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Sketch Options

Sets the default system options for sketching.

To set the default sketching options:

  1. Click Options , Sketch or Tools, Options, Sketch.

  2. Select from the following options, then click OK.

  • 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. Rotates views to be normal to the sketch plane whenever you open a sketch on a plane.

  • 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 or Copy 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 entities' original position while you drag a sketch.

  • Show curvature comb bounding curve. Displays or hides the bounding curve used with curvature combs.

  • 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.

  • 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.



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Web Help Content Version: SOLIDWORKS 2012 SP05

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