CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > General Forums > Main CFD Forum

SIMPLE method small time step

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   June 29, 2016, 07:20
Default SIMPLE method small time step
  #1
New Member
 
DSR
Join Date: Sep 2014
Posts: 11
Rep Power: 8
dsr_cfd is on a distinguished road
Hi, I have created a CFD code following the SIMPLE method. It is a co-located grid and uses Rhie-Chow interpolation. The problem is, I need to take rediculously small time steps for it to be stable.

Has anyone ever had this issue? Fixes?

Any response will be much appreciated!
dsr_cfd is offline   Reply With Quote

Old   June 29, 2016, 09:18
Default
  #2
Senior Member
 
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 5,688
Rep Power: 60
FMDenaro has a spectacular aura aboutFMDenaro has a spectacular aura aboutFMDenaro has a spectacular aura about
Quote:
Originally Posted by dsr_cfd View Post
Hi, I have created a CFD code following the SIMPLE method. It is a co-located grid and uses Rhie-Chow interpolation. The problem is, I need to take rediculously small time steps for it to be stable.

Has anyone ever had this issue? Fixes?

Any response will be much appreciated!
what discretization are you using in time? first order explicit? How about the Re_h?
FMDenaro is offline   Reply With Quote

Old   June 29, 2016, 09:45
Default
  #3
New Member
 
DSR
Join Date: Sep 2014
Posts: 11
Rep Power: 8
dsr_cfd is on a distinguished road
First order implicit. I've tried with multiple Re, but it seems the time step is always limited by a CFL of 1.0. Which seems very low for an implicit solver.
dsr_cfd is offline   Reply With Quote

Old   June 29, 2016, 21:33
Default
  #4
Senior Member
 
Arjun
Join Date: Mar 2009
Location: Nurenberg, Germany
Posts: 980
Rep Power: 25
arjun will become famous soon enough
Quote:
Originally Posted by dsr_cfd View Post
Hi, I have created a CFD code following the SIMPLE method. It is a co-located grid and uses Rhie-Chow interpolation. The problem is, I need to take rediculously small time steps for it to be stable.

Has anyone ever had this issue? Fixes?

Any response will be much appreciated!

Your program has a bug and it could be anywhere. Instablity in cfd solver could creep in from anything from small to big.

It is not possible to point out bug from your information.
arjun is offline   Reply With Quote

Old   June 30, 2016, 07:30
Default
  #5
New Member
 
DSR
Join Date: Sep 2014
Posts: 11
Rep Power: 8
dsr_cfd is on a distinguished road
But is it safe to say that there is definitely a bug? That I should be able to run with much higher time steps?
dsr_cfd is offline   Reply With Quote

Old   June 30, 2016, 08:05
Default
  #6
Senior Member
 
flotus1's Avatar
 
Alex
Join Date: Jun 2012
Location: Germany
Posts: 2,731
Rep Power: 38
flotus1 has a spectacular aura aboutflotus1 has a spectacular aura about
Quote:
First order implicit. I've tried with multiple Re, but it seems the time step is always limited by a CFL of 1.0
With his kind of behavior, the first place to look for the error is your implementation of the temporal discretization.
flotus1 is offline   Reply With Quote

Old   June 30, 2016, 08:43
Default
  #7
New Member
 
DSR
Join Date: Sep 2014
Posts: 11
Rep Power: 8
dsr_cfd is on a distinguished road
Could it be related to the rhie chow or pressure correction methods which both use the coefficient value from momentum (which depends on the time step)? Or any other suggestions? My temporal discretization method comes straight from the Versteeg textbook.
dsr_cfd is offline   Reply With Quote

Old   July 1, 2016, 21:30
Default
  #8
Senior Member
 
Michael Prinkey
Join Date: Mar 2009
Location: Pittsburgh PA
Posts: 363
Rep Power: 22
mprinkey will become famous soon enough
What is the nature of the instability? flow variables going to infinity? If so, which one starts it? Or do linear systems fail to converge? If so, which field? Or does the nonlinear iteration fail to converge?
mprinkey is offline   Reply With Quote

Old   July 4, 2016, 06:44
Default
  #9
New Member
 
DSR
Join Date: Sep 2014
Posts: 11
Rep Power: 8
dsr_cfd is on a distinguished road
The pressure correction equation goes unstable first. If I just do heat conduction, I can use a large time step. The instability seems to occur during velocity-pressure coupling.
dsr_cfd is offline   Reply With Quote

