In this exercise you will:

• create a valid profile
• toggle lines to construction
• toggle lines to fixed
• apply constraints
• extrude
• chamfer
• mirror a solid
• save parts
• assemble parts
• duplicate parts
• Centre Axes
• Align faces

• Select the Lateral plane

• add a new sketch naming it Profile

• view onto the Profile sketch (Shift + w)

• select the Straight line tool

• draw a vertical line

• select the line using the Select Line tool

• from the Constraints menu select toggle fixed

• select the Sketch Dimension tool

• add a constraint to the length of the line

• select the Select constraint tool

• set the constraint for the length of the line to 100

• select the Straight line tool

• attach an inclined line to the top of the 100 line

• constrain the length of the inclined line to 70

• constrain the angle between the lines to 135 degrees

NOTE Toggle fixed prevents the part from moving when other objects are attached to it.

• draw a line inclined down to the left from the top of the 70 line

• constrain the length of the new line to 110

• select both inclined lines

• from the constraints menu select Perpendicular

• draw a vertical line down from the end of the 110 line

• draw a horizontal line towards the left from the bottom of the 100 line

• use the Delete Line Segments tool to trim any overhanging lines

• select the Straight line tool

• move to the coincident point of the 70 and 100 lines (where the two lines cross)

• draw a line down to the left at approximately 45 degrees

• from the Line menu select toggle construction

• select the new construction line and the 110 line

• from the Constraints menu select Parallel

NOTE Toggle construction changes drawing objects to construction lines. Construction lines are ignored when a profile is being created.

• select the line tool

• move to the bottom of the 110 line

• draw a line down to the right at approximately 45 degrees

• from the Line menu select toggle construction

• select the new construction line and the 70 line

• from the Constraints menu select Parallel

• select the Circle tool and draw three circles approximately as shown

• use the Line Select tool to select a circle and the adjacent construction line

• from the Constraints menu select Tangent

• repeat this operation to make all three circles tangent to the construction lines

• use the Sketch Dimension tool to apply a constraint to a circle

• select the Constraints tool to set the diameter to 12

• repeat this for each circle

Extrude the profile

• from the Features menu select Extrude

• extrude the profile a distance of 12

• select the two vertical and two inclined edges

• from the Features menu select Chamfer

• set the distance of chamfer to 6

• from the File menu select Save

• save the design giving it the name RIGHTEND

• from the File menu select Save Copy As

• give the copy the name LEFTEND

Create second end

• Open the file LEFTEND

• rotate the end similar to that shown

• select the bottom surface

• from the Features menu select Modify Solids then Mirror Solids

• untick the Keep original solids box

• from the File menu select Save

Create Dowel

• open a new design

• on the initial sketch draw a circle

• constrain the circle to a diameter of 12

• extrude a dowel 300 long

• from the File menu select Save

• name the design Dowel

Assemble Parts

• open a new design

• from the Assemble menu select Add Component

• locate and select the RIGHTEND in the list of files

• use the Select Parts tool to select the RIGHTEND

• from the Constraints menu select Toggle Fixed

NOTE Toggle Fixed prevents this part from moving when other parts are added to the design and constrained in relation to it.

• from the Assemble menu select Add Component

• locate and select the LEFTEND in the list of files

• from the Assemble menu select Add Component

• locate and select the DOWEL in the list of files

• select the Select Parts tool

• select the dowel

• from the Edit menu select Duplicate

  • select the Rectangular tab
  • set Number to 3

  • select Spacing to 20

• click OK to duplicate the dowel

• select the Select Faces tool

• select the surface of one dowel and the inside surface of a hole as shown

• from the Assemble menu select Centre Axes

• centre the axes of all dowels

• select the end face of one dowel and the face of the right end

• from the Assemble menu select Align

• repeat the alignment process for each dowel

• select the surface of the middle dowel and

• the inside surface of the middle hole in the left end

• from the Assemble menu select Centre Axes

• rotate the design using the arrow keys

• select the end of the middle dowel and the outside surface of the end

NOTE

• The outside surface is the surface which is chamfered.
• The outside surface of the end may not be facing outwards.

• From the Assemble menu select Align

select the outside of another dowel and

• the inside of the matching hole

• from the Assemble menu select Centre Axes