[alfianalfarisi]

Hello all, I am Naval Architecture undergraduate student from Indonesia, I'm doing my final project to claim my bachelor degree, but I'm facing problem when doing so

I'm facing
+--------------------------------------------------------------------+
| ERROR #004100018 has occurred in subroutine FINMES. |
| Message: |
| Fatal overflow in linear solver. |
+--------------------------------------------------------------------+
in my ship analysis to get the ship resistance. This error appear wen it reach 12th iteration.

I'm having no problem doing the same analysis with default mesh size, its 43 meter because I'm having 170m long ship to analyze. Then when I give face sizing to my ship to 1meter size it errors about 20 iterations, then when I give it a try with refinement the error appears again in 12th iteration.

I've trying to read any clue from this forum but I still don't get what shall I do to solve this.

Can anyone help me out here? Thank you

[ghorrocks]

Have you looked at the FAQ: https://www.cfd-online.com/Wiki/Ansy...do_about_it.3F

[Steffen595]

dodgy mesh, not enough RAM. Or boundaries not right, does it say it has to make 100% walls in an outlet? or there are some wild velocities somewhere? Run again, stop manually after 10 iterations 9because you know it will crash at 12) and have a look in POST. Maybe there are endless swirls (eddies) , if you do streamline.

[alfianalfarisi]

Originally Posted by ghorrocks

Have you looked at the FAQ: https://www.cfd-online.com/Wiki/Ansy...do_about_it.3F

I've tried to read it before I post this

The physic set up, I think the material, boundary been set up correctly, but still I don't get about what turbulence model and equation shall be used for my analysis but Ive tried to modify it using different turbulence model.

The mesh quality I think I've been get better mesh

the initial condition, I don't get it how to set this solution

Double precision or not, I've been try it several times

Small time steps to start, I dont get it how it works but Ive been tried it too

[alfianalfarisi]

Originally Posted by Steffen595

dodgy mesh, not enough RAM. Or boundaries not right, does it say it has to make 100% walls in an outlet? or there are some wild velocities somewhere? Run again, stop manually after 10 iterations 9because you know it will crash at 12) and have a look in POST. Maybe there are endless swirls (eddies) , if you do streamline.

The mesh? I think I have a good mesh, the RAM I think 32gb ram is more than enough,
I dont know the boundary, but, I've try with different ship model, and using the same step and method I use, it face no problem.

Hmm, wild velocity, I've tried to check it up, but there's nothing suspicious

[karachun]

Originally Posted by alfianalfarisi

The mesh? I think I have a good mesh

Can you prove that? Some mesh statistics from solver log will be fine.

[Steffen595]

https://www.youtube.com/watch?v=SyU5W-CshP8
this one suggests changing the inflation layer thickness.
how did you set up the model, inlet and outlet?
can you make a picture of your mesh? And one of the velocities in POST?
here is another interesting video:
https://www.youtube.com/watch?v=FT0CCxRROpc
but I reckon something else is fishy. Check pressure at inlet and outlet, that kind of thing.
Did it work with your initial mesh with 43m?
Did you get your units right?
Edit: sometimes its better to start a fresh simulation. Sometimes you overlooked something. Or you clicked around too much and something is stuck somewhere.

[alfianalfarisi]

Originally Posted by karachun

Can you prove that? Some mesh statistics from solver log will be fine.

Here I attach them, actually Ive done several times analyzation, how do you think then?

Mesh Statistic 2.PNG
Mesh Statistic.PNG

[alfianalfarisi]

Originally Posted by Steffen595

https://www.youtube.com/watch?v=SyU5W-CshP8
this one suggests changing the inflation layer thickness.
how did you set up the model, inlet and outlet?
can you make a picture of your mesh? And one of the velocities in POST?
here is another interesting video:
https://www.youtube.com/watch?v=FT0CCxRROpc
but I reckon something else is fishy. Check pressure at inlet and outlet, that kind of thing.
Did it work with your initial mesh with 43m?
Did you get your units right?
Edit: sometimes its better to start a fresh simulation. Sometimes you overlooked something. Or you clicked around too much and something is stuck somewhere.

https://www.youtube.com/watch?v=SyU5W-CshP8
I've tried this solution, but I think that this dont give me any help

Yes, I set it inlet and outlet

I'll get the picture tomorrow, I have the file in my university laboratory.

