Hi All, I want to calculate the mixing time is an agitated vessel using CFX4.4. I introduced the tracer as a pulse input, where I expect the concentration of the tracer at a monitoring point to increase with time up to a maximum, and this should mark my mixing time. However, in my case the concentration of the tracer at the monitoring point, which is far away from the input point, increases then decreases continuosly up to the end of my iterations (12,000).

Where does this tracer go?

regards nyatoto

Hi Nyatoto

First of all - are you sure that you set the monitor point in the one spot where you can observe the expected tracer development ?. Have you tried to make surface plot during the simulation to make sure that your transport is physical correct.

I my experience the tracer development is not allways as expected from textbooks - there are surprices ! Moving the monitoring point a bit around can yield quite different tracer curves.

The question you need to get answered is wether the tracer transport you see is physical correct or there is some numerical errrors.

In my opinion you shold not consider the maximum of your tracer curve as the only significant time for mixing, but also consider the retention time of your tracer. Say the time it take for 50 % of the tracer to leave your vessel. Also make a mass balance to make sure that there is not something numerical going on. Is the injected mass equal to the mass leaving the vessel ?

If you not allready have done so I can recomend that you read Octave Levenspiels book on Chemical reaction Engineering: There is an excellent section on analysis of non-ideal reactors

Regards

Michael

Hi Michael,

Thanks for you comments. I have tried those options you mentioned. I tried two points, probably I need to try more. I have done the fringe plot and the pattern I saw is what I expect. Let me first clarify a few points here: -Mine is a stirred tank, typically simulated as BATCH reactor in CFD. -I use the PULSE method, feeding 114mg for 1 sec. I saw on the fringe plot that the tracer was correctly fed and was highly concentrated at the feed point. - After the 12,000 iteration I saw, again with fringe plot, that the tracer was now uniformly distributed. -I have a 19litre vessel.

You have mentioned about the non ideal flow patterns that are explained by Levenspiel and more simply and explicitly by Fogler. Yes, I would consider RTD too if it was a continuous flow. However, i checked in the out put that the flow in (at INLET) and out (at OUTLET) were both zero, that is after the feed was switched off.

I initially thought that probably the amount was too small and I increased it to 1.14 g (in a 19litre vessel). This should give a minimum concentration above my mass tolerance limit,or does this matter?

More ideas please!

regards, nyatoto

Hi Nyatoto,

The question is for how long (time step wise) have you run your mixing time simulation? It could be that the system is sitll not fully homogenised.

From what you described it looks like the sensor response is OK. (high peak of concentration and then normal decrease.

The concentrations should level off. Use the +-10% mixing time and compare it with experimental results. If you are running a multiple impeller problem then your simulated mixing times will be around 2 to 3 times longer than the experimental data.

I from my experience I would I have more than just than one monitoring (sensor) point (around 15?).

Kuba

Hi Kuba,

Many thanks for your response. I think there is a strong point in what you are saying, Kuba. I was suspicious of my convergence. First I run my simulation for 300 time steps, 40 Iterations per time step ie 12,000 total iterations, one time step=180 deg/rev. I got a convergence which was not good, minimum sum of the residuals was 10^-3 (for k) and max was 0.5 (for epsilon, VERY bad!). I changed to 60,30 deg/rev, the convergence was worse than the first case. Then I tried 3Deg/rev (ie one grid/per time step) result were not good either.

There are a lot of oscillations, I have reluctantly used Under relaxation factor as low about 0.1 for all parameters (including pressure!!??). This gave me some less oscillations and a little better convergence. I have switched from BLOCK STONE to AMG solvers, the latter is painfully slow if set for all variables.

Iterations per time in the range of MAXIT>10 gives me wild oscillation. I am now using MAXIT=6 , again very reluctantly!!. I would be comfortable with something like MAXIT>30.

After trying all those, I decided to feed tracer in the the system that gave me the best convergence. This was out of desperation because I know a good convergence does not necessarily represent a good solution.

Before I compare my result with experimental ones, I need to have a logical result in my simulation. Mine is still not. I am tying to get better convergence then I will use more point, finally compare my result with experimental ones.

I suspect I still need to fine tune something in order to obtain a better convergence. BUT HOW?? Please HELP!

thanks for your time, nyatoto

Hi Nyatoto,

If 10 or more iterations per time step is giving wild osilations than using less iterations per time step will still give meaningless results. The problem being that the solver is not converging and using fewer iterations will not improve convergence. Also since you set the under relaxation factor to 0.1 the convergence will be slow and a greater number of iterations per time step will be needed, not less.

If the time step is set to give more than a few degrees per time step than cylindrical coordinates should be used, otherwise convergence will be a problem.

Also, you might need to fine tune the geo to improve convergence.

Regards, John

At what Re and rpm are you?

The procedure you described is ok. I would increase the number of iterations to 20 and underelaxation to 0.3. Use a lot of timesteps and revolutions with a small time step.

Hi John and KubaB,

I am using 3D cylindrical coordinates.

How do I fine tune the geo? Do I have to regenerate the geometry in build, remesh and pass to VOLMSH again? You notice that a stirred tank may be regarded as a complex geometry. "PERCENTAGE OF WELL ORDERED BLOCK IS 0.0". For this reason, I could use AMG, however, given that I have an SG, I decided to use BLOCK STONE AND/OR GENERAL AMG (CONNECTIVITY TOLERANCE increased from 10^-14 to 10^-10).

I use 250 RPM of a Rushton turbine with 300mm diameter tank (T), impeller diameter,D=0.33T. Thus, the Re=4.16x10^4 for water.

