[Dimone]

Hi, everyone.

I'm solving coupled (CFX + ANSYS APDL) problem. For some reasons some times the solution stops occasionally (e. g. due to poor fluid domain mesh morphing). The thing I would like to achieve is to be able to restart the problem from the point, where it stopped (in the most simple case - without any changes to setup; in more complicated case - as one with poor mesh morphing - restart after remeshing of fluid domains).

The thing I've got from CFX documentation is that I need multiframe restart scheme. Which assume, that multiframe restart files are written by ANSYS during solution.

Here I've came to my problems. CFX documentation tells, that the only thing to be done to enable writing of multiframe restart files is to add "RESCONTROL,DEFINE,ALL" string to .inp file before "SOLVE" command. I've tried this, but in this case the only one ANSYS.R001 file is written at the end of solution. But this is not what I need. Because I would like to be able to restart solution, if it stopped in non normal way, i.e. none ANSYS.Rnnn files present and I cannot restart solution from previously completed timestep.

The thing I need is to have ANSYS.Rnnn files for each timestep calculated by CFX+ANSYS (the same manner, as there are nnn_full.trn files for each step of CFX transient analysis, which allows to restart solution from any previous point (I mean restart CFX side part of analysis)).

I've tried to use more detailed RESCONTROL command definitions such as:
RESCONTROL,DEFINE,ALL,1,0
RESCONTROL,DEFINE,ALL,LAST,0
etc.
As I understood from ANSYS output it treats each timestep as separate load step, so I think, that one restart file is needed per load step (but as you can see above, I've tried to output all restart files from all substeps either).

I've found either, that .inp file generated by Workbench contains command
resc,,none
which disables output of restart files. But it is above the one, which I was inserting, so it should be overridden with my version. Anyway I've tried to remove it or replace with my version of command.

None of my trials were successfull, i.e. in all cases I've got the only one ANSYS.R001 file at the end of succesfull solution.

If somebody knows, how to make ANSYS produce restart files ANSYS.Rnnn for each timestep, please, help me.

Thanks in advance.

[singer1812]

Dimone:

You can't just restart from where the solution crashed, you need to start at the last output of the rescontrol/full cfx output point. In order to do a multiframe restart, without remeshing, you will need:

Ansys restart files *.rXXX,*.rdb, and *.ldhi and the CFX *.res (*.trn) files.

ALSO, the output times of the ansys restart files MUST coincide with a full output of a CFX output. So make sure those line up. You are only getting one *.rXXX file becuase it is getting over written with each output. Look up the APDL command rescontrol to counteract this.

You need to make sure your start time coincides with these files.

Doing a restart with remeshing is a much more complicated proceedure, and I don't recommend trying this until you master ANSYS FEA using APDL thouroughly. It involves:

1) INISTATE in order to keep track of the stress/strain field in the structure to use for resetting up the field in an "add-on" analysis.
2) Querying the Ansys results for the nodal velocities to setup the correct momentum in the structure upon restart
3) 2 Psuedo Ansys runs in order to setup the stress field, the momentum, and the correct restart time
4) ICEM or FE Modeler to update the Fluid mesh based on the deformation
5) Managing all of the above files and pulling the pertainent ones together for a "restart"

Master the normal restart, and don't worry about the remeshing part. Ansys will officially tell you it cant be done, and it might be sometime before they start doing this sort of thing.

I usually do the FSI controlled from the ANSYS APDL side (not CFX-PRE) so I can't reliably help you on the menu paths to set all of this up.

[Dimone]

singer812, thanks for your comments.

Originally Posted by singer1812

You can't just restart from where the solution crashed, you need to start at the last output of the rescontrol/full cfx output point.

I understand this. Thats why I'm looking for a way to obtain ANSYS.Rnnn files for each timestep (full set of *.trn files I already have).

Originally Posted by singer1812

In order to do a multiframe restart, without remeshing, you will need:

Ansys restart files *.rXXX,*.rdb, and *.ldhi and the CFX *.res (*.trn) files.

I understand this. And I have all of those files except for *.Rxxx ones for needed timesteps. Moreover, I have none of them until the succesfull finish of simulation (see bellow).

Originally Posted by singer1812

ALSO, the output times of the ansys restart files MUST coincide with a full output of a CFX output. So make sure those line up.

Certainly. That's why I need *.rxxx files written at the end of each stagger iteration process (at each timestep) - to be able to select the most appropriate one for restart.

Originally Posted by singer1812

You are only getting one *.rXXX file becuase it is getting over written with each output.

