There are many different types of constraints that can be created in a sketch. For explanations of the tools in the constraints menu, explore the sections below.

For information about the Make Construction tool found in the constraints menu, see Make Construction.
When a pattern is created within a sketch, a Sketch Pattern constraint is automatically added. For more information on this constraint type, see Sketch Pattern Constraint.
Parallel
Parallel lines have the same distance continuously between them.
To create a Parallel constraint, select two or more lines in the sketch and select Parallel from the constraints menu.
Perpendicular
Perpendicular lines have a right (90°) angle between them.
To create a Perpendicular constraint, select two lines and select Perpendicular from the constraints menu.
Lines do not need to share a common point or intersect with each other to be made perpendicular. Guide curves are shown to indicate a perpendicularity between disconnected lines.
Tangent
A line is tangent to a curve and perpendicular to the radius when it touches it at exactly one point. A line that is tangent to an arc (or circle) will be perpendicular to the arc's radius. Arcs and circles can also be tangent to each other. When curves are tangent to each other, they touch at exactly one point.
To create a Tangent constraint, select two sketch elements, either a line and a curve, or two curves, and select Tangent from the constraints menu.
Tangent elements do not need to be in contact with each other. When tangent elements are separated, guide curves are shown to indicate where the tangency applies.
Coincident
When geometric elements are coincident, it means they are overlapping. In Shapr3D, you can make sketch endpoints coincident with other elements in your design to make them connected.
To create a Coincident constraint, use one of these techniques:
 Select an endpoint and another element in your design, then select Coincident from the constraints menu.
 Drag an endpoint onto the element you want to connect to.
Endpoints can be made Coincident to other endpoints, lines, curves, and edges.
Endpoints that are connected to elements with a Coincident constraint are shown with a filled center. For more information, see States of sketch points.
Midpoint
Use a Midpoint constraint to connect an endpoint with the center of a line. This relationship will ensure that if the length of the line change, the endpoint will always remain at the center of the line.
To create a Midpoint constraint, use one of these techniques:
 Select an endpoint and line, then select Midpoint from the constraints menu.
 Drag an endpoint onto the center of a line (indicated in purple).
Endpoints that are connected to elements with a Midpoint constraint are shown with a filled center. For more information, see States of sketch points.
Concentric
Concentric arcs share the same center point.
To create a Concentric constraint, select arc or circle elements and select Concentric from the constraints menu.
Horizontal/Vertical
Horizontal and vertical directions in a sketch are aligned with the axes of the sketch plane.
To create a Horizontal/Vertical constraint, select a line (or multiple lines), then select Horizontal/Vertical from the constraints menu. The line(s) will be aligned with the axis closest to their original direction.
You can automatically create Horizontal/Vertical constraints while sketching when the constraint setting for Autoconstraining is turned on. For more information, see Constraint Settings.
Equal
When lines are equal, they are the same length. When arcs and circles are equal, they have the same radius.
To create an Equal constraint, select similar elements, such as multiple lines or multiple arcs, then select Equal from the constraints menu.
Symmetry
Symmetrical elements lie on opposite sides of an axis of symmetry and behave as mirror images of each other.
To create a Symmetry constraint, follow these steps:
 Select two similar elements, such as two arcs or two lines.
 Select Symmetry from the constraints menu.
 Select a line or an edge for the axis of symmetry.
Disconnect
Disconnect is used to break the connection between connected points. For more information on using Disconnect, see Adding and removing constraints.
Tip: Connected sketch points are shown with a filled center. For more information, see States of sketch points.
Lock
The Lock constraint fixes a selected element in its current position.
To use the Lock constraint, select a sketch element, then use one of these techniques:
 Select Lock from the constraints menu.
 Select the Lock icon in the design space (this icon is only available when a point is selected).
Locked sketch points are shown as a solid blue color. For more information, see States of sketch points.
Locked elements can be unlocked by selecting them and using the Unlock icon or option in the constraints menu. For more information, see Adding and removing constraints.