[pkgupta]

Recently I have been working on a multiphase solid-liquid flow in horizontal pipe in CFX. I observed the following:
1. When my pipe length was 100D (D=pipe diameter), the solver messaged "placing wall at the outlet". Here I had used tetrahedral+prism meshing for full 3D pipe.
2. Then I extended my pipe domain to 140D, and this time it worked smoothly for the tet+prism meshing.
3. However, when I replaced the mesh with ICEM Hexahedral mesh, keeping same L=140D, full pipe, I am receiving again the error at the start of the solution, "Wall placed at the outlet...."




Can anyone throw some light on why I am receiving different response from CFX solver for same physics problem. Of course the mesh is changed, but that's the purpose of mesh independence study.



My main issue is why CFX solver issuing error when the mesh structure is HEXAHEDRAL (prepared in ICEM CFD)?

[Opaque]

I think you are confusing matters. Mesh independence study is not about changing mesh types, it is about mesh refinement.

You have not stated if your hybrid mesh is more or less refined than your hexahedral mesh.

For any mesh type, you should be able to refine the mesh, i.e. reduce the mesh spacing, such as the solution no longer changes.

If you switch mesh type, you must be careful you are within your already mesh spacing; otherwise, you must continue your mesh refinement study until it shows it is mesh independent (type and spacing)

[pkgupta]

Thank you for your kind reply and clarification. Yes, you are correct. Mesh independence means refining the mesh.


And sorry for posting my question here. I thought this is CFX forum. Could you please tell me where exactly shall I post problems on CFD?

[ghorrocks]

This is the CFX forum, you posted your question in the correct place.

Another way of looking at it is that if changes like changing the mesh type makes a significant difference to the result then your mesh is far too coarse as changes like this are affecting things. When you have achieved mesh independence then small changes in the mesh do not affect the result.

Also note that mesh quality is probably changing between the inflation+tet versus hex mesh. Some simulations are very sensitive to mesh quality - this often applies to multiphase models, and you are doing a multiphase model so you may be more sensitive to mesh quality than the default settings.

[pkgupta]

Thanks Glenn! However, I did try your suggestion, and still the problem persists. In my meshing, I kept the exact same grid spacing near the wall.


The tet+prism mesh is running smoothly in SERIAL processing mode.


Here is the CFX output log of the failed simulation for the Hex-mesh:
Total Number of Nodes = 179456 Total Number of Elements = 70800
Total Number of Hexahedrons = 170800
Total Number of Faces = 15888

No isolated fluid regions were found.
| A wall has been placed at portion(s) of an OUTLET |
| boundary condition (at 38.5% of the faces, 24.3% of the area) |

| ERROR #004100018 has occurred in subroutine FINMES. |
| Message: Fatal overflow in linear solver. |

| The ANSYS CFX solver exited with return code 1. No results file has been created.
End of solution stage.

This run of the ANSYS CFX Solver has finished.

================================================== =============


I tried SERIAL, PARALLEL, keeping mesh distance equal but nothing works. For the HEX mesh, the solver senses some flow reversal at outlet even though the domain outlet is well away from such regions of flow,as the flow is certainly fully developed


Can you please help me out on why CFX giving such error?


Thanks in advance!

[ghorrocks]

Your total number of nodes is 170k. This is a very small mesh so this is more evidence to suggest your mesh is far too coarse.

There is no point in trying to infer conclusions from a mesh which is far too coarse. It will give you very inaccurate answers, so your conclusions will be very inaccurate.

You have to get a mesh independant solution first.

[pkgupta]

Thanks for your Quick reply Glenn!


I understand that meshing may not be proper. Okay, let me put some more details here on what I have tried so far:


Geometry: Straight pipe, D= 103 mm; L = 140D, wall roughness=2 micron


Physics: Solid-liquid concentrated flow through pipe, volume concentration ranges from 10% to 45%; particles size = 270 micron; flow velocity = 3 and 5.4 m/s; KTGF model, k-e model with scalable wall functions.


Analysis: Steady state, 3D



Boundary conditions: Inlet - velocity inflow; outlet - pressure outlet (static pressure); wall - rough wall


Observations:



(1) Tet+prism mesh: nearly 437340 elements, Inflation set for maximum thickness = 10% of pipe Diameter, no. of layers = 9, growth ratio = 1.4


When I carried out simulations with TET mesh, SERIAL processing, solutions converged. I validated the results with known experiments, and they are within 10% agreement


(2) ICEM Hexahedral mesh: In order to reduce computational burden, I took HALF PIPE (Symmetry conditions), this time first grid height = 0.5% of pipe D; no. of layers = 13; Total no. of elements = 432000. All other conditions remain identical.
Solutions converged in both SERIAL as well as PARALLEL processing mode.


