In this article we step through detailed instructions to create a sheet metal part in inventor.

NOTE #1: "Inventor HSM" is now known as "Inventor CAM".

Pre-requisites

Before commencing this article you will need:

• Software installed and configured (for more information refer to our CAD Setup article)

Overview

The steps involved in this article can be broken into the following sections:

(a) Open Inventor and start a sketch

(b) Create a circle for a bearing

(c) Create some more circles

(d) Set dimensions between the circles

(e) Horizontally constrain the circles

(f) Create arcs to complete the perimeter 

(g) Tangent constrain the arcs

(h) Set the radius of the arcs

(i) Trim out the unwanted internal parts of circles

(j) Reapply constraints

(k) Apply equal constraint to geometry that should be symmetrical

(l) Finish the sketch

(m) Select extrude (note: inventor has a guess at what you want to extrude and displays that automatically, if the wrong region or no region has been extruded then hover over the drawing to highlight the different regions that can be extruded, when the correct region is highlighted then left-click to select)

(n) Save part

The sections that follow elaborate on each of these steps.

Open Inventor and start a sketch

1: Launch Inventor

2: If prompted for serial number and product key use the ones emailed to you when you completed the installation (if you followed the instructions above then you will have two emails, one contains the serial number and product key for Inventor, the other email will the serial number and product key for Inventor HSM (see note#1)

3: Select "New" > "New"

4: Select "Templates" > "Metric" > "Standard (mm).ipt" (note the "ipt" extension for a part)

5: Select "Create"

6: If prompted with a "Style Conflict" popup, select "OK"

7: Select "Start 2D Sketch"

8: In the drawing space, select the plane in which you want to create the sketch (e.g. XY)

Create a circle for a bearing

1: Select "Sketch" > "Circle"

2: Left-click on the point 0,0 (centre of the drawing area)

3: Left-click anywhere away from the origin to draw a circle of random size

4: Select "Sketch" > "Dimension" then left-click on the circle

5: Left-click again outside the circle

6: Enter "28.875 mm" in the dimension editor and then "Enter" (or select the tick)

7: Select "View" > "Zoom"

8: Left-click in the drawing area and move mouse backwards and to zoom out so that you can see the full circle

9: Left-click again to turn off zoom function

Create some more circles

1: Using the above method create and dimension five more circles:

• a 60 mm circle with same centre as the first one
• a 5mm circle outside and to the left of the first two circles
• a 5mm circle outside and to the right of the first two circles
• a 30mm circle with same centre as the left 5mm circle
• a 30mm circle with same centre as the right 5mm circle

Set dimensions between the circles

1: Select "Sketch" > "Dimension"

2: Left-click the centre of the left 5 mm circle then left-click the centre of the first circle

3: Drag out the dimension line and enter 50 mm

4: Repeat with the right 5 mm circle

Horizontally constrain the circles

1: Select "Sketch" > "Horizontal Constraint" tool

2: Left-click on the centre of the first circle then left-click on the centre of the right 5 mm circle

3: Left-click on the centre of the first circle then left-click on the centre of the left 5 mm circle

4: Select "Esc" to exit constraint mode

5: Check that at this point all circles are constrained (i.e. all blue)

Create arcs to complete the perimeter 

1: Select "Sketch" > "Arc"

2: Left-click on top of left 30 mm circle then left-click on top of 60 mm circle

3: Left-click on bottom of left 30 mm circle then left-click on bottom of 60 mm circle

4: Left-click on top of right 30 mm circle then left-click on top of 60 mm circle

5: Left-click on top of right 30 mm circle then left-click on top of 60 mm circle

Tangent constrain the arcs

1: Select "Sketch" > "Tangent" constraint tool

2: Left-click on the top left arc then left click on left 30 mm circle

3: Left-click on the top left arc then left click on left 60 mm circle

4: Repeat the last two steps for each of the other three arcs

Set the radius of the arcs

1: Select "Sketch" > "Dimension"

2: Left-click on the top left arc and enter 45 mm

3: Select "Sketch" > "Equal" constraint tool

4: Left-click on the top left arc then left-click on the bottom left arc

5: Left-click on the top left arc then left-click on the top right arc

6: The outside perimeter should now be smooth and all items in the sketch should be constrained

Trim out the unwanted internal parts of circles

1: Select "Sketch" > "Trim"

2: Left-click on the internal part of the left 30 mm circle

3: Left-click on the internal part of the right 30 mm circle

4: Left-click on the left of the 60 mm circle

5: Left-click on the right of the 60 mm circle

6: Select "Esc" to exit trim tool

Reapply constraints

1: Notice that some of the constraints have been "lost", lets correct this . . .

2: Select "Sketch" > "Dimension"

3: Left-click on the top arc, enter 30 mm for the radius

4: Left-click on the bottom arc, enter 30 mm for the radius

5: Select "Sketch" > "Tangent" constraint tool

6: Left-click on top-left arc then left-click on top arc

7: Left-click on top-right arc then left-click on top arc

8: Left-click on bottom-left arc then left-click on bottom arc

9: Left-click on bottom-right arc then left-click on bottom arc

10: The outside perimeter should now be smooth and all items in the sketch should be constrained and there should be no spurious internal lines

Apply equal constraint to geometry that should be symmetrical

1: Resize the right 30 mm circle, make it 45 mm, what happens to the left 30 mm circle? Should be nothing, revert the right circle to 30 mm

2: Remove the diameter dimension from each of the two left circles

3: Use the "Equal" constraint tool to make the two 30 mm circles the same diameter

4: Use the "Equal" constraint tool to make the two 5 mm circles the same diameter

5: Resize the right 30 mm circle to 45 mm again, what happens to the left 30 mm circle this time? It should resize in unison with the right circle. The same for the 5 mm circles.

Finish the sketch and extrude

1: Select "Finish Sketch"

2: Select "3D Model" > "Extrude"

3: Set to 3 mm

4: Left-click on the part, it should now have 3 mm thickness

5: Select "OK"

Save part

1: Select "File" > "Save As"

2: Enter file name (e.g. my.first.bearing.plate.ipt) then select "Save"