CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   FLUENT (http://www.cfd-online.com/Forums/fluent/)
-   -   convergence in transient analysis using FLUENT (http://www.cfd-online.com/Forums/fluent/114635-convergence-transient-analysis-using-fluent.html)

sumeet kotak March 14, 2013 11:35

[HELP!!!]convergence in transient analysis using FLUENT
 
hello frnds....

i m doing analysis using ANSYS fluent n doing transient analysis.

i am very confused related to that
1. is it necessary the solution to be converged before completing each n every time step?
2. if not converged after every time step is it affect the accuracy of the result?
3. upto which limit the step size can be reduced to obtain accurate result in optimized time?
4. maximum limit for the no. of iteration/step size?

please reply as early

thanks in advanc

sumeet kotak March 19, 2013 00:17

can anyone help me in regarding with above que.....?


regards.

flotus1 March 19, 2013 03:06

Quote:

1. is it necessary the solution to be converged before completing each n every time step?
Yes. This does not apply to the first few time steps if the initial solution was not obtained by a steady state simulation, but rather on a global guess.

Quote:

2. if not converged after every time step is it affect the accuracy of the result?
Yes. Same exception as in 1.

Quote:

3. upto which limit the step size can be reduced to obtain accurate result in optimized time?
You can reduce the time step size as far as you want. The problem will be that you need more time steps to cover the same physical time.

Quote:

4. maximum limit for the no. of iteration/step size?
As a rule of thumb, the time step size should be chosen sufficiently small to reach convergence within 5-10 iterations.
So if it takes more iterations to converge, it would be more efficient to reduce the time step size than increase the number of iterations.

blackmask March 19, 2013 03:29

You need to ensure the convergence to some accuracy within each time step when you need the accurate transient information of your flowfield. Otherwise, the residual will act as forcing terms in your original (RA)NS equations.

By step size do you mean the number of iterations? As long as the residuals would drop to an acceptable level, which is rather problem-specific but usually means drops by 2~3 order of magnitude within each time step.

I don't think there would be an upper limit for the number of iterations. For simple flow and geometry I think it is possible that the residuals reduced to machine zero after sufficient many iterations. But in practice the residual stayed at a much higher level.


Quote:

Originally Posted by sumeet kotak (Post 414021)
hello frnds....

i m doing analysis using ANSYS fluent n doing transient analysis.

i am very confused related to that
1. is it necessary the solution to be converged before completing each n every time step?
2. if not converged after every time step is it affect the accuracy of the result?
3. upto which limit the step size can be reduced to obtain accurate result in optimized time?
4. maximum limit for the no. of iteration/step size?

please reply as early

thanks in advanc


oj.bulmer March 19, 2013 09:56

It is worthwhile to explore the adaptive timestepping approach, wherein the timestep is automatically calculated for you.

OJ

sumeet kotak March 20, 2013 04:02

thanks. for all of yours valuable rply..... helps me lot...




n one more thing i would like to ask that upto which limit we can reduce under relaxation parameters.... n any effect of it on results..?

once again thanks for giving previous one question's replay....

regards

flotus1 March 20, 2013 04:44

If you reduce the relaxation factors, the solution changes slower over the iterations. So you need more iterations to reach the same accuracy.
But if you have enough iterations, the solution will be the same.

You should only reduce the relaxation factors if you are facing convergence issues.

RodriguezFatz March 20, 2013 05:31

Hey,

Let me add some things:
Whether you need convergence at every time step or not really depends on your case! The other day someone here in the forum had problems with an air beam impinging into water. He "lost" water from his bowl during the simulation because the first iterations did not converge. On the other hand, if you simulate some globally unstable flow (e.g. bluff body) where you want to study the vorticies behind the bluff body, every fluid particle will leave the domain at some point, so iterations of "old" time steps don't matter at all.

You could try to half the time step size and see if your result changes strongly.

sumeet kotak March 22, 2013 07:34

[QUOTE=oj.bulmer;414983]It is worthwhile to explore the adaptive timestepping approach, wherein the timestep is automatically calculated for you.

In adaptive time step, time step may get automatically as per requirement, If I am not wrong....
But Sir I am using custom field variable to find out mass deposited

mass deposited=density*area*Velocity*time step size

In above mention case can I use adaptive time step method...??

oj.bulmer March 22, 2013 07:48

Adaptive timestepping decides the timescales globally. Now whatever timestep is being used for current iteration, will be used in your formula for that iteration by FLUENT.

OJ

sumeet kotak March 23, 2013 02:04

thanks to all off you for ur valuable reply.... it helps me lot to gain my knowledge.....

now I am facing new problem.......!!
once I got convergence at step size 0.005 n solution getting converged after every 5-10 iteration but now no. of iteration required to converge is increasing and goes to 20-30......!!!!!!

why is it happen.....??? any specific reason...!!!!
I am simulating electron beam physical vapour deposition system using species transport model using reaction is on.... n transient simulation is completed upto 3 second.....

one additional problem

I have equations in residual like
1.continuity
2.x, y, z momentum
3. energy
4. y2o3
5.yo
6.y
7.o
8. o2

the residual value for all above are below specified value except oxygen (o2).... specified value is 1e-3

n after every 3 iteration showing msg

temperature limited to 1.000000e+000 in 1 cells on zone 2 in domain 1


my project is on track means getting convergence but suddenly facing above problem..... seeing help...:(
thanks in advance...

Far March 23, 2013 03:22

Quote:

Originally Posted by oj.bulmer (Post 414983)
It is worthwhile to explore the adaptive timestepping approach, wherein the timestep is automatically calculated for you.

