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 Sketcher 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
  10. One side is finished. We now need to find a way to mirror the body.

Potential mirror options:

  • The PartDesign Mirrored command fails because it cannot handle SheetMetal features for some reason. So that does not work.
  • The Part Mirror command creates a mirrored part, but this is no longer unfoldable. So that does not work either.
  • One way that can work is to use a clone. This still can't be mirrored, but it can use axial symmetry (turn it 180°).
  • Another way that works is to use a link object.

Mirror using a clone:

  1. Select the body from the tree view.
  2. Use the PartDesign 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 fuse both halves.
    Fused halves
  4. Activate the Unfold command to get an Unfold object.
    Clip and Unfold object Unfold object
  5. Done!

Mirror using a link object:

  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
  8. 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)

SheetMetal properties

This section tries to explain the properties of each SheetMetal object with simple images, where applicable.

BaseBend object

Selected sketch + Make Base Wall → BaseBend object with default settings


Edit Datalength: Default length → Reduced length


Switch DataMid Plane from false to true: Extrusion in one direction → Symmetric extrusion


Switch DataReverse from false to true: Default direction → Inverted direction


Select DataBend Side: Outside (default) → Inside Middle


Edit Dataradius: Default radius → Enlarged radius.
This property is the inner radius of the bends created at the vertices where two edges in the sketch have a non-tangential transition.


Edit Datathickness: Default Thickness → Enlarged thickness