Sketch Entities and Planes
Choose where a 2D sketch lives, then build its shape from simple entities and construction geometry.
Choose the sketch plane before drawing the shape
Choose the sketch plane before drawing the shape
A 2D sketch is a set of points and curves on one plane. The plane places the sketch in the model; the sketch's origin and axes give you references for locating its geometry.
- Standard plane: Front, Top, or Right is a useful starting reference for a new part. Choose the view that makes the intended profile easiest to describe.
- Model face: use an existing planar face when the new sketch belongs on that face. A curved face is not itself a 2D sketch plane.
- Reference plane: an added plane can locate a sketch where the standard planes and existing faces do not.
The origin is a point, not a plane. Starting a line or circle at the origin can anchor its position, but you still need a sketch plane. You may start elsewhere when that suits the design; then constrain the location relative to a deliberate reference.
Look normal to the sketch plane: straight at it, rather than at an angle. Horizontal and vertical refer to the sketch's axes, even when you rotate the model on screen.
Supporting detail: Addendum 1 — Sketch placement in Onshape.
Use the simplest entity that describes the shape
Use the simplest entity that describes the shape
| Entity | What it describes | What to control |
|---|---|---|
| Line | A straight segment between two endpoints. | Position, direction, and length. |
| Circle | A complete round curve. | Center position and radius or diameter. |
| Arc | Part of a circle. | Center, radius, and where the arc begins and ends. |
| Rectangle | Four connected lines with right-angle corners. | Position, orientation, width, and height. Tool-created relations often supply some of these. |
| Slot | A constant-width path with rounded ends. A simple straight slot has two parallel sides and two semicircular ends. | Path position and direction, width, and length. State whether length means overall length or distance between end centers. |
| Spline | A curve shaped by fit points or control points and handles. | Point locations and curve shape. Use it when a line or circular arc cannot express the intended contour. |
Rectangle and slot tools create useful groups of geometry. They do not guarantee that the resulting sketch is fully defined. Inspect their relations before adding more.
Supporting detail: Addendum 2 — Find the tools by their software names.
Construction geometry guides the sketch without outlining material
Construction geometry guides the sketch without outlining material
A centerline is a common use of construction geometry: a reference for a center, symmetry, angle, or axis. Construction geometry participates in dimensions and relations, but does not serve as the ordinary boundary of a filled profile.
In SOLIDWORKS, Centerline creates construction geometry. In Onshape, use Construction to toggle selected sketch entities or to create construction geometry. Use a construction circle for a layout circle just as you would use a construction line for an axis.
Supporting detail: Addendum 3 — Vendor reference for construction geometry.
Check connections before moving on to a feature; Practice
Check connections before moving on to a feature
Two endpoints that look joined may still be separate. A tiny gap can prevent a profile from closing. Use a coincident relation to make the connection intentional, then inspect the sketch.
Closed and fully defined are different checks. A closed circle can still move or change size. A fully defined chain of lines can still be open. Later features such as extrude or revolve use sketches in different ways; choose the profile that the intended feature needs.
Continue with Geometric Relations in Sketches and Fully Defined Sketches and Design Intent. For view interpretation, see Orthographic Projection and the Glass Box; for drawing dimensions, see Dimension Anatomy and Placement.
