Result dependance on Iterations per Time Step, URANS 2D cylinder.

Leonardo.flores · April 25, 2018, 15:45

Hello,

I am performing a mesh independence of a 2d Cylinder, kw SST model, Reynolds related to cylinder= 1.4e5 and Y+=0.9. And have this problem when increase iterations per time step, from 20 ( suggested by fluent) to 50, 70 or 100 my results change dramatically.
iterations per ts.png

My CourantFL is 0.3, and time step = 0.0001.

Solution methods are: PISO, Pressure PRESTO!, momentum, turbulent kinetic energy and specific dissipation rate are 2d Order upwind. And Transient formulation Second Order Implicit.

The problem I think is the continuity residuals... they stay very high.... and solution doesnt converge in every timestep because of it.

I say high because some papers consider converged when reach 1e-6... and I am getting 1e-4 with 100 iterations!

residuals.png

What would you do?

Thank you for reading.

Leonardo.flores · April 26, 2018, 02:53

All right. So I found my mistake.

Was a big mistake: my Courant number was 300, not 0.3. And because of that, my time step was way too big.

So to keep a CFL=1 my time step has to be 3e-07. And that is too small... will take weeks to calculate.

Now I am considering CFL = 30, time step = 1e-05. Need 8 iterations to converge and everything seems good.

Any comentary would be great. Thanks.

LuckyTran · April 26, 2018, 03:01

When you used PISO, did you set all your underrelaxation factors to 1?

Don't do PISO with too many iterations (it defeats the point of PISO) and don't use PISO with large time-steps (it's unstable unless you lower the urf's, but this again defeats the point of PISO). For large time-steps & when you want to take many iterations anyway, use SIMPLE or the COUPLED solver.

Leonardo.flores · April 26, 2018, 03:12

Hello LuckyTran, I am keeping under relaxation Factors as default... I saw some people change pressure under relaxation from 0.3 to 0.7. But I am afraid of it since I will use CFL = 30 (I dont know if you could read my last reply, I found my mistake calculating the CFL).

I only knew PISO was good for unsteady simulations, thank you for the advice about the number of iterations. Right now I solved my problem and have about 8-10 iterations per time step.

LuckyTran · April 26, 2018, 03:50

8-10 iterations per time-step is in general not bad, but I think you have some have room for improvement. The way you are using PISO is SIMPLE-like approach and that's why I suggest to use SIMPLE.

PISO is SIMPLE with an extra correction step at the end. That's why it's better to go with SIMPLE if you plan to do many iterations. You don't need to waste these extra correctors. Remember, SIMPLE and PISO are cousins! One iteration of PISO is almost like 2 iterations of SIMPLE, but in PISO you don't update the outer solution until you do the 2nd corrector.

It's preferable to go with the fewest number of iterations (1 or 2, 3 for highly complex cases), with largest urf's, and largest time-step that PISO can still converge with (this is the Courant number < 1 regime) or switch to SIMPLE, use urf's and also largest time-step without diverging.

Leonardo.flores · April 26, 2018, 04:59

Thanks! I actually do want to have larger time-steps, or the simulations will never end! (have only 8 cores). So, I will try the following: Higher Time step=1e-4, SIMPLE, pressure urf 0.7. But courant number would be about 300. I am trying this with a coarse mesh and hope it doesnt diverge. By now I am getting about 7-8 iterations per time step with this configuration

. Will try with finer meshes and post a reply.

Btw, do you know any literature reference or paper recommended about this?

LuckyTran · April 26, 2018, 10:46

If using SIMPLE, I would have kept the 0.3 and 0.7 urf's for pressure and momentum. Or I would change it to 0.5, 0.5.

With a finer mesh, your time-step would have to be even smaller and overall simulation time goes up even more (due to needing more time-steps and having a bigger mesh). Either buckle down for a long simulation or give up. This is why it's even more important to play with your case and learn how it responds when your first set it up.

You can find SIMPLE/PISO algorithm even on wikipedia these days. "Anyone can become a scientist if they know what to search for."

PISO Usage and URF's in Fluent Manual
PISO explanation in Fluent Manual
Merged PISO/SIMPLE in OpenFOAM

Leonardo.flores · May 15, 2018, 22:14

Well, I finally could get some coherent results with 6 grids, from coarse to "fine".
Smallest Courant I could handle is 30. I actually kept SIMPLE method and 0.3 and 0.7 urf for P. and M. (higher values for P. urf gave me problems with finer meshes).

By now I am trying to find a method so I could get stabilized results faster. So I start with a steady simulation, then set high time steps (Courant = 3000), and making it smaller until get stabilized values with a small time step (Courant=30). And I am getting about 15 iterations per time step... and I think this is ok. Results very close to similar studies.

Thank you for your advice LuckyTran.

April 25, 2018, 15:45	Result dependance on Iterations per Time Step, URANS 2D cylinder.	#1
Leonardo.flores Member Leonardo Join Date: Nov 2017 Posts: 37 Rep Power: 9	Hello, I am performing a mesh independence of a 2d Cylinder, kw SST model, Reynolds related to cylinder= 1.4e5 and Y+=0.9. And have this problem when increase iterations per time step, from 20 ( suggested by fluent) to 50, 70 or 100 my results change dramatically. iterations per ts.png My CourantFL is 0.3, and time step = 0.0001. Solution methods are: PISO, Pressure PRESTO!, momentum, turbulent kinetic energy and specific dissipation rate are 2d Order upwind. And Transient formulation Second Order Implicit. The problem I think is the continuity residuals... they stay very high.... and solution doesnt converge in every timestep because of it. I say high because some papers consider converged when reach 1e-6... and I am getting 1e-4 with 100 iterations! residuals.png What would you do? Thank you for reading.

