FreeCAD Memo - Tutorial "Mug"

Modeling a mug - Step 2

Updated : August 22, 2017

Creating a handle

Then we will create a hndle of the mug.

  1. Creating a sketch plane for the handle shape.

    Switch workbench to Part Design workbenchWorkbench_PartDesign and create a new sketch planeSketcher_NewSketch.
    On the creating sketch plane dialog, select "XZ-plane" and click OK.
    Dialog for creating a sketch plane (XZ-plane) Dialog for creating a sketch plane
  2. Drawing the handle shape

    Sketcher_CreatePolylineDrawing polyline : Select the tool 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

    Sketcher_ConstrainLockConstraining a coordinate : Click an end point of the polyline on the top side and execute the tool. 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

    Sketcher_ConstrainLockConstraining a coordinate : Click an end point of the polyline on the bottom side and execute the tool. 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

    Constraint_HorizontalConstraining a edge to horizontal : Select the edge of polyline on the top side and constrain to horizontal.
    Constraint_VerticalConstraining a edge to vertical : Select the edge of polyline on the right side and constrain to vertical.
    Constraining the edges to horizontal, vertical Constraining the edges to horizontal/vertical

    Sketcher_CreateFilletCreating fillet : Execute the tool and click 2 edges of a corner to create fillet. Create fillets on both corners and click mouse right button to finish creating fillet.
    Creating fillet Creating fillet

    Constraint_HorizontalDistanceConstraining a horizontal dimension of the edge : Select the edge on top side and execute the tool to constrain a horizontal dimension to 30 mm.
    Constraint_VerticalDistanceConstraining a vertical dimension of the edge : Select the edge on right side and execute the tool to constrain a vertical dimension to 25 mm.
    Constraining the horizontal/vertical dimension of edges Constraining the horizontal/vertical dimension of edges
    Constraint_RadiusConstraining corner radii : Select fillet of each corner and execute the tool 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

    Sketcher_NewSketchCreate a new sketch plane.
    On the creating sketch plane dialog, select XY-plane as a sketch orientation and set 50 mm as offset value. Click OK to create a sketch plane.
    Dialog for creating a sketch plane (XY-plane) Dialog for creating a sketch plane
    The sketch plane The sketch plane
  4. Drawing a sketch of the handle profile

    Sketcher_CreateSlotDrawing a slot : Execute the tool and select 2 points to draw a slot.
    Drawing a slot Drawing a slot

    Constraint_SymmetricConstraining the sketch to symmetrical : Select 2 centers of the slot and X-axis of the sketch plane then execute the tool. So the centers of the slot will be constrained symmetrical with the X axis as a line of symmetry.
    Symmetrical constraining Symmetrical constraining

    Constraint_RadiusConstraining a radius : Select the top side arc of the slot and constarin the radius to 5 mm.
    半径の拘束 Constraining a radius

    Sketcher_ConstrainLockConstraining a coordinate : Select a upper left point of the sketch and execute the tool to constarin the coordinate to (77.5mm , 2.5mm).
    Constraining a coordinate Constraining a coordinate

    The sketch will be fully contained and be displayed with green lines. Then click Close on Task tab to finish sketch edit.
    Finish editing the sketch Finish editing the sketch
  5. Sweeping the profile of handle to create solid

    Switch workbench to Part workbenchパートワークベンチ for using a sweep tool.

    Part_SweepSweeping : Execute the dialog to display a dialog. On the dialog, select the profile sketch and specify it to sweep target with right arrow button.
    Specifying a sweep target Specifying a sweep target
    The sweep target sketch The sweep target sketch
    Selecting sweep path : Click Sweep Path and select a sketch edges to be used as sweep path. Multiple edges can be selected by clicking with pressing Ctrl key. Click Done to finish selecting.
    Selecting sweep path Selecting sweep path
    Sweeping : Check Create solid and click OK to sweep.
    Sweeping result Sweeping result

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