Learning Forum

[ferranj2]

Greetings.

I need to conduct a dynamic analysis of a spinning rotor with a customized, time-varying pressure load at multiple RPM settings.
To generate the time-varying pressure load, I want to run CFD of the rotating deformed rotor blade in Fluent using rotating meshes.

To that end, I first apply an RPM of interest as a load in a Static Structural component (in it, I have cyclic symmetry and contact constraints).
In Static Structural, I request a Total Deformation Result.
I use named selections to label the parts of the rotor blade that will be exposed to fluid flow.
Using these named selections, I can get the Total Deformation over those surfaces.
In turbomachinery, this can be referred to as a "cold-to-hot" correction.
Here's where I'm stuck: I want to take those deformed surfaces to a meshing environment (preferably an external one called Pointwise), add the Fan Casing, Rotor Fairing, a Bypass Splitter, and a row of Outlet Guide Vanes to create the model for Fluent.
Caveat: The mesh I use in Static Structural is a second-order mesh, so the surface that I want to take to the mesher is composed of quadratic triangles and potentially, quadratic quadrilaterals.

I've looked online to no avail.
While searching, I've run into one-way and two-way decoupled FSI schemes, but nothing like applying a "cold-to-hot" blade correction to CFD.

Screenshots:

Cyclic Symmetry + Contact Constraints Model:

Deformation Results that I want to use for CFD mesh:

CFD mesh that I would like to make for Fluent but with deformed blades (blades below are undeformed):

[Aniket]

have you checked:

Export deformed geometry from one system to another. | Ansys Knowledge

this shows two methods, first one exports deformed mesh directly, but in your case, you should export STL as shown in the video at the end, and take it to other software such as Discovery or SpaceClaim to assemble it with other meshes

The following articles would be useful creating a solid again from the STL:

https://ansyskm.ansys.com/forums/topic/discovery-spaceclaim-3d-printing-prep-stl-facet-editing-stl-smoothing-reducing-and-regularizing-with-spaceclaim/

https://ansyskm.ansys.com/forums/topic/solid-model-creation-from-stl-in-spaceclaim-2/

https://ansyskm.ansys.com/forums/topic/discovery-spaceclaim-3d-printing-prep-stl-facet-editing-stl-smoothing-reducing-and-regularizing-with-spaceclaim/

-Aniket

Forum Rules & Guidelines

[ferranj2]

Thank you for the links, however, they weren't what I needed. To be fair, I needed to reword the original question. I was able to find a workaround (really a "trick") with named selections.

So:

1) Prior to solving the model, define a named selection that is based on surfaces.
2) Solve the model.
3) Click "Solution (A6)" and towards the top right corner of Mechanical, press the "Worksheet" button.
4) In the worksheet, press the "Solver Component Names" radio button.
5) Right-click the named selection defined during (1), drop-down appears, left-click "Create Total Deformation Result." A new Total Deformation Results appears under the solution of Static Structural 
6) Left-click the newly created Total Deformation Result and change the "Scoping Method" from "Geometry Selection" to "Named Selection".
7) Retrieve the result.
8) "Export as STL" the newly retrieved result.

Step (6) above was the key. 
That one baffled me, because in the worksheet, the result was created based on the surface-based named selection.
I tried this with second-order elements and it seems to work (Tri6's get split into four Tri3's, that's all).