Exporting mode shape into CFD mesh

  • 155 Views
  • Last Post 15 March 2019
  • Topic Is Solved
ricardooliv22 posted this 08 March 2019

Dear all,

I wish to make a Fluid-structure interaction simulation for a blade.

In order to obtain the aerodynamic damping of a certain mode, I need to perform an unsteady CFD simulation of the flow around the structure in question while it is vibrating with a certain amplitude and with the mode in question.

In conclusion, after performing the modal analysis I need to export the desired mode shape and project it onto a dynamic CFD mesh to perform the unsteady simulation.

Since I havent yet found a specific way of doing this I was hoping someone in here would have the answer for this question.(I want to use CFX for this CFD simulation)

Thank you for your time,

Ricardo Oliveira

Order By: Standard | Newest | Votes
ricardooliv22 posted this 11 March 2019

Dear abenhadj,

Thank you for the reply.

The video you present shows how to export a deformed geometry from a static structural analysis.

Unfortunately this is not what I am looking for. I'm looking for a way of exporting the shape of a certain mode (from a modal analysis) and projecting it onto a dynamic CFD mesh in CFX.

Best,

Ricardo Oliveira

rgpatchi posted this 12 March 2019

Dear Ricardo,

To export the mode shape and frequency from a modal analysis in a format friendly to CFX use the EXPROFILE command inside the /POST1 processor.

Note this command isn't supported in Distributed ANSYS, so you need to have "Distribute Solution (if possible)" unticked in Tools->Solve Process Settings->My Computer --> Advanced.

In a Mechanical Modal analysis this means adding a command snippet under "Solution" in tree (i.e. with result objects).

 

Please have a look at EXPROFILE command in ANSYS Help documentation for further information:

https://ansyshelp.ansys.com/Views/Secured/corp/v193/ans_cmd/Hlp_C_EXPROFILE.html

 

The commands needed will be something like:

SET,1,1              ! mode 1

CMSEL,S,BLADE          ! select blade named selection nodes

ESLN                     ! select attached elements

EXPROFILE,SURF,MODE,0,'MESHDISP',DISP1,CSV              ! export normalised mode shape on surface with field name 'meshdisp', file name disp1 extension CSV

ALLSEL             !select all

 

where BLADE is a named selection of faces representing the blade surface.

 

More info on the process here:

https://ansyshelp.ansys.com/Views/Secured/corp/v193/ans_cou/Hlp_G_COUunidir_1.html

 

Check that you're not using an unsupported mode-extraction method such as unsymmetric, damped or qr-damped. This is unlikely unless your modal analysis is doing something fancy like rotordynamics or acoustics.

 

Hope this helps. Please do let me know if you have any questions.

 

Best Regards,

Rohith

ricardooliv22 posted this 12 March 2019

Dear Rohith,

Thank you for the reply, this seems exactly like what I am looking for!

I will keep you updated on my developments.

In the mean time,do you think there could be a way that you share the information posted (on the links) in a different form? Because being a student I do not have access to the forums mentioned..

Best!

Ricardo

SandeepMedikonda posted this 12 March 2019

Students should be able to access ANSYS Help. 

Please see this post.

ricardooliv22 posted this 14 March 2019

Dear Rohith

After trying to implement your method I have come across some dificulties since no output file is being generated.

This message appears after the simulation but I cant really find any valuable information on the solution information file.

I used the code as you presented (and created a named selection for the blade) so I dont really know where I amgoing wrong.

No CFX project is associated in workbench. Might this be an issue?

 

Best,

Ricardo

 

 

ricardooliv22 posted this 15 March 2019

Update: 

I was not checking the post output correctly.

 

Having checked it, I realized that I was not using cmsel correctly.

Now that I am its all working fine!

 

Thanks!

Close