Is there a way to save a sketch for another model

I have just completed a model for a sheet-metal part that has been extruded to a dimension of .030" thick , it has a snowflake design pierced out of the center, and has several protrusions that are bent up at angles, etc., around the outer edge. I now need to use the same sketch that forms the profile of this model and I need to extrude it the opposite way (into a female extrusion), and I want to know how to salvage the original sketch so that I do not have to do it all over again. Solidworks must have made allowances for something like this situation. If I roll back the design tree to the original extrusion, and go to edit the sketch, I cannot exit the sketch to extrude it the way I want to, because when I exit the sketch, it reverts back to the extruded model. I even tried to delete all the steps that were taken back to the original extrusion, in hopes that I could do what I want to do with it then do a save as to something other than what it is now named. I am hoping that someone here with more experience at Solidworks than I do, (which is not a whole lot), will give me a clue as to a procedure that I must use to salvage this sketch, and bring it into a newly named part. I am thanking that person/persons in advance. Ben

Easy method is to dimension your first sketch with no relationships to reference geometry, creating a sketch thats fully defined, but floats with respect to sketch origin. Then dimension to the origin, thus making the sketch fully defined. You can then select that sketch in the feature manager tree, hit the standard edit-copy command.
Open your new part and select the plane that you want the sketch placed upon. Edit-paste. Your sketch is now inside the new part. Constraints and dimensions get maintained, with the exception of dimensions to origin, which can be made easily.
Easier would be to make a different configuration of the same part. That way changes made to the driving sketch will propegate to both mating parts.
Lastly, you could accomplish the same through an assembly. Put the first part in an assembly, then insert a new part into the assembly ( this will be the mating part ) and use the convert entities sketch tool. The advantage here is that changes to your original part will still propegate, however, you have the option to break the reference to the first sketch, thus locking your second profile from changing when you change the first.

You have some options. You'll have to see which works best.
You can use copy/paste, but ther will be no link to the original.
If you have an assembly that contains both parts, you can use a derived sketch. Read up on those in the help to see how they work.
You could also look into using sketch blocks to save the sketch out to a block file which both parts could maintain a link to without an assembly. That seemed brittle when I tried it in the past.

Not quite understanding all of what you are trying to accomplish, I think you should be able to use the original sketch and "Convert Edges" into a new sketch. This way your sketches will be in context and any changes to the first sketch will also change your features further down the feature tree.
Are you creating a sheet metal part and its corresponding tooling or are you creating two distinct sheet metal parts?
A bit more detail on what you are trying to accomplish would help us give you a better answer.
Regards,
Anna Wood http://designsmarter.typepad.com/solidmuse http://www.phxswug.com
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