TAGGED: convergence, residuals, time-step, time-stepping-method, transient
February 9, 2021 at 10:18 amRaffael_MitrouSubscriber
I am having severe problems with convergence and my time stepping settings (under "run simulation").
I am doing a transient VOF 2-phase simulation (phase1=nitrogen, phase2=liquid). The special thing about my simulation is that I have a filling process (liquid enters through inlet into tank with v=0.1m/s) in the beginning for a few seconds (e.g. 10) and then the liquid enters through an interface into a porous zone where it gets soaked, which takes 2-3 hours. The porous zone and the tank are initially completely filled with nitrogen at p=40mbar.
In the following, you can see my case scheme with its BCs:February 9, 2021 at 12:45 pmKarthik RAdministratorHi,nInstead of attaching your screenshots, please embed them into your post. Simple copy and paste should work. Ansys employees are unable to download files on this forum.nSince you are running a Transient VoF case, you don't have to set your absolute convergence criteria to 1e-6. A convergence of 1e-3 or 1e-4 every single time-step should give you a good start. Also, are you able to converge each time-step by running just 20 iterations per time-steps? If this is not the case, you might have to increase the number of iterations per time-step.nRegarding time-step - try using the implicit formulation. You might be able to march faster in time with larger time-steps. Based on the time-step size of 1e-4, what is your current CFL?nRegarding the divergence, are you monitoring your solutions using additional plots? If so, do they show an anomalous behavior? It is probably a convergence issue you are facing. Please see my comments on convergence criteria and converging every single time-step.nI hope these comments help.nKarthiknFebruary 9, 2021 at 1:15 pmFebruary 9, 2021 at 1:32 pmRaffael_MitrouSubscriberHello Karthik and thank you for your quick response and the tips!nA very helpful tip! I will first try 1e-04 for the absolute convergence criteria. If it works, I will go with 1e-03.nActually, I set the Max. Iterations/Time Step to be 120 as you can see in the screenshot above. Maybe you overlooked that!?nWhat do you mean by the implicit formulation of the time step? How can I define this? CFL is default and set to 2 (see screenshot above).nI use to have one monitor for my contour of phases (that's what I mainly want as a video/animation) and one monitor for the residuals. Since I don't have a continuous flow with an output, I can't monitor mass imbalances, if it is that you are referring to. Are there other parameters I should monitor to check convergence?nThanks again! Kind regards!nRaffaelnnFebruary 9, 2021 at 2:20 pmRobAnsys EmployeeIf you're forcing liquid into the domain the gas has to go somewhere. Either it compresses or there has to be an outlet: to a point the solver error (poor convergence) will lose some mass, but that may then lead to the divergence you're seeing. nRe the mesh, have a look at dynamic adaption and VOF predefined criteria in the 2020R2 or 2021R1 versions. That may allow a coarser mesh overall but the solver can then refine the interface. nFebruary 9, 2021 at 3:05 pmFebruary 9, 2021 at 3:55 pmDrAmineAnsys EmployeeLimit the time step size in the adaptive panel so that it does not jump / Better to monitor number of iterations per time step and time step used every time step. nMoreover Are you sure about your porous zone parameters? Do you think that phase slip is not important here? Which version are you using?nFebruary 9, 2021 at 5:42 pmRaffael_MitrouSubscriberArray I looked both options up and they seem to be quite usefull. Array Since I use ANSYS 2019R3 I may not be able to use those options, right?nVOF predefined criteria (Domain > Adapt > Refine / Coarsen... with VOF activated): Here is what I found (also for other interested users)...nAnd my Adaption controls box:nIs it possible to use this option with ANSYS 2019 R3?nI also initialized prior to looking up the settings.nArraynLimit the time step size in the adaptive panel so that it does not jump --> How can I do that? I set a min. and a max. time step size that seemed reasonable to me. What do you mean by jump?nBetter to monitor number of iterations per time step and time step used every time step. --> Do I set this monitor like so: Solution > Monitors > Report Files & select report definition: iters-per-timestep?nnnFebruary 9, 2021 at 5:45 pmRaffael_MitrouSubscriberArray nMy porous zone parameters (resistance factors) are taken from previous works, so they are kind of half guess values? I surely have to adapt them later on...nWhat is the concept of phase slip? I haven't heard of that before.nI am using