FAQ Sketch Relations

Concepts

  1. Why can I not have redundant dimensions or distance mates?
  2. What are sketch relations?

Procedures

  1. Can I turn off automatic relations?
  2. How do I toggle the display of sketch relations?
  3. How do I avoid getting relations that I don't want?
  4. What do I do if I get a relation I don't want?
  5. What are snaps?
  6. How do I set snaps?
  7. What is an over defined sketch and how do I fix it?
  8. What are dangling relations or dimensions and how do I fix them?

Answers: Concepts

  1. Why can I not have redundant dimensions or distance mates?
    The software treats dimensions as parametric, modifiable entities. If you could add dimensions to entities already defined by relations or mates, you could violate the relations or mates by modifying the dimension. For example:
    Fully defined sketch.
    A redundant perpendicular relation is added. The sketch is still fully defined.
    A redundant dimension is added. The sketch is over defined.

    Changing the dimension later to something other than 90° would conflict with the relations. To prevent this potential conflict, the software makes the sketch over defined, requiring you to delete the dimension, make the dimension drive, or delete the relations.

    In addition, resolving conflicts is more difficult when redundant relations exist. You can delete the perpendicular relation and the adjacent horizontal or vertical relation. The SketchXpert functionality displays all possible solutions.

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  2. What are sketch relations?

    Sketch relations are geometric constraints between sketch entities or between a sketch entity and a plane, axis, edge, or vertex. Relations can be added automatically or manually.

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Answers: Procedures

  1. Can I turn off automatic relations?

    Yes

    Click Tools > Sketch Settings, and clear Automatic Relations.

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  2. How do I display sketch relations?

    Click View Sketch Relations (View toolbar) or View > Hide/Show > Sketch Relations to display sketch relations. If you clear View > Hide/Show > Sketch Relations, but you select a sketch entity in an open sketch, the sketch relation icons appear.

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  3. How do I avoid getting relations that I do not want?

    Turn off automatic relations. See Can I turn off automatic relations? above.

    - or -

    Click No Solve Move (Sketch toolbar) so that when you move sketch entities, the dimensions and the relations in the sketch are not solved.

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  4. What do I do if I get a relation I do not want?
    Use these techniques:
    • With relations displayed, delete the relation in the graphics area.
    • Delete the relation in the Properties PropertyManager, under Existing Relations.
    • For dimensions, delete them from the graphics area.
    • Delete the relation using the Display/Delete Relations tool (Dimensions/Relations toolbar).

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  5. What are snaps?

    Snaps are sketch settings that control how entities snap to each other. There are two types of snaps:

    Sketch snaps

    Global sketch settings that apply to all sketch commands.

    Quick snaps

    Single operation sketch snaps that you set as you sketch.

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  6. How do I set snaps?

    In the Standard toolbar, click Options > Systems Options > Sketch > Relations/Snaps, then set the snap options.

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  7. What is an over defined sketch and how do I fix it?

    The definition of an over defined sketch:

    • Dimensions or relations conflict with each other.
    • Dimensions over-constrain the sketch.
    • Dimensions you modify that create invalid geometry.

    Delete the relations or dimensions that conflict with your design intent. Use SketchXpert to assist you.

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  8. What are dangling relations or dimensions and how do I fix them?

    Relations or dimensions dangle when the entity (external to the sketch) to which the relation or dimension is applied either changes or is deleted. The dimension or relation is unresolved.

    For example, you dimension to the corner of a block in a sketch. Then you insert a cut feature that removes the corner before the sketch. The dimension dangles because the corner no longer exists.

    Delete or repair the dimension. You can right-click a dangling relation and click Auto Repair Sketch Relation or Dimension to repair the selected dangling relation from the context toolbar.

    In the Display/Delete Relations PropertyManager, you can use Find Replacement and Replace to fix a dangling relation in a sketch. Use Repair All Dangling to automatically fix all dangling relations.

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