OJ

Yes I agree. But it always stops at the minimum time step you set. There are many time scales in your simulation which you are not interested to resolve for your requirements.

However adaptive timestepping is good in situation where you want to achieve some time step (minimum time step in settings) in automatic fashion.

Far March 23, 2013 04:01

Quote:

Originally Posted by flotus1 (Post 414875)

As a rule of thumb, the time step size should be chosen sufficiently small to reach convergence within 5-10 iterations.
So if it takes more iterations to converge, it would be more efficient to reduce the time step size than increase the number of iterations.

I have couple of questions:

1. What should be the time step size for pressure based solver with simple, simplec type pressure-velocity coupling.

2. What should be the time step size for pressure based coupled solver

3. what should be the time step for coupled solver.

4. What if we enable 2nd order Implicit time formulation.

5. Should we ensure CLF number less than 1 for accuracy?

6. What is the convergence criteria for transient simulation? It is achieved when residuals are reduced by three orders for each time step or some other parameter like mass flow rate? For mass flow rate what should be convergence criteria? 0.1% imbalance (I read it in post on forum) or even tighter?

7. How much error should be acceptable while making the time step sensitivity analysis?

8. It is said that time step restriction is reduced for PISO scheme i.e. we can use larger time step. What does it mean? Does it mean that for coupled pressure based solver we have more relaxation in choosing time step?

flotus1 March 23, 2013 16:35

I dont feel competent to answer all of the questions, but I can do my best on some of them. If anyone wants to add something or disagrees with my statements, feel free to do so.

1. What should be the time step size for pressure based solver with simple, simplec type pressure-velocity coupling.

Depends on the type of flow. The timescale of a transient boundary condition or the expected frequency of vortex shedding will determine the reasonable time step size.
The solver itself can handle any time step size.

2. What should be the time step size for pressure based coupled solver

If you use the coupled solver you obviously want to capture pressure waves. So their frequency determines the time step size.

4. What if we enable 2nd order Implicit time formulation.

I would always choose a second order accurate time formulation.
Maybe someone else knows when to use first order.

5. Should we ensure CLF number less than 1 for accuracy?

This is a stability constraint for the explicit solver and would lead to unreasonably small timesteps for the implicit solvers.
But it is good value to guess the timestep for LES.

7. How much error should be acceptable while making the time step sensitivity analysis?

This is really up to you. When I carry out a sensitivity analysis for time step size or grid spacing, I usually just show that the solution converges with better discretization.

dinesh September 30, 2013 13:33

Transient time
 
Quote:

Originally Posted by RodriguezFatz (Post 415209)
Hey,

Let me add some things:
Whether you need convergence at every time step or not really depends on your case! The other day someone here in the forum had problems with an air beam impinging into water. He "lost" water from his bowl during the simulation because the first iterations did not converge. On the other hand, if you simulate some globally unstable flow (e.g. bluff body) where you want to study the vorticies behind the bluff body, every fluid particle will leave the domain at some point, so iterations of "old" time steps don't matter at all.

You could try to half the time step size and see if your result changes strongly.

I am doing transient analysis of a radiation problem. My query is when i start the itr, for the first 4-5 iteration the solution converges in 15-20 itr but further the solution converges at each time step. What does this mean. I start my sol itr with time step 0.05 and had gone upto 10s but the situation remain same. i.e at each time step soln converges. i doubt it.
plz suggest

sumeet kotak October 14, 2013 03:13

Quote:

Originally Posted by dinesh (Post 454327)
I am doing transient analysis of a radiation problem. My query is when i start the itr, for the first 4-5 iteration the solution converges in 15-20 itr but further the solution converges at each time step. What does this mean. I start my sol itr with time step 0.05 and had gone upto 10s but the situation remain same. i.e at each time step soln converges. i doubt it.
plz suggest

According to my observation related to my transient analysis problem
once you achieved stable solution, your problem getting converged after regular interval of no. of iterations (i.e. 5 iterations/ time steps) irrespective to the no. of time steps u had set and run your solution till the results upto which time u required.

If I was wrong at any, experts please suggest

Regards

dinesh October 14, 2013 07:16

Transient timand iteration
 
Quote:

Originally Posted by oj.bulmer (Post 415677)
Adaptive timestepping decides the timescales globally. Now whatever timestep is being used for current iteration, will be used in your formula for that iteration by FLUENT.

OJ

I am doing transient analysis of a radiation problem. My query is when i start the itr, for the first 4-5 iteration the solution converges in 15-20 itr but further the solution converges at each time step. What does this mean. I start my sol itr with time step 0.05 and had gone upto 10s but the situation remain same. i.e at each time step soln converges. i doubt it.
plz suggest

Azy June 2, 2014 10:54

Hi all,

I am running a transient simulation. my solution just converged during 3 first iteration and it goes well up to the 30th one, and then it just diverged! could any one help me that about the possible cause?

i'm using the time step of .003, and i just monitor the solution by residuals.

Thank you in advance

Azy June 2, 2014 10:59

Quote:

Originally Posted by flotus1 (Post 415191)
If you reduce the relaxation factors, the solution changes slower over the iterations. So you need more iterations to reach the same accuracy.
But if you have enough iterations, the solution will be the same.

You should only reduce the relaxation factors if you are facing convergence issues.

I'm just confused, when ever i changed my momentum in relaxation factor, my residuals just decreased so fast! so i couldn't understand that when every one say that it makes the process slower. could u help me about it?

Khalil September 21, 2014 06:45

Can anybody tell me that in case of heat transfer process I solved steady state case and achieved a certain temperature. While solving unsteady case the temperatures goes higher than as it was in steady state solution. :confused:


All times are GMT -4. The time now is 19:13.