Sketch Options

Sets the default system options for sketching.

To set the default sketching options:

Click Options > Sketch or Tools > Options > Sketch.

Reset Restores factory defaults for all system options or only for options on this page.
Auto-rotate view normal to sketch plane on sketch creation and sketch edit Rotates views to be normal to the sketch plane whenever you open a new or existing sketch on a plane.
If the option is selected, the following behavior occurs:
  • When you open a new or existing sketch, the view rotates to be normal to the sketch plane.
  • When you exit a sketch:
    • If you keep your changes, the view remains normal to the sketch plane. For example, click in the Confirmation Corner or Insert > Exit Sketch.
    • If you discard your changes, the view reverts to the orientation it was in before you opened the sketch. For example, click in the Confirmation Corner or Edit > Exit Sketch without Saving Changes.
Use fully defined sketches Requires sketches to be fully defined before they are used to create features.
Display arc centerpoints in part/assembly sketches Displays arc centerpoints in sketches.
Display entity points in part/assembly sketches Displays endpoints of sketch entities as filled circles. The color of the circle indicates the status of the sketch entity:

Black

Fully defined

Blue

Under defined

Red

Over defined

Green

Selected
Over defined and dangling points are always displayed, regardless of this option.
Prompt to close sketch Displays a dialog box with the question, Close Sketch With Model Edges? if you create a sketch with an open profile, then click Extruded Boss/Base to create a boss feature. Use the model edges to close the sketch profile and select the direction in which to close the sketch.
Create sketch on new part Opens a new part with an active sketch on the Front Plane.
Override dimensions on drag/move Overrides dimensions when you drag sketch entities or move the sketch entity in the Move PropertyManager. The dimension updates after the drag is complete.
This option is also available in Tools > Sketch Settings > Override Dims on Drag/Move.
Display plane when shaded Displays the sketch plane when you edit a sketch in Shaded With Edges or Shaded mode.
If the display is slow due to the shaded plane, it may be because of the Transparency options. With some graphics cards, the display speed improves if you use low transparency. To set a low transparency, click Tools > Options > System Options > Performance and clear High quality for normal view mode and High quality for dynamic view mode.
Line length measured between virtual sharps in 3d Measures the line length from virtual sharps, as opposed to end points in 3D sketches.
Enable spline tangency and curvature handles Displays spline handles for tangency and curvature.
Show spline control polygon by default Displays a control polygon to manipulate the shape of a spline.
Ghost image on drag Displays a ghost image of a sketch entity's original position while you drag a sketch.
Show curvature comb bounding curve Displays or hides the bounding curve used with curvature combs. Example: Setting Curvature Comb Bounding Curve Option
Enable on screen numeric input on entity creation Displays numeric input fields to specify sizes when creating sketch entities. To use this option, you can also right-click in a sketch and click Sketch Numeric Input.

This option is helpful for building design intent into sketches because you do not have to exit the sketch entity tool to dimension the entity.

When Enable on screen numeric input on entity creation is selected, you can also select Create dimension only when value is entered. This option dimensions the sketch entity only if you enter a value and press Enter or Tab.

These options are not available for slot sketch entities.
Preview sketch dimension when selected Displays a sketch dimension preview when a sketch entity is selected.You can select the dimension to edit it. When you click anywhere else in the graphics area, the preview dimension disappears.
To turn on sketch dimension previews, click Tools > Options > System Options > Sketch and select Preview sketch dimension when selected.
Over defining dimensions

Prompt to set driven state

Displays a dialog box with the question, Make Dimension Driven? when you add an over defining dimension to a sketch.

Set driven by default

Sets the dimension to be driven by default when you add an over defining dimension to a sketch.

Use Prompt to set driven state alone or with Set driven by default. Depending on your selections, one of four actions occur when you add an over defining dimension to a sketch:
  • A dialog box appears that defaults to driven.
  • A dialog box appears that defaults to driving.
  • The dimension is driven.
  • The dimension is driving.
Turn off Automatic Solve Mode and Undo when sketch contains more than this number of sketch entities Enables and disables Automatic Solve Mode and Undo, and modifies the threshold limit.
Hide missing geometry error for suppressed dimensions Hides the warning caused by missing relations or missing model geometry when you suppress a part's dangling dimensions within an assembly.