TAGGED: ansysfluent, floatingpointexception, multiphase, transient, vof


February 4, 2021 at 11:02 pmmottSubscriber
Hello all,
I am looking at the fuel slosh in an automotive fuel tank using the VOF model with SST komega turbulence to track the surface of the fuel to ensure constant fuel delivery to the output. I am not using any UDF (time constraint left it for 'further work') and instead am using gravity to model the lateral acceleration in a worse case scenario.
I ran the original design through and the simulation worked fine with results gathered. However after adding an additional baffle with 4mm holes, remeshing and running it through with identical solver settings I am now getting a floating point error after 2 time steps.
//
Flow time = 0.01999999955296516s, time step = 2
168 more time steps
Updating solution at time level N...
Global Courant Number [Explicit VOF Criteria] : 4.80402
done.
iter continuity xvelocity yvelocity zvelocity k omega time/iter
100 1.0984e02 4.3675e03 8.3489e04 3.3093e04 4.3467e04 1.5751e03 0:00:23 50
Error at Node 0: floating point exception
Error at Node 1: floating point exception
Error at Node 2: floating point exception
Error at Node 3: floating point exception
Error at Node 4: floating point exception
Error at Node 5: floating point exception
Stabilizing xmomentum to enhance linear solver robustness.
Stabilizing xmomentum using GMRES to enhance linear solver robustness.
Divergence detected in AMG solver: xmomentum Stabilizing ymomentum to enhance linear solver robustness.
Stabilizing ymomentum using GMRES to enhance linear solver robustness.
Divergence detected in AMG solver: ymomentum Stabilizing zmomentum to enhance linear solver robustness.
Stabilizing zmomentum using GMRES to enhance linear solver robustness.
Divergence detected in AMG solver: zmomentum Stabilizing pressure correction to enhance linear solver robustness.
Stabilizing pressure correction using GMRES to enhance linear solver robustness.
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 omega to enhance linear solver robustness.
Stabilizing omega using GMRES to enhance linear solver robustness.
Divergence detected in AMG solver: omega
Divergence detected in AMG solver: xmomentum
Divergence detected in AMG solver: ymomentum
Divergence detected in AMG solver: zmomentum
Divergence detected in AMG solver: pressure correction
Divergence detected in AMG solver: k
Divergence detected in AMG solver: omega
Divergence detected in AMG solver: xmomentum
Divergence detected in AMG solver: ymomentum
Divergence detected in AMG solver: zmomentum
Divergence detected in AMG solver: pressure correction
Divergence detected in AMG solver: k
Divergence detected in AMG solver: omega
Divergence detected in AMG solver: xmomentum
Divergence detected in AMG solver: ymomentum
Divergence detected in AMG solver: zmomentum
Divergence detected in AMG solver: pressure correction
Divergence detected in AMG solver: k
Divergence detected in AMG solver: omega
Divergence detected in AMG solver: xmomentum
Divergence detected in AMG solver: ymomentum
Divergence detected in AMG solver: zmomentum
Divergence detected in AMG solver: pressure correction
Divergence detected in AMG solver: k
Divergence detected in AMG solver: omega
Divergence detected in AMG solver: xmomentum
Divergence detected in AMG solver: ymomentum
Divergence detected in AMG solver: zmomentum
Divergence detected in AMG solver: pressure correction
Divergence detected in AMG solver: k
Divergence detected in AMG solver: omega
Error at host: floating point exception
===============Message from the Cortex Process================================
Compute processes interrupted. Processing can be resumed.
==============================================================================
Error: floating point exception
Error Object: #f
Registering ReportDefFiles, (*removed*)
Calculation complete.
//
I have tried a variety of suggestions in the forums but to no avail. I increased the time step from 0.01 to 0.001 but instead I get an instant SIGSEGV error before calculations start. When I've been troubleshooting this SIGSEGV error comes up whenever its not a floating point. I have tried reducing the momentum and turbulent kinetic energy underrelaxation factors but I either get no change or an instant SIGSEGV error again if I drop them low. I tried using double precision and got the same floating point error after 2 time steps.
My mesh quality is: orthogonal quality avg=0.762 min=0.153 ,skewness avg=0.236 max=0.847. This is slightly worse than my first model but it should be acceptable from what I've read?
I'm not using any inlets or outlets; I saw research projects/papers in the past do it that way and it worked fine for me first time, could this be causing any problems?
Here's a pic of the model for reference, sorry for the not optimal view can include more. The baffles are modelled as infinitely thin.