(3) ICEM Hex mesh:This time I considered FULL PIPE with all the conditions identical (even for the meshing, and first cell wall distance).


But, no matter what change I made as per suggestions, the CFX solver either
- exits with error code 1
- wall placed at outlet, solver exits
- and some times even without any error, solver exits saying all residual meet their convergence criterion.


I hope this time it is detailed for other to know what problem I am facing.


I can certainly do MESH REFINEMENT study, but no matter what refinement I do for the near-wall cells, the SOLVER exits, with either of the three messages.


Any suggestions please......what is going wrong here

[ghorrocks]

There is no problem with CFX modelling full pipes with hex meshes. I can say that with some confidence

There is a some problem with your setup. There are many, many things it could be. You are just going to have to look at the details and work it out - or apply some engineering judgement and decide you don't have time to work it out, the other two approaches are working so I will just use them.

A further point - What is the KTGF model? CFX does not have a KTGF mode. Are you modelling the multiphase with a Lagrangian or Eularian approach? Please be aware that the lagrangian model in CFX is not suitable for volume fraction loadings as high as 10-45%. The only particle model CFX has which can handle particle loadings that high is the eularian-eularian model (as it has particle collision models - is this what you call KTGF?).

[pkgupta]

Thanks Glenn! As you said, I need to dig deeper to excavate useful info from the available resources.

Yes, I too am confident that CFX will work as I have read many articles reporting such flows.

I shall come back after doing my work to report.

Thanks again!

And BTW, KTGF is Kinetic theory for granular flows. I was using Eulerian-Eulerian modeling

[ghorrocks]

I presume you have read the CFX Theory manual, the section on Multiphase/Solid Particle Collision Models. That is the section of CFX which covers that physics.

[pkgupta]

Hi! Glenn. Glad to be back with good news!


You were right about the mesh density. When I increased my mesh to 0.8 million cells, all my cases for two-phase solid-liquid flow converged. However, to achieve convergence at higher solids volume concentration, I had used "parametric continuation"; i.e., using the output results from previous simulation (for lower solids concentration) as initial guess field for the simulation at next higher solids concentration. This way I was able to achieve good results (compared with experimental) for solids concentration of 10% through 45%.


But I have one more clarification. Though the outlet boundary is far away from flow disturbing conditions (here 140D length), without parametric continuation, the solver was again placing wall at the outlet, and sometimes FINMES error, and other times solver exit without any error (but residuals taking extremely low 1e-14 etc.)


So, if I keep initial guess field value for velocity as a very low value, will the above problem appear? In all my simulations, the velocity is 5.4 m/s. But if I start the solution with a lower velocity, say, 1 m/s or 0.5 m/s, will the outlet problem go away?

[ghorrocks]

You cannot say in general what you need to do to fix initial condition problems. If there was a universal fix, then wouldn't it be implemented in the code already?

The exact initial condition required to get your thing to work will be specific to your case. But I can say that it is common for a requirement for an initial condition to be at least close to the final solution to obtain convergence. Sometimes just specifying an initial velocity field (so the flow knows what direction it should be moving in) is enough, sometimes you need to be quite close to the final solution, sometimes your simulation will converge fine regardless of what initial condition you give it.

But the point I made at the start still holds - you should not infer conclusions from a simulation which is on an inadequate mesh. So until you complete a mesh refinement study and get a mesh fine enough to be accurate you are wasting your time looking at anything else.

[pkgupta]

Hello, Glenn!


How fine should the mesh be? And on what criteria the mesh refinement is ascertained?

For a sufficiently lengthy domain, a course mesh of 0.3-0.4 million hexahedral cells gives proper solution for single phase flows.


However, when I switch to two-phase solid-liquid flow, Eulerian-Eulerian modeling, even a mesh with 0.8-1 million cells seems insufficient!!


So, how do we decide it? I have already tried refinement with respect to y+, and varying no. of grids in axial, radial and circumferential directions, but still the CFX solver hangs due to various reasons, the prominent ones are - wall placed at outlet, and FINMES, floating point error, etc.


Replacing outlet with opening b.c. is definitely not doing me the favor!




However, when I read through various posts here, I found your comments/suggestions, and among it, there was a mention about the wake.