Old   July 4, 2016, 06:58
Default
  #10
Senior Member
 
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 5,688
Rep Power: 60
FMDenaro has a spectacular aura aboutFMDenaro has a spectacular aura aboutFMDenaro has a spectacular aura about
Quote:
Originally Posted by dsr_cfd View Post
The pressure correction equation goes unstable first. If I just do heat conduction, I can use a large time step. The instability seems to occur during velocity-pressure coupling.

just check after one time step if your pressure solution appears regular and if the gradients added to the partial velocity field satisfy the continyuity equation.
FMDenaro is offline   Reply With Quote

Old   July 4, 2016, 07:08
Default
  #11
New Member
 
DSR
Join Date: Sep 2014
Posts: 11
Rep Power: 8
dsr_cfd is on a distinguished road
If my time step is too big (not really even that big), my pressure correction equation diverges (first time step, first loop).
dsr_cfd is offline   Reply With Quote

Old   July 4, 2016, 09:11
Default
  #12
Senior Member
 
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 5,688
Rep Power: 60
FMDenaro has a spectacular aura aboutFMDenaro has a spectacular aura aboutFMDenaro has a spectacular aura about
Quote:
Originally Posted by dsr_cfd View Post
If my time step is too big (not really even that big), my pressure correction equation diverges (first time step, first loop).

that demonstrates you have some bugs in the code..check the BC.s for the pressure
FMDenaro is offline   Reply With Quote

Old   July 4, 2016, 09:53
Default
  #13
New Member
 
DSR
Join Date: Sep 2014
Posts: 11
Rep Power: 8
dsr_cfd is on a distinguished road
Ok thanks. What should I expect for time step (based on cell size, velocity, etc.)?
dsr_cfd is offline   Reply With Quote

Old   July 4, 2016, 11:13
Default
  #14
Senior Member
 
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 5,688
Rep Power: 60
FMDenaro has a spectacular aura aboutFMDenaro has a spectacular aura aboutFMDenaro has a spectacular aura about
Quote:
Originally Posted by dsr_cfd View Post
Ok thanks. What should I expect for time step (based on cell size, velocity, etc.)?

After a single time step do you satisfy the continuity equation?
FMDenaro is offline   Reply With Quote

Old   July 4, 2016, 23:54
Default
  #15
Senior Member
 
Michael Prinkey
Join Date: Mar 2009
Location: Pittsburgh PA
Posts: 363
Rep Power: 22
mprinkey will become famous soon enough
If you are using the SIMPLE method, then the algorithm is completely implicit and (in principle) there is no timestep limit. In fact, taking the limit of dt->inf should lead you to the normal steady SIMPLE formulation. This, of course, assumes that the SIMPLE algorithm (outer iterations) converge at each timestep.

I am aware of no theory...or even heuristic...that gives time-step guidance with regard to the convergence of SIMPLE. There are requirements on pressure and velocity underrelaxation factors for the steady state case under assumptions of simple models...no reactions, no buoyancy, etc.

I agree with the others advice. Verify that the face fluxes after pressure correction application results in conservation of mass. If that is not true both globally and in every cell, then your first problem to solve is there. There may be other bugs, but you will not be able to check because the fluxes driving the convection of other properties will be garbage.

And remember that because this is colocated, the cell values of velocity are (almost) irrelevant. The face fluxes are the primary metric with regard to pressure correction and mass conservation.
mprinkey is offline   Reply With Quote

Reply

Tags
cfd, rhie-chow, simple, time step

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
AMI speed performance danny123 OpenFOAM 21 October 24, 2020 04:13
Stuck in a Rut- interDyMFoam! xoitx OpenFOAM Running, Solving & CFD 14 March 25, 2016 07:09
[Other] Contribution a new utility: refine wall layer mesh based on yPlus field lakeat OpenFOAM Community Contributions 57 February 1, 2015 08:25
How to write k and epsilon before the abnormal end xiuying OpenFOAM Running, Solving & CFD 8 August 27, 2013 15:33
pisoFoam with k-epsilon turb blows up - Some questions Heroic OpenFOAM Running, Solving & CFD 26 December 17, 2012 03:34


All times are GMT -4. The time now is 14:56.