It seems for me, that it is not the case. It would be OK, if the situation described by you take place, as I would have at least .Rnnn file for latest succesfully completed timestep. But when I was watching for the files in corresponding folder, this file appears only at the end of the solution. So if the solution stops in its middle, I do not have *.Rnnn file for previous successfully calculated timestep. And this is exactly the issue, which I try to solve (and asking for help about it in this post).

Originally Posted by singer1812

Look up the APDL command rescontrol to counteract this.

Actually, it seems for me, that I read already all documentation relate to multifield restart from both sides: ANSYS and CFX. I did not find the answer, thats why I'm asking for help here.

Originally Posted by singer1812

Doing a restart with remeshing is a much more complicated proceedure, and I don't recommend trying this until you master ANSYS FEA using APDL thouroughly. It involves:

1) INISTATE in order to keep track of the stress/strain field in the structure to use for resetting up the field in an "add-on" analysis.
2) Querying the Ansys results for the nodal velocities to setup the correct momentum in the structure upon restart
3) 2 Psuedo Ansys runs in order to setup the stress field, the momentum, and the correct restart time
4) ICEM or FE Modeler to update the Fluid mesh based on the deformation
5) Managing all of the above files and pulling the pertainent ones together for a "restart"

You are absolutely right about, that it is really involving procedure. But as I understand (I'm studying the subject at the moment), the first and second points are handled with restart files (note, that I do not need to remesh structural part of problem). The third point, as it seems to me is handled with CFX Solver Manager using "Restart ANSYS" option.
Third point is also quite complicated, but I've managed with it (using ICEM CFD as you mentioned).
The fifth point should be just managed carefully (and there should be understanding of what file represents what, and what is it used for. So it seems to me, that if I can made a simple intermediate restart, I can either make the restart with remeshing either, but this is topic for another post.

Originally Posted by singer1812

Master the normal restart, and don't worry about the remeshing part. Ansys will officially tell you it cant be done, and it might be sometime before they start doing this sort of thing.

It's interesting, that ANSYS do not oficially support it... Posibly it is because of complexity of the procedure. But it seems to me, that I really need it, so, I will study the problem futher.

Originally Posted by singer1812

I usually do the FSI controlled from the ANSYS APDL side (not CFX-PRE) so I can't reliably help you on the menu paths to set all of this up.

I think, starting the coupled problem from ANSYS APDL side - is the next target for my study, if I would not be able to solve the problem from CFX-Pre side. Although I did not want to start get into it, as it is more complicated and requires more techincal understanding, more manual work and more carefulness.

Although I did not solve my issue, I greatly appreciate your comments, thanks a lot, singer1812.

[singer1812]

Oh, I missed something. In an MFX analysis, you are not using rescontrol, it is ignored. Look up MFRC. That should solve your restart files issue.

And regarding the remesh restart:
No, the restart files will not take care of #1 and #2. You are not able to use the restart files "as-is" in order to do a remeshed-restart. Technically, you are setting up a brand new problem, with the IC's identical to the end point of the old problem, and going on from there. Ansys is right in saying that you can't do a "restart" with a remesh in the normal manner.

Ed

[Dimone]

Ok, thanks, I'll look at MFRC command (I did not see, that in MFX analysis RESCONTROL command is ignored). Sad, but I cannot try it right now (I'm already at home), so I will continue my challenge tomorrow.

About restart with remeshing, you might be right, I thought about that (but just had no ability to try without restart files). But I made some investigation in that direction and was able to get output information about deformations stress and velocities (momentums) and (using some self written python scripts) convert those information into definition of new problem (at least, stresses were mapped successfully, as I remember). So, it seems to me, that I can accomplish this at least in this manner.

Thanks a lot once again.

[Dimone]

Finally, the solution indeed was to use MFRC command.

Using the command

MFRC,1,0

in solve block (instead of "RECONTROL,DEFINE,ALL,1,0") makes ansys write restart files (*.Rnnn) each time step.

One more comment:
This command is new in ANSYS 12.0 and it seems, like ANSYS documentation writers team did not update all the topics related to restart of coupled analysis. So, I did not find references to this command in common topics (I was confused especially by CFX manual - topic on restart coupled analysis - which tells, that for multiframe restart RESCONTROL command should be used). But the command presents in command reference and it actually tells, that in MFX analysis RESCONTROL command is ignored.

Thanks a lot to singer1812 again.

