Hi all,

I just want to confirm my understanding about the additional variables. As what I understand, the results (e.g. pressure, velocity, void) are the same with or without additional variables. Am I right? When you set the additional variable as transport equation, it uses the results of the solution (e.g. rho, velocity) to solve the additional variable but the solution for the main flow is not affected. Please tell me if I understood it right. Thanks guys!

I want to rephrase my question. If I have an additional variable which uses transport equation, is that transport equation only for that additional variable and it's not the one being used by the solver for the main flow? Such that with or without additional variables, the solution will be the same unless you use those variables as sources or boundary conditions.Am I correct? I hope I made my question easier to understand. Pls. enlighten me guys! Thanks!

Hi Ariel,

AV's are transported, but they have no effect on the hydrodynamics unless you specify their effect through a source terms to the mass and momentum equations.

This also means that you can solve AV's with a different timestep (the AV equations will solve faster by increasing the timestep on the AV under advanced control in the solver control panel).

You can also solve for AV's after obtaining a solution for the flow field without having to solve the flow. to do so, go to the advanced solver control and set "solve fluid = f". If your flow is turbulent and/or your are solving for energy, you can also turn them off with "solve turbulence = f" and "solve energy = f".

The same applies for AV's solved using the "Diffusion Equation", "Poisson Equation" and algebraic equations.

-CycLone

Dear Cyclone,

Thank you so much for that! Your explanation is much better than the CFX documentation. Actually, our model is dispersed droplet in vapor in a pipe and our professor asked us to try if we can change the condition Vnormal = 0 at the wall (slip or free slip) for the droplet. I thought it could be done by assigning wall velocity in the normal direction but the results show that from the center, the velocity normal increases and then it converges to zero near the wall and then abruptly increases to the given wall velocity. The goal is not to retard the droplet velocity along the normal direction (as if it "goes out of the wall").

I know it's not a problem in Eu-Lagrangian but my professor wants me to try it using Eu-Eu. Do you think it is possible using source terms (sink) with additional variables? I'm really having hard time thinking about it. Thanks for the help!

ariel

Hi Ariel,

For that you would need a different velocity field for your droplet phase. Instead of using an AV, run it as an inhomogeneous Eularian-Eularian multiphase model, with your droplet material as the dispersed phase. If you set it up this way you will find a slip condition is available for the dispersed phase.

-CycLone

Hi Cyclone!

Thanks again for the reply. Actually I've been simulating it as Homogeneous Eu-Eu with dispersed droplets.I've been playing around between free slip and no slip. But what my professor wants to change is the condition that the velocity normal to the wall is zero (which is the case for both free slip and no slip). When I use free slip, the droplet axial velocity doesn't retard at walls but at the same time we want also to do it along the radial direction. Do you think it's possible for Eu-Eu? When I simulated it as free slip for droplet walls, the results were almost the same as for no slip. My inlet velocity is only along the axial direction. Do you think the velocity in the radial direction would have much effect in the results? Sorry for the long email. Thank you so much for your time!

ariel

Hi Ariel,

If the velocity normal to the wall is non-zero, then you have mass flux through the wall. You can accomplish this by adding a source term to the mass equation at the wall boundary, but are you sure this is what you want to do?

As for the inlet, changing the inlet profile could significantly change your solution.

-CycLone

Dear Cyclone,

Thank you so much again! My professor thinks that maybe the hydrodynamics is significantly affected by that wall boundary condition (velocity normal to the wall for droplet is zero). He thinks that because of that condition, the droplets are forced to move near the center thereby significantly affecting the flow(in our case,droplet has larger inertia compared to vapor).This is the main reason why he wants the droplet to "move out" of the domain when it reaches the wall. But I know Eu-Lagrangian is the appropriate model but he wants me to try it using Eu-Eu which I find to be very very difficult since we don't know any mass flux correlation. I tried using mass flux = rho*vel*void but it's insignificant since the droplet void near the wall is very small. I also tried using several constant mass flux but the solution is very unstable.

The results show that pressure has negligible radial variation. Can it explain that our fear about droplet is not actually a concern? Thanks a lot Cyclone. Thanks again for the time!

Ariel

Hi Ariel,

The wall boundary condition certainly does effect the flow; walls essentially define your problem. The question is whether the wall is having the wrong effect on your droplets.

If the droplets should be collecting on the walls, you may need to add a source to account for that. Otherwise I would first verify that you are adequately resolving the flow next to the wall. Because of the no-slip condition, there is a very steep gradient normal to the wall. If you simply extend the mesh that you have in the free stream to the wall, you are unlikely to have enough elements normal to the wall to resolve this gradient (the so called wall 'boundary layer').

I recommend that you first go back and add inflation next to the wall. Try specifying a first node height which is about 1/200th the transverse wall element size. With an inflation expansion ratio of 1.3, this should give you a smooth transition to the volume mesh size in about 20 or so layers (so set the number of layers to ~25).

You should find that this significantly changes your solution. Hopefully for the better.

-CycLone

Dear Cyclone,

Thanks again for your wonderful advise. I've checked the quality of my mesh and I think it's close enough to your recommended values. Our main problem is the representation of source terms, I've already tried several correlations but the solver is always unstable or if not the results have large deviation compared to experiment. Finally, my professor agreed to do a Lagrangian model. I think he's convinced that unless we have a suitable source parameter, we can't do our objective using Eu-Eu. So we are going to compare the results of the two models. I think, Lagrangian is acceptable in our case since the maximum droplet volume fraction is less than 10%. Thank you so much again for all the advise! It's an enormous help to me!

Regards, Ariel