Learning Forum

[Eman Basheir]

Hello everyone, excuse me I'm having an «error object... floating point exception » . 

The calculation process goes for a while then it stops and I get that message. 

I'm simulating a fluid flow (biomass byrolysis) using ANSYS Fluent, with following details:

• Eulerian-Eulerian multiphase model.
• Three phases- with one reaction equation.
• Viscous model -K-epsilon.
• Turblance multiphase model- disperesed.

Kindly see the following error massage:

Divergence detected in AMG solver: pressure correction Stabilizing k to enhance linear solver robustness.

Stabilizing k using GMRES to enhance linear solver robustness.

 

Divergence detected in AMG solver: k Stabilizing epsilon to enhance linear solver robustness.

Stabilizing epsilon using GMRES to enhance linear solver robustness.

 

Divergence detected in AMG solver: epsilon Stabilizing gas-species-0 to enhance linear solver robustness.

Stabilizing gas-species-3 to enhance linear solver robustness.

Stabilizing gas-species-4 to enhance linear solver robustness.

Stabilizing gas-species-5 to enhance linear solver robustness.

Stabilizing gas-species-6 to enhance linear solver robustness.

Stabilizing temperature to enhance linear solver robustness.

Stabilizing temperature using GMRES to enhance linear solver robustness.

temperature limited to 1.000000e+00 in 99842 cells on zone 4 in domain 2

temperature limited to 1.000000e+00 in 99842 cells on zone 4 in domain 3

temperature limited to 1.000000e+00 in 99842 cells on zone 4 in domain 4

Stabilizing vof-1 to enhance linear solver robustness.

Stabilizing vof-1 using GMRES to enhance linear solver robustness.

 

Divergence detected in AMG solver: vof-1 Stabilizing vof-2 to enhance linear solver robustness.

Stabilizing vof-2 using GMRES to enhance linear solver robustness.

 

Divergence detected in AMG solver: vof-2

 

WARNING: Invalid cp (0.00

0===============Message from the Cortex Process================================

 

 

Error at Node 3: floating point exception

Compute processes interrupted. Processing can be resumed.

 

000e==============================================================================

 

+Error at Node 2: floating point exception

 

Error at Node 1: floating point exception

00

Error at Node 0: floating point exception

J/kgK) for carbon-solid at temperature -nan(ind) K

Thanks

[Rob]

Thanks, what are the three phases? 

The problem is with the model stability. Basically, the solver is unstable because of something, that's caused the stabilisation routines to be used and they've eventually failed. If cp=0 because of a temperature dependent property that needs checking, but equally that's only reported after the temperature field has hit 1K. 

Check the mesh quality (cell quality and mesh resolution etc). If that's OK try running single phase. Then multiphase and so on. 

[Eman Basheir]

the the three phases are: Biomass, gas, sand.

the sand is inert and only it is work as heat carrier. the biomass is heated and then it produce the gases , sorry I am begineer I need some details, so you means I have to delete these phases and started with single phase for examle the biomass only ?.

I checked the mesh quality and it is as follow:

Mesh Quality:

 

Minimum Orthogonal Quality = 2.53196e-01 cell 24135 on zone 4 (ID: 99760 on partition: 2) at location (-4.75776e-01, 1.09642e+01, -1.32245e+00)

 

Maximum Aspect Ratio = 1.26151e+01 cell 24135 on zone 4 (ID: 99760 on partition: 2) at location (-4.75776e-01, 1.09642e+01, -1.32245e+00)

Kindly advise me.

 

[Rob]

Cell quality looks OK. How well resolved is the mesh?  When complex models fail it's best to turn things off until it works. Then look at the flow field to check for areas that may be causing problems with the more complex set up. Resolve these and continue turning physics on. 

As a beginner I recommend getting some practice with something other than a 3 phase bioreactor - they're not simple models. 

What volume fraction of sand are you patching into the domain? 

[Eman Basheir]

ok, thanks for support.

 

[Eman Basheir]

The proplem was solved by modifying the under- relaxation factor as follow:

Under-relaxarion factor	case	Default
Pressure	0.2	0.3
Density	0.3	1
Body forces	0.3	1
Momentum	0.3	0.7
Volume fraction	0.3	0.5
Granular Temperature	0.1	0.2
Energy	0.3	1

 

Do you think these modification could effects the results accuracy , If so what else I can do?

[Eman Basheir]

noting that the error always appeared in the 53 seconed 

[Rob]

You've increased the values so it shouldn't alter the accuracy. I would watch the monitors (not residuals) carefully for any odd jumps/changes though. 

[Eman Basheir]

I decreased the values compared to the default, and there were odd jumps( remember that after these modifications the error wasn't appear and the run proceed until the end.

[Eman Basheir]

[Rob]

Oops, I was reading left to right.  In a transient case you're usually better off leaving the UR alone and dropping the time step. It's a bit dependent on what's driving an instability. Decreasing the UR tends to mean you'll need more iterations to reach the correct solution. 

As an aside, do NOT use brackets and other command characters ( " £ $ etc in filenames & paths. Fluent tends to react badly to these. It's something we always forget to mention as most of the staff are Unix/Linux trained or have been trained by those that are. The longer term users (I'm not old, yet...) don't use spaces either:  - or _ are fine. 

[Eman Basheir]

Thanks for the advice, already I decreased the time step to 0.005, so your advice now is to use the default values of  under relaxiation factor and decrease the time step more for example to 0.001 and increase the iterations, am I understand your point?

[Rob]

I'd decrease the time step further, chances are you've got something happening quickly that's making the model unstable. Once you can see where/what that is it may be possible to do something about it. 

[Eman Basheir]

ok, I will do that , thanks

[Eman Basheir]

Hello Rob, I hope you are doing well, I noticed that the before the floating point exception error appears, I recived this notification:

temperature limited to 1.000000e+00

What is causes of this issue? 

[Rob]

Fluent has a limiter for pressure, temperature and turbulent itensity to avoid the solution reaching silly values without any warning. So, in your case the solver will be struggling, hit 1K which will mess with any temperature dependent properties, is then diverging and the final error is the floating point. I assume there are a load of multigrid messages in the TUI before the solver falls over?

The cause is likely mesh or boundary condition related, but then linked to time step. With three phases and combustion/phase change you're going to need to carefully look at the mesh and all settings.