So, my guess is that in my case of two-phase solid liquid flow, the wake or turbulence created by the solid particles might be the cause of "wall placed at outlet..." And this I observed with the convergence behavior. For relatively smaller particle size of 90 microns, the solver ran smoothly. But when the particle size is increased to 270 microns, the solver started giving the message "wall placed at outlet", which I tried to overcome by increasing the mesh density.


Now, currently I am running another case but with increased particle size of 440 microns, and again the same mesh where I had obtained good solutions (albeit using parameter continuation) started messaging "wall placed at outlet" just after 3-4 iterations!!


So, I tried reducing the auto timescale, currently at 0.05, the iterations are going on slowly......


From your vast experience, can you throw some light on what's happening with this case, and whether my hunch that larger particle size create disturbance (turbulence) which might be causing "wall placed at outlet". And what's the remedy, if any?


Thanks in advance!

[ghorrocks]

Question 1: Mesh sensitivity:

To do a mesh sensitivity study, do a run of your current mesh and note the output parameters you are interested in. It could be pressure drop, separation location, particle size, anything. Then remesh using half the element edge length (this means a hex element will become 8 hex elements, and a tet element will become 5 tet elements - so your mesh should have around 5 times to 8 times more elements) and run it again. Compare against the parameters of interest from the previous run. Are you happy to accept the difference in those values? If yes then you have found a mesh which will give you the accuracy you want. If no, then halve the element edge length yet again (so 25 to 64 times more elements than the first mesh) and try again. Continue refining until you get the accuracy you want.

You will find that the meshes required get very big very quickly. CFD is famous for that - that is why a lot of the super computers in the world are for CFD. If you short-cut this and just use a coarser mesh then realise you are saying that you accept a larger error.

Question 2: What is going on with convergence, walls at outlets and particle size?

You would have to explain what you are doing in more detail for me to answer that. Please post an image of what you are modelling, your CCL or output file and some post-processing images of what you are currently getting with the recirculation, flow conditions etc.

[pkgupta]

Dear Glenn!


Thanks again for your kind response!


Yes, I shall try to follow your advise on Question 1 regarding mesh refinement. So far I was trying to get a mesh which I can run on my personal Desktop PC with 8-core 64 GB RAM.



As for Question 2: I will send you soon the details of modelling and output file.


Thank you!

[pkgupta]

Hi! Glenn!


I am sorry I have not been successful in obtaining a starting mesh enough to get a converged solution for a two-particle solid-liquid flow case.
I am limited by the available computing resources at my disposal.


Since there was no starting mesh, I could not do the mesh refinement.


However, I am attaching the OUT file for the same case here for your kind reference:


file:///X:/ANSYS_CFX_Cases/m1b_001.txt

[pkgupta]

Oops! Here is the Link to OUT file

[ghorrocks]

You could always try coarsening the mesh and see what happens.

But if this says you do not have enough computing resources to get the accuracy you want then you have your answer - this model is not possible with the resources you have available.

[pkgupta]

I tried coarsening the mesh, but still the same error, "Wall placed at outlet...."


Then I refined my mesh from 661500 elements to 2396160 hexahedral elements. Yet the same error persists, after 3 iterations only!


Could you extract any useful info from the OUT file?


I am still not very convinced about mesh size? In one Journal paper published in 2009, the authors reported mesh of 385600 elements only, but used Transient simulations. And the paper has reported several cases on mono-size solid-liquid flow validations against experiments.
On that basis only I am wondering why CFX is unable to produce results even with the finer meshes than the reported one in 2009!


After today's run with 2396160 elements, it is clear that it is not the mesh problem. Something else is going on here which we are not able to point to.


Hope you would have some answers...

[ghorrocks]

The "Wall placed at an outlet..." thing is a warning, not an error. The simulation will proceed despite the statement. If the wall is OK then the simulation is fine and you do not need to do anything about it. If the wall is a problem then, some options:
* Use an opening instead
* Have a look at your simulation and work out why you are getting backflow. It is probably a recirculation which goes to the outlet. Then think about what you have seen. Is it realistic? If yes, then your model is correctly capturing the physics but your outlet boundary is a poor choice. I would move the outlet boundary further downstream and/or change it to an opening. If no, then why is your model generating the spurious recirculation? The problem is the recirculation, not the outlet boundary.

CFX is a powerful CFD code with just about any option you could want. And it is accurate and fast. If it is not accurate and fast for you then you have not set it up correctly.