Work with Sketches

• In the browser, right-click a sketch, and select Edit Sketch. The parent component is also activated.
• In the graphics window, right-click and select a sketch tool from the context menu.

A mini-toolbar displays when a sketch is active. It has buttons for Reorient Sketch, Look At, and Stop Sketch.

Reorient sketch displays the Move triad so you can realign it by selecting geometry, a work feature, or a sketch entity.

Look At Sketch Grid changes the camera position so the sketch is parallel to the screen.

Stop Sketch exits the active sketch.

The sketch grid displays when a sketch is active. The grid spacing automatically updates as you zoom in and out, so the snap distance is appropriate for the zoom factor. Precision increases as you zoom in, and prevents the spacing from being too small when you zoom out.

The grid spacing displays on the snap bar in the lower right-hand corner. If you prefer a static value, you can manually override the grid spacing. The override is maintained unless the grid is not visible when you zoom in. The spacing is temporarily changed, and the original override value is used when you zoom out again.

The status bar contains buttons for Sketch Grid Mode, which turns visibility on and off, and Snap Mode, which turns snapping on and off. Snapping is disabled when the sketch grid is not visible.

Sketch constraints are created automatically (inferred), as you sketch. Design intent and relationships between sketch entities are captured.

If you do not want to create constraints automatically, press CTRL while sketching. Coincident constraints on points are still created, but relationship constraints, like horizontal or perpendicular, are not created

You can add constraints to existing sketch entities. When under-constrained entities are selected, a constraint glyph displays. You can click the glyph to apply that constraint, or pause over the glyph to display a list of valid constraints.

The Constraint button on the status bar turns the constraint visibility on and off. Constraints are still inferred when constraint visibility is off.

Fusion has two types of dimensions: transient and persistent. Transient dimensions do not control the size of the entity. Persistent dimensions control the size of an entity, so you cannot change the size by dragging or changing related entities.

Transient dimensions display only when you click an entity. They report the current size of an entity. You can change the size of an entity by dragging or changing related entities.

Persistent dimensions display when a sketch is active. You can change only the size of an entity by clicking on the dimension and entering a new value or turning persistent off.

Precise Input

Precise Input provides value entry boxes so you can specify the entity size. By default, value entry boxes display as you create sketch entities. The primary value highlights, and you can type a new value. If you want to enter a secondary value, such as the angle of a line, you can press Tab to highlight that box. If you enter a value and Tab to the next box, that value locks. It does not update as you move the cursor or enter a value in the other box.

The Precise Input button on the status bar turns the value entry boxes on and off.

Lock Geometry is a method to fix geometry without adding constraints and persistent dimensions. Locked geometry displays in green.

1. Click Reorient Sketch. The valid triad controls display.
2. Click a manipulator to move or rotate the sketch.
   • The arrow manipulators align the X or Y axis with a linear object.
   • The arc manipulator rotates the sketch.
   • The ball manipulator moves the sketch to the selected point.
3. Press OK to accept the changes

1. On the ribbon Solid or Surfaces panel, click Move.
2. In the browser, or in the graphics window, select a sketch.
3. Use the triad to move and rotate the sketch plane.