
[Sponsors] 
Simulating a steadystate/laminar/incompressible/newtonian flow 

LinkBack  Thread Tools  Search this Thread  Display Modes 
March 6, 2019, 11:23 
Simulating a steadystate/laminar/incompressible/newtonian flow

#1 
New Member
Estelle
Join Date: Mar 2019
Posts: 10
Rep Power: 3 
Hello everyone,
I am totally new on OpenFoam. I practiced on tutorials and thanks to some videos/forums. Nevertheless I am facing a problem: Which solver do I have to use to simulate a steadystate, laminar, incompressible, newtonian flow? Thanks, Estelle 

March 6, 2019, 11:29 

#2 
Senior Member
Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 4,041
Rep Power: 49 
simpleFoam works. Probably there's even simpler ones that also work.


March 7, 2019, 11:11 

#3 
New Member
Estelle
Join Date: Mar 2019
Posts: 10
Rep Power: 3 
Yes you're right. I made it work today, I juste changed the turbulenceProperties file to a laminar simulationType ans it has been ok.
I would like to make the transient form work too (icoFoam) ! Until now it does not. 

March 7, 2019, 16:01 

#4 
Senior Member
Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 4,041
Rep Power: 49 
if you don't have any luck with icoFoam, the transient version of simpleFoam is pimpleFoam (merged pisosimple algorithm) or pisoFoam.


March 8, 2019, 04:29 

#5 
Member
VS
Join Date: Nov 2012
Posts: 86
Rep Power: 10 
pimple,piso and icoFoam are good candidates for what you want to do. Try to give some more details on why icoFoam is not working for your case. Solving basic issues in this early stage will give you more than just changing solvers.


March 11, 2019, 06:07 
icoFoam simulation  Poiseuille cylinder

#6 
New Member
Estelle
Join Date: Mar 2019
Posts: 10
Rep Power: 3 
Hello,
I managed to use simpleFoam for my simulations in steadystate! The problem now is for the transient part of my study. As I am a very beginner I tried to use both pimpleFoam, pisoFoam (lam,LES or RAS) but it instantly crashes each time, and I still do not succeed in using icoFoam. Here's a very simple case I tried to make run with icoFoam: a cylinder with D=1e04m and L=7e03m for a Poiseuille flow (nu = 5e05 mē/s) with the condition deltaP=30bars between the inlet and the outlet. The maximum velocity should be 5.36m/s when it converges. I joined the files P/U/transportProperties/blockMeshDict/controlDict. Help :') Thanks for your answers, Estelle 

March 11, 2019, 11:38 

#7 
Senior Member
Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 4,041
Rep Power: 49 
See if you can dig out the Courant number from the log. It's probably stupidly high.
try a very small deltaT, like 1e06 s. What's the ddtScheme setting in fvSchemes dict? Euler hopefully? What's your fvSolution dict? Also try the dam break tutorial or pitzdaily tutorial for some hints. 

March 11, 2019, 11:56 

#8 
New Member
Estelle
Join Date: Mar 2019
Posts: 10
Rep Power: 3 
Here are the fvSchemes and fvSolution files,.
Is not it what I am doing by setting the "endTime" to 10e+6 and "deltaT" to 1 in controlDict? It is the same than putting respectively 1 and 10e6, no? Yes, it is Euler for ddt. I already did these tutorials. the problem is that I am not working with the same scales at all. My conduct is 105 meters large and my fluid is oil =/ so I have results very different from the tutos. 

March 12, 2019, 10:01 

#9  
Senior Member
Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 4,041
Rep Power: 49 
Quote:
Large deltaT is numerically unstable, especially if you are using piso. Your maximum Courant number needs to be around 1ish for PISO to be stable. If it exceeds 1 by too much (i.e. 2 or 3) it will blow up. The Courant number prints at the beginning of the timestep, but since you initialized with 0 velocity everywhere it won't be helpful until you can get some timesteps in. That's why I suggest to use a stupidly small deltaT to see if you can make it past 1 timestep without it crashing immediately. 

