CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > OpenFOAM > OpenFOAM Running, Solving & CFD

planeWall2D tutorial: error running chtMultiRegionSimpleFoam

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

Like Tree4Likes
  • 2 Post By Dreoasteh
  • 2 Post By Dreoasteh

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   September 19, 2017, 07:09
Post planeWall2D tutorial: error running chtMultiRegionSimpleFoam
  #1
Member
 
Marc
Join Date: May 2017
Posts: 42
Rep Power: 9
Dreoasteh is on a distinguished road
Hello,

I've been trying to run the planeWall2D tutorial in OpenFOAM 4.1 in order to understand how to set up a chtMultiRegionSimpleFoam case. However, there seems to be a problem running the case when the solver chtMultiRegionSimpleFoam is invoked.

This is the error from the chtMultiRegionSimpleFoam log:

Code:
--> FOAM FATAL ERROR: 
Unknown Function1 type uniform for Function1 meanValue

Valid Function1 types are:

7
(
constant
csvFile
polynomial
sine
square
table
tableFile
)



    From function static Foam::autoPtr<Foam::Function1<Type> > Foam::Function1<Type>::New(const Foam::word&, const Foam::dictionary&) [with Type = double]
    in file /home/ubuntu/OpenFOAM/OpenFOAM-4.1/src/OpenFOAM/lnInclude/Function1New.C at line 60.

FOAM exiting
How could I go about solving this issue?

Thanks you!

Edit: other chtMultiRegionSimpleFoam cases (like the ones provided in the tutorials that come with OpenFOAM) do run without this error.
vs1 and jackjiang1989 like this.

Last edited by Dreoasteh; September 20, 2017 at 08:11.
Dreoasteh is offline   Reply With Quote

Old   September 28, 2017, 05:28
Default
  #2
Member
 
Marc
Join Date: May 2017
Posts: 42
Rep Power: 9
Dreoasteh is on a distinguished road
Found the problem! It was in the boundary condition definition for p_rgh.

At least in my build, this boundary condition is not supported/gives errors:

Code:
        type            fixedMean;
        value           uniform 100000;
        meanValue       uniform 100000;
Dreoasteh is offline   Reply With Quote

Old   November 9, 2017, 04:35
Default
  #3
New Member
 
Join Date: Nov 2017
Posts: 1
Rep Power: 0
Archy is on a distinguished road
Hi Marc,

i have the exact same error. The case still does not work when i change the boundary conditions you mentioned above. How exactly did you change the bc?

regards
Archy
Archy is offline   Reply With Quote

Old   November 9, 2017, 10:48
Default
  #4
Member
 
Marc
Join Date: May 2017
Posts: 42
Rep Power: 9
Dreoasteh is on a distinguished road
Hi Archy,

Well basically you can:
    1. Write the proposed BC correctly:
      In system/*Air/changeDictionaryDict instead of:
      Code:
              rightLet
              {
                  type            fixedMean;
                  meanValue uniform 1e5;
                  value           uniform 1e5;
              }
      Write:

      Code:
              rightLet
              {
                  type            fixedMean;
                  meanValue       1e5;
                  value           uniform 1e5;
              }
      Which works for me
    2. Or you can define another boundary condition such as:

      Code:
          rightLet
          {
              type            fixedValue;
              value           $internalField;
          }
      Or explore other options. This pdf has a nice explanation of different BC which might be useful.
chenhu and sweet_satan like this.
Dreoasteh is offline   Reply With Quote

Reply

Tags
chtmulitregionfoam, conjgate heat transfer, fatal error, openfoam 4.1

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
tutorial files KITetima FLUENT 8 November 23, 2019 16:05
AMI - Propeller Tutorial diverging kingmaker OpenFOAM Running, Solving & CFD 2 November 4, 2016 02:57
Tutorial For Workbench CFX Remesh ashtonJ CFX 2 April 26, 2014 21:19
Fluent Tutorial Guide Ch. 17: Non-Premixed Combust, THTR MAE7509 FLUENT 0 January 22, 2014 20:59
STAR-CD Tutorial shekhar aryal STAR-CD 4 March 22, 2010 03:25


All times are GMT -4. The time now is 06:01.