[nihil2718]

Greetings,

I am working on the simulation of flow inside a centrifugal fan, the first stage of design validation was a steady-state simulation where everything ran smoothly.

For the next stage of my design, I must run a transient simulation (this is because I need to do acoustic analysis), however, despite a lot of attempts the solution diverges after a couple iterations, can't even complete one time-step. (I always get the floating point exception)

Has anyone faced a similar issue? Please find details below

Steady-state info

1. Pressure Inlet
2. Mass flow outlet
3. k-w SST turbulence model
4. rotational speed = 25,000 RPM
5. Interface= frozen rotor
6. Monitor was placed to check the convergence of the pressure rise across the fan

As stated everything good with steady state.

For transient simulation I started with the same B.C's and a time step of 6.67e-6 (aware that I should do sensitivity analysis on this later on), I also started with the DES turbulence model and after failing with that, I tried some computationally simpler ones without success.

I think that summarizes everything, I appreciate any guidance or tip.

Regards

[vinerm]

Is this in Fluent or CFX. Though valid, frozen rotor is not a terminology we use in Fluent. Is it full model or periodic model?

[nihil2718]

Originally Posted by vinerm

Is this in Fluent or CFX. Though valid, frozen rotor is not a terminology we use in Fluent. Is it full model or periodic model?

Hello Vinerm, thanks for your reply. I am doing it in Fluent (so MRF it is) and it is a full model. I already did both steady and transient in CFX without any problem.

[vinerm]

Could you share a snapshot of two settings in your case?

1. Cell Zone Conditions
2. Boundary condition for the interface (is it interior between rotating and stationary frame or an interface?)

[nihil2718]

Please find below the information,

1. Cell zones
There are two cell zones, impeller and casing, both fluid. For the transient simulation impeller zone has mesh motion activated.

2. Boundary conditions at interface

What I did here was just create and name the interface after loading the mesh in Fluent (the name of the interface is "this is it").

[vinerm]

That's good but I apologize for not being more descriptive. I need to look at the conditions you have for cell zone. So, you need to open cell zone conditions and not just the tree, the option where frame motion and mesh motion are applied.

[nihil2718]

Not at all!, my apologies for missing that info. Please find the cell conditions attached.

Let me know any other info you want to check.

Thanks

[vinerm]

Now, check two things.

1. Is the axis of the rotor really aligned with z-axis as given in the mesh motion setting? Since axis is not visible in the images, I can't say that. Also check if the axis passes through the origin. For MRF, these settings, if improper, will let the case run but lead to wrong results. For moving mesh, case will not run.

2. Type of interface. What kind of settings have you used when defining the interface? Could you share that image as well? Before sharing, you may look at the first point. If that is the issue, you do not need to share the image and your case should run fine after defining proper reference point and rotation axis.

[nihil2718]

1. Yup, double checked, 100% sure it is aligned with the z-axis

2. I attached the image when I defined the interface

Regards

[vinerm]

It seems to be all good. Last thing to check is if the motion is correct. With mesh motion setup, Fluent allows you to move the zone without any simulation. This is doable from Run Simulation panel (also from Dynamic Mesh panel). Display the mesh of the rotor alone and then use Display Zone Motion to observe the rotor move. Check if it moves properly or not. If it does, then the case would require a thorough check. If it does not show the expected motion, then you would be able to find the reason. Ensure to save your case file before displaying the zone motion because Fluent does not bring it back to the same position once the zone has moved.

[Andrea1984]

Hi Jorge,

this puzzles me since usually unsteady algorithms are more stable than steady ones.

What p-v coupling algorithm are you using? What is the Courant number value associated with your time-step? And what discretisation schemes are you using in time and space?

Also, are you using a psuedo-transient formulation for your "steady-state" run?

Cheers,
Andrea

[nihil2718]

I checked the mesh motion and it seems fine the impeller rotates properly.

I keep thinking what can be the source of the problem but can't come with anything significant. If you come across any other parameter/setting I could check, let me know. Thanks again for the interest!

Regards

[nihil2718]

Originally Posted by Andrea1984

Hi Jorge,

this puzzles me since usually unsteady algorithms are more stable than steady ones.

What p-v coupling algorithm are you using? What is the Courant number value associated with your time-step? And what discretisation schemes are you using in time and space?

Also, are you using a psuedo-transient formulation for your "steady-state" run?

Cheers,
Andrea

Hi Andrea, thanks for your message.

