[lxlylzl]

O.K. I'll give it a try and let u know soon.

[lxlylzl]

Hi RodriguezFatz

With 96K hex mesh, and using 2nd order upwind, my solution finally converged with single phase and with DPM too (image attached) !


But with 196K hex mesh, same issues are there (image attached) .
In this case, the only changes I made was with the time step and no. of iterations per time step equal to 20 (in the above case i used its value as 30).


Why results are not converging with different meshes? Is this due to some meshing problem?

[flotus1]

I can't see an image of the residuals for the 196k mesh.

[lxlylzl]

Hi flotus1,
I'm sorry, here it is, with 256K hex cell (I didn't save it for 196K mesh).

[flotus1]

Originally Posted by lxlylzl

In this case, the only changes I made was with the time step and no. of iterations per time step equal to 20 (in the above case i used its value as 30).

You LOWERED the time step for the finer mesh, right?

To judge if it could a meshing problem, some information and pictures about the meshes used would be nice.

[lxlylzl]

Hi flotus1,
Yes, I LOWERED the time step for the finer mesh. I haven't saved those images. Since I'm working in trial phase, I haven't saved the file in gambit's default format. I saved meshes of different sizes in .msh format.

[RodriguezFatz]

Again, if you have numerical problems: Go to the safest level of all approximations, i.e. 1st oder upwind spatial and purely implicit time schemes. If this doens't work you can think about other things (grid, ...).

[lxlylzl]

Fine RodriguezFatz, now I'm going to try 1st order upwind.

[lxlylzl]

Now I've started with 1st order upwind.

Well with 2nd order upwind, for 256K mesh, now with reduced time step, my residuals (I've taken 1e-05) are as shown in attachment.

[lxlylzl]

Thanx RodriguezFatz

Using 1st order upwind from momentum onwards, the solution converged (image attached). Why wasn't it converging in 2nd order upwind?

RodriguezFatz, which cyclone you are working upon and on which model?

[RodriguezFatz]

Originally Posted by lxlylzl

Thanx RodriguezFatz

Using 1st order upwind from momentum onwards, the solution converged (image attached). Why wasn't it converging in 2nd order upwind?

RodriguezFatz, which cyclone you are working upon and on which model?

I'm not simulating a cyclone at all. I just use the DPM model.

Different numerical schemes use different approximations for the derivatives. Thus, they replace a derivative with the differential quotient [eg (Phi(x+dx)-Phi(x)) /dx ] plus a certain error term. Now this error term can change the original (Navier-Stokes) equation to a different one, making ugly things possible, such as resonance. 1st order upwind establishes some amount of damping, that counteracts the ugly effects. Obviously, in your case, 2nd order doesn't.

[lxlylzl]

I got it RodriguezFatz. Well, I think I should go for grid independence check first, before taking any decision because on some meshes I'm getting convergence using 2nd order upwind, while for others it requires 1st order upwind. Do these schemes provide more accuracy when we move to higher ones? Please suggest me few books regarding this. Thanx a lot for your support.

[RodriguezFatz]

Plainly, this one:
http://www.cfd-online.com/Books/show...&full_review=1
It is one of three really, really good cfd books I can recommend. And it has everything you need about numerics and some great other chapters as well!
I actually read it in German, but I guess the English version is the same...

[masoodina]

hi x|y|z . i ll be really glad if you help me .

do you think its necessary to use "interaction with continuous phase" ?? why

and why are you using unsteady solver ??

2 . i used injection from surface and entered just velocity of the particles .
do i have to enter flow of particles ?? ( i dont have this data )

[lxlylzl]

I think, it depends on your problem type and whether you want any particle interaction or not (I mean 1st order coupling or 2nd order coupling, etc.). Regarding unsteady state, the flow inside the cyclone is swirl dominated with high anisotropic. So to track every parameter accurately, you need to go with unsteady condition. Moreover discrete phase motion in also unsteady and you need to work with Lagrangian approach to keep its track.

Regarding flow of particles, I had the mass flow rate, so I used it. I'm not sure but if you don't specify mass flow rate and go for injection from surface and enter velocity of the particles only, you may need to specify the time for injection.

By the way, which model you are using and what are your boundary conditions? This may help to classify your problem. Are you using steady state?

[lxlylzl]

Thanx RodriguezFatz.
The book is really nice !

[masoodina]

for now im using rsm steady . if i get good answers i would work on les too .

thanks for answering . but i have seen many papers running cyclone with steady solver .
i think i may solve it in two ways . one with flowrate and one with no flowrate .

i get answers and particle path with no flowrate , but im not satisfied .;(

and by the way i have many incompleted particles , do you have any idea how to decrease it ?