[ghorrocks]

Have you read the FAQ I quoted earlier on this? https://www.cfd-online.com/Wiki/Ansy...do_about_it.3F

In your case the instructions to use double precision numerics and a smaller time step are the way forward. Also, you need to check all the other things as well.

[SeVV]

Thank You very much for reply. I`ve just changed the total simulation time to 0.01 s and the timesteps to 0.001 s and solver has finished calculation without any errors. These are so small values. Is it notmal/typical situation?

[ghorrocks]

Yes, that is normal. That is why it is in the FAQ.....

[SeVV]

Sure, I`ve read this helpful FAQ, especially the part about the "overflow" solver error. I was reducing the value of timestep but I didn`t expect that this value should be such small.
I`m still considering whether the steady-state simulation isn`t a better solution for this case than transient. I`ve just read that it is also allowed to perform a steady-state simulation in situation when steady conditions are assumed to have been reached after a relatively long time interval and I suppose this case is going to be stable after some time. What do You think about it?

[ghorrocks]

If you only care about the final steady state flow (if there is a steady state flow) then you should do a steady state simulation. They are much faster and easier.

[SeVV]

I was obtaining the "overflow" error in steady state simulation too. I`ve tried to improve the mesh quality, especially (as I read in FAQ) the aspect ratio. The simulation now is going to about 30-40 iterations and then the "FINMES" erros occurs. I`ve read the topic about it (Finmes error) and as You suggested there I was trying to change the turbulence model. Performing the simulation with few turbulence model I`ve tried to use (k-epsilon, SST, k-omega) and it still causes the "FINMES" error (different turbulence model allows to reach different iteration number). What else can I improve in this case? I`m attaching the output file with SST turbulence model try (it was too big so I`ve compressed it).

[ghorrocks]

Your simulation uses extremely small time steps. How large is this thing you are modelling? If it is of the scale of a few cm across then this is a sign that your simulation is highly unstable and it is having to use really small time steps to try to converge it - but ultimately failing as it gives a overflow error eventually.

Your model is quite complex with a multiphase model, porous regions and several domains. I would simplify it and check the models work by themselves. For instance, does it work with the porous regions and all the domains, but with single phase air as the only fluid? Or if you remove the porous regions does it work then?

Mesh quality could also be a contributor.

[SeVV]

The diameter of full grinding wheel is 40 mm (I use the quater of it) and the diameter of workpiece and ambience domain is about 50 mm so it isn`t really big but these are real dimensions. The single phase simulation was working when I was trying it few months ago but results were not so good (due to "just any" setup - I suppose). I will try to remove the porous domain today and see does it work.
Anyway I was trying to improve the aspect ratio of mesh because there are still few elements of aspect ratio value of 10, maybe it is still a problem for the solver to converage the simulation?
I`m trying to reduce the value of aspect ratio and as I read it is the ratio of longest element diameter by the shortest element diameter. It means that the best way is to obtain the equilateral triangle. I`m using the path independent type of mesh (I`ve read that it is good for imported geometry and mine was created in autodesk inventor). The problem is that I`m trying to determine the 60 deegrese angle but I don`t know how to force it in the mesher to obtain equilateral triangle shape elements where it is possible.
By the way, I successfully ran the simulation solver once when I was trying to proceed the transient simulation (simulation time 0,01s and timestep 0,001s) but the result was not so good..
Im attaching the URL to a short avi video below:
https://mega.nz/#!hWRCQK5Z!HRbPIKBcO...NV8rPwHqEJb9xs

[ghorrocks]

The purpose of running the simpler simulations (single phase, no porous region) is to determine what is causing the convergence difficulties. Then you know what part of your simulation you need to work on.

Make sure you use adaptive time stepping for all your simulations. If you just guess a time step you are bound to get it wrong and get misleading results. So run the single phase and no porous region simulation with adaptive time stepping and see how they go.

[SeVV]

Ok I`ll try it, thank You. But as I understand, the timestep setup is available only in transient simulations (which are more difficult to converage?) and maybe it is better to stay in steady state simulation type? Correct me if I`m wrong, please.

[ghorrocks]

If you only care about the steady state result then do a steady state simulation. Transient simulations are more complex and much slower so you would only use them when you had to.

[SeVV]

I`ve checked following combinations of steady-state simulation:
-changing the porous domain to fluid (air) domain -> overflow error;
-reducing the simulation to single phase (air only) -> solver completed and looks very realistic;
-performing the simulation as the multiphase (air+water); setting the same temperature to all domains; selecting the "homogeneous model" for the turbulence model and for multiphase in "fluid models" lap-> solver finished but results are poor (for example there is no velocity change in the water domains).

I`ve found some information about steady state time controling: https://www.sharcnet.ca/Software/Ans.../i1313401.html
But to be honest, I`m not sure which timescale control should be more appropriate in this case.

