Learning Forum

[Pollovr]

Hello, I'm currently performing a classical two-way system coupling. It's a baffle (solid) in the middle of a tank (fluid) half empty. The goal is to simulate how the water impact deflects the baffle (classical sloshing inside a tank). My problem is that every time I set up the Fluent simulation and refresh the system coupling box (which is mandatory), it doesn't patch the water region. The simulation works perfectly but with no water. It's like it's re-doing the initialization but without the water phased selected. I've tried to set it up in the Fluent solutions directly but it doesn't work.n

[Stephen Orlando]

You can add the /solve/patch command to the Original Settings command as shown here. nn

[Pollovr]

Thank you, Steve, nCould you expand on that please? I've never used system coupling nor commands, just the Fluent interface. On that Original Settings line that you've highlighted, what should be written?n

[Stephen Orlando]

You'll need /solve/patch with the appropriate inputs. Take a look at the Fluent Text Command List documentation for more information.nhttps://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v202/en/flu_tcl/flu_tcl.htmlnnI recommend going over this tutorial in the Ansys documentation that shows a 2-way FSI simulation with Fluent and Mechanical.https://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v202/en/sysc_tut/sysc_tut_oscplate_wb_fluent.htmlnSystem Coupling Tutorials \\ Tutorials with Workbench-Setup Workflows \\ Tutorials with Workbench Setup and Execution \\ Oscillating Plate FSI with Fluent and MechanicalnnYou can also look at the following for the same tutorial but run with the System Coupling GUI or Command Line Interface that is run outside of Workbench. The new System Coupling GUI (run outside of Workbench) is available by searching for System Coupling 2019R3 (or newer) in the Start menu.https://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v202/en/sysc_tut/sysc_tut_oscplate_cli_fluent.htmlnSystem Coupling Tutorials \\ Tutorials with Command-Line Interface (CLI) Workflows \\ Oscillating Plate FSI with Fluent and MechanicalnnFSI simulations with very soft materials or membranes are prone to numerical instabilities. In 2020R1 we have introduced a stabilization method in System Coupling called the Quasi-Newton Stabilization Algorithm. Note that this has to be used with the new System Coupling GUI or Command Line Interface that is run outside of Workbench. More information here:https://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v202/en/sysc_ug/sysc_gen_scservice_dt_supplemental_iqnils.htmlnSystem Coupling User's Guide \\ System Coupling Data Transfers \\ Supplemental Processing Algorithms \\ Quasi-Newton Stabilization AlgorithmnnIt is very important to build up the FSI simulation in stages as opposed to setting up the 2-way FSI right at the start. This document Best Practices for Coupled Fluid-Structure Interaction (FSI) describes this process and is available here:https://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v202/en/sysc_ug/sysc_bestpractices_fsi.htmlnSystem Coupling User's Guide \\ Best Practices for System Coupling \\ Best Practices for Coupled Fluid-Structure Interaction (FSI)n

[Pollovr]

I'm just trying to patch a Cell Register called region_water with the water phase at a value of 1 (the region would be full of water). How would I write the commands?nn

[Pollovr]

I've been looking around and I assume it should be something like /solve/patch region_water volume fraction phase_water*yes 1 but every time that I try to do so, an error telling me that an invalid cell zone id/name was given. Where I can find the name of this region?.

[Rob]

Run through the command in the TUI to see what is being asked. You may find the different models require slightly different syntax. Using * in labels is also likely to cause problems! n

[Pollovr]

When I write this in the console it returns this. But I can't find the cell zone id/name of the cell register I've created (region_water)n

[Rob]

The register doesn't have a cell ID. Use () to close the list and read the next line that comes up. n

[Pollovr]

This is what happends:nn

[Rob]

That isn't asking the mesh region it's the phase domain, so likely mixture and phase-2 (or whatever you called it): hit Enter to see the options. In the earlier post you'd got beyond that stage. n

[Pollovr]

I see what you mean, here is what it comes up:nIf I keep on pressing Entern/solve/patchnnDomain>nmixture phase-waternnDomain> phase-watern()ncell zone id/name(1) [()] 1nInvalid cell zone.ncell zone id/name(1) [()] region_waternnError: eval: unbound variablenError Object: region_waternInvalid cell zone.ncell zone id/name(1) [()]nnNOTE: If you plan to patch the volume fraction ('mp') variable,nsince patching the reconstructed interface shape has beennrequested, please only pick one register at a time!n(0)nregister id/names (1) [0] region_waternregister id/names (2) [()]nnVariable> mpnValue [1] 1n45225 cells markednnturbulent viscosity limited to viscosity ratio of 1.000000e+05 in 45225 cellsnnAnd it patches everything that I'm looking for!! But how can I write that down into a single command line so I can put it in the Original Setting?.

[Pollovr]

As seen in the second comment of the post. nBecause when I do it line by line, between asking me the cell zone id/name and the register id/name I have to press ENTER and when I try to do so in one line (as /solve/patch/phase-water/region_water/mp/1) it asks me for the cell register. Is there any way to skip that step or tell Fluent to press enter?n

[Rob]

Try n/solve/patch phase-water region_water mp 1The / is for a menu command that (generally) takes you to another menu level. If it's an answer to a prompt you don't need the / n

[Pollovr]

It doesn't work:nI've tried /solve/patch/phase-water region_water mp 1 and it spits out the same answer.n

[Pollovr]

I think I got it: /solve/patch/phase-water () (region_water) mp 1n

[Rob]

Oops, I missed the terminator for the cell zone list. Try the above, and if it fails try n/solve/patch phase-water () region_water mp 1nslightly different to your version. n

[Pollovr]

IT WORKS!!!! n/solve/patch/phase-water () (region_water) mp 1nJust one question, when I go to Case Modification --> Orignal Settings How many number of iterations/Time steps should I put? Because the goal is to have the region patched at the beginning and let the coupled calculations runs, so I assume it has to be just one. I don't want fluent patching the same region over and over every time stepn

[Rob]

I'd set the patch to trigger at time step/iteration 0. n

[Pollovr]

It seems to be working, but now I have another problem... I don't know if it's related but I've created another discussion to make things clear:n/forum/discussion/23297/2-way-fsi-vof-floating-point-errorn

[ZX]

I am doing VOF+FSI as well, so first of all, thank you for your method. After I input your method '/solve/patch/phase-water () (region_water) mp 1', I can patch the water region in FSI simulation as well. nHowever, after I finished the calculation, there is no animation in CFD-post. Instead, there is just a constant image. In the Calculation Activities in Fluent solver, I set saving every time step. But in the CFD-post, there is no time step, just a picture instead of anime. Could you please tell me how to solve this problem? Thank you.nn

[Rob]

Check in the folder to see what you've saved. Are you saving .cas.gz or .cas.h5 files? n

[ZX]

Yes, it's the save problem, thank you.n

[Rob]

Sorry, not sure what you mean. n