Exercise 1:  Extrude – Add and Subtract Material

Step 1:  Create new Design file. 

Step 2:  Save using filename Table.

Step 3:  Select workplane Base and sketch Initial 

Step 4:  Orient plane to begin sketch by selecting the icon

              You should see the following screen:

Step 5:  Select sketch rectangle icon

 LMC[1] and drag to any position to form a rectangle.   

Step 6:  Create the dimensions for length and breadth by selecting Sketch Dimension icon

              select one side of the rectangle, drag the cursor out to place the dimensions. 

  Do the same for the other side of the rectangle.

Step 7:  To modify the dimensions, LMC on the dimension and then double-click.  The

  following box will appear:


            Likewise, change the breadth to 750.

Step 8:  Re-orient to look at the sketch in 3-D view as shown by selecting   

Step 9:  Select Extrude function and extrude the rectangle by keying in 500mm as circled in the diagram:

Note that the default is Add Material and Above Workplane
 


Step 9:  Select OK or simply hit the Return key.

Now, we are going to create the legs of the table by subtracting material from this rectangular extrusion.
 

Step 10:  Select the Face icon.


  Select the front face of the rectangular extrusion by clicking on the perimeter that  

  is highlighted.  You will know you have selected the right face when it turns red.

Step 11:  RMC[2] to activate menu and select New Sketch.  You should see the following

    screen as shown:


Step 12:  Sketch a rectangle with dimensions as shown and extrude by dragging point across. 

    Make sure this extrusion clears the other side of the table.

Click and drag this point across.
 


Step 13:  Select OK when done.

Step 14:  Select the other face of the rectangular extrusion and follow the same steps to

   subtract material as shown:

 


Step 15:  The table model is complete with the four legs as shown:

Step 16:  Save and Close File.

Practice:  Create a new design file Glass_Top and extrude a rectangular glass top (750 x 500) of thickness 8mm for the table as shown: 

 


To create a pencil holder by revolving a half-cross-sectional profile.
 
Exercise 2:  Revolve and Trim Sketch

Step 1:  Create a new design file. 

Step 2:  Save file with filename Pencil_holder.

Step 3:  Select Frontal Plane

 and RMC[3] and select new sketch.  The following menu will appear


Step 4:  Orient the sketch plane to begin sketch. 

Step 5:  Create a vertical line for axis of revolution.  RMC and toggle it to Construction line.

  Dimension it to 100mm. 

Step 6:  Constrain the line from moving by applying the G-clamp.

 


Step 6:  Create half the profile of the pencil holder about the same height as the axis of revolution.

Trim off the excess lines using
 


           

If the profile is does not have any gaps, stray or overlapping lines, the internal area will be highlighted and the profile can then be extruded or revolved. 

 



Step 7:  Re-orient to 3-D view and select Revolve function.  Revolve the profile to 360o as

  shown:

 


Step 9:  The pencil holder is revolved as shown.

Step 10:  Save and close file.


Trim off excess lines and arcs to obtain a close profile.
 

Revolve 360o to obtain solid as shown.
 

Sketch on Lateral or Frontal Plane. Add constraints and dimensions as desired.
 
 


Exercise 3:  Creating Rounds and Chamfers


Step 1:  Open existing file Pencil_holder.

Step 2:  Select Edge icon:

Step 3:  Select the edges that will have the same fillet radius.  To continue selecting one edge

  after another, press the SHIFT key down.


Step 4:  RMC and select the Rounds function.  The following menu will appear:


Step 5:  The rounds are formed as shown:

Step 6:  To create chamfers, select edges to be chamfered using Edges icon as before.

Step 7:  RMC and select Chamfer Edges function.  The following menu will appear:

              You can choose Equal setback, Unequal setback or Angle setback (which are self-

  explanatory) and key in the required values.

Step 8:  Create the following chamfer on the pencil holder model.

 


 


Exercise 4:  Shell Solids, Duplicate and Pattern


Step 1:  Create a new Design file, Pencil_case.

Step2:   Create a rectangular extrusion with the following dimensions 100 x 40 x 10. 

 Round the four edges with fillet radius = 5mm as shown:

Step 2:  To hollow out a cavity, select the Face icon and select the top face of the extrusion.

Key in the thickness of the box.
 
Step 3:  RMC and select the Shell Solids icon.

