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FreeCAD: Tutorial Smartphone Cover (1/3)

Update: April 12, 2018
FreeCAD 0.17

Summary

What we will create?: Smartphone cover

Smartphone cover
Smartphone cover

Model information

A size of smartphone: 123.83×58.57×7.6 mm
A space between smartphone and case: 1 mm 、壁厚さ  1.2 mm
A radius of corner roundness: 11.6 mm

Note: These values are not based on an actual smartphone. If you want to create a smartphone case for REAL smartphone, tune-up the values for the smartphone.

iphone-top
Kelvinsong http://commons.wikimedia.org/wiki/File:IPhone_5S_front_camera.png

Mouse operation

SelectPanZoomRotate
mouse_select_CAD mouse_pan_CAD mouse_zoom_CAD mouse_rotate_CAD or mouse_rotate_CAD2

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

Creating a basic solid

  1. Creating a sketch plane

    Switch workbench to Part Design workbenchWorkbench_PartDesign.

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

  2. Creating a basic shape

    Select rectanglerectangle icon and select 2 points on sketch plane to create a rectangle.

    base1
    Creating a rectangle

    Select filletfillet icon and click 2 edges forming corner. Create a fillet at the four corners by repeating the same operation.

    base2
    Creating fillet
  3. Specifying sizes

    Select the arc and select radius constraintConstraint_Radius to set size of fillet 12.1 mm. Set all fillets to same size by repeating the same operation.

    Constrain fillet radius
    Constrain fillet radius

    Select 2 points from upper edge and lower edge and select vertical distance constraintConstraint_VerticalDistance to set the length of the edge to 124.83 mm. Similarly, select 2 points from left edge and right edge and select horizontal distance constraintConstraint_HorizontalDistance to set the length of the edge to 59.57 mm.

    Constraints vertical/horizontal length
    Constraints vertical/horizontal length

    Select a point on the sketch and constrain it to the origin of sketch plane with coincident constraintConstraint_PointOnPoint. By this operation, the sketch will be fully contained and be displayed with green lines.

    Constrains the position
    Constrains the position
  4. Exiting sketch edit

    Click Close on Task tab to exit sketch edit.

    Exiting sketch edit
    Exiting sketch edit
  5. Extrusion

    Select the created sketch in model tree and execute padpad icon. On a dialog, set 7.6 mm as extrusion length and click OK.

    Before padding
    Before padding
    Padding result
    Padding result

Hollowing the solid

Click a top face of the created shape and select thickness toolthickness tool icon. On a dialog, set 1.2 mm as thickness and click OK.

Select a top face of shape
Select a top face of shape
Hollowing result
Hollowing result
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