Flange on extruded feature

[cubalibre000]

Hi,
I would like to make a flange as the image attached, but I can't.
Have you any suggestion ?

Thank you

 

[JohnRBaker]

The extrude feature does NOT have a 'square' end, it's off by 6 degrees. And now that I see why that's the case I think I see what it is that you're trying to do. Well you can NOT do it directly, but here is how I just did it.

First delete the Extrude feature and set SB Flange(4) to the be the 'Current Feature'. Now add the flange that you intended to add originally (I assume that you wish it to eventually align with the other flange so make the angle 96 degrees). Now leave NX Sheet Metal, go to...

Insert -> Synchronous Modeling -> Relate -> Make Coplanar...

...select the bottom side of the flange you just added to the model as the 'Motion Face', select the bottom side the flange that you would like it to align with as the 'Stationary Face', toggle the 'Offset' option in the 'Face Finder' and hit OK. Now go back to the Part Navigator and make the Flat Pattern feature the Current Feature, and you should be all set.

Note that even though the Synchronous edit was performed OUTSIDE the NX Sheet Metal task, your Flat Pattern should still have updated correctly to show the fully developed blank for your Sheet Metal part.

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

 

[cubalibre000]

Thank you John,
your solution works well.
Only one question :
Why have you decided to keep separated the sheet metal environment to the modeling application ?
I find some situations where I need to switch to the modeling environment to complete my design and return in the sheet metal application.
This switch and the relative message, it's a little frustrating for our designers, in 8 work hours.

Regards...

 

[JohnRBaker]

Originally NX Sheet Metal was designed to be a separate extra-cost module and so it was created so that it would be easy to implement in that way and enforcable without a lot of confusion as to when you were in the module and when you were not. However, after all of the initial work was done, including the toolbars and dialogs, it was decided to not charge for it (note that it's still doing a license check, just that everyone is getting free access since the check is basically being ignored by the license server). As a result of this it has the look and feel of being something separate from regular NX Modeling. Unfortunately, unless there is some critical overriding need, I suspect that we will NOT be making any significant changes in this behavior since there would be little to gain and it would in fact prove problematic since we DO charge for the 'Aerospace Sheet Metal' module which is actually built on top of a common architecture with NX Sheet Metal (just with valid license checking).

Anyway, this is something that we're all just going to have to basically learn to live with.

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