[solomedic]

hello everybody, I am doing two way fsi in ANsys Workbench 13 coupling ansys mechanical and CFX . No error is shown in setup of both mechanical and CFX but when running the solver it gives me the following error, can you direct me whats the real problem

ERROR #001100279 has occurred in subroutine ErrAction. |
| Message: |
| CFX encountered the error: Read. Fatal error occurred when reque- |
| sting Total Mesh Displacement for INTERFACE. |
| |
| |
| |
| |
+--------------------------------------------------------------------+

+--------------------------------------------------------------------+
| ERROR #001100279 has occurred in subroutine ErrAction. |
| Message: |
| cplg_SendCommand failed to send the command: ERROR -- CFX encount- |
| ered the error: Read. Fatal error occurred when requesting Total |
| Mesh Displacement for INTERFACE. |
| |
| |
| |
+--------------------------------------------------------------------+

+--------------------------------------------------------------------+
| Writing crash recovery file |
+--------------------------------------------------------------------+

+--------------------------------------------------------------------+
| ERROR #001100279 has occurred in subroutine ErrAction. |
| Message: |
| Stopped in routine cplg_SendCommand |
| |
| |
| |
| |
| |
+--------------------------------------------------------------------+

+--------------------------------------------------------------------+
| An error has occurred in cfx5solve: |
| |
| The ANSYS CFX solver exited with return code 1. No results file |
| has been created. |
+--------------------------------------------------------------------+

End of solution stage.

+--------------------------------------------------------------------+
| The following transient and backup files written by the ANSYS CFX |
| solver have been saved in the directory D:/temp/cfx/BETTER MESHED |
| AGARD_1028_Working/dp0/CFX/CFX/Work1/Fluid Flow CFX_002: |
| |
| 0_full.trn |
+--------------------------------------------------------------------+


+--------------------------------------------------------------------+
| An error has occurred in cfx5solve: |
| |
| ANSYS Solver terminated with return code 256 |
+--------------------------------------------------------------------+


+--------------------------------------------------------------------+
| The results from this run of the ANSYS solver have been written to |
| D:\temp\cfx\BETTER MESHED |
| AGARD_1028_Working\dp0\CFX\CFX\Work1\Fluid Flow CFX_002.ansys |
+--------------------------------------------------------------------+


+--------------------------------------------------------------------+
| Warning! |
| |
| The ANSYS CFX Solver has written a crash recovery file. This file |
| has been saved as D:/temp/cfx/BETTER MESHED |
| AGARD_1028_Working/dp0/CFX/CFX/Work1/Fluid Flow CFX_002.res.err |
| and may be an aid to diagnosing the problem or restarting the run. |
| More details should be available in the solver output section of |
| the output file. |
+--------------------------------------------------------------------+


+--------------------------------------------------------------------+
| The following user files have been saved in the directory |
| D:/temp/cfx/BETTER MESHED |
| AGARD_1028_Working/dp0/CFX/CFX/Work1/Fluid Flow CFX_002: |
| |
| mon |
+--------------------------------------------------------------------+


+--------------------------------------------------------------------+
| Warning! |
| |
| After waiting for 60 seconds, 1 solver manager process(es) appear |
| not to have noticed that this run has ended. You may get errors |
| removing some files if they are still open in the solver manager.

[Dimone]

Hi, solomedic.

It is not totally clean for me, what is the problem. But as error is related with reading interface nodes displacements, I would suppose one of the following:

1. For some reason ANSYS process was not started.
2. There are some troubles with definition of interfaces. It unlikely to be, as you say, that there are no errors in CFX-Pre, but still... By the way, do you have one FSI interface or multiple?
3. I'm not sure, if ANSYS<->CFX exchange data through files or TCP sockets (as I remember - sockets is the right answer). Anyway there may be some problems, if your antivirus/firewall programm blocks this communication (either firewall blocks TCP ports or antivirus blocks writing files. I met the latest case with ansys, but in another context). But of course, if you have other FSI examples, for which simulation is completed successfully, this is not the case.

I do not see any other causes of the problems...

Did you try to complete CFX tutorial for two way FSI (from workbench)?

If you have the same problem while completing tutorial, then the problem is global (most likely, antivirus/firewall or ansys apdl is not started or some other problems with ansys insallation)

If you do not have such a problem with tutorial example, but have it in your own probject, then the problem is in your definitions. Here I can suppose following cases:

1. Geometry for mechanical and fluid parts of the problem mismatch each other (different scale, or they have offset relatively to each other or you've just applied FSI interface on different (not matching) surfaces in mechanical (APDL) and fluid (CFX) parts of the problem. Or if you have multiple FSI interfaces, then may be you messed up them, while definition of the CFX part of the problem. Note, that CFX do not check geometrical matching of the interfaces. It just check existance of at list one FSI definition in your CFX problem for coupled analysis. So if definitions of FSI surfaces in APDL and CFX parts mismatch each other, you will not get errors within CFX-Pre.