I attached and image with the info you requested for how I am trying to run the transient simulation. I am not quite sure what to answer in my selection of the time-step, I went for a relative short time-step (basically one time step for every degree the impeller rotates) as a starting point and was planning to do a sensitivity analysis on it later on.

How would you define the Courant number for this case?

For the steady-state I did use the pseudo-transient formulation with default settings, I used quite extensively to create the characteristic curve of the fan.

Regards

[vinerm]

If the impeller rotates as expected, then the only thing left is numerical setup. Since the time-step is already very small, problem could be with initialization or meshes at the interface. Since you already have MRF results, initialize using those and not from scratch. Secondly, check if meshes on both sides of the interface are similar to each other in size (possibly, you have already ensured it).

[Andrea1984]

Hi Jorge,

I am not a Fluent user anymore but you should have a Convective Courant Number variable available to plot (if it is not, you should be able to create it using a custom field function). It is true that your time-step "sounds" small in absolute terms, still I would make sure that the maximum Courant number is below 1, especially when using PISO for pressure-velocity coupling. I would also suggest to test other pv-coupling algorithms less sensitive to the Courant number value such as SIMPLE or SIMPLEC.

Finally I would switch all the spatial and temporal discretisation schemes to first order until you fix your convergence problems. I am particular suspicious of the BCD for the convective term in the momentum equation. Why BCD and not 2nd order upwind (if you want to retain 2nd order accuracy)? After all, you are performing a (U)RANS simulation, BCD is more for LES and can lead to stability issues.

Andrea

[nihil2718]

Originally Posted by Andrea1984

Hi Jorge,

I am not a Fluent user anymore but you should have a Convective Courant Number variable available to plot (if it is not, you should be able to create it using a custom field function). It is true that your time-step "sounds" small in absolute terms, still I would make sure that the maximum Courant number is below 1, especially when using PISO for pressure-velocity coupling. I would also suggest to test other pv-coupling algorithms less sensitive to the Courant number value such as SIMPLE or SIMPLEC.

Finally I would switch all the spatial and temporal discretisation schemes to first order until you fix your convergence problems. I am particular suspicious of the BCD for the convective term in the momentum equation. Why BCD and not 2nd order upwind (if you want to retain 2nd order accuracy)? After all, you are performing a (U)RANS simulation, BCD is more for LES and can lead to stability issues.

Andrea

Hi Andrea,

Well I was using that particular configuration of spatial and temporal discretization schemes because for my analysis I need DES turbulence model and those are the schemes recommended in the users guide.

I did a rough estimate of my model to see what the Courant Number should be and it turns out it should be on the order of 10^-7, so I run a simulation with the steady-state one as initial values and still got divergence(I follow your advice and decided to run everything with first order accuracy and just the k-w SST model for turbulence). I attached an image of the residuals and of my monitor.

Any ideas on what could be the problem?

Regards

[nihil2718]

Originally Posted by vinerm

If the impeller rotates as expected, then the only thing left is numerical setup. Since the time-step is already very small, problem could be with initialization or meshes at the interface. Since you already have MRF results, initialize using those and not from scratch. Secondly, check if meshes on both sides of the interface are similar to each other in size (possibly, you have already ensured it).

I took for granted that the size at the interfaces were similar, however I am not sure to tell whether it is appropriate or not, I attached the interface sides for each component and I appreciate your comments on it.

Regards

[vinerm]

Looking at the front image won't help. You need to observe the elements in the plane of rotation. That will show edges of the mesh capturing the curvature, similar to an octagon circumscribing or inscribing a circle. Both boundaries should have enough elements along the curvature or else there will be one element going inside the other and that will cause trouble.

[Andrea1984]

Hi Jorge,

I can't think of any obvious reason for this behaviour. I thought about possible issues with your mesh at the interface but this should show in your steady-state calculation as well.

Have you tried SIMPLE instead of PISO (retaining first order discretisation for everything?).

Also, why are you using 1000 iterations per time step? Is this in conjunction with some residuals-based criterion? I tend not to use the latter for transient simulations. I usually adjust the number of iterations per time-step based on a drop of about 2 orders of magnitude is the residuals. Normally I start with a low time step (max Co ~ 0.1 or even lower if necessary) and high number of iterations per time step (around 100), and then gradually increase the former and decrease the latter until I reach a good compromise between convergence and runtime.

Andrea