Get sketch "out" of Extrude feature

I have an extrude based on a sketch.

How do I undo the extrude and leave the sketch in my feature tree?

I want to split the extrude in two steps, but want to keep the sketch.

 

Since 2003 we are able to share sketches. All you have to do is expand the
feature and select the sketch, then hit extrude to add another extrude using
the same sketch. Any shared sketch will have a hand under the sketch
symbol. Did you know that you don't have to use the whole sketch anymore.
There is an option to select contours and regions. Using regions can
sometimes allow you to use overlaping contours in a sketch and still extrude
them.

Corey

 

If you delete the extrude the sketch should be left behind. Make sure
the "delete absorbed features" box is unchecked.

 

Delete the extrude in the feature tree and sketch will stay.

 

Barry,

Here is one technique. There are other ways when dealing with
multibodies but construction geometry in my opinion are the simpliest
Step 1
A. If you just created the sketch and are in the Extrude feature you
can use the Cancel Red X mark and return to the sketch.

B. If you already created the Extrude feature, you can select the
feature from the FeatureManager and delete the feature, do not check
the box to delete absorbed features.

Step 2.
The original sketch will remain. Right-click the sketch in the
FeatureManager and select Edit Sketch. Window Select the entire
sketch. All entities are green. Select the Construction box. Your
sketched entities will all turn to construction geometry. Close
Sketch1.

Step 3
Right-click on the Sketch1 located below the Feature name in the
FeatureManager.
Use Show to display Sketch1.


Step 4.
Create the first feature. Select the sketch plane. Ctrl-Select the
construction entities from Sketch1 required to create the closed
profile (for a solid) or open profile (for a thin). Select Convert
Entities. Entities cannot overlap or the sketch is invalid.


Step 4

Create the second feature. Select the sketch plane. The Sketch1
should still be visible.

Utilize Convert Entities to extract the required entities for the
second feature. Extrude the feature.



Regards, Marie

 

You can use the 'Select Contours' in the feature properties and use
the same sketch for some features.

Akiva Litinsky
CAD App. Eng.
Systematics - Tel Aviv

 

It can be dangerous though. As can 'Select Contours'. If you have a
part that uses alot of these, small changes in early sketches can really
mess things up further down the tree. I'd say 'Convert Entities' holds
fewer surprises.

Select contours is however quite nice when you don't want to trim every
line so you have the exact profile you want.

Jim S.

 

If you convert entities, you are still bound by the laws of sketching
with respect to open countours, three or more lines meeting at a single
point, etc in order t make a valid feature from the converted entities.
Select contours gives you more rope to hang yourself with, but you
have the convenience of not having to 'pretty up' the sketches before
making features.

Keep in mind I'm talking about using select contours when additional
sketch geometry is present, and doesn't necessarily represent a
converted edge or face. I didn't make that clear in my prior post.

If you use contour selection to do the same types of operations for
which you used to convert entities, there is little difference.

Jim S.