# Converging the solution

 Register Blogs Members List Search Today's Posts Mark Forums Read

 June 25, 2015, 09:07 Converging the solution #1 Senior Member   Aja Join Date: Nov 2013 Posts: 493 Rep Power: 13 Hi, As I explained in the my previous threads, I designed a turbine and Now I am simulating expressed turbine in fluent. But solution is not converged. I changed under-relaxation factors and discretization schemes, but I don't know that why solution is not converged. Case and Data files are placed in the following link, I am really grateful that you check these files and guide me and If It is possible, please place useful links about this problem until we can converge this simulation. http://www.4shared.com/rar/klHltuXVba/Amir88-BC3.html My tool of simulation is a Laptop(Fujitsu) with 6 G ram and core i7 CPU 2.2GHZ. really thanks, Best, Amir

 June 25, 2015, 09:30 #2 Senior Member   Cees Haringa Join Date: May 2013 Location: Delft Posts: 607 Rep Power: 0 How did you decide the simulation did not converge? aja1345 likes this.

June 25, 2015, 09:58
#3
Senior Member

Aja
Join Date: Nov 2013
Posts: 493
Rep Power: 13
Quote:
 Originally Posted by CeesH How did you decide the simulation did not converge?
Hi,

because take to long time.

In fact, solution is not divergent but I think that this process is very long time. and I can't reach to convergence. How can I reach to convergence rapidly? I think that Values of under-relaxation factors and discretization schemes are not correct.

Thanks

 June 25, 2015, 11:05 #4 Senior Member   Cees Haringa Join Date: May 2013 Location: Delft Posts: 607 Rep Power: 0 But how do you judge whether the simulation converged or not? That has nothing to do with time. You need to have some basis on which you say, now the outcome has converged, or it has not (and will not). So how did you decide that? What is your criterion for convergence?

June 25, 2015, 12:06
#5
Senior Member

Aja
Join Date: Nov 2013
Posts: 493
Rep Power: 13
Quote:
 Originally Posted by CeesH But how do you judge whether the simulation converged or not? That has nothing to do with time. You need to have some basis on which you say, now the outcome has converged, or it has not (and will not). So how did you decide that? What is your criterion for convergence?
Hi,

what is your exact meaning of 'That has nothing to do with time'?

I don't judge and I am New in fluent. maybe It is converged or not converged. But what is important to me, It is converged rapidly. According to recent simulations in this case, It took to a long time. I placed case and data until you guide me about this problem. The criterion is 1e-6.

Thanks

 June 26, 2015, 04:50 #8 Senior Member   Cees Haringa Join Date: May 2013 Location: Delft Posts: 607 Rep Power: 0 There's a difference between a correct solution and a converged solution, and also a mesh-independent solution. A converged solution means the solution doesn't change significantly anymore when adding more iterations. A mesh independent solution means that, increasing the mesh density further, the results will not change significantly anymore. A correct solution means the solution is well in agreement with experimental data. But these are three fully different things. You should first strive for your solution to converge; so, make sure a stable answer without significant oscillations or changes over a number of iterations is found. Then the solution is converged, but it does not have to be correct, or mesh independent. Then, check for mesh dependency: Does the solution change when you add more elements to the mesh? For example, say I have a stirred tank (because I happen to have one), and I have 5 meshes - checking for the power number. The meshes (1-5) have 100.000 - 500.000 elements in increases of 100.000. I may find the following: 100.000 elements - Po = 3.5 200.000 elements - Po = 4.7 300.000 elements - Po = 5.2 400.000 elements - Po = 5.4 500.000 elements - Po = 5.45 Based on this data, I can say that increasing the mesh density from 400.000 to 500.000 elements does not make my solution very different. Hence, mesh 4 is good enough. For certain applications, mesh 3 might suffice too, but mesh 1 and 2 are certainly not good. So, with mesh 4 I checked the solution to be mesh independent. Now that I know that, I will continue to use mesh 4, and check if the solution is correct. Now in literature I find a value of the power number for this setup, and it is 4.7 This means that although the solution on mesh 4 converged, and the solution is mesh independent - it is not correct. There is a big offset in power number! This indicates that the turbulence model I was using, or the discretization method I was using, cannot properly capture the physical behavior of the tank. Knowing this, I can look for a better physical model. (Note: The PO of 4.7 does not mean mesh 2 was better! In mesh 2 the solution was mesh-depending, so there is certainly an error there! In this case the physical and numerical error balance eachother making it look like the mesh does very well, but in fact, it does pretty bad!) So to summarize, always work in this order. if your solution does not coverge, there's no point in checking mesh dependency or physical accuracy. if the solution converges but is not mesh independent, there's in no point in physical interpretation. only if your solution converges and is sufficiently independent of the mesh, you can truly interpret the physical results. aja1345, attiquejavaid08, Ansys2015 and 7 others like this.

