[Gert-Jan]

For now, let it run over the weekend.

However, I don't want to frigthen you, but you are dealing with really difficult physics (and CFD). In fact the speed of sound can drop significantly in mutliphase problems. I wouldn't be surprised if the speed of sound of a mixture with 10% of gas will be below 50 m/s. Then your results with >100 m/s for gas and oil can be unrealistic since the flow can be chocked.

So at least you need to perform calculations using Total Energy and make sure your speed of sound is implemented correctly.

To start, look at Fundamentals of Multiphase Flows from Christopher E. Brennen, paragrpah 9.3.

[SeVV]

But how can I achieve the speed greater than 50 m/s? This is the maximum velocity of rotating grinding wheel in this process. And why we need to monitor the sound speed? Is it connected with the CFX limitation to subsonic flows? I can see that this is what the chapter 9.3 of mentioned book is about so I will read it and maybe than it will be more clear to me, thank You very much.
I miss one thing. I set the value of 10 m/s of oil mist inlet velocity but it is for test only. I don`t know this value. I only know the mass flow rate (nozzle manufacturer papers). The poroblem was that when I was setting the value of bulk mass flow rate to 2.85 g/s (ca. 2.75 for air and 0.1 for oil) results were very poor without any signs of oil mist flow. But before I run the settings which I show You previously (1m m/s of on oil mist inlet) I`ll try again with bulk mass flow rate instead of the velocity on the inlet and run it for longer period of time to see what is going on. I am using 'double precision' so it takes a lot of time. I am attaching the graphs after almost 40 iterations (still in progress). The local time step factor is set to 2.5 for now.

[ghorrocks]

Your previous results show velocities of up to 100m/s. Gert-Jan raises the important point that the sonic velocity of multiphase flows can be much less than of the pure fluids. This means you may need to consider compressible flow effects, and if that is so that means you need to run a full total energy equation in your simulation so you cna capture compressibility effects - this will complicate things further.

The convergence graphs you attach show you are a long way from convergence. You will need to run a lot more iterations.

Regarding your inlet condition - it looks like you should do a simple model with just this boundary condition so you can get this right before you return to your full complex model. You have to get these details correct and understood on a simple simulation before working on the full simulation.

[SeVV]

Thank You for information. I will try to enable total energy equation and proceed the simulation. Now I am attaching the graphs of simulation which is running for over 2 days. I`m afraid it wouldn`t be any better, would it? Almost 1800 iterations and it doesn`t look to going to converge. I think I need to terminate it?

[Gert-Jan]

Try reducing the timescale factor to 0.25.

[SeVV]

Ok, I`ll try it. Should I have to keep the local time scale or change the type to physical? And should I stop the solver, change the time step and continue or run it again from the beginning? And can I refrain from switching on the total energy equation at this point?

[Gert-Jan]

- Changing to physical timestepping can be done on the fly, but requires some specific knowledge. I would suggest to change it in Pre, write a new def file and use your current solution as an initial guess.
- Total energy can only be implemented in Pre.

[ghorrocks]

This question is now an FAQ: https://www.cfd-online.com/Wiki/Ansy...gence_criteria

I do not agree that physical time stepping requires specific knowledge. You need a starting point, and physical knowledge can help there, but from there you just adjust according to how convergence is going. If it is monotonic but slow you increase it, if it is jagged and oscillating you decrease it. As you adjust it it is OK to start with a guess because you can refine it from there.

[Gert-Jan]

I meant that you need specific knowlegde to be able to CHANGE IT ON THE FLY from Local Timestepping to Physical Timestepping. And on the fly, I mean change it while running, without stopping your calculation, which might save you some time.
But if you don't know how to do this on the fly, CFX might crash. Therefore it is safer to stop your calculation, change it in Pre, write a def with physical timestepping, run this def with your current solution as an initial guess.

