About Part Sketching

All part models created in Autodesk Inventor start with sketches, which you create by drawing geometric elements such as points, lines, shapes, and arcs.

What's New: 2021

The sketch becomes the basis for sketched features, such as extrusions, revolutions, lofts, coils, or sweeps, which add volume to the sketched part.

Note: A placed feature, by contrast, consists of a defined mechanical shape that serves an engineering function in a part or assembly. Examples of placed features include holes, chamfers, and fillets.

Sketches can include reference geometry or construction geometry. Reference geometry is usually part of a feature, such as an edge or a vertex, which you project from the sketch of the feature to a new sketch. Construction geometry is used to help in the creation of sketches or features but isn’t used to define profiles or paths.

Elements of a Sketch

Understanding the elements of Inventor sketches will help you draw them accurately and model parts and assemblies correctly.

When working on a sketch, you can specify a planar face, work plane, or sketch curve:

• A planar face is a flat part face.
• A work plane is a construction feature that defines the parametric location of a sketch plane in 3D space. It’s useful when no planar face exists, such as when sketching on curved or toroidal faces.
• Sketch curves refer to the geometric objects you draw, such as lines, arcs, circles, ellipses, and splines.

A sketch profile is a closed loop defined by sketched or reference geometry that represents a cross-section of a feature. An open profile defined by sketched segments, arcs, or splines can define a surface shape or extend to boundaries to close a region.

The sketch path is the trajectory of a sweep feature. A path can be an open or closed loop consisting of lines, arcs, ellipses, or circles, with a specified starting point.

Creating Stable Sketches

A critical aspect of sketching is making sure that your geometry is stable. That’s why Inventor automatically applies some constraints to sketch geometry as you sketch. You can also add geometric constraints manually. Constraints affect:

• The orientation of the geometry to the sketch coordinate system. For example, if you draw a line that’s almost vertical, Inventor automatically makes it vertical.
• The relationship between sketch geometry. For example, you can add constraints to make shapes or lines perpendicular, parallel, tangent, or concentric. Or you can create proportional relationships between sketch curves.

You can also use dimensional constraints to stabilize sketches. Parametric dimensions control the size and position of sketch geometry and help prevent distortion when you resize sketch elements.

2D vs. 3D Sketches

Two-dimensional sketches are drawn on a plane along X/Y coordinates. In a 3D sketch, you can create geometry at any point in 3D space.

Use a 2D sketch to create planar geometry for features like extrude and revolve and to create 2D cross-sections for 3D lofts and sweeps.

Use a 3D sketch to create paths for wiring, tubing, sweeps, and lofts, or to create surface edges.

You can create 2D sketches in part (IPT), assembly (IAM), or drawing (DWG) files. You can create 3D sketches only in part (IPT) files.

Best Practices for Sketching

Before starting a sketch, consider its use and purpose so that you create it in the correct environment. Good uses for 2D sketches include:

• In parts, creating transition planes in a loft, projecting geometry from a different plane to use in a profile, for sharing geometry with more than one feature, and projecting profiles onto a surface to create complex shapes.
• In assemblies, adding holes through multiple subassemblies, extruding cuts through multiple parts, and creating a weld bead in a weldment.
• In drawings, creating hold notes, creating title blocks, creating sketch symbols, and adding manufacturing details.

In contrast, a wire route references multiple components, so you might want to create a 3D sketch in a part file of an assembly to reference component placement. In another scenario, you might create a cross-section in a 2D sketch and then create the centerline or sweep path in a 3D sketch.

The Sketch Environment

When you create sketches in Inventor, you work in the sketch environment, which simply means that all of the tools and commands you need are available in the ribbon in the Sketch tab (2D sketches) or the 3D Sketch tab (3D sketches).

The sketch environment also includes the graphics window, where you work directly on your sketch, and the browser, which shows a sketch icon as soon as you create a sketch, even before you create any geometry.

For 2D sketches only, the Line command is automatically activated when a new sketch is started. The command is not automatically activated when editing a sketch.

Tip: Right-click any sketch geometry in the graphics window and choose Find in Browser. Inventor highlights the sketch of the selected geometry in the browser.

Sketch dimensions display based on the state of the dimension:

• Orange = when mouse is hovering over the dimension
• Blue = when the dimension is selected
• Black = when the dimension is visible and not selected

If at any time you click Cancel Sketch all actions are discarded. For create workflows, that means going back to the point before the sketch was created. For edit workflows it means going back to the state before the sketch was edited.