[ghorrocks]

In CFX the Eularian model has the fluid flowing over a fixed mesh and the phases are tracked as volume fractions which convect, diffuse and interact with the other phases. In CFX the Lagrangian model models the particles as points with a position in the mesh, forces act on those particles and move them.

Read the documentation on when to use both types of model. If you are going to do multiphase simulations you really need to understand these basic concepts.

And the choice of multiphase model also depends on what the flow looks like and what results you want. Am I correct in saying that when this is operating you have regions of pure air, regions of pure oil, a foamy oil region, and a oil mist region? If so this makes it tricky as mist and foam require totally different multiphase models.

[ghorrocks]

In CFX the Eularian model has the fluid flowing over a fixed mesh and the phases are tracked as volume fractions which convect, diffuse and interact with the other phases. In CFX the Lagrangian model models the particles as points with a position in the mesh, forces act on those particles and move them.

Read the documentation on when to use both types of model. If you are going to do multiphase simulations you really need to understand these basic concepts.

And the choice of multiphase model also depends on what the flow looks like and what results you want. Am I correct in saying that when this is operating you have regions of pure air, regions of pure oil, a foamy oil region, and a oil mist region? If so this makes it tricky as mist and foam require totally different multiphase models.

[SeVV]

Excuse me for so long delay in posting. I was studying the documentation and trying to understand it. Now I know that I want to use a dispersed fluid flow for Oil domain and if it is possible I want to try proceed with inhomogeneous model just to have results of oil and air velocity values separately.

Glen, You`ve wrote:
"Am I correct in saying that when this is operating you have regions of pure air, regions of pure oil, a foamy oil region, and a oil mist region? If so this makes it tricky as mist and foam require totally different multiphase models."

Generally I`m sure that You are right but I`m not sure about the occurence of foamy oil region? Is it the stage of oil mist generation? (pure oil is being aerated by the air (and here we have a foamy oil??) what causes the formation of oil mist?
In results which I want to obtain in my simulation I don`t need to care about the formation of oil mist, I`m only interested of its velocity and area of occurence.
I`ve spent many hours of trying to fine my grid and eliminate any other issues in proceeding with inhomogeneous model and here it is what I`m obtaining now (attached picture 1). I don`t understand why both the oil and air is barely flowing out from the channels (the velocity value from 5 to 20 m/s doesn`t have any influence on it). The situation was completly different when I was 'blowing' with single phase air only - the air and oil streams were much more extensive and also penetrated the grinding wheel (porous domain). What could be wrong with my setup? May it be connected with the timescale of steady state simulation? Now I`ve set the value of about 0,0001.

[ghorrocks]

Foam is like a bubble bath. Some oils form foams easily. Mist is isolated droplets. The important thing is that in foams the bubbles bump up against each other so any relative motion between air (in the bubbles) and fluid (in the films between bubbles) is strongly determined by the bubbles pushing against each other. In mist the air/fluid slip is strongly determined by aerodynamic drag on the droplets. Hence the physics of both these multiphase flows is totally different. That is why it is important to match the multiphase model to the flow conditions.

Your time scale seems very small compared to the size of your domain and the velocities you report. It could be that your flow simply has not converged yet. Increase the time scale and run it longer.

[SeVV]

Glen, in my case the solution was to change the time scale from automatic to physical (what I`ve overlooked) and to increase the time step as You`ve said. I`ve checked the fluid residence time (as You`ve wrote about in FAQ) and use the half of the value as a starting point. Now the time step is 0,01 [s]. I had to decrease the value of dispersed fluid droplet mean diameter (from 0,002 to 0,001 mm) because otherwise FINMES error has occured. Now I`m trying to enable the rotation of the grinding wheel and I have an issue with the interfaces between rotating and stationary domains. I`ve tried to find the analogous application in the CFX-pre tutorial but it seems to be different.
I am attaching the drawing where I`ve marked and described all interfaces and information which domains are rotating. Can You help me with setting the interfaces please? Which type of interfaces should I use? I think that some kind of "sliding" interfaces would be the best solution? Please find attached drawing.

[ghorrocks]

If you are simulating this in a transient simulation your only choice is transient rotor-stator. If you are simulating this is steady state you have more options.

[SeVV]

I am simulating as a steady state simulation. I am using the frozen rotor interfaces (is it good approach?). I don`t know what am I doing wrong but when I set the single phase flow simulation (with AIR or OIL only) results looks fine for me and I wish my final results will look similar (picture 1 - single phase). But when I add the another phase (AIR + even WATER) my results is very unproperly (picture 2 - multiphase). I don`t have idea what factor need to be improved but I`m trying to change mesh, reduce or increase time scale and iterations number.. I didn`t see any tip according to this situation in the FAQ and nowhere else on the forum. Maybe You know what kind of issue am I dealing with, Glen?
Best Regards

[ghorrocks]

Can you show an image showing what you expect the multiphase results to be. Also explain what multiphase model you are using, and why you chose that one.

[SeVV]

I`ve spent 2 whole days on this simulation and I think that I`m closer to the finish line. I think that it should looks like on attached images (im1, im2, im3, im4). It`s not perfect but I think it is very close. Below I`m describing the model as good as I can:
- Multiphase flow inhomogeneous flow (cause I can get separate oil and air velocities) but with homogeneous SST turbulence model.
- Air (provided by two pipes from the outside) is modeled as a Countiunuous Stream (13.3 m/s normal velocity set on inlets).
- Oil mist (0.9 of air volume fraction and 0.1 of oil volume fraction) modeled as Dispersed fluid with mean diameter of 0.02 mm (10 m/s normaln velocity set on inlets).
- Grinding wheel is rotating with angular velocity of 2285 rad/s and is modeled as a porous domain with volume porosity = 0,45.

