If you’re new to Autodesk Inventor, start by modeling one simple part: a 2D sketch, dimensions, an extrude, a fillet and a couple of holes. That covers the workflow you’ll use for almost every part. This lesson walks through it step by step.
This is the first lesson in my Autodesk Inventor series. We’ll model one small part from scratch: a small 1/4″ thick part with rounded ends, a plain hole and a counterbored hole. Along the way you’ll use the tools you’ll need in every Inventor model after this:
- Starting a part and a 2D sketch
- Dimensioning a sketch
- Trim and Extend
- Extruding a sketch into a solid
- Fillets
- A hole made with a sketch and Extrude
- A counterbored hole made with the Hole tool
Tip before you start: if the mouse wheel zooms the “wrong” way for you, here’s how to reverse it.
How do I start a new part?
- On the Get Started tab, click New.
- Choose Standard.ipt and click Create.
How do I start a sketch?
- On the 3D Model tab, click Start 2D Sketch.
- The origin planes appear. Click the XY plane (it highlights green).
Draw the outline
- On the Sketch tab, click Line.
- Click once in the lower left part of the screen.
- Click again somewhere to the right. That’s your first line.
- Keep going and draw the bottom part of the shape.
When you draw the last line of the box, watch for the green dot. It means Inventor snapped to the end of the other line.
You’ll also see small perpendicular and parallel symbols pop up while you draw. They tell you the line you’re drawing is perpendicular or parallel to another line, and Inventor adds that as a constraint.
- To get out of the Line command, right-click and choose OK, or press Esc.
How do I dimension a sketch?
- Start Dimension: Sketch tab > Constrain panel > Dimension.
- Click the bottom line. The dimension sticks to your cursor. Move down and click to place it.
- Type 2 and press Enter. The line becomes 2″ long.
- Do the same on the side line with 0.25.
- Finish the rest of the shape with the Line tool.
Trim
- Start Trim: Sketch tab > Modify panel > Trim.
- Hover over the piece of line you want to remove. It turns dashed. Click it.
The segment is trimmed:
Extend
- Delete the extra line you don’t need anymore.
- Start Extend: Sketch tab > Modify panel > Extend.
- Hover over the line you want to extend. It highlights and shows a preview. Click it.
The line extends to the next line:
Finish the sketch
Add the rest of the dimensions.
For the 0.25″ thickness, you can dimension between the two line ends, where you see the green dots:
When you’re done, right-click in the workspace and choose Finish 2D Sketch.
Your sketch should look something like this:
How do I extrude a sketch?
Now we turn the 2D sketch into a 3D part.
- Start Extrude: 3D Model tab > Create panel > Extrude.
- Enter 1 in the Distance A box and click OK.
Round the ends with fillets
- Start Fillet: 3D Model tab > Modify panel > Fillet.
- Hover over an edge of the part. When it turns green, click it.
You’ll see a preview:
- Click the other edges you want rounded.
- Click OK in the dialog.
Make a hole with a sketch and Extrude
This is the long way to make a hole, but it teaches you how to sketch on a face of a part, which you’ll do all the time.
- Hover over the face where the hole goes. Its edges turn green.
- Right-click the face and choose New Sketch.
Inventor turns the view so you’re looking straight at that face:
- Start Circle: Sketch tab > Create panel > Circle.
- Hover over the rounded end until its center point shows up. Click the center and type 0.5 for the diameter.
The circle is drawn:
- Press Esc, right-click and choose Finish 2D Sketch.
You’re back in 3D:
- Start Extrude again (3D Model tab > Create panel > Extrude). The dialog opens:
- Flip the direction so it goes down into the part, make sure it’s set to cut, and set Distance A to 0.25 (the thickness of the part). Click OK.
The hole is done:
How do I make a counterbore with the Hole tool?
The Hole tool is the faster way, and it handles counterbores, countersinks and threads.
- Right-click the face at the other end and choose New Sketch.
Inventor goes back to sketch mode:
- Start Point: Sketch tab > Create panel > Point.
- Hover over the rounded end until the center point shows:
- Click the center point.
- Press Esc, right-click and choose Finish Sketch.
The point shows on the part in 3D:
- Start the Hole tool.
- Click the point. A hole preview appears. Choose Counterbore and enter 0.50 for the counterbore diameter.
- In the Behavior section, enter the values shown below and click OK.
The finished counterbore:
Check the part with Orbit
To make sure both holes go all the way through, turn the part around.
- Click Free Orbit: View tab > Navigate panel > Orbit.
- Hold the left mouse button and drag. Drag up and the part rolls up. Press Esc to stop orbiting.
Save the part
Save it so you can use it later: File > Save As.
What beginner mistakes should I avoid?
- Not fully constraining sketches. Add dimensions until the sketch is fully constrained. Inventor tells you on the status bar how many dimensions are still needed.
- Drawing to exact size. Draw roughly, then fix sizes with dimensions.
- Using Extrude for every hole. It works, but the Hole tool is faster and makes standard holes.
- Forgetting to save. Save the part early in its own project folder.
That’s lesson 1. Next up: Lesson 2: More basic stuff.