When I used 20,30,40 and 50 iterations per time step, the convergence was fine within a time step, however, the errors were accumulating and bouncing back to the initial conditions, if not worse, when i moved to the next time step. I, therefore, fell into the temptation of using small iterations, pushing the calculation to some steady state. This i could do well if all a needed was a steady state solution. However, with my tracer case, i just must get good convergence within a given time step. 'This is where water starts breaking the dam'.

I use SIMPLEC, any body with experience of using PISO in a stirred tank (SG)?? Would it be better any way??

I feel that I should now focus on the INNER ITERATION, say, increasing NTURB etc, however, I do not have any experience with this.

Thanks for your time,

Regards,nyatoto

I do not have any experience in mixing tank problems, but just some experience in transient calculations. So If my comment are no help then - sorry.

A good idea could be to check you Courant number

CU = d_t*Umax / d_cell (time step * maximum velocity / minimum cell lenght)

I think it should be around unity.

What kind of time scheme are you using consider using if not already BACKWARD DIFFERENCE QUADRATIC TIME DIFFERENCING is more accurate/or robust. In this case your Courant number could be around 5.

It is my experience for my cases that a number of 15 iterations per time step is sufficient also less depending on the time step. I rather reduce the time step if I have problems.

Regards Jan

Ok so your residuals look somethihng like this?? Sorry my graphical skills are not so good

\ |\ |\ \ | \ | \ \ | \ | \

\| \| \

If these are the graphs of residuals you get as you see the solution develope with each time step then you are ok. It is supposed to be like this.

Kuba

Hi Jan, I use HYBRID and/or HIGHER UPWIND because of the linear interpolation at the interface. I had used QUICK in my steady state modelling, but when I compared my results, I saw that i did not have much gain using QUICK. Probably the gain in using the 3 order accurate QUICK was lost at the interface.

I will try COURANT NUMBER.

Any experienced mixing expert!? thanks

Regards Nyatoto

Yes! It looks like that. However, even after 12,000 total iterations, I do not see (in CANVAS and OUT PUT) much change (<10). It just keeps dancing there!! Should i just be petient? What typical CPU time should I expect in order to see some mass residual convergence of say upto 10^-4 kg/s?

thanks Nyatoto

Hi Nyatoto:

Give this a try. Increase the number of iterations for each time step. This will reduce the mass residuals. If you set the number of iterations high enough you will get to a mass residual convergence that you are looking for. As you have noted, the residuals will "dance" with each time step. The dance reflects the movement of the rotating core within the vessel. Another way to look at it that there is not a steady state solution to the problem.

Regards, John

I was not talking about differencing scheme, but your "time" scheme. The default is a linear time differencing which is only first order. Read in the manual under transient parameters.

Hi Jan, Sorry, for not having got you clearly. I have not tried the BDQ Time Differencing yet. As for now, I have got some network problems, so I cant run my CFD. As soon as it is back and running I will get back to you.

John, You are right. The problem is indeed not steady and is modelled as such. You suggested that I use more time steps, could you please suggest some figures. You can see from my earlier postings that I have tried 4,20,30,40,50. I do not want to go to 100 or more for obvious reasons.

thanks for your time. Nyatoto

Nyatoto:

You say that you used 20,30,40 and 50 iterations per time step and that the convergence was fine within a time step. So how did the mass residual respond to 20,30,40 and 50 iterations per time step?

John

Hi John, Thanks for getting back to me. When I used the 20.....50 time steps, the convergence per time step was fine but but it was always bouncing back. Something some people would like to describe as acccumulation of error from one step to the next. The net result was that it was diverging, after all that bouncing up and down.

There is one thing I would like to know, I am sure there are a lot of guys out there who have experience with a stirred tanks, what order of magnitide of CPU time and total iteration for such system should I expect to have?

One might say it is system specific, yes. Mine is a standard Rushton tubine stirred tank (4 baffles, six blades, H=T, D=0.33T, h=0.2D, etc). I have some other internals that I have not included as yet. Just a simple stirred tank!

regards. nyatoto

Convergence per time step is fine. The simulation has run for more than 150 agitator revolutions. Residuals always bounce back at the begining of each new time step.

All the above sounds normal to me. A few thoughts.

Consider monitoring with USRTRN the velocities at several cells near the Rushton tubine but located in the stationary portion of the mix tank. Set the time step to give 3 to 5 degrees per step, so you can see how the movement of the blade impacts the local fluid velocities. Run for two or three full agitator rotations. Plot the data from USRTRN. If the solution is converged, you should see a repeating cyclical pattern in the velocities at the cells being monitored. There should be six cycles per revolution corresponding to the six paddles on the Rushton turbine.

If you restart from a dump file, be sure to read the grid from the dumpfile so the grid and solution field are matched.

Good Luck.

John

Hi Jan & John and other family members,

I have tried your suggestion of using quadratic time differencing; 15 and 30 iterations per time step, for 432 time steps. There is a modest convergence. I am running it again with more time steps.

John, I will try your suggestion of using USRTRN, however, I am not sure that I quite undertand your suggestion about the CYCLES PER REVOLUTION. Where do you specify this? What I have is just Z CYCLES PER REVOLUTION for the unmatched grid. My repeating geometry is a half tank so I set 2 cycles/rev. Provide more light please.

thanks

Nyatoto

If you are modeling half the geometry then 2 cycles per revolution is correct. But my previous comment was not referring the the cyclic connections. It was in reference to the flow field in the fixed portion of the vessel and how to determine if the model has reached a "stable" flow pattern. My comment was in response to your question on how may iterations did you need to run to get a converged solution. How about sharing your key learnings regarding convergence for your mixing tank model?

Thanks