Sketching

About sketches

A sketch is a set of 2D curves on a plane. Most part features start from a sketch. A closed region in a sketch becomes a profile. You can extrude, revolve, sweep or loft a profile.

You can put a sketch on:

An origin plane (XY, XZ or YZ).
A work plane.
A planar face of the part.

Start and finish a sketch

On the Features tab, click Start 2D Sketch.
Select a plane or a planar face.
The Sketch tab opens. Draw the curves.
Add constraints and dimensions.
Click Finish Sketch to keep the changes.

To leave the sketch and discard its changes, click Cancel Sketch.

To change a sketch later, right-click the feature in the model browser and select Edit Sketch.

Create curves

Tool	What it does
Line	Draws connected lines.
Circle	Draws a circle from its center and a point.
Three Point Circle	Draws a circle through three points.
Three Point Arc	Draws an arc through three points.
Center Point Arc	Draws an arc from its center, start and end.
Tangent Arc	Draws an arc tangent to the end of a curve.
Two Point Rectangle	Draws a rectangle from two corners.
Center Rectangle	Draws a rectangle from its center and a corner.
Slot	Draws a slot from two centers and a width.
Polygon	Draws a regular polygon.
Point	Adds a sketch point.
Ellipse	Draws an ellipse.
Spline	Draws a spline through control points.
Text	Adds text as closed profiles that you can extrude.

Modify curves

Tool	What it does
Trim	Removes the part of a curve between two intersections.
Extend	Extends a curve to the next curve.
Project Geometry	Projects model edges onto the sketch plane.
Construction	Changes the selected curves to or from construction geometry.
Fillet	Rounds a corner of two lines with a tangent arc.
Chamfer	Cuts a corner of two lines with a line.
Offset	Copies a chain of curves at a distance.
Move	Moves the selected sketch geometry.
Rotate	Turns the selected sketch geometry about a point.
Scale	Makes the selected sketch geometry larger or smaller.

Construction geometry helps you position other curves. It does not make profiles.

Pattern curves

Tool	What it does
Mirror	Copies the selected geometry symmetrically about a line.
Copy	Copies the selected geometry to a different position.
Grid Pattern	Copies the selected geometry in rows and columns.
Polar Pattern	Copies the selected geometry around a center.

Constraints

A constraint sets a geometric relation between curves.

Constraint	What it does
Coincident	Makes two points meet.
Horizontal	Makes a line or two points horizontal.
Vertical	Makes a line or two points vertical.
Parallel	Makes two lines parallel.
Perpendicular	Makes two lines perpendicular.
Tangent	Makes two curves tangent.
Equal	Makes two lines the same length, or two arcs the same radius.
Concentric	Gives two arcs or circles the same center.
Midpoint	Puts a point at the middle of a line.
Fix	Locks the selected geometry where it is.
Symmetric	Makes two points symmetric about a line.
Collinear	Puts two lines on one line.

To show or hide the constraint symbols, click Show Constraints.

Dimensions

Use Dimension to add a dimension to the selected geometry. A dimension can be driving or driven:

A driving dimension sets the size of the geometry.
A driven dimension only shows the size. It does not change the geometry.

For a value, you can type a number, a number with a unit (for example 2 in), or an expression that uses other parameters. For more data, refer to Parameters and rules.

Good practice

Make the profile closed. An open chain of curves does not make a profile.
Add enough constraints and dimensions to hold the shape. Then the sketch keeps its shape when you change a value.
Use Project Geometry to refer to existing model edges.
Use construction lines for center lines and symmetry lines.