CFD Online Logo CFD Online URL
Home > Forums > Software User Forums > ANSYS > FLUENT

why can't use segerated solver?

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

LinkBack Thread Tools Search this Thread Display Modes
Old   June 2, 2006, 22:56
Default why can't use segerated solver?
Posts: n/a
Hello,everyone! what's the difference between the segerated solver and the coupled solver? i can use the coupled solver to compute. but when i use the the segerated solver to compute, there will be an error like this:"absolute pressure limited to 1.000000e+000 in 18 cells on zone 2 turbulent viscosity limited to viscosity ratio of 1.000000e+005 in 81 cells" why? the material is idea-gas, thanks to every who can answer my question. my email is ""
  Reply With Quote

Old   June 2, 2006, 23:57
Default Re: why can't use segerated solver?
manoj korde
Posts: n/a
You check ur initilization condition Also u can increase the limit for turbulent viscosity ( It can be change from Solutuin control limit panel) i hope this will solve ur problem

  Reply With Quote

Old   June 3, 2006, 01:03
Default Re: why can't use segerated solver?
Posts: n/a
thank you i have tried what you said ,but it does not work. maybe, it doesn't converge

  Reply With Quote

Old   June 5, 2006, 08:51
Default Re: why can't use segerated solver?
Posts: n/a
Choice of solvers depends heavily on the model being solved. The segregated solver solves based on the pressure, while the coupled solver solves based on density. This makes the segregated solver better at low speed flows and the coupled solver better at solving transonic / supersonic cases. I wouldn't recommend the coupled solver at any flows below Mach .4 (until the pressure based coupled solver comes out in the next release of Fluent). I've used the Segregated solver up to Mach 1.5 with great results, but the higher speed, the more mesh dependent you become (because the segregated solver tends to "smooth out" shocks), so you have to pay a lot of attention to your meshing.

The coupled solver tends to be more stable with the defaults settings. The segregated solver tends to be very sensitive to the allowable limits. When trying to get a solution with the segregated solver, DO NOT increase the turbulent viscosity ratio limit (unless you have a great reason to based on past experience or the physics of your current model truly exceeding that limit, but I've never even heard of that being realistic). Instead limit the pressure and temperature limits to reasonable limits (i.e. Plimits = Pstatic +/- (2 * dynamic pressure), and calculate the appropriate temps). You need to give the solution "room to move" while it reaches a solution, but you don't want to give it enough room where it goes out to some totally impossible numbers, and the limits help prevent this.

The other thing to look at is to find the area that's giving the TVR warning (use the Plot->Contours, select the volume and then play with the limits so that you can just see the areas that have very high TVRs) and check the mesh in these areas. Is it refined enough? Is there highly skewed elements? High aspect ratios? Are the surfaces messed up for some reason? These kinds of things.

Hope this helps, and good luck, Jason
  Reply With Quote


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
A New Solver for Supersonic Combustion nakul OpenFOAM Announcements from Other Sources 19 February 27, 2024 09:44
[Other] A New Solver for Supersonic Combustion nakul OpenFOAM Community Contributions 20 February 22, 2019 09:08
thobois class engineTopoChangerMesh error Peter_600 OpenFOAM 4 August 2, 2014 09:52
Quarter Burner mesh with periosic condition SamCanuck FLUENT 2 August 31, 2011 11:34
why the solver reject it? Anyone with experience? bearcat CFX 6 April 28, 2008 14:08

All times are GMT -4. The time now is 02:51.