If you give more background information, I will try to make more specific directions.

[solomedic]

Hi Dimone,

yes Ansys is not started because before solving a single iteration it gives me this error. I have multiple faces that are interface like trailing edge,leading edge,top bottom faces and tip of the wing.
yes it is through TCP socket. that firewall can be a case, I will check it and then I will reply to you. I have done alot of other examples but they were two weeks back, So there may be that now firewall is enabled?? I did the two way fsi example in workbench and no errors were found in that and then I did static divergence of flat plate.

As per your supposition

I am doing the 2way fsi in ansys workbench so the geometry cant mismatch because while doing 2way fsi in workbench it links the same geometry to both ansys MECHANICAL and CFX.
as you said if there are multiple interface they can be messed up, Does it mean that the sequence in which I select the interface in mechanical I should follow the same sequence in CFX? like if I select the leading edge first and then tip and then trailing edge in Mechanical as interfaces so in CFX should I have to select Leading edge,then tip and then trailing edge as interfaces in CFX as well?

I will check by doing a simple run that if that is caused by a firewall or if we have to selct faces in same sequence.
and I dont see any other cause of this error

thanks Dimone

[solomedic]

Hi dimone I try to run an old case by keeping the firewall on,it is solved normaly then I made the firewall of and then again it gives me no error and ran smoothly as before, so the problem is not with firewall.it is something else

[Dimone]

Originally Posted by solomedic

yes Ansys is not started because before solving a single iteration it gives me this error.

It is not neccessary, that ansys is not started although you do not have results. And looking at things, you write further, it seems, that this is not the case (you can just check out processes in process manager to make sure).

I am doing the 2way fsi in ansys workbench so the geometry cant mismatch because while doing 2way fsi in workbench it links the same geometry to both ansys MECHANICAL and CFX.

Ok, it's clear

I have multiple faces that are interface like trailing edge,leading edge,top bottom faces and tip of the wing.

...

as you said if there are multiple interface they can be messed up, Does it mean that the sequence in which I select the interface in mechanical I should follow the same sequence in CFX? like if I select the leading edge first and then tip and then trailing edge in Mechanical as interfaces so in CFX should I have to select Leading edge,then tip and then trailing edge as interfaces in CFX as well?

Multiple interfaces and multiple faces, on which the interface is present is not the same thing. By word interface I mean fluid-solid interface boundary condition (single item in project tree), which can be assigned to (associated with) multiple faces. While you select faces to associate with INTERFACE BC it is no matter, in which order they are picked.

But you can have multiple fluid-solid INTERFACE BCs. Each INTERFACE in this case is labeled by ANSYS (usually, labels are FSIN_1, FSIN_2 etc...). Each interface is associated with their own set of faces.

Then, when you define fluid part of the problem in CFX-Pre and define "WALL" boundary with mesh displacement defined by "Fluid-Structure-interface" (do not remember, how it is named exactly, but I hope, you've got the thing) - there you have combo-box (expanding list) with those FSIN_1 etc... And you should select one to associate this WALL condition of CFX problem with INTERFACE previously defined in mechanics application.

If you have only one interface, you cannot mistake, as there is only one option to select from (note, however, that you must have exactly one wall with this mesh displacement option and its geometry (faces selected for it) must match corresponding faces of INTERFACE defined in mechanics.

If you have multiple INTERFACE-BCs in you mechanics application, you must have exactly the same number of walls with exactly the same faces selected within CFX-Pre. And you must select the right FSIN_n interface while defining the interface.

Note, that for coupled analysis CFX-Pre only checks for existance of at least one WALL condition with FSI-defined mesh displacement. But it DO NOT CHECK, if you have WALLs corresponding to each mechanical INTERFACE and it DO NOT CHECK, that faces selected for INTERFACE (mechanical) and WALL (CFX) do match each other. So if you make some mistakes in this regard, CFX-Pre will not warn you, that you have invalid model.

Hope, this will help.

[solomedic]

Thanks Demone for your help.

Ok I got Multiple interfaces,No I have a single wing that is a single interface.

the problem seems to be solved because the solver has done a couple of iterations now, the problems seems to be with mesh. In the previous run which gave me errors the mesh was very unstructured (i tried previously to make the mesh good but was not able to get a good mesh because it is vey thin wing-Agard 445.6 wing that has naca 65004 airfoil)
but this I somehow able to get a good mesh and the solution started,no other change I made in the setup.

Because of unstructured mesh in the previoius runs I think Ansys and CFX was not able to transfer data at interface, Can it be a reason?

