NX4 How to create a flat pattern?

[jmgford]

I have created several sheet metal parts and created flat patterns ofthem in the model. How do I select them in the drawing so I can show the part in a bent state on one sheet and show the flat pattern on another?

Also, how do you display bend lines?

 

[JohnRBaker]

Are you using the new NX Sheet Metal and if so, have you created a 'Flat Solid' of your sheet metal part file?


John R. Baker, P.E.
Product 'Evangelist'
UGS NX Product Line
SIEMENS PLM Software
Cypress, CA

http://www.siemens.com/ugs

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

 

[jmgford]

Yes, I am using sheetmetal, and I have created a flat solid.

 

[hudson888]

Usually if you have the sheet metal license you can go into Application>Sheet metal>Forming flattening, and tools flat pattern. This will create curves of a flat pattern.

It is quite good for most simple applications and somewhat capable of keeping up to date with changes to the part design associatively.

There are advanced techniques associated with unfolding shapes that are other then flat with simple flanges. This usually means pressed sheet metal parts.

What John has alluded to is that with an unfolded solid you had extract the curves etc as required. If you are already at that stage then your next step should be straightforward.

The flat pattern technique that I described has the advantage that you could equally derive the flat pattern for parts not created with sheet metal flange features.

Best Regards

Hudson

 

[JohnRBaker]

What I WAS GOING TO SUGGEST is that when one creates a Flat Solid the system automatically creates an additional Reference Set named 'FLAT_SOLID'. Now after you've created your first drawing sheet with the views of the formed sheetmetal part, open your second sheet and use Insert -> View -> Add View from Part... and select the file name of your original sheet metal part and place that view on the second sheet. Now it will initially look like the base view on your first sheet, but that's OK. Now open the Assembly navigator and you will note two components, but one of them will have a icon idendifier that looks like block over a drawing sheet (also it will be white and not yellow). Anyway, select that component and the with the MB3 (right mouse button) over the selected component select Replace Reference Set and select 'FLAT_SOLID'. After that update all the drawing views and you should now have a view of the flattened solid on you drawing.

Note that for NX 5, we are now going to automatically create an actuall drawing view using wireframe geometry and it will properly define fonted lines for the break lines as well as provide automatic annotation for the angle and direction of the breaks. This drawing view can then be added to the drawing instead of having to add the second component and change reference sets.


John R. Baker, P.E.
Product 'Evangelist'
UGS NX Product Line
SIEMENS PLM Software
Cypress, CA

http://www.siemens.com/ugs

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

 

[jmgford]

John,

When i attempt to add the second part view, I get an error message that it is cyclical?

 

[JohnRBaker]

You have to be working in the Master Model mode where the Drawing is an 'assembly' with the part file as a single level component.


John R. Baker, P.E.
Product 'Evangelist'
UGS NX Product Line
SIEMENS PLM Software
Cypress, CA

http://www.siemens.com/ugs

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

 

[edwink]

how do i create a flat solid? i cant seem to figure it out.

 

[JohnRBaker]

If you're in NX Sheet Metal, to create a flat solid, select the last icon on the main Sheet Metal toolbar or go to Insert -> Sheet Metal Feature -> Flat Solid... (again, the last item on the drop-down menu). You then selet a face that the 'unfolding' will be relative to, as well as an edge to define the X orientation of the file model.


John R. Baker, P.E.
Product 'Evangelist'
UGS NX Product Line
SIEMENS PLM Software
Cypress, CA

http://www.siemens.com/ugs

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