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FreeCAD: Extruding a cross-sectional shape along the curve (Sweep)

Update: February 12, 2017
FreeCAD 0.17

In this example, I explain how to create a solid by extruding a cross-sectional shape along the curve. Following shapes can be created by this method.

Bend Spiral Branches
  1. Click [File]-[New] in menu bar and create new document.

  2. Select [View]-[Workbench]-[Part Design] in menu bar to switch to Part Design workbenchPart Design workbench.

  3. First we create a curve. This curve is used as pathway of extruding.

    1. Create new sketch planeSketcher_NewSketch on XY-plane.

      Create Sketch Plane Creates sketch plane
    2. Create two linesSketcher_Line and an arcSketcher_Arc as shown in following figure. You can set these positions in rough because these will be adjusts in the restraint operation.

      Sketch Step 1
    3. Connnect the three wires with Coinciden constraintConstraint_PointOnPoint.

      Sketch Step 2
    4. Connect a center of circular arc and joint points of the wires with linesSketcher_Line and apply Vertical constraintConstraint_Vertical and Horizonal constraintConstraint_Horizontal to these points.

      Sketch Step 3
    5. Select two lines forming the arc and switch them to auxiliary linesSketcher_ToggleConstraint. Auxiliary lines are displayed in blue color.

      Sketch Step 4
    6. At the end, select a end point at left lower and set it's coordinate to (0, 0) with Lock constrainSketcher_ConstrainLock. After adjusting each point's coordinate by dragging them, click Close at Task tab in Combo View to exit sketch editing mode.

      Sketch Step 5
  4. Next we create cross-sectional shape to be extruded.

    1. Select the document in Tree View and create new sketch planeSketcher_NewSketch on ZY-plane.

      Create Sketch Plane-YZ Creates sketch plane
    2. Create a circleSketcher_CreateCircle as shown in following figure. You can set positions in rough because these will be adjusts in the restraint operation.

      Sketch Step 6
    3. Select a center of the circle and set it's coordinate to (0, 0) with Lock constrainSketcher_ConstrainLock.

      Sketch Step 7
    4. Select the circle and apply Radius constraintConstraint_Radius. In this example, we set radius to 5. After that, click Close at Task tab in Combo View to exit sketch editing mode.

      Sketch Step 8
  5. Following figure shows the two sketches that has been created above steps.

    Sketch Step 10
  6. Select [View]-[Workbench]-[Part] in menu bar to switch to Part workbenchPart workbench. In the workbench, Select SweepPart_Sweep.

  7. At first, select a cross-sectional shape (Sketch001) and click to set the cross-sectional shape as sweep-target.

    Sweep Task
  8. Then click Sweep Path and select a pathway of extruding in 3D View. If you want to select more than one line, select lines with pressing Ctrl key. Click Done to finish selecting.

    Sketch Step 10
  9. After selecting the pathway, check Create solid at bottom left of the dialog and click OK on Sweep dialog to create a solid by sweeping.

    Bend

Any cross-sectional shape can be extruded along the curve with this sweep method. In following figure, a regular pentagon has been extruded along with a spiral that has been created with Creating primitivesPart_CreatePrimitives in Part workbench.

Spiral

You can sweep while changing the cross-sectional shape (It is usualy called "Sweep Blend") by using multiple cross-sectional shapes.

Sweeping-Blend1 Sweeping-Blend2

If a pathway of extruding has branching, the pathway cannot be extruded one sweep operation. So sweep each pathway and connect the two solids by a boolean operationPart_Fuse.

Branches