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FreeCAD: Tutorial Mug (2/3)

Update:May 27, 2019
FreeCAD 0.18

Creating a handle

Then we will create a handle of the mug.

  1. Creating a sketch plane for the handle shape.

    create a new sketch planecreate new sketch plane icon and select XZ-Plane in the dialog. Click OK to create sketch plane.

    New sketch plane dialog
    "New sketch plane" dialog
  2. Drawing the handle shape

    Select the polylinepolyline icon and click 4 points to draw a sketch of a handle. Click mouse right button to finish drawing.

    Drawing a sketch of a handle
    Drawing a sketch of a handle

    Click an end point of the polyline on the top side and execute lock constraintconstraint icon. Type (42mm , 75mm) as the coordinate.

    Constraining the coordinate of end point on the top side
    Constraining the coordinate of end point on the top side

    Similarly, click an end point of the polyline on the bottom side and execute lock constraintconstraint icon. Type (42mm , 25mm) as the coordinate.

    Constraining the coordinate of end point on the bottom side
    Constraining the coordinate of end point on the bottom side

    Select the edge of polyline on the top side and constrain to horizontalHorizontal Constraint icon. And select the edge of polyline on the right side and constrain to verticalVertical Constraint icon.

    Constraining the edges to horizontal/vertical
    Constraining the edges to horizontal/vertical

    Select filletfillet icon and click 2 edges of a corner to create fillet. Create fillets on both corners and click mouse right button to finish the operation.

    Creating fillet
    Creating fillet

    Select the edge on top side and execute horizontal dimension constrainthorizontal dimension constraint icon to constrain the dimension to 30 mm. Similarly, select the edge on right side and execute verical dimension constraintverical dimension constraint icon to constrain the dimension to 25 mm.

    Constraining the horizontal/vertical dimension
    Constraining the horizontal/vertical dimension

    Select fillet of each corner and execute radius constraintradius constraint icon to constrain a corner radius to 10 mm.

    Constraining corner radii
    Constraining corner radii

    When both corner radii were constrained, the sketch will be fully contained and be displayed with green lines. Then click Close on Task tab to finish sketch edit.

  3. Creating a sketch plane for a profile of the handle

    At first select "body" in model tree and create a new sketch planecreate a new sketch icon.

    On the creating sketch plane dialog, select XY-plane as a sketch orientation. Click OK to create a sketch plane.

    Dialog for creating a sketch plane
    Dialog for creating a sketch plane
    Sketch plane
    Sketch plane

    When sketch editing mode starts, check "Auto Remove Redundants" on dialog to enable redundant elements removing.

    Auto Remove Redundants
    Auto Remove Redundants
  4. Drawing a sketch of the handle profile

    Select slotslot icon and select 2 points to draw a slot.

    Drawing a slot
    Drawing a slot

    Select 2 centers of the slot and horizontal axis of the sketch plane then execute symmetric constraintsymmetric constraint icon. So the centers of the slot will be constrained symmetrical with the horizontal axis as a line of symmetry.

    Symmetric constraint
    Symmetric constraint

    Select the top side arc of the slot and constarin the radiusRadius constarint to 5 mm.

    Constraining radius
    >Constraining radius

    Select a upper left point of the sketch and execute lock constarintlock constarint icon to constarin the coordinate to (77.5mm , 2.5mm).

    Constraining the coordinate
    Constraining the coordinate

    The sketch will be fully contained and be displayed with green lines. Then click Close on Task tab to finish sketch edit.

    After finishing sketch edit, select the sketch (Sketch002) in model tree and change Z coordinate of "Attachment Offset" - "Position" property on Data tab to 50 mm to offset it.

    Offsets sketch
    Offsets sketch

    So the sketch of the handle profile has beeen drawn.

    Sketch of the handle profile
    Sketch of the handle profile
  5. Sweeping the profile of handle to create solid

    Select the profile sketch (Sketch002) in model tree and execute Additive Pipe (sweeping)Additive Pipe icon to show the dialog.

    Dialog for sweeping
    Dialog for sweeping

    Click Object button below "Path to sweep along" and select the sweep path sketch (Sketch001) on 3D view. Sweeping result will be shown on 3D view. Click OK to execute sweeping operation.

    Sweeping results
    Sweeping results
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