FreeCAD: Tutorial Mug (2/3)

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 plane and select XZ-Plane in the dialog. Click OK to create sketch plane.

   

2. Drawing the handle shape

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

   

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

   

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

   

   Select the edge of polyline on the top side and constrain to horizontal. And select the edge of polyline on the right side and constrain to vertical.

   

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

   

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

   

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

   

   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

   Select the vertical edge of the created sketch in the 3D view and make a datum plane. A datum plane is an imaginary plane that can be used as a reference plane.

   

   Make sure that "Normal to edge" is selected for Attach Mode in the dialog and click OK to make a datum plane.

   

   

   Select the created datum plane in the 3D view and make a new sketch to make a new sketch on the datum plane.

   

4. Drawing a sketch of the handle profile

   Select slot and select 2 points to draw a slot.

   

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

   

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

   

   Select a upper left point of the sketch and execute lock constarint to constarin the coordinate to (-5mm , 2.5mm).

   

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

   So the sketch of the handle profile has beeen drawn.

   

5. Sweeping the profile of handle to create solid

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

   

   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.

   The datum plane will not be used in following, so select "DatumPlane" on the model tree and press the space key to hide it.