How do I Draft a revolve that is different from its cross section

[ingallspw]

I have a part the has a revolved section. Later in the model history a cylindrical feature was added. Most of the revolve remains and needs to be toleranced but I just want the revolve's features and not the cylinder.

What would be ideal is if I could drop the modeling sketch into the drafting application.

Is there any way to do that?

Thank you all in advance!!!

Keegan Bear
Horton Inc.

 

[JohnRBaker]

Anytime after you create your revolved feature (and making sure that the sketch is 'external', meaning that you can see it as a separate item in the Part Navigator), go to...

Format -> Reference Set...

...and select the Model ("MODEL") Reference Set and then select the Sketch and hit 'Close'.

Now when you create you drawing, the Sketch curves will also be visible in all of the drawing views. If you want to see it in one or two views, you will need to 'erase' it from the other views which can be done either by doing a View Depended edit or by placing the sketch on a different layer in the master part model and then using Visible in View to hide it in the views that you do not wish to see it.

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

To an Engineer, the glass is twice as big as it needs to be.

 

[hudson888]

Keegan,

I had trouble visualising what you wanted to do, maybe a part or a few images might help.

Best Regards

Hudson

www.jamb.com.au

Nil Desperandum illegitimi non carborundum

 

[ingallspw]

Hudson, I attached an example.

http://files.engineering.com/getfil...-888b-d17993ae4f85&file=finish_VS_drafted.jpg

There are many othere fatures intersecting the revolve in real life (more behind the cylindar extrustion) and I only want the sketch.



John,
Do i need to start a new drawing from scratch for this to appear in the drafting app?


Thanks to both of you!!!

 

[JohnRBaker]

If you already have your drawing created, go back to the master part and do what I described, then go back to the drawing and just force a Drawing Update and the sketch should show up.

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

To an Engineer, the glass is twice as big as it needs to be.

 

[hudson888]

Technically you can do what John says. I usually use layers and reference sets with master model concept drawings. So I'd probably use visible in view to capture the sketch or just cheat by creating some "dummy geometry" in the drawing file on another layer, and then use visible in view to filter what appears on the drawing.

I'd have to say that this would be very rare and non standard drafting practice for us, and if we wanted to show two stages of a process then we'd probably create two files for casting and machining, or finished and less finished parts. There is something to be said for reflecting the manufacturing process in your designs. I tend to think that by and large NX has tools intended to support those activities. I can't advise more since seeing the part and knowing what you want isn't the same as knowing why you would want to do a certain thing.

Best Regards

Hudson

www.jamb.com.au

Nil Desperandum illegitimi non carborundum