Step 5:  The box is shelled as shown:
 
 


If you do not choose any surface before shelling it, then a hollow will be created inside the box as shown:

Now, we are going to create holes using Duplicate function.

Step 1:  Select the Face icon, select the front face and activate a new sketch on this face.

Step 2:  Sketch a circle at one corner of the face as shown and dimension the centre from the two edges:

The default is Rectangular.  Key in the number of holes and spacing between holes in the two directions: X and Y.
 
Step 3:  Before extruding the hole, RMC to select the Duplicate function.

Step 4:  The result is as shown:

Step 5:  Extrude the holes using subtract material as shown:

Step 6:  Select OK and obtain the resulting model as shown:


Step 1:  Extrude a hole on the front face as shown:

Step 2:  Select the hole to pattern.  RMC and select Pattern function.

Step 3:  Select 1st direction to pattern:

LMC on green arrow will toggle direction.  Make sure arrow is pointing in the direction of pattern.
 

Key in the number of holes and spacing between holes.

 
 


Step 4:  Select 2nd direction to pattern:

 


Step 5:  Select OK and obtain the following holes as before:

Additional Exercise: 

Create a mirror holder as shown:
 


Extrude this profile symmetrically by sketching on the Lateral plane
 
You could try using the following steps:

Round off all the edges as shown.
 

(a)  Create a recess for the mirror using extrusion.

(b)  Create the pattern using Duplicate – Circular.

       Then either extrude to get holes or protrusions.
 
 


Exercise 5:  Redefine and Mirror


Step 1:  Open existing file Pencil_case.

Step 2:  Use Save Copy As to create another file and name it Pencil_case_cover.

Step 3:  Close file Pencil_case and open file Pencil_case_cover.

Step 4:  To delete the holes, select Features and select Pattern1 which is the holes creation.


Step 5:  Click on the Update icon. 

Step 6:  The patterned holes are deleted with the original hole remaining as shown:

Step 7:  Delete the original hole using the same method.

Step 8:  To change the height of the cover, redefine the extruded box. 


Step 9:  Change the height of the cover.

Step 10:  Click Update icon to update changes made. 

Step 11:  Redefine the thickness of the Shell to 0.5mm.  Update when done.  The resulting

    pencil_case_cover is observed:

Next, we are going to create some designs on the cover and then mirror them.

Step 1:  Rotate the box so that bottom is at the top.

Step 2:  Select the Face icon and then select the top face.

Step 3:  RMC to activate a new sketch on this surface.

Step 4:  Sketch a close profile using Spline to sketch and then extrude. 

Step 5:  Select Features and RMC on extrusion 6.  Select mirror from the menu.

Step 6:  Change to Workplane on the Mirror Feature menu


Step 7:  Select Workplane on this menu and click on the Lateral:

Step 8:  The feature is mirrored across the Lateral plane as shown:

Exercise 6:  Loft, Sweep and Offset Planes

 


Step 1:  Create a new design file and saved it as Vase.

Step 2:  Using the Initial Sketch on the Base plane, create an ellipse as shown:

Step 3:  Select New Workplane from the Workplane menu:

 


Step 4:  Activate a new sketch on this workplane and sketch a rectangle

Step 5:  Create another new workplane 100mm offset from the previous workplane.

Step 6:  Create a new sketch on this workplane and sketch a circle:

Step 7:  Select Loft function from the menu and click the 3 profiles as shown:

 


Step 8:  Select Ok and obtain the resulting vase:

Step 9:  You can now select the top face and Shell the vase.

 


Step 1:  Create a new partfile and save it as Paper_clip.

Step 2:  Select Frontal plane and activate New Sketch to sketch the profile.

Step 3:  Sketch a circle of diameter 1mm at 0,0.  You will have to zoom out a few times to

  sketch this circle as the diameter is very small.

Step 4:  Select the Base Plane and Initial sketch to sketch the trajectory. 


Trim the horizontal lines using 

 

Use Arc icon to create tangent arcs.
 


Step 5:  Select the Sweep command from the Features pull-down menu and select

  Along Sketch Path.  The following menu will appear:

 

 


(1)  Create a helical sweep on the profile shown:

(2)              Create a mouse using Loft and the cable using

Sweep as shown:

Exercise 7:  Deform, Project and Angled Planes

To use Deform to give a dome shape to a flat surface. 

To create a profile at an angle to this deformed face and project onto it.

