[Bharadwaj B S]

Originally Posted by misagh

hi,we have under relaxation factor(<1) and also over relaxation factor(>1).
how to adjust the factors is so complicated and cant be explained easily.
you can visit this address:
www.bakker.org/dartmouth06/engs150/05-solv.ppt
p.p 16-17-...
i found it really useful.
best regards.

Kudos man. Thanks for an awesome presentation.

[sebastianbn]

Hey!
I'm trying to load a previous result (steady state) done in a coarse mesh into a finer one, but it seems it doesn't work... I read that I should drop the URF at least for the first iterations, which I did, but then when setting the default ones again, the solution crashes.

Do I have to run the whole calculations with lower URF?

Cheers!

[randolph]

Originally Posted by Phil
;140717

Each of the variables(mass,mom,density) represents an equation the solver is trying to solve. Each iteration the values obtained for the variables should get closer and closer together - converge. FOR SIMPLE PROBLEMS ESPECIALLY COLD FLOWS WITHOUT COMBUSTION YOU SHOULD SIMPLY KEEP THE RELAXATION FACTORS AT DEFAULT.

Sometimes for many many reasons the solution can become unstable so a relaxation factor is used - takes part of value from previous iteration to dampen solution and cut out steep oscillations.

If you are having convergence trouble start the solution on default then when it starts going to shit(becomes unstable) put pressure 0.2 momentum 0.5 turbulence KE 0.5 turbulence DR 0.5 - this should be in the manual. This should sort out most issues much worse and you need a better mesh or something isn't correct.

RELAXATION FACTORS MAKE SOLUTION TAKE ALOT LONGER TO CONVERGE SO ONLY USE WHEN YOU REALLY NEED TO.

Generally start off without RF's then when solution becomes unstable later on bring them in where needed - whichever equations (residual graph) are unstable, meaning not a nice smooth line but up and down rapidly. Start off moving down from 1 to 0.8 or 0.8 to 0.6 etc. For energy equation start off with 0.9 it takes hundreds or thousands of iterations to converge with relaxation factors in.

ALWAYS REMEMBER--------- ALWAYS START WITH DEFAULTS. ONLY WHEN SOLUTION BECOMES UNSTABLE DO YOU RELUCTANTLY LOOK AT THE RESIDUALS AND BRING IN APPROPRIATE RF's.

hope this helps

Why would you relax pressure more than momentum?

Isn't that SIMPLE family algorithm overshoot velocity instead of pressure?

[ViLaks]

Hi All,

I am solving a natural convection problem (Transient). Aim is to find the temperature drop within a volume in 2 hours. I am using Fluent for the simulations.

What I am observing is that the transient behaviour is different when I use different values for solution controls. In Picture 1.png, I have used default values for Solutions controls, whereas in Picture 2.png, I have under relaxed Body forces and Energy to 0.8 (Default: 1). There is no other change in the case/mesh/geometry. Now, can someone explain what is happening here and which is correct. As per my understanding, the Solution controls are for faster / slower convergence and stability issues. They should not affect the solution

[vinerm]

You are right; URFs are meant for stability and do affect the convergence rate. But they also behave like diffusion controls. In other words, if very low URFs are used, it takes more iterations for a field to reach not just convergence but also conservation. Energy time scales are larger, i.e., it takes longer for thermal energy to diffuse. Therefore, higher URFs are used for it. When lower URF is used, it would require more iterations to reach same conservation level. So, you have to ensure that when URF is reduced, you run for more iterations in each time-step and convergence target for energy is achieved. You may also reduce the convergence target to 1e-7.

[ViLaks]

Originally Posted by vinerm

You are right; URFs are meant for stability and do affect the convergence rate. But they also behave like diffusion controls. In other words, if very low URFs are used, it takes more iterations for a field to reach not just convergence but also conservation. Energy time scales are larger, i.e., it takes longer for thermal energy to diffuse. Therefore, higher URFs are used for it. When lower URF is used, it would require more iterations to reach same conservation level. So, you have to ensure that when URF is reduced, you run for more iterations in each time-step and convergence target for energy is achieved. You may also reduce the convergence target to 1e-7.

Thanks for your prompt reply, Vinerm.

The energy residual has converged to 1e-7.
You mean to say, if I use higher number of iterations per time step, my profile in 2.png will be similar to 1.png? If that is the case, then it is incorrect because experimental data follows a profile similar in 2.png.

Regards
VL

[vinerm]

What I mean is whether you use low URF or high, you need to ensure that the convergence within each time-step is good. If you are getting wrong results with high URF for energy, most likely the time-step used is higher than expected.

[ViLaks]

Originally Posted by vinerm

What I mean is whether you use low URF or high, you need to ensure that the convergence within each time-step is good. If you are getting wrong results with high URF for energy, most likely the time-step used is higher than expected.

So, ultimately the inference is URFs affect only the stability and convergence of the results.

Yes, my time step is in fact pretty high. But I have used it in purpose because it was not creating problems like these in the past. I have also validated results with different time steps and I am using the one which gives me the results at the earliest.

Anyways, thanks for the reply.

Regards
VL

[vinerm]

Most of the time, users do a grid sensitivity analysis, but it is incomplete. Grid is spatial as well as temporal. By grid sensitivity analysis, users usually imply spatial. However, temporal is equally important.

[Ramon Quiñonez]

Hi. I am simulating non premixed combustion with propane for stabilisers, I reduced my URF as specified in the manual, however left the momentum and turbulence DR as 0.8. My residuals went down pretty well, and then after 150 iterations they went up for at least 300 more iterations. However after 450 iterations they are normalising, and then they go down smooth again. Does this affect my solution? I am using a 3D model with more than 4 M nodes, realisable kE, and laminar flamelet.

Thanks!

[ViLaks]

Originally Posted by Ramon Quiñonez

Hi. I am simulating non premixed combustion with propane for stabilisers, I reduced my URF as specified in the manual, however left the momentum and turbulence DR as 0.8. My residuals went down pretty well, and then after 150 iterations they went up for at least 300 more iterations. However after 450 iterations they are normalising, and then they go down smooth again. Does this affect my solution? I am using a 3D model with more than 4 M nodes, realisable kE, and laminar flamelet.

Thanks!

I havent worked on combustion problems. But looking at the residuals, it should not affect your solution. But ensure that you run for much more iterations and see if the residuals shoot up again, even if it does, if the trend is same, do not worry. Use surface monitors to check for correctness of your simulations
Regards
Vignesh