[solomedic]

Sorry for posting Irrelevant message here but I am posting it here so Dimone you can see it and you can reply. Few people reply when you post a newer separate post.

The Question is that: I am doing Divergence of wing and some time the wing is converged like the graph of mesh displacement of some point on wing raises to a certain values and then become constan but at some other higher velocities it(mesh displace of some point) shows an ever increasing trend and then gives me an error of folded mesh, so should I consider that velocity as Divergence Velocity?

the other thing that for cases it gives me folded mesh error the mesh diplacement of some point at tip of the wing is like of order 15,20mm.
so Does it make some sense that by this displacement at tip the wing is broken?

the wing has span of .76m.

[Dimone]

Yes, problems with mesh can cause very different error types. And the problem is that they often hard to identify as problems with mesh (except for folded mesh). One word about terminology: structured and unstructured mesh is specific terms, which define mesh generation method. I think, when you say "very unstructured", you mean "distorted" or just "mesh of poor quality" (whatever "mesh quality" means in your particular case).

Folded mesh error is just what its name say. When you have folded mesh error, it means, that one (or more) element was folded or even inversed inside out. It do not have any special physical sense - like "wing is broken". It just says, that "solution has diverged" in this special sense. You can try to vary mesh morphing settings or initial mesh (but take into account, that "better mesh" not always means finer mesh).

You can also try to manage remeshing restart (sayng this I make your posts in-topic by the way ). But this requires very good skills with CFX and ANSYS and good understanding of what is going, when you start coupled analysis and which options you have. All this staff cannot be covered in single answer. If you choose try remeshing restart, I only can suggest you to examine all related topics in manuals (note, that you will need either CFX and APDL docs). Any way it took quite long time to get understanding of that. NOTE: I was working with ANSYS 12.1. May be in 13-th release the things are better. But anyway remeshing restart in coupled analysis is really complicated topic. You can check out my questions in this therad and answers and if you understand, what they are about, I think, you can manage with remeshing restart.

[solomedic]

Yes I should have said it distorted mesh.
there is just a single option that should the mesh morphing be Onn or Off? so should I make it onn?

so if the folded mesh does not give the divergence then how will I know what is the divergence speed,anyother parameter?

I will check that Meshing Restart.

[Dimone]

there is one mesh morphing option - mesh stiffness. It is in the properties of the domain. (although, I did not find it too useful for the mesh morphing problems arisen in my solutions). You can try it.

Actually, I do not understand, what is "divergence speed"... (if it is something from the aerodynamics, I should say, that I'm not specialist there).

[solomedic]

Divergence is aeroelasticity term, as flutter is dynamic aeroelastic phenomena, divergence is static aeroelastic phenmenon. Divergence simply means that the aerodynamic forces due to flow are so much larg that resotring elastic forces can not equate them and the wing continously deforms under aerodynamic loads till the wing is broken,so I consider,the min speed at which the folded mesh happens as divergence speed.
yes I have mesh morphing and also enabled that increase mesh stiffness near small volumes. by increasing stiffness of small volumes the areas which are crtical are fine meshed so these are remain fine meshed to some extent by this option

[Dimone]

Ok. Then mesh folding has nothing in common with "divergence", as you descrived it. Actually, I do not see some criteria, how you can detect if for 100%. You can try to perform simulation up to the situation, when the wing is deformed significantly, but first, it still will not be 100% criteria - just you thinking "oh, I think, here it is", and second, it can be quite complicated to complete such simulation due to large deformations and difficulties related to mesh morphing. Possibly, if you find better criteria, you will not need to wait until the wing is highly deformed. May be it is possible to monitor some special parameters of system, which will indicate occurance of you "divergence" at the very beginning (i.e. when deformations are not so significant). But this is only my speculations.

[solomedic]

hi dimone again an irrelevant question and hope you will not shift this one to restart analysis
I am now going for flutter of a wing ? do u hav any exoerience on that, I dont now how to start with it,it is also a two way fsi phenomenon, but it requires some load step so which load step(harmonic,step?) should I apply?
I making it myself relevant,how can I restart from last time step without remeshing? I just type MFRC command in cfx pre?

[Dimone]

No, as I said already, I'm not specialist in aerodynamics at all (an in wings phenomena in particular, whatever those exist). All I can say, it is impossible to perform harmonic analysis in coupled simulation (here by harmonic analysis I mean simulation, where you have harmonic excitation and harmonic responce). The only availabe option is transient analysis. Although, you of course can define harmonic load and perform transient coupled analysis.

Actually, I do not understand, at what point you need restart.

MFRC is APDL (not CFX) command.