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Unit 02 · Lecture 2

Understanding sketch constraints (Part 1)

A sketch that looks right isn’t finished until nothing in it can move. This lesson builds a mounting plate with four corner holes and shows how to constrain each element step by step, until Inventor reports Fully Constrained.

Video 14:27Reading 8 minLevel: beginnerUpdated 26 October 2026

Lecture video, 14:27. The written steps below follow the video, with timestamps so you can jump to each part.

What you will build

A 200 × 100 × 20 mm plate centred on the origin, with four Ø10 mm through-holes, each 20 mm from the two nearest edges.

You will learn

  • The four rectangle types and when to use a centred one
  • Why the sketch origin is the only fixed point
  • Dimensioning features relative to other geometry
  • Reading the constraint status bar
  • Closed profiles, and why open ones won’t extrude as solids

Before you start

Finish Lecture 1 first. You should know how to start a sketch on the XY plane and extrude a profile.

Step by step

  1. 01

    New part, sketch on XY

    0:00

    Create a new part from Standard (DIN).ipt and start a 2D sketch on the XY plane (the Top view).

  2. 02

    Draw a centred rectangle

    0:45

    Open the Rectangle drop-down. There are four types: Two Point, Three Point, Two Point Center and Three Point Center. The plate must be symmetric about the origin, so choose Two Point Center.

    Click the sketch origin (X0 Y0), type 200, press Tab, type 100 and press Enter. The rectangle is now anchored to the origin.

  3. 03

    Add four Ø10 circles near the corners

    1:30

    Draw a circle near each corner and give each a diameter of 10 mm. Don’t worry about exact placement yet. The dimensions will place them.

  4. 04

    Locate each circle with dimensions, not helper geometry

    3:50

    You could draw 20 mm construction lines or small squares to find the hole centres, but that adds clutter and doesn’t teach you anything. Use the Dimension tool on the Constrain panel instead: click the circle’s centre point, click the nearest vertical edge and enter 20. Repeat with the nearest horizontal edge and enter 20.

    Do this for three circles and leave the fourth undimensioned on purpose.

  5. 05

    Compare the colours

    4:34

    Look closely. The three dimensioned circles have changed colour, and the fourth has not. Inventor draws geometry that can still move or change size in a different colour from geometry that is fixed. Try dragging the fourth circle: it slides around and its size changes. The others don’t move.

    Give the fourth circle its diameter (10) and its two 20 mm distances. Now none of the circles can move, grow or shrink. Restricting geometry like this is what constraining means.

  6. 06

    Watch the status bar reach “Fully Constrained”

    9:03

    The bottom-right corner of the window shows how many dimensions the sketch still needs. Delete the dimensions of one circle and it reports 3 dimensions needed: one diameter and two positions. Add them back one by one and the counter drops, until it reads Fully Constrained.

  7. 07

    Extrude: count the profiles

    10:31

    Finish the sketch and press E, the shortcut for Extrude. (Every tool’s shortcut appears in brackets after its name.) Inventor finds five closed profiles: the plate area between the holes, plus the four circles.

    Select only the plate area, leave the circles unselected so they become holes, and extrude 20 mm.

Why constraints matter

The origin is the only true fixed point

When you start a sketch, the only location Inventor already knows is the sketch origin. Anchoring the rectangle there fixes its position, and its 200 and 100 dimensions fix its size.

Relative constraints chain together

The circles are dimensioned to the rectangle, and the rectangle is fixed to the origin, so the circles are fixed too. It’s the same logic as A = B and B = C, therefore A = C. Build every sketch as a chain that leads back to the origin.

Closed vs. open profiles

A solid extrusion needs a closed profile. If you draw a triangle with one side missing, Extrude won’t let you select it. The exception is surface mode in the Extrude dialog, which can extrude open shapes into surfaces instead of solids. Surfaces are a later topic. For now, keep surface mode off and close your shapes.

Common mistakes

Practice exercise

Model a 120 × 80 × 10 mm plate centred on the origin, with a Ø30 hole in the middle and four Ø8 holes 12 mm from the nearest edges. Get the status bar to Fully Constrained before you extrude.

Then edit the sketch: change the plate to 140 mm long. If the corner holes move with the edges, your dimensions were placed correctly.

Check yourself

Which rectangle type keeps the plate symmetric about the origin?

Two Point Center, started on the sketch origin.

How many dimensions does a free circle need to be fully constrained?

Three: its diameter and two position dimensions (horizontal and vertical).

Why are the circles fixed even though they are only dimensioned to the rectangle?

Because the rectangle is anchored to the origin. Relative constraints chain back to the one fixed point.

Extrude finds five profiles in this sketch. Which do you select to get a plate with four holes?

Only the plate area, the region outside the four circles.

Written by the CADsmit instructor from the lecture recording and checked in Autodesk Inventor Professional 2027. Last updated 26 October 2026. Spotted an error? Tell us.