 

 


Step 1:  Create a rectangular extrusion of dimensions 100 X 60 X 30mm.

Step 2:  Select the Face icon     and then select the top face of the box.

Step 3:  Select Modify Solids from the Feature menu and select Deform Face.

 


Step 4:  The top face is deformed as shown:

Now, we are going to create a profile at an angle to this surface.

Step 1:  Create a plane at and angle of 45o.


Step2:  Select New Sketch on this angled workplane.

Step 3:  Sketch the following profile:

Hint:  Sketch a rectangle, trim away the top edge and use Arc to draw the tangent arc.
 


Step 4:  Select Project from the Features menu:


Step 5:  The solid is formed as shown:

Practice:  Create a cup using the steps shown:
 

Create a handle using Sweep.
 

Deform and Round the inner base.
 

Join handle to cup using Project.
 


Exercise 8:  Assembly and Album

Exercise 8-1:  Assembly of Wooden Blocks

Step 1:   Create new design file for assembly.

Step 2:   Select menu Assembly > Add Component .   Select file called BLOCK.

  The component will be assembled on your design.

Step 3:   Add another component by using the same block again.

   Assembly > Add Component     -   Click on the same file BLOCK again.

   Now two identical parts was assembled on the assembly on the same location.

Step 4:  Click on the part and drag with the mouse to move one part away as shown below.

Select these two faces.
 


Fix this part.
 

Step 5:  Assembly > Fix Components   -   to fix the lower part in location.

Step 6:  Select > Faces   -   Click on the two faces as shown above. 

 To select the second face,  press the shift key.

Step 7:  Assembly > Mate    -   This command will mate the two faces.

The screen will appear as below.

Select these two faces to do a align offset
 

Select these two faces to align it
 

Step 8:  Select the two side faces as shown above with the shift key depressed.

Step 9:  Assembly > Align  -  This will align the two faces.

Step 10:  Finally do a align offset of the two front faces by 10 mm.

   Your assembly is completed as shown below.

Step 11:  Save the assembly as WOODASM.

Exercise 8-2:  Assembly of box with rotable cover

Step 1:  File > New > Design  -   To start the assembly.

Step 2:  Add the components Pencil_Case_Bottom and Pencil_Case_Top.

Step 3:  Click on to the box and drag with the mouse to separate it as shown below.

 


Step 4:  Fix the pencil_case_bottom.

Step 5:  Select > Faces  - Select the two side faces as shown above and align it.

Step 6:  Select > Edges  - Select the two edges and constraint by centre axes.

Step 7:  Select > Parts   -  Click on the upper part to select it.

Step 8:  With the mouse button depressed, move your mouse, you will see that lid will rotate

  about the constrained edge.

Step 9:  Save the file as PENCIL_CASE_ASM.

Exercise 8.3 - Assembly of the Mirror and frame


7 Align these two faces.
 

3 Fix this.
 

Step 1:  File > New > Design

Step 2:  Assembly > Add Component   -  Select the mirror frame part that you had created.

Step 3:  Assembly > Fix Component    -  To fix it in position.

Step 4:  Assembly > Add Component   -  Select the mirror part.

Step 5:  Click on it to move it to a convenient position.

Step 6:  Click the two faces as shown and do a centre axes.

Step 7:  Click on the top face and align it to the mirror frame.

Step 8:  Save the design as MIRRASM.


Exercise 9:  Creating Album

Step 1:    With the table assembly still opened, select File > New > Photo Album

Step 2:    Select Image > New Image > OK

Step 3:    Select > Parts   -  Click on the table part.

Step 4:    Down drop the Images box on you right and choose Materials.

Step 5:    Click on Non-metals.  Left click on wood > Apply Material

Step 6:    Click the Update button to update the image.

Step 7:    Click on the table-top.

Step 8:    Left click on glass > Apply Material.

Step 9:    Update.

Step 10:  For the mirror, select the face.

Step 11:  Left click on mirror > Apply Material.

Step 12:  Update.

Step 13:  Continue to apply materials until you are satisfied with the display.

Step 14:  Select Image > Image Properties, Studio > Lighting.  -   Choose Room Lighting,

OK.

Step 15:  Select Image > Image Properties, Effects > Background  - Snow, 0K.

Step 16:  Update.

Or you can also change the background by the custom menu on your left, left click on brick

> Apply Background.

Step 17:  Update.

Step 18:  Save Album TABLEASM.