Is it any possibility to obtain more than one keyframe after solving the steady state simulation?

[ghorrocks]

It looks like the porous region is a cause of problems. There are many options which assist in convergence for porous regions, you should read this section of the documentation carefully and try some options.

Time scale is steady state is straight forward: If you have convergence problems, use a smaller time step. If it is converging but slowly then use a larger time step. Some other comments are in the FAQ: https://www.cfd-online.com/Wiki/Ansy...gence_criteria

keyframes on steady state simulation: What do you want keyframes of? A steady state simulation just has a single result.

[SeVV]

Why do You think that the porous domain causes the problem? The issue was still present when I`ve changed the porous domain to fluid domain everything seems to look fine when I`m reducing it to singlephase.
So when I will enable the rotation of grinding wheel and the workpiece (in opposite direction) the steady state simulation result will show me just the single frame in which the steady state will be achieved?

[ghorrocks]

Sorry, you are right. I misread your last post.

If the rotating wheel and workpiece is linked with a GGI then I presume you are using frozen rotor frame change model. This will simulate the flow taken from the flow at that position in the rotation.

[SeVV]

I`m still trying to achieve proper results of just flow without the grinding wheel rotation in steady state simulation. I`ve observe very strange (for me) situation of the velocity values. I don`t understand why the velocity of both air and oil (now it is the water for simplicity) is raising after outflowing from the channels. As I know the velocity should be higher in the regions with higher pressure (in this case inside of the pipe channels) than in the regions with lower pressure (in this case in the area of fluid outflow to the ambience). I`ve tried to change the value of reference pressure (0 and 1 atm) but that has not changed anything. What could be wrong with this simulation?
I am attaching few images of CFD-POST results.
Best regards.

[ghorrocks]

I do not understand what you are modelling or how you are modelling it so I have no idea.

But the general principle for debugging CFD simulations is to start with simple models and check they are correct, and then add the physics one step at a time checking that the results are good all the way along. Then if something weird happens you have some idea of where to look for a solution.

[SeVV]

Thank You for suggestion. I`m proceeding with adding simple steps one after another and It`s getting better. Now I`m considering which morphology type (dispersed fluid or particle transport fluid) should I use to simulate the oil mist which consists of oil droplets carried by the air stream?
I`ve found following definitions:
A dispersed fluid
is a fluid that is present in discrete regions that are not connected. Examples are water droplets in air or gas bubbles in a liquid.

Particle Transport Fluid is used for fluids when using the Particle Transport Model. The morphology option can be set to Particle Transport Fluid or Particle Transport Solid in CFX-Pre. Gas and liquid particles should use the Fluid Particles option. Currently both models produce the same results because the same drag law is used for fluid and solid particles.

It`s not clear for me should I treat the oil droplets as a fluid particles carried by the air stream or as a dispersed fluid?

Thank You again for Your help.

[ghorrocks]

A dispersed fluid uses a Eularian model. A Particle Transport Fluid uses a Lagrangian model. Whether the Eularian or Lagrangian model is suitable for your case is a fundamental decision so you should make sure you have read the documentation carefully so you know what these options mean.

[SeVV]

I`ve found some description of Eulerian and Lagrangian approaches here:
https://www.sharcnet.ca/Software/Ans...g_eul_360.html
As I understood (in simplifying), the Eulerian aproach is using the static area of mesh and the fluid flows throught this grid, when in Lagrangian aproach the mesh is moving withe the fluid flow, right? It`s still difficult to feel the difference in using it to describe the real process. For sure it is important what I need to achieve as a result?
Let me show three pictures of what I am trying to simulate.
Picture 1 shows the Grinding Wheel with the 'surrounding-nozzle' put inside the grinding wheel (one orange channel provides oil and the second orange channel provides compressed air to the nozzle which together gives us the oil mist on the nozzle outlet).
Picture 2 shows the grinding wheel inside the workpiece in ready-to-grinding position with two visible nozzles which provides the compressed cold air.
Picture 3 shows the formation of oil mist which is a little bit hardly visible.

Which method (Eulerian or Lagrangian) and which model (homogeneous or inhomogeneous) will be more appropriate in case when I want to achieve following results:
-the velocity of oil mist,
-the velocity of air stream,
-location of oil during the grinding process (general location - just to know how the oil behave and where is it collecting, not the specific location of every singular oil particle),
-the temperature changes on grinding wheel external surface and on workpiece inner surface.

I˛ve found in the Ansys CFX tutorial the following sentence: 'Disabling the homogeneous model allows you to specify a unique velocity field
for each fluid.'. As I understand, this is the tip for me. If I want to see the velocity of oil mist and air stream separately I need to use inhomogeneous model, right?

Best Regards