ANSYS 2019 R3.nFebruary 9, 2021 at 6:02 pmDrAmineAnsys EmployeePlease start them with no porous zone.nYou reduce maximum time size to 1 ms for example and use conservative time step change factors. Think about using barotropic gas material.nPhase slip is slip velocity between phases.February 10, 2021 at 5:36 pmRaffael_MitrouSubscriberArrayno How can I start without porous zone? I defined it in the Zone Condition of the corresponding zone and activated porous model and laminar there.no Referring to the time step change factors I found this:n"Variable time stepping is not ideally suited to second order time formulation because the second order formulation does not take into account the time step size variation. However, by keeping the minimum time step change factor in the range 0.5–0.8 and the maximum time step change factor in the range 1.2–1.5 it can be used without severely affecting the second order time accuracy."n--> Therefore I chose min 0.5 and max 1.5. Is that considered conservative?no Where can I set the Phase Slip? Any recommendations?nFebruary 12, 2021 at 7:50 amDrAmineAnsys EmployeeYou just deactivate the porous option from Cell Zone Conditions.nWithin the actual version rely on second order time discretization and adaptive time stepping.nPhase Slip is relative velocity between phases: VOF model does not account for that. Forget about this point for now.nFirst thing you need to try is to disable porous function and run with constant time step size to ensure that everything is running smooth. Second step you add porous option (here we need to talk again). Third step is to optimize setup.nnBetter to switch to a newer version which adds more stability features for VOF calculationnFebruary 12, 2021 at 10:00 amRaffael_MitrouSubscriberArrayI tried a few things out and now my simulation is running and completed. I think that we can skip your advice of deactivating porous media, right?nI simulated 100 seconds (physical time) and created an animation of the electrolyte volume fraction.nFollowing two screenshots of the electrolyte volume fraction at t=50s and t=100s:nSo the thing is that from the point seen at t=50s I would imagine the liquid to be soaked into the porous zone and I want to simulate this wetting process until t=160min. Also it seems that the liquid is disappearing. I will be monitoring the inlet surface at next to see if there is flow in the upper y direction by any chance. Do you have any other ideas about that?nAnother problem: the calculation time is too long for try and error since my deadline is coming closer. Any ideas how I can reduce calculation time?no Max. Iterations/time step is already low at 20.no Maybe I can increase max. time step size in the adaptive time stepping settingsfrom 10s to maybe 60s or so?no Absolute criteria (residuals) also quite high (for all parameters): 1e-02no Maybe my mesh is too fine in the right zone (tank) since my focus is rather on the long-term wetting processes in the porous zone (left zone)!?no Solution methods: I have set everything to 2nd order except for the transient formulationwhich was first order. Shall I change it to 2nd as well?no For my porous zone (cell) I have the following settings. The Viscous Resistance and Inertial Resistance factors were taken from another work as first guess values. Any ideas how or to what extent I can change them? Or doing try and error until I find my simulation to be similar to my reference process? --> In this case I again need to reduce my calc. time...nnFebruary 12, 2021 at 11:07 amRobAnsys EmployeeCheck the resistance coefficients, they're quite high. As for changing them, there's a section in the manual outlining the various methods to calculate the values based on what you know about the material. nFebruary 17, 2021 at 1:19 pmRaffael_MitrouSubscriberCould too high values for the resistance coefficients cause the electrolyte volume to decrease?nMy expectations: The electrolyte volume should increase until the inlet is closed (at t=2.4s) and should then be constant.nI monitored the volume-averaged electrolyte volume (see screenshot):nIn the beginning, the electrolyte volume increases which is correct. However, it then seems as if there was a leakage in my simulation as the electrolyte disappears / amount of volume decreases. The following screenshot shows the volume fraction of electrolyte (red color) against the nitrogen (blue color).nDo you have any ideas why this is happening?.Convergence:nFor the absolute criteria, I set 1e-02.nnThanks in advance.nKind regards!nnFebruary 19, 2021 at 1:34 pmRaffael_MitrouSubscriberdo you have any ideas related to my problems previously explained?nPS: I changed to fixed time steps.nFebruary 19, 2021 at 1:48 