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FreeCAD: Sweep with a 3D sketch

FreeCAD 0.20

Summary

In the Part Design workbench, you can combine multiple sketches with a subshape binder binder icon to create a 3D sweep path and it can be used to create a additive pipeadditive pipe icon.

Fig. Additive pipe with 3D sweep path
Additive pipe with 3D sweep path

Steps

  1. Start FreeCAD and create new documentNew document icon.

  2. Select PartDesign workbenchSketcher workbench.

  3. Create new sketch planeSketcher_NewSketch and select XY-Plane in shown dialog. Click OK to create new sketch plane.

    Fig. Creates new sketch
    Creates new sketch

  4. Draw a sketch as shown below with PolylinePolyline icon and FilletFillet icon.

    Fig. Draws polyline
    Draws polyline

  5. Click Close at Tasks tab in Combo view to exit sketch editing mode.

  6. Select "Origin" in Tree View and push a space key to show it.

    Fig. Shows Origin (in Tree View)
    Shows "Origin" (in Tree View)
    Fig. Shows Origin (in 3D View)
    Shows "Origin" (in 3D View)

  7. Select an end point of the sketch in 3D view and create datum planedatum plane icon. Push Reference2 button and select XZ plane in 3D view.

    Click OK to create a datum plane that parallel to the XZ plane with the sketch endpoint as the origin.

    Fig. Datum plane parameters
    Datum plane parameters
    Fig. Creates a datum plane
    Creates a datum plane

  8. Select the datum plane in 3D view and create new sketchSketcher_NewSketch on the datum plane.

    In a similar way as first sketch, draw a sketch with PolylinePolyline icon and FilletFillet icon. Then set an end point of the sketch to the origin of the sketch plane with coincident constraintcoincident constraint icon.

    Fig. Edits a sketch
    Edits a sketch

  9. Click Close at Tasks tab in Combo view to exit sketch editing mode. Now all sketches that will be used as a sweep path have been created.

    Fig. sketches for a sweep path
    Sketches for a sweep path

  10. Select the end point of the created sketch and create an another datum plane「データム平面」アイコン. Push Reference2 button and select XY plane in 3D view. Click OK to create a datum plane that parallel to the XY plane with the sketch endpoint as the origin.

    Fig. Datum plane parameters
    Datum plane parameters
    Fig. The datum plane
    The datum plane

  11. Select the new datum plane in 3D view and create new sketchSketcher_NewSketch. Then draw a circle「円の作成」アイコン centered at the origin. This circle will be used as profile to be swept.

    Fig. Draws a profile sketch to be swept
    Draws a profile sketch to be swept.

  12. Click Close at Tasks tab in Combo view to exit sketch editing mode.

  13. When all the sketches are drawn, it look like as shown below. Since the datum plane will not be used hereafter, select them on Model tree and push space key to hide them.

    Fig. The sketches (on Model tree)
    The sketches (on Model tree)
    Fig. The sketches (in 3D view)
    The sketches (in 3D view)

  14. A sweep path consisting of multiple sketches cannot be swept as is, so it must be combined into one.

    While holding down the Ctrl key, select the sweep path sketches "Sketch" and "Sketch001" on the Model tree and create a subshape bindersubshape binder icon. Then the sketches will be combined into one subshape binder.

    After creating the subshape binder, select "Sketch" and "Sketch001" on the Model tree and push space key to hide them.

    Now we can sweep the sketches to make solid.

    Fig. Subshape binder (on Model tree)
    Subshape binder (on Model tree)
    Fig. Subshape binder (in 3D view)
    Subshape binder (in 3D view)

  15. Select "Sketch002", the sketch for the sweep profile on the model tree and create additive pipeadditive pipe icon.

    Confirm that "Sketch002" is set as the profile and Push Object button in "Path to sweep along" then select subshape binder in 3D view to set it as path to sweep.

    Fig. Additive pipe parameters
    Additive pipe parameters
    Fig. Additive pipe (preview)
    Additive pipe (preview)

  16. Click OK at Tasks tab in Combo view to create additive pipe with sweeping.

    Fig. Additive pipe (on Model tree)
    Additive pipe (on Model tree)
    Fig. Additive pipe (in 3D view)
    Additive pipe (in 3D view)

  17. After creating the additive pipe, if you re-edit the sketch and change the dimensions of each part, the final shape will be updated according to the change.

    Fig. Re-edits the sketch to update the shape
    Re-edits the sketch to update the shape

References