Transient Blade Row model Fourier transformation error
 

Hello everyone.
I am trying to analyze gas turbine 1st stage with transient blade row model. I am using fourier transformation and Rotor-stator option(beta feature).

In the display monitor, the message at below has displayed.




ERROR #999100267 has occurred in subroutine gKCsFCCsPS.
Message:

Unable to compute interface connectivity between the following domain interfaces:

Phase Corrected domain interface : R1 to R1 Periodic 1
Sampling domain interface : R1 Internal Interface 2

for this serial/partitioning run. Likely causes are:

1) The mesh has been transformed using single precision arithmetic at some point.
2) The single precision solver/partitioner is being used instead of the double precision solver/partitioner as recommended for the Fourier Transformation model.

If 2) is not the case please increase the expert parameter "ps mapping check tolerance" to a Value larger than the current value: 1.000E-04.



I confirmed that mesh has been transformed using double precision, and also double precision solver is being used.
So I looked for "ps mapping check tolerance" but there wasn't any tolerance like that in expert parameters.

I am using ANSYS 15.0 and If someone have any idea of this, please give me any advice. Thank you.

I am not sure, but I think the Phase Corrected Interface and the Sampling Interface are not physically matching.

The name for the Sampling Interface being suggest it is referring to tip gap interface (usually named <Component> Internal Interface <N>) instead of the sampling interface between the two passages.

Hope the above helps,

Hello!

Do you solve the problem yet? I'm using CFX 16.0 TBR-FT now and facing the same problem. Could you help me on this please? Thank you very much.

Same problem in Fourier Transformation method
 

I am simulating a Francis turbine using FT Method and I have the same problem , have you solved the problem? If yes, How do you solved the problem?

Anyone solved it?
Thanks

Error
 

Has someone solved this error? Also me have the same problem, I followed the youtube guide modeling impeller vaneless volute but the partitioner interruptes with the same error

Two things to keep in mind:

When doing replicating the mesh for the passage, you must use the Turbo Rotation option. Do not use the Rotation option unless you are going to type 16 decimal digits for the rotation angle.

Once the definition file is created, you must always run in double precision for Fourier Transformation cases.

Both items are mentioned in the documentation for transient blade row guidelines.

Thanks for your advises. But after having these two things in my CFD setting, I still got this problem. Wired.

Hi Ahmed,

Have you solved this problem?

Best regards,
Young

Hello dear Young :) I do not remember why I did write this reply :D anyway tell me about your machine type and the problem again, also, you can watch my tutorials about CFX setup, they may help you more...the playlist is attached, it contains all the simulations...Danke!

https://www.youtube.com/watch?v=QfSe...xqdJbZmagGCTop

Hi Ahmed, thank you very much for your reply. I like your videos. They are quite informative. But there is no exactly same case as mine. I am doing a flutter calculation of radial turbine.

The problem is solved anyway. I will note it down later in this post.

Best regards,\Yang

Possible solution to this error
 

Dear all,

After fighting against this error for days, I found my solution. So I just note it down here. If someone happened to encounter the same problem, check this first.

The reason for my error comes from the steady state CFD calculation, which is used to initialize transient CFD calculation. It should be calculated with double precision. But before, I did not notice that from the CFX tutorial.

Actually, this is also mentioned in CFX manual.

Best regards,
Young

Thanks, :)

I checked the double precision button for both steady state and transient blade row; as well as changing cfx (beta) to cfx https://www.cfd-online.com/Forums/cf...formation.htmlbut still the error exists. What else do you think could cause this problem?

The Fourier Transformation model requires two passages. The usual way for obtaining the two passages is to mesh a single passage, and replicate the passage one more time by one pitch.

In CFX-Pre, there are two option for the replication:

Rotation: it requires the angle to be rotated, i.e. one pitch. If using this option, you must enter as many significant digits as possible, and even then it does not guarantee it will be perfect.

Turbo Rotation: it requires information about the blade row: passages in 360, passages to be modeled, and passages in the provided mesh. This method has minimal roundoff, and it is the most used for turbomachinery modeling.

The above must be done from the steady-state solution setup, and throughout any variants of the setup.

It is not only about running the ANSYS CFX Solver in double precision.

Thank you for your reply.
Although it didn't solve my problem, I'll consider it whenever I have to replicate a mesh.
I also cannot find the expert parameter: "ps mapping check tolerance"

Is your mesh conformal (1:1), or largely non-conformal between the periodics, and the sampling interface?

Both of them are conformal. Do you think I should change it?