what is under relaxation factor?
 

Hi all,

1. What is under relaxation factor? 2. what does its effect towards solution? 3. why we need to specify a lot of factor. i mean need 2 specify for example; mass,mom,energy,density,turbulent....... 4. How do we know the correct factor to be used?

5. Can anybody suggest where i can get properties for wood chips? properties such as thermo prop. like conductivity, porosity......

thanks in advance rayy

Re: what is under relaxation factor?
 

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

Re: what is under relaxation factor?
 

very detail answer. Thanks Phil.

Combustion Relaxation Factors
 

I had to lower, my URFs for a combustion model in order to get it stable. Now, I am trying to increase them back to default to make them better.

Is there a particular order in which I should increase them so the solver which would help it converge easier?

Thanks!
Michelle

It depends on the problem. Most of the time the default numbers are the best. Just when there is a fluctuation in residual, you should decrease URF of it. Decrease until fluctuation have been vanished.

relaxation factor
 

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.

Under and over relaxation factors control the stability and convergence rate of the iterative process.The under relaxation factor increases the stability while over relaxation increases the rate of convergence.


xk+1 = w.xcal + (1-w).xk
yk+1 = w.ycal + (1-w).yk

For 0<w<1, the method is known as successive under relaxation.
For 1<w<2, the method is known as successive over relaxation.

where xcal is the value calculated based on xk

helpful article
 

Eects of under-relaxation factors on turbulent flow simulations

Under-relaxation factors
 

Hello,

I'm simulating a steady state case. Risiduals are fluctuating. And i have no choice else to reduce under-relaxation factors to hence stability. But, I really do not understand the influence of this factor. For example for the momentum in natural convection, if we reduce to 0.1, it is like we take the same old solution of the momentum equation and we ignore the new solution. Is it like this??

thank you an advance

Help for CD Nozzle
 

I am trying to solve a flow in convergent-divergent nozzle. Initially due to divergence I reduced the under relaxation factor and obtained the result. My doubt is whether I can use the result obtained as it is or again if I have to change the URF to default and run the iteration again to get the result. Help me

Urf for nozzle!?
I think flows in nozzles should model with density based solver!
In density based solver there isn't URF,instead you can reduce the courant number to controlling convergence!

Nozzle with Pressure based solver
 

Initially I tried with density based solver and it didn't worked. So I switched to pressure based solver and got the result. But the result was for reduced URF. My doubt is whether I have to run back the iteration with default UFR. Kindly help me.

In my idea, it's better that use density based for yor problem
But if you want to use pressure based solver, I think it's better that your problem converges with more URFs and 2nd order for less numerical error!

Under relaxation factor
 

Oh okay thank you. I am facing a different problem. I got solution convergence with 100 times reducing all the URFs. Again what I did is increased the URF to the default value, and iterated again (but without initialization). Now I got a different solution. So I am completely confused. Which solution I can take as the final value. Kindly help me. Thank you very much for the quick replay.

Dear ramesh!
Usually flows must converge with URFs close to defult,but when the solution isn't stable and diverge we can control the solution with reducing URFs! So when solution converge, it's better to continue solution with defult values and check the new results with previous results!
So I think your problem must converge with bigger URF!

Under relaxation factor
 

Thats okay sir. But my question is different. Initially with default URF I couldn't get the convergence. So I reduced the URF values and got convergence. Again what I did is increased the URF to default value and redone the iterations without initialization. This also after 5000 iterations gave me the convergence. Now my doubt is which convergence results I have to consider as the final one. Kindly help me....

As I said, in most cases bigger values and closest to defult are more reliable than small values!

Under relaxation factor
 

Thank you very much sir.......

Thanks Phil. Excellent Explanation

Thanks Amin

It took a month to know which solver I should use.. You are right, it is density based solver for Flow in Nozzles.

Shane

Thanks man
 

Kudos man. Thanks for an awesome presentation.

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!

Why would you relax pressure more than momentum?

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

Effect of URF on Solution
 

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

URFs
 

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

Implications
 

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

Sensitivity
 

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.

Residuals smooth, crazy, smooth
 

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