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DB@HuscoInt12-Amethyst
12-Amethyst
January 9, 2026
Question

Easier Ways to Create Circular Bends or Crimps in Solid Parts (Not Sheetmetal)

  • January 9, 2026
  • 3 replies
  • 151 views

In Creo 9.0.10.0, creating circular bends or crimps with varying thickness is often a bit clunky, as it requires cutting material and then re-adding the crimp or bend feature, usually as a revolve or sweep. I’m looking for a simpler, more efficient way to do this, similar to how Sheet Metal bends work, where bends can be suppressed in a simplified representation at the part level. This would be especially useful for parts that currently use family tables or flexible modeling. I’ve looked into the X-Section Property Control options in the Spinal Bend feature, but I’m not sure if any of those settings can be used for multi-directional bending. Specifically, can things like moments of inertia or centroid coordinates allow a bend towards the center of an axis or csys. I'm hoping to find another method that can directly apply the deformation like a bend to the existing length of material without cutting out features. Any advice from the community on using Warp, Spinal Bend, or other commands to make this easier. Thanks

Attached is a section view of a part with a crimp I'm trying to accomplish.
Attached is another section with the current results of using spinal bend.

3 replies

T
22-Sapphire II
tbraxton22-Sapphire II
22-Sapphire II
January 10, 2026

It is not clear from your post but are you looking to have model(s) that represents the drawn ferrule (or cup) geometry with and without the crimping operation? The varying thickness constraint immediately has me leaning towards a surface model that is offset and solidified. I don't think I would start with a solid model and then add the crimped geometry. If you want to drive all of the geometry from a master model then inheritance features might work for this IMO better than a family table in this case). What is the use case in Creo or downstream outside of Creo that is driving you to represent the geometry in both states?

D
DB@HuscoInt12-AmethystAuthor
12-Amethyst
January 12, 2026

These are housings that are crimped using a machine and we need to show the formed model in the assembly and the preformed model on the drawing. For constant thickness parts like sheet metal its easy with the flat rep and master reps.

 

With housings that are variable thickness I'm really interested in a workflow that is similar for solid parts. We are currently using flexibility for new parts and legacy models still use family tables. (all sheet metal models have been updated to use simp reps)

My main goal is to find a method that is the same for both modeling modes so you don't have to do two different things.

The method for flexibility with an entire feature set is clunky and you should be able to bend circular edges around an axis using a spine or warp. (If not then I will turn this into a feature request) 

T
22-Sapphire II
tbraxton22-Sapphire II
22-Sapphire II
January 12, 2026

A couple of comments based on my experience. Warp is not an "engineering design" feature so as a general rule I would not use it to control anything for manufacturing purposes. Have you looked at a toroidal bend feature to get the crimped geometry? The toroidal bend feature applies two bend transformations at the same time. It is not a sheet metal feature but I am assuming that you are not modeling the housings in sheet metal mode so in that case it should be available to you.

 

Creo does not have functions to generate metal forming ops "automatically" crimping, swaging, and the like are not sheet metal operations so I would not expect a Creo sheet metal part to handle this type of forming operation as a bend table is not capable of yielding accurate geometry results. When designing parts that require progressive die operations (swaging, deep drawing etc.)  I have always used part mode to define the geometry I want to receive as a finished part.

 

Here are a couple of parts (orange and red) that were designed in Creo and formed from 6000 series aluminum. They were modeled in part mode with consideration given to manufacturing constraints of the processes used to make them.

 

tbraxton_0-1768238742843.png

 

kdirth
21-Topaz I
kdirth21-Topaz I
21-Topaz I
January 12, 2026

When I need something like this, I usually look toward using flexibility.

 

To create the model I would:

  • Create the model uncrimped.
  • Suppress the crimp area features.
  • Create a crimped version of the crimp area.
  • Suppress the crimped version and unsuppress the uncrimped features.
  • Define Flexibility in the model properties, selecting features for both uncrimped and crimped features and dimensions that I want to control.
  • Define flexibility when placing model in assembly, suppressing the uncrimped features, unsuppressing the crimped features and adjusting dimensions as needed.
There is always more to learn.
A
anursinghCommunity Manager
Community Manager
March 9, 2026

Hi @DB@HuscoInt,

 

I wanted to see if you got the help you needed.

If so, please mark the appropriate reply as the Accepted Solution. It will help other members who may have the same question.
Of course, if you have more to share on your issue, please pursue the conversation. 

 

Thanks,
Anurag 

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