About Exploding Sketches

The Explode capability allows you to edit and modify a sketch obtained by Copy>Paste>As Result With Link.

Exploding the sketch converts every wireframe geometry associated to the datum feature into a standard 2D geometry feature and the copy feature is then removed from the specification tree. Consequently, there is no more associativity between the exploded sketch and its reference sketch.

To explode a sketch, right-click it from the specification tree and select Sketch.XXX object > Explode...

When done:

• The sketch is not-up-to-date.
• The order and the number of geometrical elements appearing in the specification tree after an explode operation may differ from what can be seen in the reference sketch.
• Exploded sketches used by Part Design or Generative Shape Design features appear in Update Error dialog boxes. You need to reroute them one by one.

A sketch obtained by Copy>Paste>As Result With Link is a copy of its reference sketch. By default, the system keeps associativity between the resulting sketch and the original geometry as well as between resulting sketch position and the position of the sketch reference.

To manage this associativity, such sketches contain datum features which are the real features keeping associative links between the copies and reference sketches. 3D geometrical results associated to reference sketch features are duplicated and associated to these datum features.

Thus associativity:

• With the original geometry is controlled by these datum features managing associative copies of the 3D geometrical results associated to reference sketches. Consequently they cannot take into account the following data that is included in reference sketches:
  
  • Construction or axis line geometrical elements
  • Geometrical elements on which output or output profile features exist
  • Constraints and dimensions.

  Associativity with the original geometry is always kept till it is not removed using Isolate. By the way, geometrical results can be different from reference sketches until datum features are not synchronized with reference sketches.

• With the original sketch position is managed by the sketch absolute axis feature definition. By default it is defined as associative in position with its datum feature, thus with its reference sketch feature position. But you can break this associativity if needed by defining your own sketch position. Since V5R19, thanks to the Sketch As Result With Link positioning capability, associativity with original position is explicitly identified via ‘Positioned as reference’ support definition mode or can be retrieved afterwards using this new definition mode.