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

RE: Fluent Read Error

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

Reply
 
LinkBack Thread Tools Display Modes
Old   April 10, 2005, 13:12
Default RE: Fluent Read Error
  #1
Chris
Guest
 
Posts: n/a
Hello again! I managed to make a nice mesh for my 2D parabolic domain around the missile by making an elliptical "transition face" around the missile. I then chose a solver and set the boundary conditions and fluid.

When i read the .msh file in Fluent v5.5 I get "ERROR! cannot change interior.3 to interior because there is only one adjacent cell thread" What does this mean?

Chris
  Reply With Quote

Old   April 10, 2005, 15:44
Default Re: RE: Fluent Read Error
  #2
Chris
Guest
 
Posts: n/a
Can anyone confirm if it's the same problem as Jason kindly solved in:

Help! mesh error- "only one adjacent cell thread." (kuba)
  Reply With Quote

Old   April 10, 2005, 17:57
Default Re: Meshing with united faces
  #3
Chris
Guest
 
Posts: n/a
Ok I know I've replied to my own thread but this is where I am at the moment!

I'v tried a few things and I keep getting an error msg.

When I unite faces 2 and 3 I choose retain so that I can have a fine mesh around the missile and a coarser mesh for the rest of the domain. However, choosing retain means that I get FACE 4, which is everything. I dont want to mesh face 4 because it means the mesh is too coarse for it's purpose.

So when I set all of the boudary conditions etc and export the .msh file Gambit gives an error saying, "face 4 not exported because no mesh exists for it" (roughly). Also, when I specify the fluid am I supposed to choose Face 4 as well or instead of faces 2&3 or not at all?

Then when I read the .msh file in Fluent I get the same error message stating that "ERROR! cannot change interior.3 to interior because there is only one adjacent cell thread"

Can someone please advise the best way to do this? I must be doing something wrong but I don't know what!!!

Chris
  Reply With Quote

Old   April 11, 2005, 03:04
Default Re: Meshing with united faces
  #4
handou
Guest
 
Posts: n/a
don't set the boundary condition as interior. just don't set this boundary, and FLUENT will set it as interior by default.
  Reply With Quote

Old   April 11, 2005, 05:43
Default Re: Meshing with united faces
  #5
Chris
Guest
 
Posts: n/a
Thanks handou. I have a question though. What do I do with Face 4? Nothing? Please clarify! Thanks
  Reply With Quote

Old   April 11, 2005, 08:20
Default Re: Meshing with united faces
  #6
Jason
Guest
 
Posts: n/a
Ok... so the issue is that you're not supposed to be uniting the faces. What's happening is that when you unite faces it forms a single face that covers the area where the two faces were previously. Choosing retain means that you keep the original two faces too. So Face4 is the face created by the unite command, and Faces 2 and 3 are kept because you used the retain option.

The error you're getting about the interior face is because the two faces aren't "connected". It's a different operation than "unite". When you're working in 2D, you want to connect the edges where the two faces touch (in the edge commands, its the button that looks like a black plug being connected). Once you've connected them, you don't have to define a boundary condition. Gambit will ignore the edge and write a continuous mesh.

Really, you should reconsider how you build the geometry. Here's what I recommend:

1) Build or import the missile. 2) Create the large face that represents the entire control volume 3) Subtract the missile from the control volume 4) Create the elliptical "transition" face 5) SPLIT the control volume with the transition face, making sure the that "connect" option is ON and the "retain" option is OFF.

Using the split command with the "connect" option on automatically connects the edge (or edges) where the two faces come together. This way you don't have to go back and check that the edges are connected later on.

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

Old   April 11, 2005, 22:16
Default Re: Meshing with united faces
  #7
zxaar
Guest
 
Posts: n/a
just for curiosity can you read the mesh in gambit back, from .msh file. if you can do you can set the conditions again and re-export it, fluent shall not give any error then. (because if there are descripacies they will show up when u read it again in gambit, like imagine two faces were not connected but you were thinking they are connected , gambit will show u a wall between them..fluent shall also show the same but since its giving error).

try reading it again and see what u can make out of it
  Reply With Quote

Old   April 14, 2005, 13:01
Default Re: Solution! & Turbulence Viscosity Ratio
  #8
Chris
Guest
 
Posts: n/a
Ok, I have connected the two faces and this has solved my problem; No Error msg when i read the file in Fluent. I have also changed the Boundary Conditions to Pressure Far Field after some research.

Can anyone tell me what Turbulence Viscosity Ratio should be used for my simulation? Also, where can I find out how to calculate it?

I am modelling the fluid flow at M0.8 (then M1.2, then M3.0), at 11km.

