FreeCAD Memo

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

1/5/2015
Version 0.14
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.
Creates 2 solids
Creates 2 solids
Creates 2 solids
  1. Click [File]-[New] in menu bar and create new document.
  2. Select [View]-[Workbench]-[Part Design] in menu bar and move to Part 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
    2. Create two straight linesSketcher_Line and a arcSketcher_Arc as shown in following figure. You can set these positions in rough because these will be adjusts in the restraint operation.
      Draw sketch
    3. Connnect the three wires with Coinciden constraintConstraint_PointOnPoint.
      Connect sketchs
    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.
      Constraint sketchs
    5. Select two straight lines forming the arc and switch them to auxiliary linesSketcher_AlterConstruction. Auxiliary lines are displayed in blue color.
      Change line type
    6. For a finale, 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 and exit sketch editing mode.
      Constraint a point
  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.
      Creates a sketch plane
    2. Create a circleSketcher_Circle as shown in following figure. You can set positions in rough because these will be adjusts in the restraint operation.
      Create a circle
    3. Select a center of the circle and set it's coordinate to (0, 0) with Lock constrainSketcher_ConstrainLock.
      Constraints a point
    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 and exit sketch editing mode.
      Constraints a radius
  5. Following figure shows the two sketches that has been created above steps.
    Sketches
  6. Select [View]-[Workbench]-[Part] in menu bar and move to Part workbench. In the workbench, Select SweepPart_Sweep.
  7. At first, select a cross-sectional shape (Sketch001) and click right arrow to set the cross-sectional shape as sweep-target.
    Sweep dialog
  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.
    Sweep result
  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.
    Select sweep path
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 sweep
You can sweep while changing the cross-sectional shape (It is usualy called "Sweep Blend") by using multiple cross-sectional shapes.
Sweep blend sketches
Sweep blend
Note:
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.
Sweep example