Accessing protrusion trajectory sketch

[reg2117]

Forum Members,
Can someone please suggest a method for accessing the
trajectory sketch of a protrusion. I created the sketch
during the creation of the protrusion as opposed to first
creating the sketch and then referencing the sketch when
creating the protrusion.
I would like to use this sketch for another geometry.
Thanks in advance.

 

[kdem]

You can change it to an external sketch by copying the internal sketch geometry and pasting into a newsketch feature and then redefine the extrude to reference the new sketch. You could also create a sketch and reference the extrusion geometry using the Use Edge command in sketcher, delete the edge references from the reference dialog, drag the sketch in the model tree before the extrude, and edit the definition of the extrusion to use the new external sketch. If you have features that reference the extrusion geometry you need to specify new references for those features.

 

[reg2117]

kdem,
Thanks for the reply. In all of the suggestions, it
seems the final step always includes referencing a new
sketch, made by way of the old sketch or geometry. Is
there no way to show the referenced sketch in the model
tree (before the protrusion) without making a new sketch?
I could just redo the geometry such that I always
create the trajectory sketch first. It seems bizarre that
a sketch made before and a sketch made during the
creation of the protrusion should have different
behavior.
Is there a reason for this difference (i.e. the sketch
made during is completely inaccessible but a sketch made
before is accessible and no way of changing the former to
the latter)?
Thanks.
Edited by: reg2117

 

[dakeb1]

Used to be you could only use sketches within the feature. External sketches is a recent innovation. I guess the old way has been retained for those that prefer it.

 

[kdem]

Not that I know of. The reason for the differenceis the external one is a stand alone feature and the other is internal to another feature. An internal sketch defines the geometry for a feature. An external sketch is used as a reference for the internal sketch of a feature. When you create an extrusion using an external skecth ProE creates a dependent internal sketch feature.


One thing that may work for your purposes is to create a sketch feature that references the geometry of the extrusion and use thatfor your other geometry. Depending on what you're after it should update accordingly and you wouldn't need to specify new references for failing features. However, geometry variations, which is what having an external sketch is good for, could be a challenge.


As for redefining feature references, since section isn't being changed you may only lose one reference. Without knowing the geometry it's difficult to tell you what referencescould be lost.