pmRobAnsys EmployeePorous coefficient can effect stability but you'd see that in the residuals. What separates the zone that's filling with the neighbouring zone? nFebruary 19, 2021 at 2:58 pmRaffael_MitrouSubscribernWhat exactly would I see in the residuals? Do you mean I would see an increasing convergence tendency?.In the BC settings I defined interface_1 and interface_2 and from there I defined an interface under Mesh Interfaces selecting the two interfaces.nIs it possible that there is a problem with orphan cells because the mesh is too different at the interface?nI read about this topic in: 18.104.22.168. Donor Search Fails Due to Orphan CellsnHere a picture of my meshing near the interface:nThe red arrow pointing to where the interface is.nnMy idea is as follows:nI thought about coarsening the mesh at the right (where it gets filled) and refining it at the left, such that the size difference near the interface get smaller (to avoid orphan cells).nIs that a valid idea?n I am getting frustrated because I cannot solve this problem for weeks now...nPLEASE HELP! nFebruary 19, 2021 at 4:06 pmRaffael_MitrouSubscriberPS: My porous media settings:nI checked my Viscous Resistance (1/K) values as well as my inertial resistance (C2) values and they have already been correct.nI assumed a particle diameter of 8μm and a porosity of 0.4 yielding the above values.nWhat should I specify for the Relative Viscosity?nFor a porosity of 0.4 and I get these values:nBrinkman: 3.586nEinstein: 2.5nBreugem: 0nWhich model is best to choose here? I picked Breugem because its the latest publication.nFebruary 19, 2021 at 4:35 pmRobAnsys EmployeeOrphan cells are in overset only, hopefully you're not using that. If the region to the left of the interface is the porous zone then you will get some leakage as the medial will restrict flow and not stop it. There's also no need for the interface if you use multibody parts: a conformal mesh is generally better. Nothing wrong with using mesh interface where it's needed, but in this case it's not. nFebruary 19, 2021 at 5:06 pmRaffael_MitrouSubscriberFebruary 22, 2021 at 11:04 amRaffael_MitrouSubscriberArray Array I don't know how I can set this up without defining the two faces as an interface BC and why interfaces are not needed here?nSince I wish to have two cell zones, in order to define one of them as porous, I need to somehow specify this interface region in my Boundary Conditions.nAlternatively, I thought of using something like an outlet BC for the left face of the tank and an inlet BC for the right face of the left zone (=porous). Is this possible and what type of BCs exactly shall be used?.nFebruary 22, 2021 at 11:26 amRobAnsys EmployeeIf you create a multibody part or use share topology you'll get a conformal mesh with an interior rather than the interface pair. An interface just means we can have two different meshes and pass fluid from one to the other. nYou have an inlet and (pressure) outlet, so flow must pass through the porous region. Because the porous region can't completely stop the second material you'll get some of it passing into the porous region. nFebruary 22, 2021 at 1:34 pmRaffael_MitrouSubscriberArraythe steps I did are the following:nDM: After creating the two zones I Form new part and activate Shared Topology (=Gemeinsame Topology).nMeshing:nIs it ok that under Geometry my two parts are separate instead of the one part I defined in the previous Design Modeler step?nAlthough I labeled the two faces as interior during meshing instead of interface (which I did before this try) I can only choose interface in the BCs in Fluent...nIs this due to the fact that I activated Shared Topology in DM and changed some labels in Meshing and then updated my Setup instead of doing it like this at once?nOr did I misunderstand you and it is ok like that and I just need to avoid going to Mesh Interfacesto define an interface selecting the two BCs?nFebruary 22, 2021 at 1:50 pmRaffael_MitrouSubscriberPS: When I try to initialize the case, I get the following message:nnWARNING: Unassigned interface zone detected for interface 12 (--> which is my interior1 BC)nWARNING: Unassigned interface zone detected for interface 13 (--> which is my interior2 BC)nUnassigned interface zones found. Flow is not initialized.nnSo when I instead define a static Interfaceunder Mesh Interfacesanother 3 BCs are created:ninterface-interior-1-1(@Rob the BC you referred to?)ninterior1-non-overlappingninterior2-non-overlappingnAlso, I don't understand why I get these non-overlapping BC which are of type wall as I don't have non-overlapping regions. So it is like a wall of zero length?nI am quite confused with all these BCs and settings. Any suggestions are