Initializing turbulence flow with '0' k and epsilon

SRKR · July 17, 2018, 02:52

Hello all, I am simulating a flow process in which bubble is initially at rest at bottom of a liquid container. As the bubble raises up turbulence will be produced something called 'Bubble induced turbulence' but initially since everything is in static condition turbulence will be '0'. So, in order to account for turbulence as bubble moves i am using 'Standard k-epsilon' turbulence model. But, the problem is I am unable to initiate the simulation with initial values of both 'k' and 'epsilon' as '0', solver is terminating in between calculation of 1st time step. Can some one please help me, How to initialize the simulation with '0' turbulence.
Thank you in advance.

simrego · July 17, 2018, 03:30

They cannot be zero. If they are zero, you will try to divide with zero, and the solver blows up.
set to a really small value for example 1e-10 or less.

SRKR · July 17, 2018, 04:28

Quote:

Originally Posted by simrego

They cannot be zero. If they are zero, you will try to divide with zero, and the solver blows up.
set to a really small value for example 1e-10 or less.

Ya, you are correct. Got it. Thank you

SRKR · July 20, 2018, 02:39

Quote:

Originally Posted by simrego

They cannot be zero. If they are zero, you will try to divide with zero, and the solver blows up.
set to a really small value for example 1e-10 or less.

Hello Simrego, as discussed previously to give values of k and epsilon to a v.small value, I have been trying to do that but, with such low values I am getting error as "Floating point exception (core dumped)". Can you please explain about that and how to fix it.
Thank you.

simrego · July 20, 2018, 03:24

Hi!

There can be a lot of reason for that. Mesh? Maybe your initial or boundary conditions are not correct physically, etc..
Post the end of your log where you got the error and maybe someone can help you, but this is much less information than needed.

SRKR · July 20, 2018, 11:21

Quote:

Originally Posted by simrego

Hi!

There can be a lot of reason for that. Mesh? Maybe your initial or boundary conditions are not correct physically, etc..
Post the end of your log where you got the error and maybe someone can help you, but this is much less information than needed.

That's the image and I got this error only when I have very low 'k' and 'epsilon' values like '0.001'. So, I am thinking it's because of floating point limit. Is that the reason if so, how to set it.
Thank you.
https://drive.google.com/file/d/1_mB...ew?usp=sharing

simrego · July 20, 2018, 13:04

Post the image as an attachment or just copy-paste the text. We can't read this small image.

SRKR · July 20, 2018, 13:42

Quote:

Originally Posted by simrego

Post the image as an attachment or just copy-paste the text. We can't read this small image.

https://drive.google.com/file/d/1_mB...ew?usp=sharing
I think.. this image will be clear for you...

simrego · July 20, 2018, 14:07

Sorry! Didn't saw the link.

Yea, it is comes from the kepsilon::correct() function where maybe you try to divide with zero.
How much iteration can you do before crash?
I'm not an expert in it but if you sure your boundary and initial conditions are fine you could try to tune your fvSolution a bit or try with first order schemes.
Maybe some expert read this post and can help you, because at this point all i can is give you hints but no correct answer.

SRKR · July 20, 2018, 14:11

Quote:

Originally Posted by simrego

Sorry! Didn't saw the link.

Yea, it is comes from the kepsilon::correct() function where maybe you try to divide with zero.
How much iteration can you do before crash?
I'm not an expert in it but if you sure your boundary and initial conditions are fine you could try to tune your fvSolution a bit or try with first order schemes.
Maybe some expert read this post and can help you, because at this point all i can is give you hints but no correct answer.

Yeah, thank you so much for responding. I got the error in the first time step itself. Hope someone can help me with this.

pete20r2 · July 21, 2018, 20:38

Can you post the case files? I'll give it a go if you want

SRKR · July 22, 2018, 14:57

Quote:

Originally Posted by pete20r2

Can you post the case files? I'll give it a go if you want

https://drive.google.com/file/d/1Xgy...ew?usp=sharing
That's one of the sample case file zipped, with similar conditions. If you like to try you can try with that and please inform me back if you find anything useful.
Thank you.

pete20r2 · July 23, 2018, 21:39

Quote:

Originally Posted by SRKR

https://drive.google.com/file/d/1Xgy...ew?usp=sharing
That's one of the sample case file zipped, with similar conditions. If you like to try you can try with that and please inform me back if you find anything useful.
Thank you.

