Machining after flat pattern 1

[cubalibre000]

Hi,
we make an hole after the cut of the sheet metal.
It's possible to add a feature after the flat pattern ?
it's not possible, but sincerly I've seen a part in our archive with and estrusion after the flat pattern, then I don't know if an exception or can be possible.

Thank you...

Using NX 8 and TC9.1

 

[carlharr]

Hi, this is not possible because unfortunately flat pattern can't be time stamped.

We found a way around it using the master model drawing method:
- WAVE link a body in the drawing file from the model, at timestamp, before the "after cutting" operations are done
- convert the linked body to sheet metal (convert to sheetmetal command)
- create the flat pattern in the drawing file
- put the WAVE linked body on another layer, so it doesn't appear in drawing views

If you don't use master model concept, you might be able to do something like this in the same file.
You'll need to be careful to make sure SOLID ref set only contains the finished part (for your assemblies), and that weight is correct.

http://www.jcb.com

NX 7.5 with TC 8.3

 

[JohnRBaker]

So what you're attempting to do is add a hole to you model which does NOT appear in the flat-pattern, correct? As if you had cut-out the blank, formed it into its final shape and THEN drilled a hole in the sheet metal part, correct?

OK, if this is what you're looking for, go ahead and create your sheet metal part, WITHOUT the hole(s), create your flat pattern and then leave the NX Sheet Metal module and go back to Modeling. Now go to...

Insert -> Associative Copy -> Extract Body...

...and select the model and with the Setting 'Hide Original' option toggled ON and the others toggled OFF, hit OK. Now add your hole(s) as needed. Now go to...

Edit -> Show and Hide -> Invert Shown and Hidden

...and then go to...

Format -> Reference Sets...

...and select the 'Model ("MODEL")' item and then deselect the highlighted model on the screen using 'Shift+Select' and then hit Concel. Now go back to...

Edit -> Show and Hide -> Invert Shown and Hidden

...and you should see your final model with the hole(s). And if you check your Part Navigator you will see the the Hole(s) are after the Flat Pattern feature, which means that you can now create an Drawing showing both the formed sheet metal part with its Holes and the flat pattern view without the holes, as I've done in the attached example.

Now it is true that if you were to ask for the weight of the part model it would be the combined weight of both solid bodies, the original sheet metal part without the Hole(s) and the final solid body with the Hole(s). Now if you have an Advanced Assemblies module there is a way out of this and that would be to go to...

Analysis -> Advanced Mass Properties -> Advanced Weight Managerment...

...and set the 'Definition' to the 'Model' Reference Set and hit OK. Now only the solids in the 'Model' Reference Set will be considered when the Mass/Weight of this part model is computed and since you've already removed the original sheet metal solid (without the Hole(s)) from the 'Model' Reference Set, the results will now reflect only your final model.

Now if you DON'T have an Advanced Assemblies module, then you'll need to do something more along the lines of what carlharr has laid out.

Anyway, I hope this helps.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

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

 

[cubalibre000]

Jhon,
I've adopted your solution and works fine.
Thanks

Thank you...

Using NX 8 and TC9.1