April 26, 2018, 03:50		#5
LuckyTran Senior Member Lucky Join Date: Apr 2011 Location: Orlando, FL USA Posts: 5,761 Rep Power: 66	8-10 iterations per time-step is in general not bad, but I think you have some have room for improvement. The way you are using PISO is SIMPLE-like approach and that's why I suggest to use SIMPLE. PISO is SIMPLE with an extra correction step at the end. That's why it's better to go with SIMPLE if you plan to do many iterations. You don't need to waste these extra correctors. Remember, SIMPLE and PISO are cousins! One iteration of PISO is almost like 2 iterations of SIMPLE, but in PISO you don't update the outer solution until you do the 2nd corrector. It's preferable to go with the fewest number of iterations (1 or 2, 3 for highly complex cases), with largest urf's, and largest time-step that PISO can still converge with (this is the Courant number < 1 regime) or switch to SIMPLE, use urf's and also largest time-step without diverging. Last edited by LuckyTran; May 16, 2018 at 00:07.

April 26, 2018, 10:46		#7
LuckyTran Senior Member Lucky Join Date: Apr 2011 Location: Orlando, FL USA Posts: 5,761 Rep Power: 66	If using SIMPLE, I would have kept the 0.3 and 0.7 urf's for pressure and momentum. Or I would change it to 0.5, 0.5. With a finer mesh, your time-step would have to be even smaller and overall simulation time goes up even more (due to needing more time-steps and having a bigger mesh). Either buckle down for a long simulation or give up. This is why it's even more important to play with your case and learn how it responds when your first set it up. You can find SIMPLE/PISO algorithm even on wikipedia these days. "Anyone can become a scientist if they know what to search for." PISO Usage and URF's in Fluent Manual PISO explanation in Fluent Manual Merged PISO/SIMPLE in OpenFOAM Last edited by LuckyTran; April 26, 2018 at 15:06.

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
Segmentation fault when using reactingFOAM for Fluids	Tommy Floessner	OpenFOAM Running, Solving & CFD	4	April 22, 2018 13:30
simpleFoam error - "Floating point exception"	mbcx4jc2	OpenFOAM Running, Solving & CFD	12	August 4, 2015 03:20
Compressor Simulation using rhoPimpleDyMFoam	Jetfire	OpenFOAM Running, Solving & CFD	107	December 9, 2014 14:38
calculation stops after few time steps	sivakumar	OpenFOAM Running, Solving & CFD	7	March 17, 2013 07:37
pisoFoam with k-epsilon turb blows up - Some questions	Heroic	OpenFOAM Running, Solving & CFD	26	December 17, 2012 04:34

April 26, 2018, 02:53		#2
Leonardo.flores Member Leonardo Join Date: Nov 2017 Posts: 37 Rep Power: 9	All right. So I found my mistake. Was a big mistake: my Courant number was 300, not 0.3. And because of that, my time step was way too big. So to keep a CFL=1 my time step has to be 3e-07. And that is too small... will take weeks to calculate. Now I am considering CFL = 30, time step = 1e-05. Need 8 iterations to converge and everything seems good. Any comentary would be great. Thanks.

April 26, 2018, 03:01		#3
LuckyTran Senior Member Lucky Join Date: Apr 2011 Location: Orlando, FL USA Posts: 5,761 Rep Power: 66	When you used PISO, did you set all your underrelaxation factors to 1? Don't do PISO with too many iterations (it defeats the point of PISO) and don't use PISO with large time-steps (it's unstable unless you lower the urf's, but this again defeats the point of PISO). For large time-steps & when you want to take many iterations anyway, use SIMPLE or the COUPLED solver.

April 26, 2018, 03:12		#4
Leonardo.flores Member Leonardo Join Date: Nov 2017 Posts: 37 Rep Power: 9	Hello LuckyTran, I am keeping under relaxation Factors as default... I saw some people change pressure under relaxation from 0.3 to 0.7. But I am afraid of it since I will use CFL = 30 (I dont know if you could read my last reply, I found my mistake calculating the CFL). I only knew PISO was good for unsteady simulations, thank you for the advice about the number of iterations. Right now I solved my problem and have about 8-10 iterations per time step.

April 26, 2018, 04:59		#6
Leonardo.flores Member Leonardo Join Date: Nov 2017 Posts: 37 Rep Power: 9	Thanks! I actually do want to have larger time-steps, or the simulations will never end! (have only 8 cores). So, I will try the following: Higher Time step=1e-4, SIMPLE, pressure urf 0.7. But courant number would be about 300. I am trying this with a coarse mesh and hope it doesnt diverge. By now I am getting about 7-8 iterations per time step with this configuration . Will try with finer meshes and post a reply. Btw, do you know any literature reference or paper recommended about this?

May 15, 2018, 22:14		#8
Leonardo.flores Member Leonardo Join Date: Nov 2017 Posts: 37 Rep Power: 9	Well, I finally could get some coherent results with 6 grids, from coarse to "fine". Smallest Courant I could handle is 30. I actually kept SIMPLE method and 0.3 and 0.7 urf for P. and M. (higher values for P. urf gave me problems with finer meshes). By now I am trying to find a method so I could get stabilized results faster. So I start with a steady simulation, then set high time steps (Courant = 3000), and making it smaller until get stabilized values with a small time step (Courant=30). And I am getting about 15 iterations per time step... and I think this is ok. Results very close to similar studies. Thank you for your advice LuckyTran.