CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   STAR-CCM+ (http://www.cfd-online.com/Forums/star-ccm/)
-   -   Floating point exception error [High rotating speed tube] (http://www.cfd-online.com/Forums/star-ccm/129465-floating-point-exception-error-high-rotating-speed-tube.html)

wkwong February 5, 2014 23:49

Floating point exception error [High rotating speed tube]
 
Hi,

I have been encountering this Floating point exception error [overflow]/[divide by zero] whenever I run my simulation over 1200 rpm. Below that, its running well. Once over 1200 rpm it will gives me this problem. I understand that this is because the solution diverge, but I cannot identify the reason why, because all of my boundary conditions (mine is really simple project) seems correct. I need to run until 6000 rpm.

My project:
Cooling of rotating tube, rotating at 6000 rpm around an axis outside of itself and convection is allowed everywhere except the base of the tube (cone shape horizontally). Its inital condition is 369k and surrounding is 300k.


http://imageshack.com/a/img543/7150/rafe.jpg

Any help PLEASE??

Updates: I managed to get it running at 6000 rpm without getting simulation error immediately by reducing the time step to 1E-14s (unbelievable low), but the residual usually suddenly rise to super huge value after around 300 iterations and eventually I will get the same error again...

my email is masterlancer@hotmail.com

rabat February 6, 2014 01:45

Hi,

I would try to run the calculation only isothermal.
If it 's converge, than try to modified you mesh, or change the under relaxation factors.

Regards

wkwong February 6, 2014 07:27

hi, @rabat, tried and it did not even converge only isothermally, at 6000 rpm.

me3840 February 6, 2014 20:33

Is this transient or steady? A tube rotating outside of its axis sounds like an unsteady problem. Are you changing your timestep to account for the new higher rotation rate?

Does it diverge immediately or after some amount of time?

What kind of mesh are you using? Is it still adequate for the higher rotation rate?

wkwong February 6, 2014 20:43

@me3840,

It is transient. You mean make the time step smaller?

At 6000 rpm, it diverge almost immediately, within 3 iterations.

My model is
Implicit unsteady
Coupled Flow
3D
Laminar
IF97 (water)

My mesh is:
Polyhedral, Prism layer, surface remesher, surface wrapper

I have around 690k cells.. should be fine thou.

wkwong February 8, 2014 05:46

Quote:

Originally Posted by me3840 (Post 473831)
Is this transient or steady? A tube rotating outside of its axis sounds like an unsteady problem. Are you changing your timestep to account for the new higher rotation rate?

Does it diverge immediately or after some amount of time?

What kind of mesh are you using? Is it still adequate for the higher rotation rate?

I tried to decrease the time step REALLY small to around 1E-14 s and thanks to you I am able to get the simulation running without the error as mentioned previous. All the parameters's residual fall to somewhere 0.01 however, my energy and continuity residual is at 10^5 region. The simulation can continue, but why is this so?

wkwong February 10, 2014 07:12

Any would be greatly appreciate please. Thank you.

ggulgulia February 12, 2014 02:42

Hey Wkong

I think 1e-14 is too small a time step. Your simulation will take a lot of time to complete even 1e-4 second. I suggest check your courant number. Sometimes it's value is 50. If it's so, then change it to 5 and try running the simulation. 1e-5 second with 10-20 inner iteration should be good enough. You should approach the problem in as simple way as possible and then go on to add the complexities as desired when you see your simulation actually works. Therefore I recommend to change the fluid to water constant density or ideal gas liquid H2O

Secondly you have given Laminar flow for the turbulence model. Flow of water at 6000 RPM cannot be laminar. I suggest you change the model to k-e with wall y+ model.

Thirdly your mesh size for this simulation seems very small. Can you post a picture of the domain ? I need to have a look at the grid spacing near the wall boundaries and see if it could be resolved into 2-d axisymmetric problem?

wkwong February 12, 2014 11:32

Hi ggulgulia, thanks I have posted my mesh size and my model. It is a fluid region rotating about the Z axis at 6000 rpm. Base of the cone is insulated and the rest is allowed convection at 500 W/m2K

ggulgulia February 14, 2014 14:09

Hey Wkwong

I still am wondering if you are using RBM or Overset method for making the tube rotate. Regardless of that you can check the points I have mentioned below...

1. I would suggest that you check with a different turbulence model
2. Try to increase the time step to 1e-5 second
3. Check your initialization value. Sometimes the problem occurs due to improper initialization
4. Try reducing the URF for pressure to 0.5 and then ramp it up to 0.9 after 100-150 iterations.
5. Check the courant number. Sometimes the default value is 50. If it's so then bring it down to 5 or somewhere less than 5 but greater than 1.
6. Go for a first order differencing scheme for 100 iterations and then change the differencing scheme to second order implicit.


All times are GMT -4. The time now is 17:45.