Actually I've varied it too, not only using 43m, but also with 171 mm for ship, 1710 mm for the water

I think I've tried to start a fresh simulation several times though

[karachun]

Originally Posted by alfianalfarisi

how do you think then?

This is only a number of mesh elements, it tells nothing about element quality.
Can you post a Mesh quality summary or whole .out file?
Also you can post quality plot from Ansys Meshing.

[AtoHM]

karachun, it is hard to see from his post, but there are actually two images there, the second one clearly tells the issue I think.



You have orthogonality angles of merely 1.7 deg inside your domain. No suprise you get errors. I don't know what the actual lowest value allowed is, but I suggest improving the mesh at least until you reach 15 deg. Expansion factor should come down as well, especially for multiphase flows.

[karachun]

Yep, I didn't notice the second picture.

[alfianalfarisi]

Originally Posted by AtoHM

karachun, it is hard to see from his post, but there are actually two images there, the second one clearly tells the issue I think.



You have orthogonality angles of merely 1.7 deg inside your domain. No suprise you get errors. I don't know what the actual lowest value allowed is, but I suggest improving the mesh at least until you reach 15 deg. Expansion factor should come down as well, especially for multiphase flows.

I still dont get What shall I do, but I get this

+--------------------------------------------------------------------+
| Mesh Statistics |
+--------------------------------------------------------------------+
| Domain Name | Orthog. Angle | Exp. Factor | Aspect Ratio |
+----------------------+---------------+--------------+--------------+
| | Minimum [deg] | Maximum | Maximum |
+----------------------+---------------+--------------+--------------+
| Default Domain | 44.5 ok | 16 ok | 7 OK |
+----------------------+---------------+--------------+--------------+
| | %! %ok %OK | %! %ok %OK | %! %ok %OK |
+----------------------+---------------+--------------+--------------+
| Default Domain | 0 <1 100 | 0 2 98 | 0 0 100 |
+----------------------+---------------+--------------+--------------+


What do you think? oh I do single phase analization

[ghorrocks]

These mesh quality numbers are only rough guides. There is no threshold quality level you need to achieve for the simulation to be good. The threshold depends very strongly on what you are modelling - if you are modelling low Reynolds number laminar flow you can handle far worse elements than these quality guides suggest. If you are modelling surface tension or shock waves you need a mesh MUCH better than these guides. For instance, for accurate surface tension modelling to give Laplacian pressure in a droplet you cannot exceed an aspect ratio of 1.5. This is FAR tighter than these guides suggest is "OK". So I don't think these mesh quality guides are very useful most of the time as you don't know what quality you need for accuracy.

If you have time you should do a mesh sensitivity study with varying mesh qualities to see what you can handle and be accurate. But if you don't have time for that then add the residuals to your results file and run your simulation. If it crashes, save a backup file just before it diverges. Then look at the residuals in CFD-Post and see where the high residuals are. This will tell you which area of your mesh is a problem and that is the area you should improve.

[alfianalfarisi]

Originally Posted by ghorrocks

These mesh quality numbers are only rough guides. There is no threshold quality level you need to achieve for the simulation to be good. The threshold depends very strongly on what you are modelling - if you are modelling low Reynolds number laminar flow you can handle far worse elements than these quality guides suggest. If you are modelling surface tension or shock waves you need a mesh MUCH better than these guides. For instance, for accurate surface tension modelling to give Laplacian pressure in a droplet you cannot exceed an aspect ratio of 1.5. This is FAR tighter than these guides suggest is "OK". So I don't think these mesh quality guides are very useful most of the time as you don't know what quality you need for accuracy.

If you have time you should do a mesh sensitivity study with varying mesh qualities to see what you can handle and be accurate. But if you don't have time for that then add the residuals to your results file and run your simulation. If it crashes, save a backup file just before it diverges. Then look at the residuals in CFD-Post and see where the high residuals are. This will tell you which area of your mesh is a problem and that is the area you should improve.

Hmm, I'll try my best for fixing the mesh,

anyway how to do this "look at the residuals in CFD-Post and see where the high residuals are"?

I've check Output Equation Residuals, then what else to show the area with a problematic mesh?

[ghorrocks]

In CFX-Pre, under the output tab/results file there is an option to add residuals to the results file. Select this option, then rerun the simulation. When you look at the results file in CFD-Post it will have some new variables which will be the equation residuals. You can then view it like any other variable in CFD-Post, so use isosurfaces and cross section planes to see where the residuals are high as that will tell you where the problem areas are.