February 5, 2021 at 3:35 amYasserSelimaSubscriberSigSegV is an error you get when you try to access a location in the memory that is not defined.nI suspect it is the material ... how many phases do you have? vapor, liquid fuel and air?nDid you load the fuel from fluent library?nIf you are not using double precision, use it ...

February 5, 2021 at 3:44 pmmottSubscriber
SigSegV is an error you get when you try to access a location in the memory that is not defined.I suspect it is the material ... how many phases do you have? vapor, liquid fuel and air?Did you load the fuel from fluent library?If you are not using double precision, use it ...https://forum.ansys.com/discussion/comment/105673#Comment_105673
Thank you for your response.nI have 2 phases; air and noctaneliquid which is loaded from the fluent library. I have not edited any of their properties.nI shall be using double precision from now on, I wasn't sure on what is was/did till recently. I get a floating point error at 2 time steps if I only enable double precision same as before.nI have noticed that 2 walls are created when I bring my model into fluent which both interface with the contact regions mentioned in the original post. These walls don't seem to exist however as I can't view them in any way. Could this be causing any problems? I might try and remodel if nothing else.nCheersn 
February 5, 2021 at 3:49 pmRobAnsys EmployeeI'm not sure how you've got an interface there given the top and bottom sections are connected too. Check the geometry to make sure the mesh looks OK and you've not duplicated cell zones. Otherwise it should be fine. nThe interface zone will create walls for when the two sides don't overlap. As the two surfaces are in the same location and same size the walls don't physically exist. n

February 5, 2021 at 11:17 pmYasserSelimaSubscriberThe very interesting point here is that you get this error at low time step ... If it is geometry problem, it should appear at large time step as well. But this is not the case.nI suspected the material because I thought you have tables and the interpolation takes you out of bound ... but as you are using fluent database, this is not happening. nWhat on earth is requested by the solver at time step 0.001 and not 0.01 !!nnTry 0.0001 and let us know if you get this error.n

February 6, 2021 at 4:20 pmmottSubscriberThank you both for your help, I appear to have found the problem.nThere was a face on one of the fluid volumes which should have been a hole for the fluid volume in the centre. It seems that this was causing the interface surface and causing the solver to fail.nI redid the geometry so that there are only 2 fluid volumes separated by the baffles and this has removed the interface surface.nI have run the solver with the original settings and it's made it to 5,500 iterations and 111 time steps so far without an error so I think it's worked.nThanks again for the answers, I'll update here if it doesn't work but I think I know what the problem was and how to avoid it now.n

February 7, 2021 at 7:07 pmYasserSelimaSubscriberGood to know.n

 You must be logged in to reply to this topic.
Boost Ansys Fluent Simulations with AWS
Computational Fluid Dynamics (CFD) helps engineers design products in which the flow of fluid components is a significant challenge. These different use cases often require large complex models to solve on a traditional workstation. Click here to join this event to learn how to leverage Ansys Fluids on the cloud, thanks to Ansys Gateway powered by AWS.
Earth Rescue – An Ansys Online Series
The climate crisis is here. But so is the human ingenuity to fight it. Earth Rescue reveals what visionary companies are doing today to engineer radical new ideas in the fight against climate change. Click here to watch the first episode.
Ansys Blog
Subscribe to the Ansys Blog to get great new content about the power of simulation delivered right to your email on a weekly basis. With content from Ansys experts, partners and customers you will learn about product development advances, thought leadership and trends and tips to better use Ansys tools. Sign up here.
 Suppress Fluent to open with GUI while performing in journal file
 Floating point exception in Fluent
 What are the differences between CFX and Fluent?
 Heat transfer coefficient
 Getting graph and tabular data from result in workbench mechanical
 The solver failed with a nonzero exit code of : 2
 Difference between Kepsilon and Komega Turbulence Model
 Time Step Size and Courant Number
 Mesh Interfaces in ANSYS FLUENT
 error: Received signal SIGSEGV

5162

3275

2453

1308

956
© 2023 Copyright ANSYS, Inc. All rights reserved.