CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > ANSYS > CFX

Fatal overflow in linear solver in mesh deformation

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   May 7, 2016, 10:57
Default Fatal overflow in linear solver in mesh deformation
  #1
New Member
 
Ugo degli Ubaldi
Join Date: May 2016
Location: Palermo, Italy
Posts: 6
Rep Power: 9
billoable is on a distinguished road
Hello guys,
I am a student,
and unfortunately I can not solve a convergence error of my simple problem of fluid dynamics .. laminar flow
I am trying to simulate a breathing movement, in CFX 15 using mesh deformation.

breathing movement = amplitude * sin (2 * pig * t / (2 * period)) * sin (2 * pig * x / (2 * L)) + y0

I tried to change a few parameters, thicken the timestep, improve the mesh, and change the exponent of the stiffness according to the report 1 / wall. But nothing, I always get:
"ERROR # 004100018 has occurred in FINMES subroutine. | | Message: | | Fatal overflow in linear solver."

all boundaries are stationary except the selected wall in green, it is set in the periodic displacement



Is my definition of breathing movement correct?
Tips?

Thanks to everyone in advance
Attached Images
File Type: png Immagine.png (90.1 KB, 19 views)

Last edited by billoable; May 7, 2016 at 12:40.
billoable is offline   Reply With Quote

Old   May 8, 2016, 06:41
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,665
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
FAQ: http://www.cfd-online.com/Wiki/Ansys...do_about_it.3F

As this is a moving mesh simulation this FAQ will be of assistance as well: http://www.cfd-online.com/Wiki/Ansys..._went_wrong.3F (the tip on sending the mesh motion to the results file for debugging is HIGHLY recommended)

After you have looked at these FAQs please post your CCL.
ghorrocks is offline   Reply With Quote

Old   May 8, 2016, 10:53
Default
  #3
New Member
 
Ugo degli Ubaldi
Join Date: May 2016
Location: Palermo, Italy
Posts: 6
Rep Power: 9
billoable is on a distinguished road
thanks a lot for the FAQ ghorrocks!
I read the FAQ before writing this post

- Is the physics of the simulation set up correctly? yes! no error in CFX pre

- Is the mesh of high enough quality? I have used different types of mesh from the more dense to more simple.

- Is a better initial condition required? the problem, without breathing, gives solution!

- Using a coarse mesh and interpolating as an initial condition onto the final mesh? The simulation does not start

- Is double precision required? Yes

- Does the model require small time steps to start? yes

- a better fluid mesh? yes

- meshsiffness 1/wall distance? yes

- smaller timesteps? yes

- If the mesh motion is prescribed (ie not FSI or 6DOF) then you can turn the fluid, turbulence, energy and any other solvers off using an expert parameter. This means the only work the solver is doing is calculating the mesh motion. Obviously this will speed the simulation up immensely? No turbulence, no energy, no scalar. Easy laminar flow.

there are online guided tutorials for using the mesh deformation?
thank you again
billoable is offline   Reply With Quote

Old   May 8, 2016, 20:05
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,665
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
Do a google search and you should find some tutorials. There are also tutorials on the ANSYS customer page.

Can you post your CCL?
ghorrocks is offline   Reply With Quote

Old   May 9, 2016, 05:12
Default
  #5
New Member
 
Ugo degli Ubaldi
Join Date: May 2016
Location: Palermo, Italy
Posts: 6
Rep Power: 9
billoable is on a distinguished road
here is my CCL in .txt

I will try in customer service ansys, I hope to find something to make my case.

good day
Attached Files
File Type: txt for CFD online.txt (19.8 KB, 13 views)
billoable is offline   Reply With Quote

Old   May 9, 2016, 09:13
Default
  #6
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,665
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
You appear to be using mesh motion option of periodic displacement. You probably want to use the specified displacement option as you are defining the motion with your displacement function.

Your specification of the displacement function on the top face but stationary on the side walls is going to lead to highly distorted meshes and is probably not what you intend.

