Extract Sketch from Protrusion Feature

[fiebigc]

Does anyone know if it is possible to extract the sketch from a protrusion feature? I occasionally find that it would be convenient to take the sketch that was created for a protrusion feature and convert it to an independent sketch feature.

Anyone know if this is possible WF 5?

Thanks!

 

[kdem]

There isn't a menu command for this. Two options are:


1) Edit the definition of the protrusions sketch, copy the sketch entities, and create a new sketch by pasting the entities. This option will keep your dimensioning scheme for the sketch.


2) Create a new sketch using the use edge option and then delete the reference edges in the references dialog to add dimensions.

 

[kenppy]

While is sketcher mode file>save. The next time you want to use it, insert from file. BTW, while creating the first sketch, patrticularly if it's not symmetric, put a point to act as a datum for placing when importing.

 

[fiebigc]

Thanks for the suggestions. I think kenppy's suggestion is the closest solution to what I was looking for. I wish you could simply drag the sketch out of the feature in the model tree similar to pulling out a datum.

It took me a few moments to figure out how to import the sketch into sketcher. Here is what I did.

1. Start sketch feature and setup sketching plane and sketch orientation.
2. Now you should be in sketcher.
3. Go to Sketch > Data from file > File system. There will open up the file viewer to find the sketch file. The sketch file has the file extension *.sec.1.
4. The sketch will then have to be placed.

 

[kthomas]

do an edit definition, get back to the sketch and save the file. Then if you use the pallet when you start a new sketch, you geometry should be there.

 

[Nadir]

Kenppy I like thidea of putting a point in as a datum - defo going to use that. Thanks for the tip.

 

[krow72]

Kenppy - I use the same format that you stated except to make it easier on me I do a save as and name the file to something that makes since to me. That way instead of having a file named S2D0001.SEC I can name the file hexagon.sec or whatever the shape represents to me. It makes it easier to pick out.

 

[kdem]

If you're intending to use the sketch in other parts you might want to save as a seperate file. However if you are just intending to use the sketch within the same part (which is the way it sounded) there isn't realy a need to save the sketch externally and then import it. Importing from file and copy/paste do the same thing. Thechoiceof using one over the other, IMO, are what do want to achieve and which method do you prefer.