About Modifying the Sketch Setup
You can modify the sketch setup at any time in the sketcher mode, in the following ways:
• Selecting a new sketching plane
• Selecting an orientation reference
When you change the sketch setup, the active section is regenerated. The sketcher geometry appears with the new orientation settings. After regeneration, a message in the message pane indicates reference failures. This applies for undo and redo of the sketch setup.
Modifying the Sketching Plane
When modifying the sketch setup, you can create a new datum plane that you can use as the new sketching plane or orientation reference.
When you change only the sketching plane, one of the following happens:
• If the existing orientation is normal to the new sketching plane, it is retained.
• Otherwise, the existing orientation reference is replaced with the default orientation reference. The default orientation reference is an existing plane or is based on the model default coordinate system.
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 The sketch orientation is based on the model default coordinate system, regardless of the existence of a coordinate system feature. |
The Effect on Constrains and Dimensions
When you modify the orientation or the orientation references of the sketch, you do not change the sketch itself. This modification is similar to a rigid rotation of the sketch geometry entities along with the model geometry. Constraints and dimensions that define the sketch behave in the following ways:
• Horizontal and vertical constraints—Replaced with parallel and orthogonal constraints with respect to the original orientation reference. Orientation references that are not dimensioning references are automatically added to the references. You can then add the parallel and orthogonal constraints.
• Strong and weak dimensions— Preserved and retain their values.
• Point to point dimensions in the horizontal and vertical directions—Preserved but do not retain their values. Their values are adjusted to reflect the new directions.
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When you modify the sketch setup in a sketch with top level relations that involve point to point dimensions, the dimensions in the relation change and then affect the shape of the sketch. Both driving and driven point to point dimensions are changed.
In this case, modifying the orientation settings is not similar to a rigid rotation.
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If you change the direction of the sketch view, then the sketch dimensions and constraints are automatically changed. The sketch geometry goes through a rigid transformation and does not change its location relative to the model.
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To view the sketch, you can hide the model geometry located in front of the sketch while you are working on the section.
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If changing the sketching plane causes some external references to fail, a message in the message pane indicates reference failures.