Sketch Constraints

Apply geometric relationships such as tangency and perpendicularity to sketch curves.

As you create geometry, many sketch constraints are automatically applied. For instance, if you draw a line that is nearly horizontal, a horizontal constraint will be created on that line automatically, making it precisely horizontal for you. When you modify a sketch, the constraints ensure that the intended relationships between the sketch entities remain intact.

Apply or Remove Sketch Constraints

Apply sketch constraints to geometry to ensure that the intended relationships between sketch entities remain intact, or remove sketch constraints to allow more freedom to create free-form objects.

  1. In sketch mode, select the entities you want to constrain.
  2. Select or deselect an icon on the Constraint Toolbar. When a constraint is selected, it allows you to quickly select entities in the sketch to apply constraints.

    Tip:
    • Drag the Constraint Toolbar to the left or right side of the workspace to dock it.
    • Use the Show Constraint Toolbar checkbox under Sketching in File > Preferences to show or hide the toolbar.
    • Constraints are also available on the context menu: right-click a sketch entity, then select or deselect the icons at the top of the context menu to apply or remove constraints.
    Constraint Description
    Fixed

    		 Lock the position of any sketch curve.

    When a line is fixed, you can still move the end points to change the length. The end points of a line are separate entities and can be fixed independently.

    Note: To delete all fixed constraints, right-click on the constraint and select Remove Fix.
    Horizontal

    		 Click individual lines to constrain them to be horizontal.

    You can also use this constraint to align points.
    Vertical

    		 Click individual lines to constrain them to be vertical.

    You can also use this constraint to align points.
    Midpoint

    		 Click a point and any other entity (excluding splines) to constrain the point to the midpoint of the entity.
    Coincident

    		 Click a point and any other entity to constrain the point to be coincident with the other entity.
    Tip: When you hover over coincident sketch entities, a badge appears next to the cursor and a tooltip appears.

    This indicates that you can hold down the left mouse button to access the coincident picking menu, from which you can select the desired sketch entity.



    Collinear

    		 Click two lines to constrain them to lie along the same straight line.

    The second line will move to be collinear with the first-selected line unless the second line is already constrained. In that case, the first line will move.
    Parallel

    		 Click two lines to constrain them to be parallel.
    Perpendicular

    		 Click two lines to constrain them to be perpendicular.
    Tangent

    		 Click a line and a circle/arc (or two circles/arcs) to constrain them to be tangent to each other.
    Concentric

    		 Click two circles/arcs to constrain them to have the same center.
    Equal

    		 Click two lines to constrain them to have the same length.

    Click two circles/arcs to constrain them to have the same radius.
    Offset

    		 A sketch curve is offset from another sketch curve.
    Note: This constraint can only be applied from the sketch constraint context menu to remove an offset constraint.
    Symmetric

    		 Two sketch entities are constrained to be symmetric about a construction line (e.g., mirrored curves).
    Note: This constraint can only be applied from the sketch constraint context menu when two entities and a construction line are selected.
    Select Other This is not a constraint.

    Select this option when selecting overlapping sketch entities to specify which sketch entity you wish to select.
Tip:
  • To hide all constraints, deselect Show constraints under Sketching in File > Preferences.
  • If your horizontal constraints appear vertical and vice versa, use the Align Axes option in the context menu to align the sketch axes so that the x-axis is horizontal and the y-axis is vertical.
  • Select Delete All Constraints from the context menu to remove all constraints from all sketches in the model.
  • Select Remove Fix from the context menu to remove all fixed constraints in the model.

Use Inferences

Inferences are constraints that are applied automatically as you sketch to help you quickly create accurate sketches.

  1. In sketch mode, select the entities you want to modify.
  2. As you modify the entities, inferences are displayed to help you.
    Constraint Description
    Tan/Tan When you sketch a line between two circles, the Tan/Tan inference helps you make the line tangent to both circles.
    Perp/Perp When you sketch a line between two circles, the Perp/Perp inference helps you make the line perpendicular to both circles.