Half Etch in NX Sheet Metal

[baschuve]

Looking for suggestions in creating 'half etch' features using NX Sheet Metal (NX6.0.2.8). If not familiar, the requirement is for the flange feature to be half of the sheet metal thickness from tangent line to tangent line. Tried to use Extrude, however will then not allow unbend or flat solid.

Thanks

 

[JohnRBaker]

Could provide at least a 'picture/cross section' of what you're looking for?

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.

 

[baschuve]

Thanks John. Image uploaded.

Previous to NX Sheet metal, we used modeling sheet metal features to create a zero tangent length flange, that was half thickness, to simulate the half etch bend areas. This does not seem possible in NX Sheet Metal?

 

[JohnRBaker]

OK, this is about the best that I could come up with. While you can NOT use the Flat Solid function to 'flatten' the model, you can produce something which will give you almost the same result by activating the Feature Group which I've named 'Flatten', which consists of two 'Unbend' features. If you wish, you can edit this Feature Group and toggle OFF the 'Hide Feature Set Members' option and then you can see where I placed them in the model workflow. You can also use the Playback toolbar to better understand how I approached the problem.

Anyway, take a look at the attached model and let me know what you think of this approach and whether it could be used to address your type of work.

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.

 

[cmacca]

How about making the half-etch features as extrudes as you already have done but make them the final features in the part nav tree. Now make the feature before the etch extrudes the current feature and then use extract body (in modelling app), make sure assoc and fix at time stamp are checked. Now make sure this extracted body in not on the model ref set and then create a new ref set for the extracted body only. Do a flat pattern for the extracted body ie only select the face of the extracted body. Now hide the extracted body and make the last feature current. You will now have a flat pattern view of the part, the bend lines will also be the centre line of the half-etch features. If you need to add the width of the half-etch to the flat pattern you can add lines to the flat pattern, see the NX Sheetmetal help.

NX 6.0.1.5, TC 2007