March 12, 2019, 10:57 

#10 
New Member
Estelle
Join Date: Mar 2019
Posts: 10
Rep Power: 3 
Thanks ! Yes of course I understand now... I did it and the calculation runs longer but still it crashes...
My last cylinder test: D = 0.001m L = 0.07m nu = 0.00005 mē/s deltaP = 3 bars deltaT = 1e6s Re = 0.268 I really do not understand why ! 

March 12, 2019, 12:14 

#11  
Senior Member
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 5,501
Rep Power: 58 
Quote:
How do you estimate that Re=O(10^1)? The deltaP seems to high to produce such a low velocity 

March 13, 2019, 04:45 

#12 
New Member
Estelle
Join Date: Mar 2019
Posts: 10
Rep Power: 3 
You're right, I corrected it and got Re = 53.6.
I use Darcy formula to get the average velocit: U = deltap*Dē / (32* nu * rho * L) In this case, I get U = 2.68 m/s. Then, Re = U*D / nu. 

March 13, 2019, 11:46 

#13 
Senior Member
Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 4,041
Rep Power: 49 
Okay not crashing immediately. That's progress!
In your U dict try: Code:
instead of internalField uniform (0 0 0); Code:
internalField uniform (2.68 0 0); Another idea is to not use internalField uniform 0 for the initial condition of pressure. You can specify a linear profile but that requires using a tool like funkySetFields from swak4Foam. Have you tried a very small driving pressure? I.e. 3 Pa instead of 3000000? Also..... Courant number!?!?!?!?!?!?!?!? 

March 13, 2019, 12:09 

#14 
New Member
Estelle
Join Date: Mar 2019
Posts: 10
Rep Power: 3 
Well, I have to check that I get U=2.68m/s at the end of the transient time, for a 30bars deltap! So I will not change my initial conditions.
I just have to check that my simulations suits to the theory. I will have to build a real prototype with deltap = 30bars. I calculated that Umax = 2.68 m/s but I want my simulations to prove it. Yes, the case is running for very small delta p, also for bigger dimensions, and for more viscous fluids, equivalent Reynolds numbers. This is very frustrating. If I increase deltap, decrease dimensions or viscosity... Courant number explodes quite fast. My last try:  D = 1mm  L = 70 mm  deltap = 3 bars  nu = 5e5 mē/s Is running, has to reach U = 5.36 m/s. It took 5h to reach 2.7 m/s... So I am waiting. I managed to get my calculation running longer thanks to a finer mesh on the sides of the duct. 

March 13, 2019, 13:35 

#15  
Senior Member
Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 4,041
Rep Power: 49 
Quote:
You have an initial condition of 0 velocity and 0 pressure. And then suddenly impose 30 bar at the inlet. That's practically a blast wave. Quote:
Btw you can get away with slightly larger deltaT using pimpleFoam instead of pisoFoam. But if you don't get how piso works, then I don't recommend to switch to pimple. 

March 18, 2019, 09:06 

#16 
New Member
Estelle
Join Date: Mar 2019
Posts: 10
Rep Power: 3 
I managed to get the results by refining a lot on the sides of the duct.
Well yes, it is like a very huge pressure wave. And I wanted to study what happens when putting a so big pressure at once, so in transient. And how much time does that take to get steady Thanks for your help 

Tags 
incompressible, laminar, newtonian, steadystate 
Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
About Some Concepts:Laminar flow, turbulent flow, steady flow and timedependent flow  Jing  Main CFD Forum  8  October 5, 2018 18:02 
How does Fluent works in DPM, with steady flow and unsteady particle tracking ?  pkp  FLUENT  2  March 30, 2016 18:38 
Unsteady DPM / Steady Flow  Jultou  FLUENT  2  December 3, 2015 05:51 
Unable to achieve a steady flow  lost.identity  Main CFD Forum  1  April 29, 2009 11:22 
Inviscid Drag at subsonic, subcritical Mach #  Axel Rohde  Main CFD Forum  1  November 19, 2001 13:19 