Get sketch "out" of Extrude feature

SW 2004 Delete dependant feature Highlight the feature RMB and uncheck "also delete absorb features" in pop up dialogue box. This will leave you with the sketch used to create the solid feature

Or

Hide solid body Create a new sketch and by converting the parent feature sketch onto a plane or surface or start from a new sketch from scratch. Alter the new sketch as required Extrude the sketch and make sure to uncheck the "merge result" check box. Edit all other features dependant upon the parent feature and uncheck "merge result" check box for each. Now hide the parent solid body

Kman

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

Nice, (i.e. reuse same sketch to extrude without using convert entities.) Kman

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.

How does using "select contours" cause more issues than convert entities? Kman

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.