Import DXF Flat - Bend Lines

[Mechman50]

Quite often I import Autocad DXF sheetmetal flat patterns, which include bend lines. I then convert the bend lines, in the sketch, to reference lines. I then extrude and convert to sheetmetal. Now I want to use those reference lines as bend lines, but "add bend" will not allow me to select reference lines as a bend curve, and if I try projecting sketch to a new sketch to derive the bend lines, NX only projects non-reference sketch entities. What method would not force me to re-sketch the bend lines manually?

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NX 8.0.3.4

 

[JonSelby]

Apologies if I've missed the point but ...

Don't convert the bend lines to reference only.
Then when you do what you describe as an "extrude and convert to sheetmetal" just select the perimeter edges of the part for the extrude, not the bend lines.
If you set your "curve rule" (on the "top border bar") to be "connected curves" or "tangent curves" then you can whistle round the part only selecting what you need. (I'm wondering whether you have this set to "feature curves" at the moment?)

As an aside ... you might get a more robust model by creating a sheetmetal 'tab' rather than using the extrude.

Jon

 

[Mechman50]

Thank you Jon. I did find the filter "connected curves" which will allow me to leave the bend lines as non-reference.

"As an aside ... you might get a more robust model by creating a sheetmetal 'tab' rather than using the extrude." Not quite sure the advantages of using "tab" in this instance. Maybe a little more explanation?

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NX 9.0.3.4

 

[JonSelby]

Hi Mechman50

Yeah sorry ... scrub the robustness comment!
In your instance (and probably most) there is likely to be no difference.
It's probably a personal thing that I like to do things 'by the book' where I believe you would normally start a sheet metal model with a 'tab'.
Strictly speaking the 'convert to sheet metal' is for where you maybe have a model that performs one function in your design and you effectively re-use (maybe wavelink) the geometry to drive a sheetmetal part (for say a cover around it).
Being pedantic, it does result in two entries in your history tree where you could have one (which is hardly a problem) and does mean that the model can't be adapted through the sheet metal preferences.
I will often model something in 0,7mm and then find that it's maybe not stiff enough so I tweak the preferences to 1,0mm and the whole model updates accordingly.