[SeVV]

Ok, I`ve changed it from the CFX-pre to avoid solver crash.
Glen, I`ve read the information about when to use the local time step in FAQ but I`m not sure do I need to keep trying with local time step or change to physical time step in my case. For now I`ve changeg the local time step factor from 2.5 to 0.25 as Gert-Jan told me. As I understood after reading the FAQ and after reading one of Your previous post Glen, I should change the timestep for last few iterations to physical when simulation is going to converge, am I right?
Some time ago I was dealing with the physical timescale according to the fluid residence time but in my case there are many domains and two fluids so I need to refer my physical time step to the longest residence time (which I can view on the cfx-post)?

[ghorrocks]

Gert-Jan - thanks for the clarification, I understand your point now.

SeVV - Yes, the last iterations should be physical time stepping but only when it is just about converged. Your convergence charts do not look like they are approaching convergence to me.

I reckon there is a pretty good chance this simulation is not steady state and will require transient simulation to obtain convergence. You will note this is described in the FAQ. So I would try a transient simulation.

[SeVV]

I was afraid that the transient simulation will be inevitable but I am still givin it a little chance in steady state due to the graphs which I`ve obtained after changing the local time scale factor from 2.5 to 0.25 as Gert-Jan suggested. Let me join another few pictures of mentioned graphs after over 500 iterations. It is still the isothermal simulation. Is there any chance to converge? Glen, You`ve written few posts ago: "If it is monotonic but slow you increase it, if it is jagged and oscillating you decrease it". In my case, some values seems to be nearly monotonic and some are jagged (especially RMS P-Vol). Maybe running it for many longer may be effective and lead to convergence? Does any another time scale factor changes make sence?

[Gert-Jan]

I adviced you to set the Time Scale Factor to 0.25.
However, I was not aware that you were running with Local Time Scales.
My advice to use a Time scale of 0.25 was based on the assumption that you were running with Physical Timestepping.

As Glenn mentioned, you should switch to physical timestepping. You should only use Local Time Stepping to obtain a rough estimate (or initial guess) in a short period of time. It is less suitable for final solutions. And, as Glenn told you, it is likely that your solution is transient. So you should try that as well.

Regarding your convergence, it is useless to give my opinion as long as you run local timestepping. Also, you should go to Pre to create monitoromg points in which you monitor velocity, pressure, volume factions, etc during your calculation. These should become flatliners when you convergence is reaching the end.

[SeVV]

I`ve abandoned the steady state simulation for now and I`m trying to perform the transient one as You`ve adviced me.
I`ve read about the adaptive time step in the FAQ and it seems to be the safiest and most stable for beginners? I was considering what values for adaptive time step choose and and how many loop iterations set? I`ve set the adaptive time step from the 0.005 s to 0.1 s and 10 loop iterations (default setting-maybe it is to less?). Is it good approach? Another very important case are initial values of rotating domains. Is it better to set the initial value of my 3 rotation domains as rotation or as stationary? Now I`ve set it as stationary but I`m not sure is it good solutions with such a high velocity of 2285 rad/s. Maybe the expression with adaptive velocity would be more proper? I think that the biggest problem is to input the initial values of fluid pressure and velocities when setting the domain initial as rotational.
And another question, do the values of residuals, imbalance etc. need to be on such a low level as in steady state solutions or it isn`t so important in transient approach?

Best Regards.

[SeVV]

I`ve abandoned the steady state simulation because proceeding it with physical time step was not possible. Now I`m still trying to perform the transient simulation. I`m trying to set the proper time step. I`ve read in the FAQ that adaptive time stepping is helpful in this case. I`ve set the min time step value to 0.0001 [s] and max to 0.01 [s] and the initial time step to 0.0005 [s]. I`ve inserted three monitor points near the fluids outlets. I don`t know why the velocities are proper and stable only for a while and then they increase (attached image). The velocities are raising even to few thousands of m/s. I`ve changed the model to the total energy as You`ve adviced me last time. I`m still trying to establish isn`t the mesh qualiy responsible for this issue. Here are my mesh metrics which I was taking care of (mayby another parameters are also important?):
-Element quality: min = 0.2; average = 0.8;
-Aspect ratio: max = 10; average = 1.8;
-Skewness: max = 0.8; average = 0.2.

