# Transient simulations: how to tell its converged (I've read the FAQ & user guides!)

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

March 12, 2013, 04:59
Transient simulations: how to tell its converged (I've read the FAQ & user guides!)
#1
Senior Member

Mr CFD
Join Date: Jun 2012
Location: Britain
Posts: 361
Rep Power: 14
Hello,

I have a transient problem. In my problem a plate is heated from below, which heats up the liquid column above it (please see the picture). The large temperature difference between T1 and T2 causes unsteady, buoyant natural convection.

In steady state I know what parameters to look out for to ensure convergence (correct me if I am wrong):
- You must give enough iterations to allow the residuals must fall acceptably low (for single precision no more than 1e-6). I understand you can get effects such as psuedo-steady state.
- Imbalances must be less than 1%, and ideally less than 0.01%.
- You must set monitor points inside your domain to monitor points of interest such as temperature and velocity. If these level out it suggests a steady state.
- You must do a mesh sensitivity study and tailor your mesh.

I know my problem is transient as:
- I've run the simulation in steady state with a specified physical timestep (the timestep was first estimated, and then reduced or increased depending on residual behaviour).
- Steady state imbalances are not acceptable.
- Monitoring key variables such as temperature and velocity in my domain suggest the problem is transient.
- Logically I expect the physical problem to be transient.

I am homing in to the solution in the following way:
Run 1. Do a steady state pure conduction case first (as in go into expert parameters and switch fluid modelling off).
Run 2. Using the results from Run 1. I initialise and do a steady state buoyant simulation using an upwind advection scheme.
Run 3. Using the the results from Run 2. I initialise and do another steady state simulation using a high resolution advection scheme. The residuals and imbalances do not fall.
Run 4. Using the results from Run 3. I initialise and do a transient simulation using a high resolution advection scheme and a second order transient scheme (backward Euler). The residuals do fall and the imbalances do reduce acceptably low.

A picture of the transient residuals are attached. A picture of some velocity vectors are also attached. Hopefully you can get a feel for the problem.

After reading the FAQ, Ansys User Guides, and searching the forum it is still not clear what criteria must be met to ensure a transient simulation has converged! I know there is something called "Transient Statistics" in CFX, however I don't know how these are used to determine convergence.

Any input will be appreciated!

A few further notes:
- A mesh sensitivity study has NOT been conducted yet - it will be the next step (to compare transient results on Mesh 1 vs Mesh 2 vs Mesh 3 etc).
- I've set the problem to be 2D (extruded one cell thick). In reality the domain is a 3D cylinder (and that will be the next step). I want to understand the problem in 2 dimensions before I move onto 3 dimensions.

Thank you
Attached Images
 Geometry.jpg (11.5 KB, 280 views) Residuals.jpg (56.4 KB, 479 views) Velocity vectors.jpg (26.8 KB, 341 views)

 March 12, 2013, 05:12 #2 Super Moderator     Alex Join Date: Jun 2012 Location: Germany Posts: 3,400 Rep Power: 47 To me, your results look like a turbulent flow simulated with a DNS-solver at insufficient spatial and temporal resolution. Did you try to simulate your case with a turbulence model activated?

 March 12, 2013, 05:16 #3 Senior Member     Mr CFD Join Date: Jun 2012 Location: Britain Posts: 361 Rep Power: 14 Thanks for your reply. I am doing a turbulent simulation using a 2 equation model (K Omega SST) as I type this reply. This is obviously cheaper than doing a DNS simulation. However DNS may be done in the future. But I would still like to know how to tell if a transient simulation has converged. Do you know what is meant by transient statistics?

 March 12, 2013, 06:05 #4 Super Moderator     Alex Join Date: Jun 2012 Location: Germany Posts: 3,400 Rep Power: 47 The transient statistics can be used for data sampling, e.g. time-averaging of variables.

 March 12, 2013, 06:08 #5 Senior Member     Mr CFD Join Date: Jun 2012 Location: Britain Posts: 361 Rep Power: 14 Hi flotus1, How valid are time averaged results of a problem which is very transient? Also how do you view time averaged results?

 March 12, 2013, 06:13 #6 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,729 Rep Power: 143 What Rayleigh number is the flow? That is what will tell you whether the flow is turbulent or not. This flow is almost certainly 3D transient. Your 2D model is of little use other than to check the setup works, it will have little similarity to the 3D case and you cannot infer any 3D results from it. The answer to your question (how do I tell it is converged?) is a sensitivity study. Do a baseline simulation, then change the parameter of interest (convergence tolerance, imbalance, time step size, mesh size) and see if the change is less than a tolerance you are happy to live with in parameters you care about. You will find these sensitivity studies are a little iterative - the mesh size affects the time step size affects the convergence - so you might need to do a few goes at it as you home in on a set of parameters which give an accurate solution. aero_head likes this.

