Learning Forum

[Hazem]

Dear members, 

I tried solving a 2,700,000 element structured mesh of good orthogonal quality (0.93) and low skewness using the K-Omega model and PRESTO setting, during initialization it mentioned that it didn't reach convergence. I started calculating with 1000 iteration and the value of Cm seemed to stabilize before fluctuating intensively towards the last 200 iterations.

While solving it kept printing " reversed flow in 7000 faces on pressure outlet 8" What does that mean ?
Any clue regarding what could be done ?

[Karthik Remella]

Hello,

Couple of thoughts:

• Do you have inflation layers in your mesh? What y+ value does your first layer thickness correspond to? What wall treatment model are you using?


• What are your solver settings are you using? Can you try the Coupled Pressure-Velocity Coupling scheme with Pseudo-Transient?


• Could you please share some screenshots of how you have set-up your model? Are you using MRF here?


• What are your initial conditions?

Please share your model details through screenshots here on the community and we will try to help you with this.

Thank you.

Best Regards,

Karthik

[Hazem]

Thank you for your message! I'd appreciate it greatly if you could help me.

I understand Y+ is instrumental for the model(Please find a Y+ snapshot at the very end) to be solving correctly and for K-Omega it should be less than 1. in my case here it's around 200 on average of all zones ! which could be why the solution diverges quicky and stops calculating around 50 iterations now (indicates divergence even during hybrid initialization at the 6th iteration) .  I'm not using a wall treatment model and I'm not sure how to make inflation layers.

Solver settings I'm using is "SIMPLE" , I'm not sure how pseudo transient is or why would it be suitable here for the model. Also I haven't change relaxation factors from the defaults

Regarding the initial conditions, I have 6 zones (Inlet, outlet, outer domain which is the big cylinder, inner domain which is a small cylinder of rotating air just surrounding the turbine, domain wall which is the shell of the outer big cylinder, and blade walls.

the inlet is a velocity inlet with 8m/s,
outlet is a pressure outlet of zero gauge (Also tried setting it to -10pa gauge and tried making it "Outflow" and nothing changed)
inner domain takes a rotational speed of 19.2rad/s 

blade walls is a moving wall "no slip" and rotates with zero relative to the adjacent (which is the inner domain)

domain wall is a stationary wall "Specified shear" and set to 0 so it would be like a cylinder shell with shear on it.

(all of them have axes of -1,0,0 as the air inlet direction is -X)

 

this is Y+ of all zones

 

This one is for only blade walls

Thanks in advance !

 

 

[ashrafazlan011]

Hello, 
can you show me in figure displays, for inital condition

[Karthik Remella]

Hello,

Could you please try and use First Order Upwind for both Turbulence parameters? Also, can you please try the Hybrid Initialization? Once you finish your Hybrid Initialization, could you please initialize using FMG? You can do this using the following TUI command.

/solve/initialize/fmg-initialization

Also, could you please reduce your under-relaxation parameters to see if you can get convergence?

Another suggestion - you could run the first-order discretization for pressure in the beginning. Once you have a convergence solution, could you please switch the pressure to Second-Order upwind and try?

Please change the 'Pressure-Velocity Coupling' to Coupled and then you should be able to check the 'Pseudo-Transient' option. This might help. Which Fluent version are you running?

Thanks.

Best Regards,

Karthik

[Hazem]

Dear Karthik,

Thank you for your help, the suggested settings didn't help to make convergence. coupled setting had a bad effect too (I'm solving steady not transient btw)
The initialization through fmg worked well and the solution gave a slightly better convergence as the continuity was e+02 at the end. but that's not good enough.
Also the value of the coefficient of moment was way lower than expected, this is all because the Y+ value is too high.
I tried reducing it with inflation at the blade walls but this had terrible results on the rest of the hex mesh ans spoiled the quality awfully, inflation won't work with hex mesh.

I'm not looking to make the inner domain structured too, that way I'll have edges in there around the blades to do bias and reduce the Y+ through that.

Any clue how to structure this rotating domain at the geometry 

 

[Karthik Remella]

Hello,

There are a series of 4 videos that extensively discuss decomposition. Here is the first part of the series. Please use these videos to understand how to decompose your geometry better to generate a hex mesh.

https://www.youtube.com/watch?v=P19GOTQWmc0

If you wish, you could create a structured mesh everywhere except in the region close to the blade. A tet mesh might work there (perhaps). This might give you more robustness in terms of creating the necessary inflation layers.

Another way to move forward might be to use the new Fluent Meshing with Watertight Geometry Workflow. Again, this will create a good quality unstructured mesh (tet / poly). Here, you might be able to obtain more control on the meshes you are trying to create.

I know this is not a complete answer but (hopefully) it gives you a starting point.

Thanks.
Best,
Karthik