Can I ask You for any advice please?
Best Regards.

[ghorrocks]

In future please attach your output file.

Your simulation is diverging. That's all.

Have you set a maximum coefficient loops of 5? Because the previous time step does not appear converged yet it accepted 5 coeff loops and moved on, despite the convergence being very poor.

I would recommend making the minimum time step 1E-10 [s], and an initial time step much smaller than you currently use. Even if you start with a ridiculously small time step the adaptive time stepping can increase it from there. In this case you obviously need to ensure it converges properly right from the start.

[SeVV]

I've set the maximum coefficient loops of 20 and even more. Initial time step and minimum time step values were reduced as You`ve adviced too (few different options including the 1e-10). I've tried very hard but unfortunately the RMS values are quite good only till a moment when the simulation time is reaching about 9.9e-4 [s] (it takes about 15 hours of solving). After reaching this point the RMS values are growing drasticallly and does`nt want to fall. I`ve tried both isothermal and total energy models and tried of adding the buoyancy value too. Is there any another thing I could check? I am adding the output file, mayby it could be helpful.. I hope so..
Thank You in advice and best regards.

[ghorrocks]

Your initial time step is too big. It only starts converging when it has a time step of about 4e-7. I would start with 1e-7[s] for the time step to be safe and let it grow from there.

I also prefer setting the Target Minimum Coefficient Loops to 3 as the adaptive time stepping works a bit better than the default settings.

Have a look at the post processor to try to work out why it starts failing to converge at time step 700/800. You might be able to see some flow feature which is causing this.

While you are getting the basics right you should consider using a coarse mesh and/or first order time stepping. When you can get it running in a simplified form then try a full accuracy run.

[Gert-Jan]

A few things:
- I can't recall exactly what you are solving, but velocity is relatively high and geometry is relatively small. So, switch of gravity. I don't expect this playes any role. Did you make any analysis on this?
- Are you sure Cimtech has a specific diameter of 0.002 mm? i.e. 2 micron. That is very small..........
- You calculation starts to act wierd at time step 782 (First 'F' appearing in your linear solution) Make a backup and look in Post what goes wrong.
- You are running transient, but with frozen rotor. Is that a valid combination?
- You should set minimum values for your fractions. Say 1e-5. That might help a lot.
- I would choose for SST instead of k epsilon. It's validity range its larger.
- you could try the expert parameter volfrc sumapp = t

[SeVV]

Welcome again after break.

I`ve included the following suggestions:
-there is no buoyancy now;
-I`ve switched the turbulence model do SST again.

Moreover:
-I was dealing with the "Air at 25 deg. C" gas model and I`ve switched it to "air ideal gas" model;
-I`m proceeding with steady state again.

The simulation is converging in this set up after about 900 iterations.

First of all I wanted to thank You for previous help which effect is the convergence of simulation.

I have some another questions.

1. I'm trying to understand the velocity values in different approaches in CFD-Post. I don`t know how to understand the situation in which for example the air velocity has the maximum value of 63 m/s (Grinding wheel is rotating with velocity of 50 m/s) but after switching to the velocity in strn frame the maximum velocity is about 111 m/s. I`ve read that values shown in stationary frame are showing "absolute values". So how to understand, the situation, which I`ve obtained? Could You help me please with interpretation? Please find attached pictures.

2. I`m using the "frozen rotor, general connection" interface between the rotational grinding wheel domain and stationary ambience air domain. Is it proper approach in this case? Do I understand it well that using for example translational periodicity interface is proper ony in situation when we are not dealing with the full geometry (for exapmle the quarter of rotating grinding wheel)?

3. I want to set the values of:
-ambience air to 18 degree C,
-steel workpiece to 100 degree C;
-grinding wheel to 40 degree C;
-dispersed oil to 18 degree;
-compressed cold air to -2 degree C.

My most important goal is to chceck the influence of cold air and dispersed oil on the ambience and workpiece temperature in the simplest way. Which way would be the easiest in this case? Could You help me a little with initial values and set up? Is it possible to do in steady state?