I`ve choosen inhomogeneous model just to be able to view both oil and air velocities separately. I`m not sure am I right but homogeneous turbulence model is fine for me when I don`t need to know how the mist is being generated. I`ve choosen SST turbulence model because I`ve read that it is quite stable model which also allows to describe wall and center fluid velocities quite good. I`ve selected dispersed fluid for the oil mist to use Eulerian-Eulerian model because I think that I don`t need to perform the particle tracking at the moment (but now I`m considering it as well).

I`m performing a steady state simulation and I`m trying both physical and local timestep approach to obtain good solution. I didn`t knew that one of the criterium of good results is the value of RMS below 1e-4 (or even 1e-5 or 1e-6). Now I`m trying to reduce my RMS values. I`m attaching the image (solver) with plot of rms history. It was obtained when I was using the local timestep with timestep factor of 3. Can You give me some suggestion what can I improve please?

[ghorrocks]

I do not know what is the grinding wheel and oil mist ports. Also please show the volume/mass fractions.

You should not use local time stepping for final convergence. You can use it to get the residuals down some distance but for the final run to convergence you should switch to physical time stepping.

[Gert-Jan]

- Don't stop calculating until your mass imbalance is within 5%. Mostly this should be much smaller but for a multiphase calculation you can take this as a upper limit.
- Provide picture with 'Velocities in Stn Frame' as variable. Mostly these are better understandable.
- As Glenn asked, we definitely need volume fractions to be able to judge quality of your result.

[SeVV]

Glen, could You explain please what do You mean 'grinding wheel and oil mist ports'? Do You mean 'portions'? Here I am attaching the volume fractions history plot and the velocities in st frame.
Gert-Jan, how can I understand the 5% of mass imbalance? 5% = 0.05 so it is 5e-2 on the plot? Sorry if You mean something totally different..

[Gert-Jan]

You should create a new graph, where you plot the imbalances of all equations. It will give you values between approx -100 and 100%. So you can easily see how far you are off.

[SeVV]

And do I need to create this graph in the CFX-PRE or CFX-Solver?

[Gert-Jan]

You can do it on the fly. Or even when the calculation is finished:
Solver Manager > New Monitor > Imbalance > Select All IMBALANCE Variables (Right mouse button) > OK

[SeVV]

Thank You for quick instruction, that is very useful. I am attaching the imbalance plot. Am I right that it looks bad..? So the biggest problem is imbalance of volume momentum of "OIL" in "CHANNELS" as I can see? The values of V-mom imbalance in "Ambience" and and "OIL" mass imbalance in "ambience" looks bad too? What can I do to fix this? Improve the mesh and do something (but really don`t know what?) with initial values?
Thank You
Best Regards

[Gert-Jan]

You just have to calculate longer. It is an overall imbalance. Not an imbalance from cell to cell. So it has nothing to do with the mesh.

I cannot see what each line represents. But first guess would be that the steady green line@95% and the blue line @60% need improvment. The flipping dashed green line is a bit vague. The imbalance is a percentage based on a value at a boundary. If this value is close to zero, the imbalance can flip from -100 to 100. But I need more info to judge it more accurately.

Hasn't anyone told you, you need to monitor imbalance? Supervision? What course did you take? Did you look at the FAQ on CFD-online?

[SeVV]

I was setting the iterations number up to 150, maybe to 200 once. What is the upper limit worth to try? 300, 500? What can I do to improve imbalance of values described by those two lines? The steady green line@95% describes the (OIL) mass imbalance in AMBIENCE domain and the blue line @60% describes the P-Vol imbalance in ambience. What information do You need to try help in this case?

I`m sorry but I didn`t have any proffesional course. Im still reading the CFD-Online FAQ and archive posts when I am dealing with another problem. I am reading the official cfx papers and sharcnet. My knowledge in this area isn`t very big but I am still trying to learn. Very often my work on this simulation is nothing more than trial and errors method. I was unfortunatelly droped on a deep water (for me) and I need to perform this simulation as a chapter of my phd thesis. I don`t have any supervisor with knowledge in field of CFD.

[Gert-Jan]

It should be forbidden to have people operating tools like this without any guidance/supervision.

Nevertheless, why don't you just let it run for 10000 iterations over the weekend. Who cares? Probably it just needs time.

BTW, we still didn't see any pictures with volume fractions. How large is the Oil volume fraction. I see you solve energy as well. Do you run Thermal or Total Energy?

[SeVV]

I`m affraid that You`re so right with the first sentence. I am dealing with this since July and feel that it is so tough to do it well without a supervisor who would show how it works live..
I`ve attached the volume fracion image together with some CFD-post screens few posts ago. I am attaching it again here . Ok, I`ll try to let it run much longer and see what would happen. The oil volume fraction is 0.1 and the rest 0.9 of volume is an air and together it is modeled as a dispersed fluid (it is an oil mist provided centrifugally through the grinding wheel in a real process). I hope You mean these values?
I can see the energy overlap too but at the moment I don`t care about the heat transfer yet and I`ve set the isothermal model of 25 degrees C. But eventually I will try to simulate the heat transfer too. Which model (thermal or total energy) would be more proper?