June 26, 2015, 09:32
#9
Senior Member

Aja
Join Date: Nov 2013
Posts: 493
Rep Power: 13
Quote:
 Under-relaxation factors are easy: lower values mean slower convergence but more stability, higher values vice-versa. My advice: start high, and if you observe oscillations in the solution, reduce them for stability. So, end low.
Hi Ceesh,

Really thanks for your guide, I fully realized. But another questions:

1. you said that i start high value, But how much? 0.3? or 0.7? etc.

2. what is your exact meaning of 'So, end low'? Is it means that I continue with low values?

I am grateful that guide me about values of Under-relaxation factors.

Thanks,

Best,

Amir

 June 26, 2015, 10:49 #10 Senior Member   Cees Haringa Join Date: May 2013 Location: Delft Posts: 607 Rep Power: 0 Hi Amir, It depends a bit on the situation you are modeling. Typically I just start with the default values for all factors, unless I know upfront that certain equations may be difficult to stabilize. For example in stirred tanks with radial impellers, I may start with 0.2 for momentum (following Andre Bakker, you can find some advice on www.bakker.org) if I know that I won't be around the computer for a while to check how convergence is going - because I know at some point I may have to alter the value. Other than that, I suggest to start default, and if during the process you notice that one of the residuals gets 'stuck' (so is oscillating up and down without any general downward trend), reduce the underrelaxation factors. What I typically do for stirred tanks when I am around to change things, is start with momentum at 0.7 to make some fast first iterations, then after 2500 iterations change to 0.1 - 0.2 or so to finish more accurately. That's what I mean with start high, end low. I do not know of any papers discussion URFs at length, or at least, I never referenced them since they very much focus on the mathmatical implemenation, and I regard them more as a tool - so knowing the basic idea behind them suffices for me. Also I'd recommend; if the URFs need to be below 0.1 for your simulation to converge, you probably need to change your mesh. Otherwise the solution is going to take very long at best, and probably won't converge at all. This is no hard limit or so, just a lesson from experience. aja1345, attiquejavaid08 and sanjaykummar2810 like this.

June 26, 2015, 19:00
#11
Senior Member

Aja
Join Date: Nov 2013
Posts: 493
Rep Power: 13
Quote:
 Originally Posted by CeesH Hi Amir, It depends a bit on the situation you are modeling. Typically I just start with the default values for all factors, unless I know upfront that certain equations may be difficult to stabilize. For example in stirred tanks with radial impellers, I may start with 0.2 for momentum (following Andre Bakker, you can find some advice on www.bakker.org) if I know that I won't be around the computer for a while to check how convergence is going - because I know at some point I may have to alter the value. Other than that, I suggest to start default, and if during the process you notice that one of the residuals gets 'stuck' (so is oscillating up and down without any general downward trend), reduce the underrelaxation factors. What I typically do for stirred tanks when I am around to change things, is start with momentum at 0.7 to make some fast first iterations, then after 2500 iterations change to 0.1 - 0.2 or so to finish more accurately. That's what I mean with start high, end low. I do not know of any papers discussion URFs at length, or at least, I never referenced them since they very much focus on the mathmatical implemenation, and I regard them more as a tool - so knowing the basic idea behind them suffices for me. Also I'd recommend; if the URFs need to be below 0.1 for your simulation to converge, you probably need to change your mesh. Otherwise the solution is going to take very long at best, and probably won't converge at all. This is no hard limit or so, just a lesson from experience.
Hi CeesH,

Really thanks,

Can you explain about discretization? For example, I think that second order upwind for momentum make convergence will become fast in my simulation. what is your opinion?

I am grateful that also guide me about turbulent kenitic energy and turbulent dissipation rate.

Best,

Amir

 January 21, 2019, 11:15 Apdl problem #12 Member   mahya Join Date: Jul 2016 Posts: 45 Rep Power: 8 Hello I simulate a cylinder in ansys apdl I have this error solution not converged at time ansys apdl Please help me

 January 21, 2019, 14:01 #13 Senior Member   Join Date: Dec 2016 Posts: 152 Rep Power: 9 Unfortunately, I think you're asking the wrong people, dude. Not only is this post well over 3 years old, but what they were talking about isn't really close to your problem. For future reference, read this in regards on how to ask a question (Guide: How to ask a question on the forums). Then, if you really can't figure it out, go ahead and post a new question to the forum. If you tack on to old conversations, new people reading it will have no clue what's going on or where their solution is. We, as a community, are here to help one another. Also, you do realize this is a website dedicated to CFD, right? ANSYS APDL (which I'm assuming is Mechanical APDL) is a structural program and, while some people do use it to run fluid-structure interactions (FSI), we typically only talk about fluid solvers here. More specifically, since this is the Fluent forum, we talk about Fluent here. I'd recommend finding a structural forum (I think XANSYS might be good). Good luck!

June 15, 2022, 00:46
#14
Member

Vivek MJ
Join Date: Oct 2020
Location: India
Posts: 53
Rep Power: 4
Quote:
Thank you for your detailed and well written explanation.