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

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

very detail answer. Thanks Phil.

[psigcochair]

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

[eng_s_sadeghi]

Originally Posted by psigcochair

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.

[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.

[victoryv]

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

[a.zareinezhad]

Eects of under-relaxation factors on turbulent flow simulations

[Olfa]

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

[asramesh]

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

[amin.z]

Originally Posted by asramesh

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!

[asramesh]

Originally Posted by amin.z

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!

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.

[amin.z]

Originally Posted by asramesh

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!

[asramesh]

Originally Posted by amin.z

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!

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.

[amin.z]

Originally Posted by asramesh

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!

[asramesh]

Originally Posted by amin.z

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!

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....

[amin.z]

Originally Posted by asramesh

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!

[asramesh]

Originally Posted by amin.z

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

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

[sircorp]

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

Thanks Phil. Excellent Explanation

[sircorp]

Originally Posted by amin.z

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!

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