Wake induced inlet flow
 

Hey everyone, I am trying to model a blade 2D blade cascade in CFX, the cascade has a wake induced inlet flow, experimentally we did this using a squirrel cage type rotor with rods attached at specific intervals. Anyone have ideas how to model the inlet flow?
As I can't do a 2D type sliding mesh in CFX I had thought about mathematically modelling the time dependent inlet flow. What I am finding a hard time figuring out is as the inlet flow is time dependent, or basically the wake is moving from top to bottom with time. If anyone has an idea's to pitch I'd appreciate it.

Why do you need sliding mesh? You can do this is CFX using a moving mesh.

Why can't you just put the inlet flow at an angle and use a normal stationary frame of reference?

Hello SHerif,

There is a tutorial in Fluent "Tutorial 11: Using Sliding Meshes " 2D Tutorial. In fluent problem Fluid phase Velosity (which is given in Fluent around y= -Vx) imposeed under Setup => Cell Zone Conditions.

I want to do same in CFX but i have not foung Fluid Translation in CFX. How can i do it? CFX just have "Rotaion" and stationary" option in "domain"option.

I dont want to give rotaion because i am working on 2D arirfoil(blade).

Could u pls tell me how u did it? It will really helpful for me.

Thank you,

Hey Saima,
I ended up creating my wake generator using a cylinder with the axis parallel to casacade z axis. I think you can do the same, send me an email my email is basically my user name here @gmail.com.
There is linear mesh motion in CFX but if you're creating a linear wake generator it won't work as it will continually move up or down it cannot return to its initial position after traversing a period. As far as I understand.

Sherif

For arbitrary mesh motion then forget about multiple frames of reference and use the mesh motion option. Then you can describe any motion you like.

Thanks ghorrocks, but may I ask if you have two domains one moving linearly and the other stationary how would you define the interface between them for a transient type analysis.

Using a GGI, set to TRS (transient rotor-stator). That is rotating machine talk for update the interface every time step.

transient sliding interface
 

Hello sherifkadry and ghorrocks,

I'm currently simulating the similar situation in cfx. In other words, I'm trying to find out the peak pressure change on both stationary container and moving train while moving train passes in the vicinity of stationary container. The computational domain consists of the moving and stationary domain. Moving domain comprises passenger train whilst stationary domain includes stationary containers.

I've refined the hyperbolic mesh close to the boundary layer of the train whilst it is loose away from the wall. The mesh quality for moving domain is between 0.5-1. It is between 0.9-1.0 for the stationary frame.

I've also chosen translational periodicity between inlet-outlet of each domains to make sure that the information transfer is continuous. Re number for moving domain is chosen as 2.10^5, which corresponds to a 20 m/s.

I've employed the transient LES simulation with a General Connection interface between moving domian and stationary domain (GGI) in the first place to see the effect of passing train on the container. However, I couldn't see enough information transfer from moving domain into the stationary one. Do you guys have any idea of what else I shall check/consider in the model or in the boundary conditions/solver control?

Thanks in advance.

Have you used a transient rotor stator GGI as the above thread comments?

Hey Glen,

Thanks for your answer.

Yes, I've used the transient rotor-stator GGI as a frame model. I think the reason why an adequate information transfer between two domains cannot happen is because of the mesh quality. I've simply modified the mesh around the train. I used to distribute mesh around models by using hyperbolic mesh law, which allows to create a finer mesh around the train whilst it is coarse away from the wall. On the z-direction, I kept the hyperbolic mesh as same, but modified the mesh on the upstream of the flow as `uniform`. Now, the results are promising with comparison to previous attempts.

Attachment 8847

Attachment 8848

Regards,

Berkay