NX Extrusion Bend

[mike734]

Hello all. I have a straight extrusion in NX 7.5 solid modeling that I need to bend to a certain radius/angle. I saw a previous post about this but it didn't completely solve my problem. I would like to model a tool, a chisel for example, straight and then bend it to an angle afterwards instead of sweeping or revolving the bent portion. This is how it will be done in production. Any advice would be greatly appreciated. Thank you.

Mike

 

[JohnRBaker]

Could you provide at least a picture of the part before it's 'bent' and some idea of where and to what extent the 'bend' would look like, at least in some schematic/hand sketch like image?

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
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To an Engineer, the glass is twice as big as it needs to be.

 

[mike734]

Here is an image of the round rod and the surfaces that I think I need. (the sufaces are actually a revolved line and extruded line). I tried making the flat surfaces the base and the curves surface the control but then the rod goes on an angle from the original to the top of the curve. Thank you very much in advance.

 

[JohnRBaker]

Attached is an example (NX 7.5) that may not work exactly like you might wish, but I think the final result will be very close.

Open the file and edit the Solid 'bar' by double-clicking. When the Swept dialog opens, in the 'Guides (3 Maximum)' section of the dialog, select the 'Select Curve (1)' item and then de-select (shift-select) the Green curve. Now select the Blue curve and hit OK.

The result will still be a single seamless solid 'bar' since the original sketch, made of a line and an arc, was 'converted' (associatively) to a single segment spline by creating a 'Join' curve feature (the Blue curve). Also note that the length of the original sketch is controlling the length of the solid 'bar' so is you edit the sketch named 'Final Shape', changing the length of the straight section and/or the radius and angle of the curved section, when you update that sketch, the length of the 'guide' curve used to create the solid 'bar' will change as well. Note that there was NO attempt to compenstate the length of the bar, as it went from the unformed to the formed state, for the effect that deforming a shape like this would have on the actual profile and length of the deformed portion of the solid 'bar'. In other words, the result is an idealized shape.

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.

 

[mike734]

John thank you for the help. To clarify you're suggesting that in lieu of bending a previusly straight model, that I should just model the item straight. I certainly could do this but I was trying to utilize the ease of modeling when everything is straight and then incorporate a simple bend. Is this not possible? There will be much more detail on both ends of this sample rod. Thank you again.

Mike

 

[JohnRBaker]

We support functionality like that with sheetmetal (in the NX Sheet Metal modules) since there we're dealing with explicit and unique types of geometry, thin-walled and constant thickness, where we can more easily predict what the final shape will look like. Even then, the normal workflow is to design the as-desired final formed shape and then reverse-model using unfolding/unforming tools, which results in what the original flat 'blank' would need to have been to give the final formed shape.

With an arbitrary shape it's very difficult to apply a 'bend' which would result in a reasonably accurate final shape.

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.

 

[mike734]

John,

Thank you very much for all the help and time you've provided. I suppose it makes sense why NX functions this way.

Another quick question I had is how can I snap to existing geometry in the sketch module. I am able to use project curve to be able to snap a few lines on the end of existing features, but these lines are able to mvoe anyway. Am I missing something big here. It seemed innate to other systems to snap to existing geometry easily.

Thanks you,
Mike

 

[JohnRBaker]

When you've in the Sketch Task there's what's known as the 'Selection Scope' setting on the Selection Bar. Make sure that it's set to either 'Entire Assembly' or 'Within Work Part Only' and NOT 'Within Active Sketch Only'.

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.