How to make a straight part curved in an assembly?

[JL_N]

Hi,

I would like to model a straight part for 3D/2D-documentation purposes but in reality the part would be assembled in a groove on an assembly and I would like the part geometry to follow a curve on the groove. The same part would be used twice in same assembly and in two different grooves which have different curves.

My own thought was to make the part flexible and get it to follow sketched line on the groove but I can't figure out how to do that properly. Could you help to determine which would be the best way to achieve this.

Attached image to hopefully clarify what I'm requesting.

I'm using Creo 8.

Thanks

[tbraxton]

A spinal bend should enable you to create the two nonlinear geometries.

To Create a Spinal Bend (ptc.com)

[Patriot_1776]

Spinal bend would be great to have at assembly, I'd been wanting it for YEARS for this very reason, but so far in Creo 8, it's not available in assembly mode....unless I'm missing something.  I have to make the spine curve at the part level.

I think the workaround could be is to create the curve in a skeleton model at the assembly, and use that to drive the assembly parts including the spinal bend spine curve, that way all the relevant geometry is controlled in one place and is parametric, and then you can use the instance of the family table to show unbent state at the part or subassy level for a dwg, and then bend it as needed at the top assy.  My particular problem was that I had to bend a flat ribbon wire assy at the next level assy, so, that was a real PITA having to bend 5 different layers (power and then return traces, separated by an insulating layer, then the top and bottom insulating layers).  It WAS fun and challenging though.  So, yeah, it would be nice to be able to bend a subassy at an upper level assy level.  PTC, you listening?  Hello?  Anybody?  Beuller???  LOL

[JL_N]

Hi, Thanks for your response. I managed to solve my problem by using spinal bend and taking some help by video linked below by aputman.

Br,

 JL_N

[StephenW]

If your part is a sheetmetal (constant thickness) part, you can also use the flat state instance.

https://www.youtube.com/watch?v=auHnVeODh9E

[JL_N]

Hi StephenW,

Thank you for you answer, my part is not sheet metal, so this is not applicable but I appreciate your response.

Br,

JL_N

[aputman · Accepted solution]

Watch this video, at about the 3:50 mark.  It's in an old version of Pro/E but the principle is still the same.  The guy shows how to create a ziptie that can be modeled as a flexible component (driven by a parameter) using the spinal bend feature.  You can use something similar to drive the part to fit your groove.  If the groove is always circular, this would be simple.  If the groove is irregular shaped, you can copy the groove path into the part file, and create a family table of parts with various groove patterns.  Make the part flexible and enable/disable groove paths as necessary.

https://www.youtube.com/watch?v=kZ9MNP0B8ZE&ab_channel=ECognition

[JL_N]

Hi aputman,

Thank you for the linked video, I managed to solve my problem using two spinal bends and make those flexible features in the part file. Then I used each flexible feature respectively to make the two curves I wanted and after that I suppressed those in the part file to keep it straight for drawing.

Br,

JL_N