Hello,

I am using CFX5.5.1, I have created a geometry for the mixing vessel with an impeller. I am using steady state conditions and as far as I know I am using the right boundary conditions. Can someone help me as I am not getting the right flow pattern. Can anyone suggest what I am may have done wrong. I am using the rushton turbine, the flow pattern is not correct. I would be grateful if anyone had any suggestions or if anyone is also doing modelling tanks to get in touch and maybe we can discuss this.

Regards Jennifer

HI Jennifer, when you say tanks, are you referring to mixing tanks ?? Dave

Jennifer,

Can you explain exactly what is wrong with the flow pattern? More axial flow than radial flow or something like that, or are some details in the flow pattern wrong? And, how do you model the rotation of the impeller?

Astrid

Yes, sorry mixing tanks with a rushton turbine.

Jennifer

Astrid,

I am using one domain as rotating and the other as stationary. The stationary domain has no motion and the rotating domain has a speed of say 150 rev/min. In the rotating domain there is an impeller with a shaft. In the stationary domain there are some baffles. I then set up boundary conditions and domain interfaces. The domain interface is the outside wall of the rotating domain and the inside wall of the stationary domain - that is the only place where the two domains overlap. In a rushton turbine flow pattern, there two recirculations on either side, one below and one above. From the flow pattern there is no distinctive loop below or above the impeller. The flow on both sides of the impeller should be symmetrical which it is not. The flow is not defined, there is not pattern. Are you modelling stirred tanks? I would be very grateful if you could explain how to model it so I can check if I have done it correctly. Do you have any examples of the rushton turbine? Hope this makes things clearer.

Jennifer

Astrid, one more thing, there is alot of axial flow from the vector plot and hardly any radial.

Jennifer

Jennifer,

I have never nodelled a fully baffled mixing vessel with a Rushton turbine, but as a Chemical Engineer I know what you are talking about. Presuming the turbine is in the center of the tank (both axial as radial), you should indeed obtain circulation zones, axial flow between the baffles, tangential and radial flow near the impeller and some symmetry in the total flow pattern. Some questions/hints:

- What is your Re-number (based on Di)?

- Why do you use two domains, connected with GGI's, if you presume steady state?

- Did you try transient calculations? There will definitely be transient interactions between impeller and baffles.

- Are you sure you obtained sufficient convergence? Have you monitored velocities at critical positions (f.e. impeller tip)?

Astrid

Your case has many similarities with one of the tutorials - the Mixing Vessel one. Is there anything that is done in the tutorial that you have not done (except for the fact that the tutorial is multiphase)?

Dear Jennifer, I am also modelling stirred tank (multiple impeller stirred) reactor in CFX 5.5.1. Currently, I am trying to import the CFX 4.4 mesh that I did earlier into CFX 5.5.1. I am getting certain errors and would like to help you with it but I would also like to know if you have used any specific templates for your geometry creation. Nishant

I am using a standard geometry setup, T=H, D=T/3, C=H/3 I am using a rushton turbine impeller. When you set up you simulation - are you using GGI?steady state? Are you experiencing any problems with the flow pattern?

Jennifer

Hi Jennifer, I am using 'Frozen Rotor' method with full tank geometry. My simulation is still running so I cant say what the flow patterns would look like. Could you please explain you implement GGI and what is the purpose of it for your geometry? Nishant

Another important question is that how do you create the geometries for stirred tank reactor? Do you do them manually or do you use some automatic mesh generation programme? I have found that in CFX 5.5.1 , the geometry creation is quite tedious and takes a long time, especially for multiple impeller stirred reactor. Nishant

I create the geometry and mesh myself. I am also using frozen rotar - steady state. I input the appropriate boundary conditions. For GGI, I create domain interfaces for only surfaces where the rotating domain touches the stationary domain. I am not sure what I am doing wrong.

Jennifer

Jennifer,

I hate to ask this, but is your solution converged? Look at the following:

1) What are the RMS and MAX residuals at the end of your run? Look at the last iteration, did the solver converge to the tolerance you specified for the residuals, or did it just stop? If it "converged" what tolerance did you use. If you took the default, 1.0E-4 RMS, this might not be good enough. Set it to 1.0E-4 or 1.0E-5 MAX.

2) What do the global balances look like? Do all the equations have balanced flows? i.e., roughly 0.01% or less.

3) What were you using for a timestep? Auto timescale tends to be conservative. You should be using something like 1/omega. If you can get away with it use something bigger, say 10/omega.

Neale.

Hi Neale, I have a question. How many iterations one need to use for getting a converged solution? My rotational speed is 200rpm but with a timescale of 2s and 100 iterations, the simulation takes quite a long time (2 days) to give a result. Nishant

100 iterations in 2 days? How many elements do you have and how many cpu's?

For start up cases (Upwind) I usually take 100 iterations. Fr final solutions with High Resolution I add 200 iterations as a minimum, if convergence has not been achieved but mass balances are within 0.01%.

Astrid

Hmm, well, it depends on many factors. However, typically with rotating equipment you want to use a physical timescale of around 1/omega. Your omega is 200 rpm = 20.94 rad/s -> 1/20.94 = 0.045 s. So, 2 s is pretty big, that's roughly 40/omega which is a large timestep.

How does your convergence look? Is it a constant straight line down to 1.0E-4 MAX in 100 iterations or are things just bobbling around? I would say that you should be getting to that level of convergence within 100->200 iterations. The amount of wall clock time depends on your grid size and CPU as well, 2 days means you either have a slower CPU or you are running a reasonably sized problem.

Neale

Hi The machine has four EV5 CPUs running at 300 MHz. There are about 500,000 cells in the geometry. I seem to be getting convergence but have given the simulation another 200 iterations.

OK, so it's a relatively old Digital box and you are running a medium sized problem. If you can't converge to 1.0E-4 MAX residuals within 200-300 iterations then something is wrong and you should take some time to analyse the flow and residual diagnostics to see what is holding things up.

What residual targets are you trying to achieve?

Neale.

Hi Jennipher,

I have just read the string today. Probably you have found a solution already!!

I have modelled the Rushton turbine using the frozen rotor method, albeit with CFX4.4. There are a few things I noticed: 1. the location of the interface (UMB, in CFX4.4) 2. discreticing scheme vs solution algorithm (especialy when you use higher order schemes like QUICK) 3. scale of the geometry and Re, (e.g if x>1m and Re>10^5) you are not likely to get good convergence. And the flow profiles will be unreasonable!!

I am about to start working with CFX5.5.1.

Best luck Nyatoto