I am not being shown the option of solid geometry in references of toroidal bend.

[AH_10347263]

I have creo parametric 7.0.

[remy]

You expect a solid geometry option when creating a toroidal bend and it is not offered. you're disappointed. 

In order to clarify your expectations attaching the model shown in the picture will be well appreciated.

[AH_10347263]

my model is creo parametric 7.0

[StephenW]

So I believe a toroidial bend is a "modification" to existing geometry, You are not creating new geometry, you are changing what is existing.

Try looking at a youtube tutorial.

https://www.youtube.com/watch?v=3qsL7nGbxsM

[KenFarley]

We use toroidal bend (Creo 4.0) all the time.

Your screenshot doesn't show anything helpful.

To access toroidal bend it's under Engineering -> Toroidal Bend

Once the ribbon changes to the Toroidal Bend one, click on the "References" tab and click on the "Solid Geometry" (meaning "I want to bend the whole part).

Then you have to define your "Profile Section". It's a sketch with a coordinate system, X axis along the plane of the bend, Y axis pointing in the direction opposite the bend. You must also have some sort of geometry in the section - I've always just had a horizontal line aligned with the X axis of the aforementioned coordinate system. Any length on the line is fine, it doesn't matter.

If you're not seeing prompts, or ribbon changes or whatever, take a screenshot of that and maybe more specific help can be provided.

[LukaszMazur · Accepted solution]

Since Creo 7.0 introduced multibody modeling, the option "Solid Geometry" in Toroidal Bend has been replaced with the collector "Quilts and/or solid body", which is shown in your screenshot. So now, instead of clicking "Solid Geometry" to apply Toroidal Bend to all solid geometry in the model, you need to activate the collector and pick the body you want apply the bend to (you may select only one solid body).