CFD Online Logo CFD Online URL
Home > Forums > Software User Forums > Siemens > STAR-CCM+

why is k-epsilon working better for me?

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

LinkBack Thread Tools Search this Thread Display Modes
Old   February 2, 2019, 14:50
Smile why is k-epsilon working better for me?
New Member
raviad's Avatar
Adhitya Ravi
Join Date: Feb 2019
Location: Germany
Posts: 2
Rep Power: 0
raviad is on a distinguished road
Hi everyone,

I am new to CFD and I am trying to simulate air flow through a pipe fitted with a pressure compensation element (something like a orifice disc but has a much more complicated design) in StarCCM+. I want to calculate the pressure drop in the pipe flow caused by this pressure compensation element.

The cylinder has a radius of 0.5 m. The velocity at the pipe inlet is very small almost negligible (lets say the volume flow rate is 50 l/h -> velocity ~ 1e-5 m/s).

So, initially I performed a laminar steady state simulation with a 2nd order upwind scheme. I obtained convergence and the pressure drop was close to the measurement (~ 5% error). Then, I increased the inlet volume flow rates in steps of 50 l/h. For inlet volume flow rates between 100 - 300 l/h (300 l/h is the max volume flow rate i tested), I could not obtain convergence with a laminar simulation. The pressure drop oscillates randomly (it gets worse with increasing volume flow rate).

The first thing I tried is a grid independence study. The oscillations were damped a bit when I reduced the mesh size (base size from 100 mm to 70 mm) but not even close to a converged solution. But further reduction in mesh size (base size from 70mm to 60mm) had no effect on the solution. Then I tried reducing my velocity and pressure under-relaxation factor swhich also had no effect on the solution. So, I thought the convergence problem could be because the physics of the flow is not completely captured by a laminar simulation. So, I researched a bit on turbulence models and found that the SST is the go to model especially if the flow is internal and not fully turbulent. But the results of the simulation when I used a SST, the results were not so much different from laminar simulation in terms of convergence. The solution was not converged even after 6000 iterations. Then I tried SST with turbulence suppression on the initial half of the cylinder where the velocity is close to zero. But still the pressure drop was oscillating. And then hesitantly I used realizable k-epsilon for the simulation (I was hesitant because many posts here and various literature indicated that k-epsilon may give garbage result if the flow is not fully turbulent and that it is not recommended for internal flows). To my surprise I got a converged solution for all the volume flow rates with an error of < 2%.

I am happy with this. But, I still want to understand why this happens. I understood that SST is more non linear than k-epsilon and hence it may be more difficult to converge. So I simulated the problem again with SST but this time with 1st order upwind scheme and I got a converged solution. But of course the k-epsilon results with 2nd order convection scheme was better than the SST results. Then I tried a laminar simulation with the 1st order convection and I also got a converged solution. The error in the solution was in the order

Laminar (1st order) > SST (1st order) > Realizable k-epsilon (2nd order)

which is predictable. I could accept the non linearity of SST model as an explanation for why the solution was not converged. But I could not understand why the laminar simulation could not converge. Could someone help me understand this? Is there any particular reason why k-epsilon gives me better results? Also since SST is more sensitive to initial conditions, will I get even better results if I start with k-epsilon and then switch to SST (maintaining a 2nd order convection scheme) Or if I start my simulation with a 1st order SST and then switch to 2nd order SST (I plan to run these simulations)? Should I also run some transient simulations? And should I also try a transition model?

Note: When I say 2nd order or 1st order convection scheme, I mean it for both the flow solver and turbulence equation solver.

I also performed a simulation using standard k-omega model with 1st order convection (2nd order standard k-omega also did not converge) just for the heck of it and found out that the results from standard k-omega and SST k-omega are one and the same. Why is this so?

In case if you are wondering, the there were no bad cells and the cell skewness angle is less than 85 in the mesh. When I plot the y+ value, it is <1 everywhere in the domain.

Thanks in advance.

raviad is offline   Reply With Quote

Old   February 7, 2019, 12:44
Bernhard Stiehl
Join Date: Oct 2018
Posts: 30
Rep Power: 7
cheetthe1 is on a distinguished road
Yes, converged does not mean good. Nothing to do with that. Das müssen auch deutsche verstehen Converged only means that the stuff you give to the model can be calculated. Better believe the turbulence recommendations. I am going through similar situation. Just plot your dissipation rates, you will see they may be too high.
cheetthe1 is offline   Reply With Quote

Old   February 7, 2019, 13:57
New Member
raviad's Avatar
Adhitya Ravi
Join Date: Feb 2019
Location: Germany
Posts: 2
Rep Power: 0
raviad is on a distinguished road
Hi Bernhard,

Thank you for the reply. Yes, you are completely right. It was a naive question . I found out that there is no fully developed turbulence in the flow. But the flow is not completely laminar either. There are a few vortices brought into play by the asymmetrical geometry. The flow is transitional at best. These vortices are the reason behind the oscillating pressure drop.

Hence, using a RANS turbulence model introduces an unphysical viscosity which dampens out the vortices. SST tries to reduce the turbulent viscosity as much as possible to keep the flow physical but in k-e it is high. That's why k-e was converging. This is also the reason why convergence is obtained when a 1st order convection scheme is used. In the 1st order scheme (for laminar simulation or SST model) the unphysical eddy viscosity is replaced by the numerical viscosity of the scheme. So, in conclusion the turbulent model recommendations are correct.

As a solution to my problem, I used a transient laminar simulation to capture the effects of the time dependent vortices in the flow and time averaged the pressure loss.


PS: Ich bin kein Deutscher
raviad is offline   Reply With Quote

Old   December 27, 2019, 20:50
New Member
Join Date: Jul 2016
Posts: 6
Rep Power: 9
OpenFOAM-2016 is on a distinguished road
So this is kind of my question too. I am going to perform a simulation where the flow is not always turbulent. It's a transient flow where most of the time is laminar but at some points it gets turbulent by introducing a turbulent jet flow.
I was wondering what kind of model can give a better result?
OpenFOAM-2016 is offline   Reply With Quote

Old   January 3, 2020, 22:47
Join Date: Dec 2018
Posts: 36
Rep Power: 7
Chris2337 is on a distinguished road
Did you try the gamma transition model?
Chris2337 is offline   Reply With Quote


k-epsilon, sst k-omega, turbulence modeling

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
what "If" condition means in rebound brbbhatti OpenFOAM Programming & Development 0 August 12, 2014 10:18
DPM parallel is not working but serial is working johnwinter FLUENT 1 March 27, 2012 03:01
K Epsilon convergance issue Ollie OpenFOAM 2 April 18, 2011 09:28
How to get reference to k and epsilon in the epsEqn and kEqn cfd_explorer OpenFOAM Programming & Development 0 March 10, 2011 11:16
How to get reference to k and epsilon in the epsEqn and kEqn cfd_explorer OpenFOAM 0 March 10, 2011 10:58

All times are GMT -4. The time now is 17:56.