For debugging mesh motion I strongly recommend you do as the FAQ suggests and turn off all the solvers, make it output a results file every time step and run the solver to give a results file containing just the mesh motion. Then you can check the motion is what you intended. In my experience you rarely get the motion right first time so this step is essential in getting mesh motion simulations to work.
ghorrocks is offline   Reply With Quote

Old   December 1, 2016, 13:05
Default
  #7
New Member
 
Amin
Join Date: Nov 2016
Posts: 4
Rep Power: 9
amingh92 is on a distinguished road
Dear Glenn,
would you be able to mention which one of the expert parameters should be on in order to debug the mesh motion, I`m trying to simulate the movement of a train with its exhaust taken into account.
I have the train as the rigid body, with a subdomain surrounding it and the main domain which is the route of my study. I cannot get it to work though.
Please let me know if you have any suggestions for me.

Cheers,
Amin
amingh92 is offline   Reply With Quote

Old   December 1, 2016, 17:07
Default
  #8
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,665
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
The "solve fluids", "solve turbulence" and related expert parameters are use to turn the solvers off and just resolve the mesh motion.

As a side issue - why are you modelling something like that with rigid bodies? It might be more easily modelled with moving mesh, and depending on the situation you are modelling it might be modelled with a stationary mesh.
ghorrocks is offline   Reply With Quote

Old   December 1, 2016, 17:21
Default
  #9
New Member
 
Amin
Join Date: Nov 2016
Posts: 4
Rep Power: 9
amingh92 is on a distinguished road
Thanks for the reply, I`m trying to simulate a moving train at constant speed, while taking into account the wind and the exhaust which is coming out of the train.
I also tried to consider the train as moving wall, but I wasn`t able to get any results.
amingh92 is offline   Reply With Quote

Old   December 1, 2016, 17:30
Default
  #10
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,665
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
Can you post an image of what you are modelling?
ghorrocks is offline   Reply With Quote

Old   December 1, 2016, 17:39
Default
  #11
New Member
 
Amin
Join Date: Nov 2016
Posts: 4
Rep Power: 9
amingh92 is on a distinguished road
Here are two images from my geometryGeom.jpg

Geom2.jpg
amingh92 is offline   Reply With Quote

Old   December 1, 2016, 18:09
Default
  #12
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,665
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
I thought so

This can be modelled with a stationary mesh. There is no need for rigid bodies, mesh motion or anything difficult. Make the upstream inlet have the velocity of the train, and an outlet with zero pressure at the exit. Make the ground a wall with a tangential velocity equal to the velocity of the train. This means you are modelling the train in a constant velocity frame of reference fixed on the train.
ghorrocks is offline   Reply With Quote

Old   December 1, 2016, 18:36
Default
  #13
New Member
 
Amin
Join Date: Nov 2016
Posts: 4
Rep Power: 9
amingh92 is on a distinguished road
Thank you so much for the help, just to make sure though, how should I define the train itself then ?! as wall? not rigid body ?!
amingh92 is offline   Reply With Quote

Old   December 1, 2016, 19:04
Default
  #14
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,665
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
Yes, as a wall. Have a look at the CFX tutorials which model flow past a moving object - for instance the flow around a blunt body, flow over a wing, the hydrofoil and a few others.
ghorrocks is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
CFX FSI Fatal Error unbanana CFX 0 October 3, 2015 06:57
Fatal overflow in linear solver n.soumya CFX 2 August 8, 2015 22:36
fatal linear solver overflow h.mortezaee CFX 2 July 3, 2015 11:35
[snappyHexMesh] snappyHexMesh won't work - zeros everywhere! sc298 OpenFOAM Meshing & Mesh Conversion 2 March 27, 2011 22:11
First steps w moving mesh FOAM FATAL ERROR solver table is empty tehache OpenFOAM Running, Solving & CFD 2 May 14, 2007 05:59


All times are GMT -4. The time now is 03:39.