Hi,
I got it running, link is at the bottom of the post.
I changed a few things:
k IV reduced to 1e-10
epsilon IV reduced to 1e-10
p_rgh wall changed to zeroGradient (not sure if this is better, it's what I'm used to)
Initial deltaT lowered to 0.0001 (I think this was the big one)
maxCo and maxAlphaCo increased to 0.5 (for speed)

increased the tolerance and relTol on most of the solvers to 1e-6 and 1e-3 respectively. (for speed) (you can lower these to your own spec again)

I've left some extra files in there:
U.ogv: U field up to 1 second (I only have an i5 760)
splitRun: might need to make this script executable once you extract, run

Code:

decomposePar
./splitRun

then in a new terminal you can show residuals
DecomposeParDict is in system, you can read about it if you've never used it.
Use reconstructPar after the run to put all the results back together.
residuals: run

Code:

gnuplot residuals

to monitor the residuals

Trial.zip converging

SRKR · August 2, 2018, 01:31

Yup, I got it... It's only with deltaT. Lowering the value of time step I got it running. But, I got another interesting but bad way i.e. with the same time step but decreasing the write interval also didn't get any error for me and whole simulation is good and result was to the expectations, ofcourse consumed huge memory.
Thank you all for responding.

July 17, 2018, 02:52	Initializing turbulence flow with '0' k and epsilon	#1
SRKR New Member Srikar Reddy Palla Join Date: May 2018 Posts: 19 Rep Power: 7	Hello all, I am simulating a flow process in which bubble is initially at rest at bottom of a liquid container. As the bubble raises up turbulence will be produced something called 'Bubble induced turbulence' but initially since everything is in static condition turbulence will be '0'. So, in order to account for turbulence as bubble moves i am using 'Standard k-epsilon' turbulence model. But, the problem is I am unable to initiate the simulation with initial values of both 'k' and 'epsilon' as '0', solver is terminating in between calculation of 1st time step. Can some one please help me, How to initialize the simulation with '0' turbulence. Thank you in advance.

July 17, 2018, 03:30		#2
simrego Senior Member anonymous Join Date: Jan 2016 Posts: 416 Rep Power: 14	They cannot be zero. If they are zero, you will try to divide with zero, and the solver blows up. set to a really small value for example 1e-10 or less. SRKR likes this.

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
SimpleFoam k and epsilon bounded	nedved	OpenFOAM Running, Solving & CFD	16	March 4, 2017 08:30
parallel code	samiam1000	SU2	3	March 25, 2013 04:55
K - epsilon VS SST turbulence model	Maicol	Main CFD Forum	0	November 30, 2012 16:25
Orifice Plate with a fully developed flow - Problems with convergence	jonmec	OpenFOAM Running, Solving & CFD	3	July 28, 2011 05:24
SimpleFoam k and epsilon bounded	nedved	OpenFOAM Running, Solving & CFD	1	November 25, 2008 20:21

July 20, 2018, 03:24		#5
simrego Senior Member anonymous Join Date: Jan 2016 Posts: 416 Rep Power: 14	Hi! There can be a lot of reason for that. Mesh? Maybe your initial or boundary conditions are not correct physically, etc.. Post the end of your log where you got the error and maybe someone can help you, but this is much less information than needed.

July 20, 2018, 13:04		#7
simrego Senior Member anonymous Join Date: Jan 2016 Posts: 416 Rep Power: 14	Post the image as an attachment or just copy-paste the text. We can't read this small image.

July 20, 2018, 14:07		#9
simrego Senior Member anonymous Join Date: Jan 2016 Posts: 416 Rep Power: 14	Sorry! Didn't saw the link. Yea, it is comes from the kepsilon::correct() function where maybe you try to divide with zero. How much iteration can you do before crash? I'm not an expert in it but if you sure your boundary and initial conditions are fine you could try to tune your fvSolution a bit or try with first order schemes. Maybe some expert read this post and can help you, because at this point all i can is give you hints but no correct answer.

July 21, 2018, 20:38		#11
pete20r2 Senior Member Peter Baskovich Join Date: Jul 2014 Posts: 127 Rep Power: 11	Can you post the case files? I'll give it a go if you want

August 2, 2018, 01:31		#14
SRKR New Member Srikar Reddy Palla Join Date: May 2018 Posts: 19 Rep Power: 7	Yup, I got it... It's only with deltaT. Lowering the value of time step I got it running. But, I got another interesting but bad way i.e. with the same time step but decreasing the write interval also didn't get any error for me and whole simulation is good and result was to the expectations, ofcourse consumed huge memory. Thank you all for responding.