March 12, 2013, 06:23
#7
Super Moderator

Alex
Join Date: Jun 2012
Location: Germany
Posts: 3,400
Rep Power: 47
The data sampling has to be activated before starting the simulation.
I actually dont know how this is done in CFX, but the manual surely does.
From my experience with data sampling in Fluent, I anticipate this feature to be quite buggy, so dont get disappointed too fast.

Quote:
 How valid are time averaged results of a problem which is very transient
Since there are several types of unsteadyness, the question cannot be answered in general.
For transient results that are statistically steady (time-constant mean value), time-averaging makes sense.
In your case, since you are using time-averaged equations (RANS) in an unsteady manner, time-averaging as a post-processing step is, lets say disputable.
Someone correct me if I'm wrong, but the concept of using URANS-methods for solving turbulent flow with steady boundary conditions is of questionable validity.

 March 12, 2013, 06:27 #8 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,729 Rep Power: 143 Well, lets determine whether the simulation is laminar or turbulent before you go too far. What is the Rayleigh number? Dos the literature say this Ra number should be laminar or turbulent for this configuration?

March 12, 2013, 06:34
#9
Senior Member

Mr CFD
Join Date: Jun 2012
Location: Britain
Posts: 361
Rep Power: 14
Quote:
 Originally Posted by flotus1 The data sampling has to be activated before starting the simulation. I actually dont know how this is done in CFX, but the manual surely does.
If I am not mistaken in CFX output control you just need to select transient statistics, and select which variables you want to monitor.

Quote:
 Originally Posted by ghorrocks Well, lets determine whether the simulation is laminar or turbulent before you go too far. What is the Rayleigh number? Dos the literature say this Ra number should be laminar or turbulent for this configuration?
Thanks for your reply. Based on a quick "back of the envelope" calculation the Rayleigh number is in the order of 9 E +7 (90000000).

Incropera and Dewitt suggest a laminar regime between 10^4 and 10^7. And a turbulent regime between 10^7 and 10^11.

The reason I'm doing a 2D simulation is purely because I have done some heat transfer calculations estimating the surface temperatures which are based on some empirical correlations (which agree to within 10% of data). I don't expect CFD and my calculations to agree bang on, but I don't expect them to disagree by a huge amount either.

You mentioned a "baseline simulation". I'm sorry it's the first time I've heard this term - what is it?

I appreciate the mesh resolution will have an effect on the Courant number and hence the timestep.

March 12, 2013, 09:02
#11
Senior Member

Mr CFD
Join Date: Jun 2012
Location: Britain
Posts: 361
Rep Power: 14
Quote:
 Originally Posted by oj.bulmer If I may ask, why choose a 2D case over axisymemtric; given the latter is more relevant to the cylindrical tank? You should be careful here since buoyant convection flows may be unphysically sensitive to turbulence in case of 2D/axisymmetric cases. Some literature search may help here. Though, given Ra no., is it fair to say the solution is partly transitional?
Hi OJ! The solution is physically non-symmetrical. At this stage I want to see what's going on in the planer dimensions. I.e. 2D axisymmetric will give a worse prediction compared to a regular 2D simulation (assuming one is interested in the physics in the planer direction).

Quote:
 Originally Posted by oj.bulmer Your plots don't indicate anything about the imbalances. Plot of 3 timesteps (including coefficient loop values) should shed some light on convergence of each timestep more clearly, rather than 100 upwards timesteps as you show now. Convergence of every timestep is essential and will bring more credibility to your time-averaged results.
Sure thing - in many respects CFX should have the "Monitor coefficient loop convergence" set to "on" by default when doing transient simulations.

Quote:
I'll do a few more simulations based on the advice here, and I'll let you know how I get on.

 March 27, 2020, 05:21 Time step #12 New Member   Basil Varghese Join Date: Feb 2020 Posts: 3 Rep Power: 6 Is it possible to give time step size as 500, no. of time steps=20,no.of iterations per time step =50 While doing natural convection in heat sink, where this heat sink is enclosed in a domain

 March 27, 2020, 17:24 #13 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,729 Rep Power: 143 You can set those values to anything you like. But whether it is a good idea (or will converge efficiently) is another matter. The general recommendation is adaptive time steps homing in on 3-5 coeff loops per iteration, with 10 max its per time step and no minimum. Also, in future, for a new question start a new thread. BasilVarghese likes this. __________________ Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.

 Tags buoyant, cfx, convection, heat, transient