Coupled, implicit, 2D, steady, energy eqn on, Sp-Al, air = ideal gas, Sutherland law, Pfarfield, Courant No=5
  Reply With Quote

Old   April 14, 2005, 13:59
Default Re: Solution! & Turbulence Viscosity Ratio
  #9
Jason
Guest
 
Posts: n/a
I'm guessing that you mean the turbulent viscosity ratio used in the limits? I've talked to Fluent about this a few times, and they recommend leaving the default of 1e5 (even though they claim thats the viscosity ratio for wet concrete). It has a lot to do with your quality of mesh, airspeed, what you're actually doing to the flow (flow over a sharp corner can give higher values than flow over an airfoil). What I've found is that you can try lowering it (I've gone as low as 50,000, but I've never tried lower) and see how the model reacts. If it comes back and says that X number of cells are limited, but X continues to increase, then you need to increase your limit. If you get that message, but X continues to decrease, then you might even be able to decrease the limit more. From everything I've found, it's on a case by case basis. The point is to limit it to a smaller range than you have now, but not to an unrealistic range. If you limit it to an unrealistic range, you're going to cause unrealistic results.

Hope this helps, and goodluck Jason
  Reply With Quote

Old   April 14, 2005, 17:42
Default Re: Solution! & Turbulence Viscosity Ratio
  #10
Chris
Guest
 
Posts: n/a
Hello Jason,

When I set the conditions of the Pressure Far Field boundary condition. The "Turbulent Viscosity Ratio" appears in the same "box" under gauge pressure etc.

At the moment I'm just sticking with the default of 10 and constant.

Chris
  Reply With Quote

Old   April 14, 2005, 18:14
Default Re: Solution! & Turbulence Viscosity Ratio
  #11
zxaar
Guest
 
Posts: n/a
hello cris, if u are getting this warning that 'turbulent viscosity ration limited to ...' ...then it is coming because the mesh is not fine enough at the regions of high pressure gradient.

i did two calculations (just to see high mach flow), one with fine mesh and one with coarse mesh, with the same geometery , with the setting u have described,, on the coarse mesh fluent always gives this warning and case diverges, on fine mesh fluent do not give this warning, and residuals fall to some level and then try to go up (when this happen, it is time to adapt the mesh in high pressure gradient region), then residuals will again fall down, you have to be playing this game till you get converged results.
  Reply With Quote

Old   April 15, 2005, 11:51
Default Re: Solution! & Turbulence Viscosity Ratio
  #12
Chris
Guest
 
Posts: n/a
zxaar, Fluent gives me that msg when I start the itertions with courant no=5. If however, I use courant no=2 i dont get the msg.

Please Help! My solution WILL NOT converge! It keeps getting close but then diverges again. I have done 6000 iterations at courant no = 2. Then a further 2000 at Courant no = 5. If I increase the courant number after around 3000 iterations the solution diverges!

I only have until Thursday (weds realistically) to finish this project!

Can anyone please look at my .msh file and advise how to improve the mesh.

I also need advice on how to get the solution to converge?

PLEASE HELP!!!

Chris
  Reply With Quote

Old   April 15, 2005, 17:54
Default Re: Solution! & Turbulence Viscosity Ratio
  #13
zxaar
Guest
 
Posts: n/a
mesh is probably not fine enough ...well do one thing please send me the (dbs, trn, jou) with mesh removed (they will be small to send), on monday i will try to give it iteration on my machine,

anyway what is the mesh size you are using
  Reply With Quote

Old   April 16, 2005, 18:56
Default Re: Solution! & Turbulence Viscosity Ratio
  #14
Chris
Guest
 
Posts: n/a
Hello zxaar, I have created a mesh using the mesh edge function. In the main the mesh immediately around the missile (1m radius) is from interval size 0.001 at the missile to interval size 0.1 at the edge of the ellipse. From here until the domain boundaries it extends getting gradually coarser. Hence, I have a fine mesh around the missile and a coarse mesh for the remainder of the computational domain.

I am modelling the fluid flow at M0.8 (then M1.2, then M3.0), at 11km.

Anyway I will email you the files 2moro AM. Many Thanks Chris

Coupled, implicit, 2D, steady, energy eqn on, Sp-Al, air = ideal gas, Sutherland law, Pfarfield, Courant No=5

  Reply With Quote

Reply

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
polynomial thermophysical properties II sebastian OpenFOAM Running, Solving & CFD 53 April 10, 2014 05:45
Building OpenFOAM1.7.0 from source ata OpenFOAM Installation 42 May 14, 2012 20:48
checking the system setup and Qt version vivek070176 OpenFOAM Installation 22 June 1, 2010 12:34
Version 15 on Mac OS X gschaider OpenFOAM Installation 120 December 2, 2009 11:23
OpenFOAM on MinGW crosscompiler hosted on Linux allenzhao OpenFOAM Installation 127 January 30, 2009 20:08


All times are GMT -4. The time now is 13:25.