CSWA cheat sheet

Sketch entity color coding: black = fully defined, blue = under-defined, yellow or red = over-defined or conflicting.

A new part document contains three default planes (Front, Top, Right) plus the origin; the first sketch is typically drawn on the Front plane.

Extrude end conditions available: Blind, Up To Vertex, Up To Surface, Offset From Surface, Up To Next, Up To Body, Through All, Mid Plane.

Mid Plane extrudes half the entered depth on each side of the sketch plane, so the Depth value equals the total part thickness.

A closed contour is required for a solid extrude; an open contour is valid only when the Thin Feature option is enabled.

Symmetric makes two entities equal about a centerline; Equal makes two entities the same length or radius without imposing symmetry.

Convert Entities produces On Edge relations to model geometry; Offset Entities produces a parallel copy at a specified distance.

Sketch patterns (linear, circular) reference sketch entities; feature patterns reference features or bodies.

The sketch status bar reports Fully Defined, Under Defined, or Over Defined; an over-defined sketch blocks new features until the conflict is removed.

A revolve profile must lie entirely on one side of the axis; the axis may be a sketch centerline, a sketch line, or a temporary axis.

Sweep requires a profile plus a path, tied together with a Pierce relation so the profile follows the path start point.

Loft requires two or more profiles on separate planes; guide curves and centerline parameters refine the transition.

Fillet types: constant size, variable size, face fillet, full round fillet. Chamfer types: angle-distance, distance-distance, equal distance, vertex.

Shell offsets wall thickness inward by default; Shell outward reverses the direction, and selected faces are removed to open the part.

Hole Wizard hole types include counterbore, countersink, straight hole, tapped hole, and pipe tap, using ANSI Inch, ANSI Metric, ISO, DIN, or JIS standards.

Linear pattern inputs: Direction 1, Direction 2, spacing, instance count, pattern seed, and Instances to Skip.

Reference planes can be created by offset distance, angle, mid-plane between two surfaces, or through a point or line.

Mirror requires a planar face or plane; Geometry Pattern copies the resulting shape rather than re-solving the original feature.

Standard mates: coincident, parallel, perpendicular, tangent, concentric, distance, angle, lock. Advanced mates: symmetric, width, path, linear coupler, limit.

The first inserted component is fixed by default and shows an (f) prefix in the FeatureManager; right-click and choose Float to release it.

A free rigid body has 6 degrees of freedom: 3 translations and 3 rotations. A coincident face-to-face mate removes 3.

Subassemblies solve as rigid by default; setting a subassembly to Flexible allows its internal mates to move at the top level.

Interference Detection and Clearance Verification are evaluation tools that report overlapping volumes or insufficient gaps between components.

A Smart Mate is created by Alt-dragging a component so that highlighted geometry generates the mate automatically.

Exploded views are stored per configuration; explode line sketches are used to place explode lines in drawing views.

A local component pattern is solved only within its own assembly; a derived pattern is linked to the parent feature pattern and updates with it.

Move Component with Collision Detection stops motion at contact; Physical Dynamics simulates the resulting interaction between components.

View types: Model View, Projected View, Auxiliary View, Section View, Detail View, Broken-out Section, Crop View, Broken View, Alternate Position View.

Insert > Model Items imports dimensions and annotations already stored in the model; Smart Dimension inside a drawing creates a driven reference dimension.

A driven dimension appears in gray parentheses and cannot be edited; a driving dimension changes the model geometry.

A Section View is defined by a section line drawn on a parent view; hatch pattern and hatch scale are set in the Section View PropertyManager.

A Detail View is labeled with a letter (A, B, C) and carries its own view scale, which overrides the sheet scale.

Sheet scale is set in Sheet Properties; any individual view can be assigned an independent scale.

Edit Sheet Format controls the border and title block; Edit Sheet controls the views and annotations placed on the page.

A Bill of Materials table is anchored to a drawing view and lists item number, part number, description, and quantity for each component.

Balloons attach to components; balloons snapped to a magnetic line stay aligned and move together when the line is dragged.