To revolve in Inventor, sketch half of the part’s profile plus a line for the axis, start 3D Model tab > Create > Revolve, pick the axis and click OK. Use the same tool with Cut to make grooves. In this lesson we’ll do both and add a circular hole pattern.
Lesson 2 of my Autodesk Inventor series. In lesson 1 we built a part by extruding a sketch. This time we’ll make a round part by revolving a sketch around an axis, cut a groove into it, add a hole, and then copy that hole around the part with a circular pattern. Here’s the list:
- Sketch and dimension a profile
- Revolve the sketch into a solid
- Cut a groove with Revolve (Cut)
- Make a hole
- Repeat the hole with a circular pattern
Sketch the profile
Start a new part and sketch the profile below on the XY plane, the same way as in lesson 1. Use the dimensions shown, and don’t forget to draw the line you’ll revolve around.
How do I revolve a sketch in Inventor?
- Start Revolve: 3D Model tab > Create panel > Revolve.
- Click the revolve axis line.
You should see something like this:
- Click OK.
How do I cut a groove with Revolve?
Start a sketch on the XY plane
- In the model browser, expand the Origin folder and click the XY Plane.
- Right-click the XY plane and choose New Sketch.
Switch to wireframe
The sketch plane is inside the part, so switch to wireframe to see it.
- Go to View tab > Appearance panel > Visual Style and pick Wireframe.
The part changes to wireframe:
- Use Orbit to turn the part slightly, like this:
Project the edges and draw the groove
- Start Project Geometry: Sketch tab > Create panel > Project Geometry.
- Hover over the vertical line until it turns green, and click it.
- Run Project Geometry again and click the line on the right side.
These are all the lines to project:
- On the View tab, click Look At so you’re looking straight at the sketch.
- Draw the triangle as shown, then delete the projected lines you don’t need.
Revolve the groove
- Start Revolve again (3D Model tab > Create panel > Revolve).
- Select the triangle as the profile, and the axis.
- Change the Boolean to Cut and click OK.
- Switch back to a shaded view: View tab > Appearance panel > Shaded with Edges.
The part should look like this:
Make a hole
- Click the face of the part. It highlights green.
- Right-click it and choose New Sketch.
The view turns so you’re looking at the face from the front:
- Pick the Line tool.
- Draw a vertical line starting at the center.
- Dimension it to 1.5.
- Pick the Circle tool.
- Draw a circle at the end of the line.
- Dimension the circle to a 0.50 diameter.
- Delete the helper line.
- Right-click and choose Finish 2D Sketch.
- Start Extrude.
- Set the direction, distance and Boolean (Cut) as shown, and click OK.
How do I make a circular pattern?
- Start Circular Pattern from the ribbon.
- The dialog opens. Click the hole on the part. Its outline turns green.
- Click Rotation Axis and select the outside edge of the part.
Inventor shows a preview of the pattern:
- Click OK. Done.
Why won’t my sketch revolve?
- The profile is open. Check that the lines connect at every corner.
- The profile crosses the axis. A profile can touch the axis but not cross it.
- No axis picked. Pick the axis line (or a work axis) in the Revolve dialog.
How do I skip an instance in a circular pattern?
Expand the pattern in the model browser, right-click the occurrence you don’t want and choose Suppress.
Next up: Lesson 3: Creating a detail drawing.
