Modeling a mug - Step 1

Summary

What we will create? : Mug
Version of the FreeCAD to be used : 0.16

Mouse operation

Select	Pan	Zoom	Rotate View
			or

Note : FreeCAD has other modes like Inventor mode, Blender mode and touchpad mode. Please refer to FreeCAD Memo - Mouse operation setting.

Creating a basic solid

1. Creating a sketch plane

   Switch workbench to Part Design workbench and create a new sketch plane.

   With default parameter values, click OK button on the dialog.

   Dialog for creating a sketch plane

2. Drawing a sketch of cup part

   Drawing a circle : Select the tool and click 2 point to draw a circle.
   

   Drawing a circle

   
   

   Constraining a radius : Click the circle and select the tool. On displayed dialog, set 40 mm to constrain the radius.
   

   Constraining a radius

   
   

   Constraining a center of the circle : Select a center of the circle and a sketch origin. And select the tool to match the center of the circle with the sketch origin.
   

   Constraining a center of the circle

   
   

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

   finishing sketch edit

3. Extrusion

   Sketch extrusion : Select the created sketch on model tree and execute Pad tool. On a dialog, set 95 mm as extrusion length and click OK.
   

   Dialog for extrusion

   Extrusion result

4. Hollowing the solid

   Switch the workbench to Part workbench to use a tool for hollowing.

   
   Hollowing the solid : Click a top face of the created solid to select and execute the tool. On a dialog, set 4 mm as thickness and click OK.
   

   Dialog for hollowing

   Selecting a face

   Hollowing result