CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > FLUENT

Fluent: Divide error

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

Reply
 
LinkBack Thread Tools Display Modes
Old   January 16, 2014, 08:32
Default Fluent: Divide error
  #1
Member
 
Harshal
Join Date: Oct 2013
Posts: 51
Rep Power: 5
Harshal is on a distinguished road
Hello all,
I am trying to simulate the aerodynamics of a sports car. I have created the mesh in ICEM and I am now working with Fluent.

Solution method : Default SIMPLE, least sq. based, Second order pressure etc..

Model: Viscous Standard K-omega


Error: After running the simulation, after about 190 simulations, I am getting the error:
Error: / divide; invalid argument [1]; wrong type [not a number]
Error object: -inf

Observations: In the scaled residuals, the continuity graph keeps increasing steadily till it is almost vertical. Also, the wall flux graph, defined on the car body, keeps increasing till it is vertical.

I am using Fluent in double precision mode.

I would be very thankful if some one can help me in solving this problem.

Thanks again,

Harshal
Harshal is offline   Reply With Quote

Old   January 16, 2014, 12:09
Default
  #2
Senior Member
 
Join Date: Nov 2013
Posts: 943
Rep Power: 13
pakk will become famous soon enough
I would look at the results after 180 iterations. Probably one cell is giving problems, look for the cell with the most extreme temperature/pressure/velocity/density. (And in this case 'extreme' should be physically impossible, such as a temperature of 1e180 kelvin.)
Then go back to meshing and improve the mesh in that region.
pakk is offline   Reply With Quote

Old   January 16, 2014, 13:59
Default
  #3
kad
Senior Member
 
Join Date: Feb 2013
Location: Germany
Posts: 173
Rep Power: 14
kad will become famous soon enoughkad will become famous soon enough
What kind of mesh are you using and how is your mesh quality? This I would check first. Some more general recommendations:

Standard k-omega is very picky when it comes to boundary conditions for turbulence quantities. So choose them carefully. You might think of switching to sst formulation or calculating a initial solution with standard k-epsilon model. Further you should start with 1st order methods and switch them to higher order later.
kad is offline   Reply With Quote

Old   January 16, 2014, 15:17
Default
  #4
Member
 
Harshal
Join Date: Oct 2013
Posts: 51
Rep Power: 5
Harshal is on a distinguished road
Quote:
Originally Posted by kad View Post
What kind of mesh are you using and how is your mesh quality? This I would check first. Some more general recommendations:

Standard k-omega is very picky when it comes to boundary conditions for turbulence quantities. So choose them carefully. You might think of switching to sst formulation or calculating a initial solution with standard k-epsilon model. Further you should start with 1st order methods and switch them to higher order later.
Hello kad,
thanks for your reply. I have generated a mesh in ICEM using Robust Octree method. I did mesh check in Fluent and it did not show any problems. Before simulating with k-omega method, I tried with k-epsilon method and faces the same error problem.

Harshal
Harshal is offline   Reply With Quote

Old   January 16, 2014, 15:20
Default
  #5
Member
 
Harshal
Join Date: Oct 2013
Posts: 51
Rep Power: 5
Harshal is on a distinguished road
Quote:
Originally Posted by pakk View Post
I would look at the results after 180 iterations. Probably one cell is giving problems, look for the cell with the most extreme temperature/pressure/velocity/density. (And in this case 'extreme' should be physically impossible, such as a temperature of 1e180 kelvin.)
Then go back to meshing and improve the mesh in that region.
Hello pakk,
thanks for your reply. I'll check for any irregularities. However, I don't know if I can improve some specific part of the mesh. I would probably have to generate the entire mesh again. So, is there any way of fixing this problem in Fluent itself ? Or maybe there is some problem with the boundary conditions. Can you please tell me what the possible reasons could be that would cause such problems ?

Thanks,

Harshal
Harshal is offline   Reply With Quote

Old   January 16, 2014, 17:00
Default
  #6
Senior Member
 
Join Date: Nov 2013
Posts: 943
Rep Power: 13
pakk will become famous soon enough
Quote:
Originally Posted by Harshal View Post
Hello pakk,
thanks for your reply. I'll check for any irregularities. However, I don't know if I can improve some specific part of the mesh. I would probably have to generate the entire mesh again. So, is there any way of fixing this problem in Fluent itself ? Or maybe there is some problem with the boundary conditions. Can you please tell me what the possible reasons could be that would cause such problems ?

Thanks,

Harshal
Something caused divergence. It can have many, many reasons. Look at the almost-diverged data to get an indication of where the problem is, I can not help you from here.
pakk is offline   Reply With Quote

Old   January 16, 2014, 17:06
Default
  #7
kad
Senior Member
 
Join Date: Feb 2013
Location: Germany
Posts: 173
Rep Power: 14
kad will become famous soon enoughkad will become famous soon enough
There can be many reasons as we do not know your case in detail. You named the things to check first yourself; mesh and boundary conditions.
For boundary condions there are a lot of tutorials available on the internet e.g. an one hour tutorial on youtube for meshing and simulating Ahmed body car in Workbench.

Is the mesh a full octree mesh? That would not not be that good as it has bad transition and the boundary layer is not resolved well. You can replacedelete the octree volume mesh and replace it with delaunay and then add prism. Also smooth the mesh. There are several guidelines for doing so on this forum, especially check Simon's Tips and Tricks. I think it is pinned in the sticky thread.

Another common mistake: Is your mesh scaling correct?

Last edited by kad; January 16, 2014 at 22:17.
kad is offline   Reply With Quote

Old   January 17, 2014, 05:24
Default
  #8
Senior Member
 
Join Date: Nov 2013
Posts: 943
Rep Power: 13
pakk will become famous soon enough
My approach to these kinds of problems: simplify your problem until the problem disappears, then you have an idea where the problem is.

Here: do the simulation without the turbulence models, but use a laminar model. Does your solution converge then? If it does, the problem is probably related to the turbulence modeling. If not, search further, for example by taking the energy equation out of the problem (assuming things are isothermal). Does it converge then? If it does, the problem is with the energy equation.

In my experience, if I do this then 95% of the time I find out that the problems are related to a bad mesh. (Skewed elements, low orthogonal quality, etc.) That is why I would advice you to find out where in the geometry these divergence issues originate, and improve the mesh there.

I know that it is annoying and time-consuming to improve a mesh, and it is indeed possible that have to generate the entire mesh again. Still, this is in the end faster than doing numerical tricks in Fluent to deal with a bad mesh. In my experience.

You are using turbulence, with which I have less experience, so if I were you I would use kad's advice on that.
pakk is offline   Reply With Quote

Reply

Tags
divide, error, invalid argument, not a number

Thread Tools
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 On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
2 datas on one plot Akuji ParaView 46 December 1, 2013 15:06
checking the system setup and Qt version vivek070176 OpenFOAM Installation 22 June 1, 2010 12:34
POSDAT problem piotka STAR-CD 4 June 12, 2009 08:43
user subroutine error CFDUSER CFX 2 December 9, 2006 07:31
error while compiling the USER Sub routine CFD user CFX 3 November 25, 2002 16:16


All times are GMT -4. The time now is 00:46.