Learning Forum

[scabo]

Hi I am simulating solid-water in a pipe using E-E. I have defined the solid as a fluid material (from Materials>Create) and then given the density as that of sand keeping the viscosity unchanged. After that i am using a COUPLED, Pseudo time step and a steady state solution to run the flow. But the continutiiy term is diverging right from the beginning. What could be the problem with this? Do i have to modify the under-relaxation or something like this? Any help is greatly appreciated..thanks

It is showing ' Having convergence issues: Temporarily relaxing' and later on 'Divergence detected in AMG solver : Pressure Coupled', Floating point error.

[Rob]

What are the initial conditions? Try with transient too, getting an Eulerian model started in steady can be difficult if the flow field is very unsteady. 

[scabo]

 

Hi. BCs are: 1) inlet: vel of water=sand, volume fraction of sand given. Theres a supersonic/initial gauge pressure for mixture which i have kept at default value=0 and Turb intensity and viscosity ratio as it is as. 2) Outlet I have given pressure BC and backflow of sand=0. 3) Walls-no slip for water and 0.1 spec coeff for sand. I am using kE RNG as turb model and have a good O-grid mesh with inflation layers with first layer height as 15 um. I have initialised with hybrid inititialisation.  

As for schemes i am usignCoupled with2nd order for Mom, pressure and 1st order for others.

As for unsteady, some papers have done similar pipe problems using steady state, so i was trying the same.

Are all the settings okay? Do i have to change anything? thanks

 

[Rob]

What's the volume fraction of sand? Is the pipe horizontal? How big are the sand particles? Note a 15micron mesh implies inflation which implies high aspect ratio - that's not good for models where the result changes ALONG the cell. 

[scabo]

Hi, Volume fraction of sand=0.19-0.4. Yes the pipe is horizontal, 3D and circular of length 70D where D is 0.103 m. Dia of sand=.09 mm. Are u saying first layer height =15 um is too big? Actually i wanted to see how the y+ comes and then adjust y+ =30 after the first run. But it keeps failing in the first attempt, I tried reducing the under-rlaxation factors for pressure and volume fraction, but no use.

Should i try with a reduced first layer height like 5 um? Or should i initialise with something else? thanks for giving advice.

[scabo]

 

Here is the picture of the coarse mesh. But it fails with a fine mesh also

 

[Rob]

In E-G the particles can be larger than the cells but the benefits of y+ = 1 become less critical as you consider the multiphase drag. A very fine mesh for inflation means the aspect ratio is high, which isn't good for multiphase: aim for 1-2. 

Next problem is the particle loading. Given sand sinks what do you think will happen in your model? How quickly will the system fill with sand? 

[scabo]

About y+=1, I was aiming for y+=30 because I am using the kE RNG model. What do you mean by 1-2? There is sand and water coming from the inlet at conc=0.19 of sand. So, the sytem will fill with sand relatively quickly i think. I think i can try by removing inflation first? 

[scabo]

Btw for defining the granular phase in the E-E framework i have defined air as fluid material and then just changed the density in the material box for air and called it sand. I hope this is the right procedure?

[scabo]

I was just asking, in these Eulerian-Eulerian problems how low can you expect the continuity to fall?I am seeing around 1e0 and getting stable results now. But the continuity is not falling around 1e-2 or something like that.

[Rob]

Materials are fine. Aspect ratio - you need to get somewhere near a value of 1 to 2, with a near wall cell at 15 microns that's going to be a very big mesh.  

OK, so with a steady flow you expect to fill the pipe. But.... have you looked into slugging and duning effects? With a fixed inlet flow the fluid has to enter the domain. 

[scabo]

So you are saying I need a bigger first layer height to make the AR=1 near wall? Also i am now getting stable residuals with converged velocity for steady state after removing inflation layers but the y+=400. So i need to reduce the y+ to around 30 by imposing a first layer height. Is that correct?

[Rob]

I am saying you need an aspect ratio near 1-2 for the mesh. Once sand piles up near the wall how do you think that interacts with the y+ theory? 

[scabo]

Yea, i do not know what will happen to y+ when sand piles up. Then the piled up sand will act as a wall also. But i am not sure how to mesh those scenarios. I dont think the fluent manual has that?

[Rob]

No, that'll not be covered. 

[scabo]

I was also asking lets say i change the particle volume fraction or density or diamter. Can i start a new solution from a previous converged solution for the same mesh and pipe? I think it may be valid for the volume fraction but may not be for the other 2? 

[Rob]

Yes, with Fluent there's not always a need to reinitialise as we can just change a boundary condition and iterate. It's an old trick to reduce overall compute run times, we'd initialise & run, save case & data, change inlet velocity, run, save case & data etc.... Note for a transient calculation that does mean that time isn't reset. 

[scabo]

Hi, thanks. Now I have run the simulation and it is producing stable residuals and converged quantities like vel mag and solid volume fraction in a steady state. But when i am plotting the chord averaged solid volume fraction along a vertical line it is deviating from experiments. What can be the issue? My sytem is not fully mesh independent as i wanted to use a coarse mesh first-but apart from that is there any issue? I have taken first layer as 0.5 mm and 4 inflation layers and y+=40. And i am using drag and other laws from papers.., thanks

[Rob]

How long was the experiment running for? Steady state is an equilibrium state and I'd always check you were modelling the same conditions. Also, if duning occurs you may want to look at Rocky. 

[scabo]

Hi, the simulation ran for 1.5 hrs on 30 cores and then it converged. Other papers have done steady state on the same xperimetnal conditions using commercial and got better results without Rocky. May be some problem with my mesh? I am using a corase mesh (1M) on a 7 m long pipe. But i will do the mesh independence..

[Rob]

I can't comment on other models, but mesh studies are always a good place to start. 

[scabo]

Okay-let me dothe mesh indp first