In this lesson we make the five parts (A to E) that go together into an assembly in Lesson 7. Along the way you’ll practice tools you’ll use all the time in Inventor: sketching on the origin planes, Project Geometry, Shell, and the sketch constraints Equal, Concentric and Vertical. At the end there’s a table of every sketch constraint icon and what it does.
Sketch constraints are rules that control the shape of a sketch: this line stays vertical, these two circles stay the same size, these arcs share a center. You add them from Sketch tab > Constrain panel, and together with dimensions they make a sketch behave predictably when you change it.
What you’ll practice:
- Sketching on the X, Y and Z planes
- Wireframe view
- Projecting geometry onto a sketch
- The Shell tool
- Using constraints
- Constraint icons explained
Part A: how do I sketch on an origin plane, project geometry and shell a part?
Sketch on the YZ plane
Start a 2D sketch the way I showed in Lesson 1 – Getting Started:
Extrude the sketch 2 in.:
In the Model browser, expand Origin:
Click the YZ Plane in the browser tree. The YZ plane shows up in the model:
Right-click the plane in the tree and choose New Sketch from the menu:
Click the Home View button to orient the view like this:
Switch to wireframe and Look At
Turn on the wireframe view:
Ribbon > View tab > Appearance panel > Visual Style > Wireframe
The model now shows as a wireframe:
Now start the Look At tool: Ribbon > View tab > Navigate panel > Look At.
Click the YZ plane in the browser:
You’re now looking straight at the YZ plane in the sketch:
Project geometry onto the sketch
Start the Project Geometry tool from the ribbon:
Click the lines of the cylinder. Inventor projects the outline of the 3D part onto the 2D sketch plane as yellow lines:
Draw a vertical line between the midpoints:
Draw a 0.5 in. circle at the middle of the line, then delete the line:
Delete all the projected yellow lines:
Exit the tool. Your model should look like this:
Start the Extrude tool and cut the hole through the cylinder in both directions:
Click OK. Your model should look like this:
On the View tab, change the Visual Style to Shaded with Edges:
Hollow the part with Shell
Start the Shell tool:
Ribbon > 3D Model tab > Modify panel > Shell
The dialog box opens. Hover over the flat end of the cylinder and the face highlights:
Click the face:
Click OK. Here’s the model after the Shell command:
Start the Look At tool again:
Click the face highlighted in green:
Inventor turns the view perpendicular to that face:
Start a 2D sketch on that face. Draw a rectangle with the dimensions shown, constrained to the center point shown in yellow, and click Finish Sketch:
The rectangle is constrained and centered on the center point of the cylinder. Switch to the Home View:
Use Extrude as a cut to cut back into the part 1.975 in.:
Click OK. Your part should look like this:
Save the part. You’ll need it in the next lesson.
Part B: a simple pin
Start a new part as described in Lesson 1 – Getting Started. Draw a circle 0.50 in. in diameter:
Click Finish Sketch on the ribbon:
Use the Extrude tool to extrude the part 1.875 in.:
Click OK. Part B should look like this:
Save Part B in the same folder as Part A:
Part C: fillet and holes
Start a new part as described in Lesson 1 – Getting Started and draw this sketch:
Click Finish Sketch and extrude Part C 2.25 in.:
Use the Fillet tool (3D Model tab > Modify panel) to put a 1.125 in. fillet on the end of the part:
On the View tab, choose the Look At tool:
Select the face:
Sketch a 2 in. diameter circle:
Finish the sketch and switch to the Home view from the ViewCube:
Use Extrude to cut a hole all the way through the part:
The model should now look like this:
Use the Look At tool again:
Draw a 0.50 in. circle:
Cut a 0.50 in. hole:
Save Part C in the same folder as Parts A and B:
Part D: how do I use the Equal constraint?
Make two circles equal
Start Part D as described in Lesson 1 – Getting Started and draw this sketch:
Go to Ribbon > Sketch tab > Constrain panel > Equal:
Click the upper circle, then the lower circle. The circles become the same diameter. Now when you dimension the upper circle, the lower one follows:
Finish the sketch so it looks like this:
Extrude the sketch 0.25 in.:
The model will look like this:
Draw a circle on the face:
Extrude the circle 0.25 in. as a solid:
Rotate the part to see the other side:
Draw another circle on this side:
Finish the model by extruding this side too, by 0.50 in.:
Save the part in the same folder:
Part E: how do I use Concentric and Vertical constraints?
Start Part E as described in Lesson 1 – Getting Started. Draw a sketch with circles whose centers are offset and not lined up, like this:
On the Constrain panel, choose the Concentric tool:
Hold SHIFT and click each circle. Inventor makes the circles concentric:
Click the Vertical constraint on the ribbon:
Click the circle centers. The circles line up vertically:
Using what you’ve learned so far, finish the sketch and extrude it 0.25 in.:
Save Part E in the same folder:
What do the Inventor sketch constraint icons mean?
In Parts D and E we used the Equal, Concentric and Vertical constraints. Here’s the whole Constrain panel on the Sketch tab, so you can tell the icons apart:
| Constraint | What it does |
|---|---|
| Coincident | Puts a point on another point, line or curve |
| Collinear | Makes two lines lie on the same line |
| Concentric | Gives two circles or arcs the same center |
| Fix | Locks a point or line in place |
| Parallel | Makes two lines parallel |
| Perpendicular | Makes two lines meet at 90° |
| Horizontal | Makes a line (or two points) horizontal |
| Vertical | Makes a line (or two points) vertical |
| Tangent | Makes a line or curve touch a curve without crossing it |
| Smooth | A smoother (curvature-continuous) join between a spline and another curve |
| Symmetric | Mirrors two items about a line |
| Equal | Makes two lines the same length or two circles the same size |
The button at the bottom left of the panel opens the constraint Settings.
How do I show or hide constraints in a sketch?
While you’re in a sketch, press F8 to show all constraints and F9 to hide them. You can also right-click in the sketch and use Show All Constraints. Each constraint shows as a small icon next to the geometry. Hover over one to highlight what it controls, or select it and press Delete to remove it.
How do I know if a sketch is fully constrained?
Inventor tells you in the status bar at the bottom right: it shows how many dimensions are still needed, or Fully Constrained. Fully constrained lines also change color.
A fully constrained sketch can’t change by accident when you drag something. It’s not always required, but for parts you’ll edit later, it saves a lot of trouble.
What to do when constraints don’t behave
A dimension won’t go on, or Inventor says it over-constrains the sketch. Something else already controls that size. Make it a driven (reference) dimension, or delete the constraint that conflicts.
The sketch jumps when I add a constraint. Inventor moves the geometry to satisfy the new rule. Add constraints in a sensible order (horizontal/vertical first, then equal, then dimensions), and use Fix on a point that shouldn’t move.
Inventor added constraints I didn’t want. Inventor infers constraints as you draw, like horizontal or coincident. Show them with F8 and delete the ones you don’t want, or hold Ctrl while drawing to stop it from inferring.
Project Geometry lines won’t delete. Projected lines are linked to the model. Select them in the sketch and delete them, or right-click and break the link if you want to keep them as normal sketch lines.
What’s next?
Save all five parts in the same folder. In Lesson 7 we put them together into an assembly.