appreciated!nFebruary 22, 2021 at 1:50 pmRobAnsys EmployeeIf the surfaces are in the same part then you should have one edge in meshing and it's an interior. With two parts you need interface. Both work, the former is generally better as it avoids any interpolation. The latter is used as needed, here it's unnecessary. nFebruary 22, 2021 at 2:06 pmRobAnsys EmployeeWe posted at the same time. You have two edges at the same location. With share topology that shouldn't happen, and it's why you're then getting problems. The interface condition will automatically set up the pair, the interior ought to error on import as an interior can't exist on the external boundary of a domain. Which means there's something odd with the geometry. Can you check the two faces you have don't overlap. nFebruary 22, 2021 at 2:32 pmRaffael_MitrouSubscriberI simply connected the two zones using the same two nodes (see screenshot). So I don't think that there is an overlap or something like that. Are there tools to check overlapping errors?nnMy next approach would be to do it again using SpaceClaim instead and activating Shared Topology there.nI have used SpaceClaim in the past but could not find a way to label faces in SpaceClaim (which is quite easy to do in DM). I do this, to not need to do that manually later on in Fluent or having automatically created, weirdly named BCs. Is there an option to do so?nFebruary 22, 2021 at 4:47 pmFebruary 22, 2021 at 5:02 pmRobAnsys EmployeeYou can using the mesh separate options but it's not recommended for relatively inexperienced users. In SpaceClaim or Workbench Meshing you can add Named Selections, I tend to do this in Workbench Meshing. Note, Fluent Meshing is for 3d and I set the labels in SpaceClaim. nFebruary 23, 2021 at 10:56 amRaffael_MitrouSubscriberMeanwhile I set everything up to the settings which worked quite well before.nI set up adaptive time stepping with the same exact settings of that simulation I did where the electrolyte was disappearing (at that time with an interface). nnBut just after 10mins Floating point exception message comes up and the simulation fails.nI set the absolute convergence to 0.01.nIterations per time step were set to 20.nnCould it be due to false Operating Conditions? I want both zones to be evacuated to 40mbar of nitrogen at the beginning (0% electrolyte). I set this as a Gauge Pressure of 4000Pa in the Solution Initialization Box and the electrolyte volume fraction as 0, since it will be dosed from the inlet and only nitrogen should be in the zone. Is that set up correctly?nnFor the Operating Conditions Box, I chose the Reference Pressure Location to be on the symmetry line only 1mm below the upper wall of my porous zone (76m high). The Specified Operating Density is the density of nitrogen (from the Database).nnAny ideas why the simulation fails?nThanks in advance!nFebruary 23, 2021 at 2:45 pmRaffael_MitrouSubscriberArray In my console besides Floating Point Exception it said:nnturbulent viscosity limited to viscosity ratio of 1.000000e+05 in 444 cells &nDivergence detected in AMG solver: temperaturennAfter some research, I found out that maybe the Solution Limits are the reason. So under Solution --> Controls --> Limits... I found the following:nFebruary 24, 2021 at 2:31 pmRaffael_MitrouSubscriberI read the manual. But I am not quite sure what to set if I have 2 phases and 4000 Pa in the beginning and a liquid flowing into the domain with 1bar. Maybe velocity inlet BC is not suitable here? Better to try pressure inlet?nI set 4000Pa as the operating pressure now.nnReferring to the density: I specified the density in the material settings. For N2 I have taken the default values.nFor the electrolyte, I set the density to a constant of 1190 kg/m3.nMaybe here is the problem. My electrolyte can be assumed as incompressible. My other phase - N2 - is a compressible ideal gas.nShould I set the density of N2 to ideal-gas instead?.Also, I found this:nDoes it make sense to switch to the density-based solver or to try to change nitrogen material settings to ideal-gas first?nViewing 33 reply threads
Ansys Innovation Space
- 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.
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.Trending discussions
- 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
- Difference between K-epsilon and K-omega Turbulence Model
- The solver failed with a non-zero exit code of : 2
- Time Step Size and Courant Number
- Mesh Interfaces in ANSYS FLUENT
- error: Received signal SIGSEGV
Top Rated Tags
© 2023 Copyright ANSYS, Inc. All rights reserved.Ansys does not support the usage of unauthorized Ansys software. Please visit www.ansys.com to obtain an official distribution.