Constraints

A constraint is a rule about how lines, circles and points sit together: this line is horizontal, these two lines are the same length, this point is in the middle of that line. A dimension sets a size; a constraint sets a relationship. (SOLIDWORKS calls constraints relations.) Together they make a sketch fully defined, so it keeps its shape when you change a size.

How to use it#

1. With Select, click the first thing, then Shift-click the others.
2. Click the constraint in the sketch toolbar. The constraint buttons are the small symbols •, H, V, ∥, ⊥, =, M, T, ◎, ⇹ and ⚓. Hover over one to see its name and what to select.

A button stays grey until what you have selected fits it. Most constraints then show as a small symbol by the line, such as H. Coincident and Concentric show no symbol: the points simply sit together.

The twelve constraints#

Constraints added for you#

SchoolCAD adds many constraints as you draw:

• A line drawn nearly level or upright gets H or V.
• A line or shape that starts on a point is joined to it, and one that starts on a line stays on that line.
• A rectangle's sides stay horizontal and vertical (an aligned rectangle's stay at right angles), a polygon's sides stay equal, and a slot's ends stay tangent and equal.
• A tangent arc and a sketch fillet stay tangent to their lines.
• Mirror and Pattern tie their copies to the originals.

Auto-constrain and Tie loose ends#

Two buttons beside the constraints (in Constraints ▾ on a narrow screen, or ` Search tools) do the fiddly part for you:

• Auto-constrain adds H or V to lines that are nearly level or upright, joins ends that nearly meet, and makes a line and an arc that leave a corner the same way T tangent. It only adds what the sketch nearly has already, so nothing jumps. Then add the dimensions it still needs (SOLIDWORKS: Fully Define Sketch · Fusion: AutoConstrain).
• Tie loose ends joins line ends that stop just short of each other, or just short of a line or arc, so the shape closes and can be extruded. Use it when a sketch says it has a gap. Ends that are far apart are left for you to draw the missing line.

Using the origin and the parts#

You can select the origin (the point where the dashed axis lines cross), and the dashed orange edges and corners of parts, as part of a constraint. For example:

• Select the origin and the bottom line of a shape, then click Midpoint (M) to centre the shape left to right.
• Select a corner of your shape and a corner of the part, then click Coincident (•) to join them.

Removing a constraint#

Click a constraint's symbol to select it, then press Delete. Ctrl+Z takes back one you have just added.

Tips#

• With Select, drag a blue point to see how it can still move. That shows which dimension or constraint is missing.
• Use Equal instead of typing the same size twice: change one size and the others follow.
• For a symmetric design, draw a construction centre line and use Symmetric, or Mirror.
• A point made Coincident with a line can slide along the line, even past its end. Add a dimension to hold it where you want it.

If it does not work#

• The button is grey: what you selected does not fit. Check the table: Midpoint, for example, needs one point and one line. Press Esc to clear the selection and start again.
• Already constrained that way, so nothing was added. It was already true, for example a line you drew horizontal.
• That constraint fights the ones already there, so it was not added. Delete one of the others first.
• Horizontal on that line would squash the shape flat. Did you mean Vertical? You picked Horizontal for an upright line, or Vertical for a level one.
• Red lines and symbols: two rules or sizes fight each other. Click the red one and press Delete, or press Ctrl+Z.