January 20, 2022 at 8:41 amSardarSubscriber
I am writing this post in hope that someone can clarify my doubts on some issues with my simulation. Please do not turn me down, even if you have a say on one single question of those below. I have had terrible times solving my simulation. And please do not withdraw your views if you see my question is already answered.
My problem is I am having a whole lot of uncertainties, as there is no one around to help me specifically with my case, and online info is opposing or not decicive on my questions.
I am simulating a huge (6 m tall and 3.8m dia) stirred tank with two impellers in it using MRF. I am planning to see how well the impellers agitate the fluid within (criteria is velocities at tank corners). My objective is to add powders later on but I have to first get reasonable results for a single fluid model.
- I am choosing zero shear stress for tank peripheral walls. Is this a sound assumption?
- My turbulance model is k-e RNG swirling flow. I have read online that RNG does not perform well with no-slip walls, while I have to choose some no-slip walls in my model, like the impeller walls (I have deleted the impellers from the surrounding domain in SpaceClaim, but then named the cut walls "upper impeller" and "lower impeller" to get moments plots on them).
- Can I use SIMPLE first and once reasonble monitored values come up, switch solver to coupled (non-pseudo)? And if yes, should I start coupled with the same URFs of SIMPLE?
- For SIMPLE, Fluent User's Guide suggests keeping URF sum of pressure and momentum equal to one, This does not necessarilly hold for coupled. Does it? If not, is there any criterion for changing URFs in Coupled, other than changes in monitored parameters?
- Would you suggest using QUICK over 2nd order for momentum, k and epsilon?
ThanksJanuary 20, 2022 at 8:52 amDrAmineAnsys Employee1/Why: that condition might apply only for bubble to merit any sliding effects (and for now you do not have any bubbles your are just stirring things). I will keep default no-slip.
2/Should be okay. My favorite is SST Model with curvature correction. This things are best assed in model sensitivity analysis where you compare the outcome of runs conducted with different turbulence models.
3/I recommend Coupled Solver for quicker convergence. Once your get to multiphase, I recommend to first rely on PC-SIMPLE.
4/Stick to second order for equations at first. I love QUICK but it won't increase accuracy given the midpoint rule we have + merits are more observed on uniform hex meshes.
January 20, 2022 at 9:03 amSardarSubscriberThanks a lot for your reply.
As for zero shear on walls, I thought fluid is not forming boundary layers on tank wall as it is rotating continuously over it, hence the zero-shear wall condition.
Is SST by any means less expensive than RNG? That is also somethingI should take care of, as my model is huge.
You mentioned "first rely on PC-SIMPLE" on multi-phase. Does that mean I can switch to coupled later. Right?
I am using astructured mesh. So once again, if merits of such a mesh are accounted for by the QUICK scheme, would you still recommend to go with 2nd order?
January 21, 2022 at 3:42 pmRobAnsys EmployeeIf the walls are stationary and the fluid moving you'll see a flow boundary layer if the mesh is suitably resolved. If not you'll see a distorted boundary layer.
SST and RNG cover much the same function. Historically Fluent didn't have the k-w model so we always used k-e, with the RNG variant being good for mixing tanks and low energy swirling systems. I habitually use RNG but SST is equally usable.
Phase-Coupled SIMPLE is fine for multiphase. As it's a transient solution Coupled has a lesser benefit than in a steady solution. As for UR and discretisation, I'd stick with the defaults to start with, although reading the manual to understand the options is a good idea. Not sure I've ever used QUICK, and I'm surprised you got a structured mesh with an impellor in the system.
January 22, 2022 at 9:30 amSardarSubscriberThank you. . (I could not access the site because of the maintenance- I hope it is not too late.)
Do you mind a couple of other questions please?
BOUNDARY CONDITION FOR TANK OPEN TOP
Q 6 Tank is not fully filled with water in reality, i.e water then air then open top in reality. However, as I am interested in mixing performance only, and not in the air-water interaction on top of the tank, I had initially avoided patching air on top of the tank - there was only a pressure-outlet BC immediately after water without any air region. But eliminating air turned out to be problematic (?), as I got weird water flows exiting and entering into the tank from the open top BC (I also had this "reversed flow warning during simulation, although some people have said it to be normal in swirling simulations"). Is there a less expensive configuration than turning on the VOF model? And if there isn't, which means I have to add air to the model, what should I choose for top BOUNDARY CONDITION? Plus, Does it effect if I choose either of the phases as my PRIMARY and SECONDARY PHASES?
Q 7 I am having hybrid initialization, and it is apparently done, but it says something that reads like: "Checking case topology... -This case has only inlets -Case will be initialized with constant parameters Hybrid initialization is done." So, does "initializing with constant parameters" mean it is a standard initialization with probably "random" values or something? Do I better to go with standard initialization?
Thanks a million. I will get back here once my case study starts giving results and will be adding info.
January 24, 2022 at 9:47 amRobAnsys EmployeeFor the free surface you have two main approaches. Fixed lid where we assume the top is a pressure boundary or symmetry/slip-wall or use the VOF/multifluid VOF model. If you're using DPM and not experiencing excessive vortexing the former works well and is computationally cheaper. If you have vortex formation you need to model the free surface. As you're using a sparger you'll want multifluid VOF, and the phase definitions then get more interesting as you can't use DPM.
For initialisation try hybrid and then post process the model to see what's happening. If you do only have inlets then how does the fluid get out?
January 24, 2022 at 12:09 pmSardarSubscriberThank you @Rob. That's great information.
I presume by "slip-wall", you mean the specified shear condition with shear set to zero for the top BC. Right?
I am still working on single fluid, but later will be using DDPM. So for single fluid I will go with slip-wall.
As for initialization, the message "-This case has only inlets" appears when I chose a pressure inlet as my top BC, and would say "This case has only outlets" (as different from inlet) when pressure-outlet was chosen. These messages appeared when initializing the case with pressure-outlet/inlet. In the post evaluation, I have vectors as shown in my attached image, which I called in my second post as "weird water flows exiting and entering into the tank from the open top BC".
January 24, 2022 at 1:13 pmSardarSubscriberBy slip-wall I guess you mean shear stress set to zero for wall BC.
I am convinced that the initialization message: "this case has only inlets" is related to the BC (pressure-inlet) I had used for the tank top. The message changed into "this case has only outlets" when I would choose pressure-outlet.
January 24, 2022 at 1:20 pmRobAnsys EmployeeYes, a slip wall is zero stress: symmetry won't work as you need a DPM boundary on the surface. This does mean you can't use temperature dependent density, but that's probably not needed in a model of this type. DPM condition at the top will be escape. But, you also need to monitor the surface pressure to check for distortiion: remember dP = rho.g.h
Viewing 8 reply threads
Ansys Innovation Space
- You must be logged in to reply to this topic.
Simulation World 2022
Earth Rescue – An Ansys Online Series
Ansys BlogTrending discussions
- Suppress Fluent to open with GUI while performing in journal file
- Heat transfer coefficient
- What are the differences between CFX and Fluent?
- Floating point exception in Fluent
- Time Step Size and Courant Number
- Difference between K-epsilon and K-omega Turbulence Model
- The solver failed with a non-zero exit code of : 2
- Floating point exception
- Exporting Data Results
Top Rated Tags