hi all,

i am solving a natural conv. problem with a air fluid zone above a porous zone. I am good fine mesh of about 27000 cells for a 2D axi sym problem. (unsteady)

now since i am using enhanced wall + k epsilon, y+ has to be maintained around ~1 right ?

now after few hours of simulation i found y+ max to be 1.35 and hence i refined the grid with limits 0 to 1 for y+ .. to my surprise , i found that the simulation that was converging well till then, diverged ! -- WHY?

I perhaps adapted and refined the grid too much unnecessarily ? -- but still refining should not hurt - why diverge ??

please shed some light on this issue so that I dont screw up my simulations in haste of better simulation.

thanks

Hey CO2,

Can you post some more information about your set up, including bc's, solver parameters, urfs etc.

Tom

can I email you the summary file? please email me at klimm1290@yahoo.com

I have sent you an e-mail.

Tom

Okay, I have looked at you summary.

The only thing that I can notice is that your underrelaxation factors for pressure and momentum are very low (0.1). When using the PISO scheme you can effectively put all your urf to 1 and maybe if you have problems with pressure you should lower this one to 0.7. I also noticed that you have large time steps (>1sec). I feel for natural convection problems that you have to use very small time steps as large changes in the solution can cause instabilities. I think with the urf at 0.1 you are not really converging your solution - in effect you are getting false convergence as the continuity residual is forced down. I would suggest therefore very small steps and higher urfs. This may not work as you might have other problems with the simulation such as grid quality etc.

Hope this helps. Tom.

Tom,

Thanks for your comments - They are certainly most helpful. AFter getting your email, I talked with another good CFD engineer, and I have learnt a few things today. Let me summerize here for all of you to read. And if you find anything wrong, please respond.

I speak for natural convection problem - but the same might be true for other unsteady problems.

1. it is important to start with small time steps around 0.0001 sec and small urfs. may be pressure and velocity at 0.1 and others around 0.7 or 0.6 2. solution should be stabilized with small time steps. 3. the thumb rule is if you are using small urfs you should allow around 200 iterations per time step -- if you are using higher urfs, then you should allow around 30 to 35 iterations per time step. 4. you have to be careful of false convergence 5. if solution is converging before the required number of iterations, make the conv criteria stricter so that sufficient number of iterations are done per time step

now when i came across all this info today. my simulation was converging well with conti, x, y and all the rest of the conv criteria at 0.0001 energy at 1e-6 --- but time step was 1 sec and number of iterations were about 10 per time step with small urfs -- now THAT IS PERHAPS FALSE CONVERGENCE.. I should not bring all the urfs to default, and select a time step size and convergence criteria such that solution converges in about 35 iterations ..

question: I believe all the autosaved case and data files dont have very correct data -- perhaps false convergence -- so can i start with the latest data file and make sure that i get true convergence from here onwards ? or do i have to start all over again ?

the reason why i am going to larger time steps of 1 sec is because i am looking to get data for several days around 30-35 days - and with limited computational resources i can not afford a time step less that 1 sec -- in fact 1 sec is anyways too small for me -- but as you suggested earlier, if it is just wrong to use a time step size of 1 sec for natural convection problem, then let me know -- i guess in that case i just dont have any choice if the only way of getting correct results is a small time step size.

You will probably find you will need to start from t=0.

Larger time steps doesn't always mean you will get quicker results. Sometimes small time steps that converge quickly will be faster and I believe more accurate.

Tom

tom,

right, I have now all of urfs at 1 except pressure at 0.6 I am getting good convergence in about 35 iterations. I have specified conv. criteria very strict at 1e-9 -- thus making fluent to deliberately do exact 35 iterations per time step which of size 0.5 sec -- I have another simulation running with 0.1 sec time step at a different computer. both of my simulations are showing good results and convergence -- I agree that it is not always a good idea to increase time step.

I am seeing that at the end of 35 iterations conti resi settles and oscillates around 1e-5

now my question is : is it always necessary to have atleast 35 iterations per time step when you are using high urfs ?

No is the answer. If you are using small time steps then effectively the solution is changing in very small amounts through each time step. It may only take say 10 iterations to get convergence. In this case it is then possible to increase very slightly the time step. Your convergence criteria is high so I would say you can increase the time step a bit more. What are you using to judge convergence. Don't just go by the residuals as they are not always a good measure of convergence. Make some monitors on surfaces or points within your flowfield and monitor velocities and pressures at these locations to make sure the solution has stoped changing before increase in time. Let us know if the results come out well - It sounds like you are making progress!

hi,

good. I have been monitoring avg velocities, temperatures, co2 ppm etc in the most critical parts of my model. I found that even with a time step size of 0.7 sec all these quantitites stabilize after about 10-15 iterations.

when i use 0.7 as time step size, my conti resi stabilizes around 8e-5 when i use a smaller time step size like 0.1 sec, conti resi stabilizes around 1e-7 -- the rest of the quantities, monitors stablize in around 8 iterations.

i guess thus, a time step size of 0.1 sec is going to give me faster results if i allow 10 iterations per time step (max) ... plus these results are going to be more accurate than the ones obtained using higher time step size ..

what do you think?

folks,

I am just updating everyone on the status/progress on my project.

With all your help, I was able to get the stability in my model. I have finalized the grid and urfs etc. But getting results is a pain due to the vast amount of time that it is taking. For better results I have decided to run my model at 0.2 sec time step, that further adds to the time delay.

I have decided to run my model in parallel. The network admin at school is currently in the process of installing MPICH on some of the computers, so that I can start my model. I will let you know once the I start getting results!

Any further advice from you guys is welcome. Especially since this is my first time doing parallel processing.

hi folks,

When I try to solve my natural convection problem (2d. axisymmetric) on a single processor, serial mode 2GB machine, it is taking too much time. My time step size is 0.2 sec, My experiments are 30 day long .. so it is just imposssible to wait to get all the results from a single processor.... So I was thinking running fluent in parallel. We do have several available processors here and those certainly can be used. I have been reading about parallel processing related questions on this forum for the last few hours. I noticed that if I try to solve a small problem in fluent parallel, then actually I can end up spending more time in parallel as fluent spends too much time in communication. We do have a 100 MB/sec connection speed University LAN which is very good. My problem has only 30,000 cells. Should I really attempt to solve this problem in parallel .. I just can not imagine running this model for over 30 to 40 days of actual time and then comparing results .. please suggest some solution. Time step size can not be increased as i am dealing with buoyancy driven flow and I want to preserve accuracy ..