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Sketch Settings Menu
Sketch Complexity
Working in a Sketch
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Dimensions/Relations Toolbar and Menus
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Dimensioning a 2D Sketch
Maintaining Proportions in a Sketch Profile
Creating Horizontal Dimensions
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Locking Dimensions
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Creating Circular Dimensions
Creating Arc Dimensions
Creating Path Length Dimensions
Creating Dimensions Between Two Points
Formatting Dimensions in Parts and Sketches
Inserting Driven Dimensions
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Dimensioning Two Points of the Same Arc
Displaying Dimensions
Using Centerlines to Create Radial and Diametric Dimensions
Sketch Geometry Status
Sketch Status Conventions
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Override Dims on Drag/Move
Creating Zero and Negative Value Dimensions
Displaying a Ghost Image of a Missing Sketch Entity
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Glossary
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Sketch Geometry Status

Sketches include a status, and sketch entities within the sketch include a state. Sketch entity states are displayed in different colors to facilitate identification.

Sketch states include the following:

Dangling

Appears as brown in the graphics area under Relations in the Display/Delete Relations PropertyManager, and in the FeatureManager design tree.

Indicates sketch geometry that cannot be resolved. For example, deleting an entity that was used to define another sketch entity.
sketch_dangling_dimensions_ok.gif sketch_dangling_dimensions.gif
Original sketch Sketch with dangling dimensions

Driven

Appears as grey in the graphics area.

Indicates a dimension that is redundant and cannot be modified.

When you add a redundant dimension, you can select Make this dimension driven and click OK in the dialog box. The dimension changes from red (over defined) to grey.

Item Conflicts

Appears as yellow in the graphics area and under Relations in the Display/Delete Relations PropertyManager.

Indicates a redundant dimension or an unnecessary relation.
sketch_over_defined.gif

Use SketchXpert to resolve conflicting sketches.

Under Defined

Appears as blue in the graphics area.

Indicates a sketch entity which requires a dimension or relation to another sketch entity.
Generate a combination of dimensions and relations to fully define sketch an under defined sketch.

Fully Defined

Appears as black in the graphics area and under Relations in the Display/Delete Relations PropertyManager.

Indicates all required dimensions and relations to sketch entities are present, without redundant or unnecessary elements that cause the sketch to be over defined.

Invalid

Appears as yellow in the graphics area.

Indicates sketch entities that are invalid, creating a sketch without resolution in its current state.

Requires deleting some relations or dimensions, or returning the sketch entity to its prior state.

Splines cannot self-intersect, modifying the Tangent Radial Direction PM_Tangent_Radial_Direction.gif creates an invalid sketch entity.

Video: Invalid Spline Sketch

Item is Unsolvable

Appears in red in the graphics area.

Indicates the geometry cannot determine the position of one or more sketch entities.

sketch_solved_dimension.gif sketch_not_solved_dimension.gif
Sketch solved with 50 dimension Sketch is unsolvable with 80 dimension


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