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

problem with using timeVaryingUniform by icoFoam

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

Like Tree2Likes
  • 1 Post By bigphil
  • 1 Post By wyldckat

Reply
 
LinkBack Thread Tools Display Modes
Old   August 8, 2012, 17:23
Default problem with using timeVaryingUniform by icoFoam
  #1
Member
 
Amin Shariat KHah
Join Date: Apr 2011
Location: Shiraz
Posts: 86
Rep Power: 6
amin144 is on a distinguished road
Hi dear FOAMers
especially Bernhard Gschaider ( usual replier to timeVarying B.C.)

I've read almost all posts about timeVaryingUniform
But I have problem using it
I use OF 1.5-dev and I want to work by viscoelasticFluidFoam solvers
what should I do ? what's the problem ? should I compile anything?

Thanks very much

Error:

Reading field p

Reading field U

Reading/calculating face flux field phi


Starting time loop

Time = 0.005

Courant Number mean: 0 max: 0 velocity magnitude: 0
PBiCG: Solving for Ux, Initial residual = 1, Final residual = 7.46317e-06, No Iterations 5
PBiCG: Solving for Uy, Initial residual = 0, Final residual = 0, No Iterations 0



gradientInternalCoeffs cannot be called for a genericFvPatchField (actual type timeVaryingUniform)
on patch inlet of field p in file "/home/amin/OpenFOAM/amin-1.5-dev/run/cavity/0/p"
You are probably trying to solve for a field with a generic boundary condition.

From function genericFvPatchField<Type>::gradientInternalCoeffs( ) const
in file fields/fvPatchFields/basic/generic/genericFvPatchField.C at line 692.

FOAM exiting


0/p:

boundaryField
{
inlet
{

type timeVaryingUniform;
timeDataFileName "inlet.dat";
value uniform 1e5 ;
}
outlet
{
type fixedValue;
value uniform 0;
}

wallup
{
type zeroGradient;
}
walllow
{
type zeroGradient;
}

frontAndBack
{
type empty;
}
}

inlet.dat:


(
0 1
.01 5
.02 10
.03 20
.07 100
)
amin144 is offline   Reply With Quote

Old   August 8, 2012, 17:40
Default case file
  #2
Member
 
Amin Shariat KHah
Join Date: Apr 2011
Location: Shiraz
Posts: 86
Rep Power: 6
amin144 is on a distinguished road
I attached case file for simplicity
Attached Files
File Type: gz testCaseTVU0.tar.gz (69.2 KB, 11 views)

Last edited by amin144; August 8, 2012 at 18:52.
amin144 is offline   Reply With Quote

Old   August 9, 2012, 09:43
Default
  #3
Member
 
Amin Shariat KHah
Join Date: Apr 2011
Location: Shiraz
Posts: 86
Rep Power: 6
amin144 is on a distinguished road
AnyBody answer me this simple question?
amin144 is offline   Reply With Quote

Old   August 9, 2012, 10:25
Default
  #4
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,258
Blog Entries: 34
Rep Power: 84
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
Hi Amin,

Quote:
Originally Posted by amin144 View Post
I use OF 1.5-dev and I want to work by viscoelasticFluidFoam solvers
what should I do ? what's the problem ? should I compile anything?
I'm not even certain you know what you're asking!

The viscoelasticFluidFoam solver is available in the OpenFOAM variant 1.6-ext, not 1.5-dev. There you will also find tutorials on how to use this solver.
edit: wait, I'm wrong. I completely forgot that they were already present in 1.5-dev Sorry about that. But still, I can't fully understand the question...

Good luck!
Bruno

Last edited by wyldckat; August 9, 2012 at 10:30. Reason: see "edit:"
wyldckat is offline   Reply With Quote

Old   August 9, 2012, 10:27
Default I'm happy
  #5
Member
 
Amin Shariat KHah
Join Date: Apr 2011
Location: Shiraz
Posts: 86
Rep Power: 6
amin144 is on a distinguished road
Quote:
Originally Posted by amin144 View Post
I attached case file for simplicity
I could do my job by using GroovyBC and this thread:
time varying vector boundary condition using patch normal

I attached my case in order to using of others.
I should mention that I used myIcoFoam solver which it's different to icoFoam is adding the line " -lgroovyBC " to "option" file and compile new solver.

After all I'll be happy if someOne say my fault in using timeVaryingUniform
Attached Files
File Type: gz testCaseGroovyBC0.tar.gz (69.5 KB, 3 views)
amin144 is offline   Reply With Quote

Old   August 9, 2012, 10:33
Default
  #6
Member
 
Amin Shariat KHah
Join Date: Apr 2011
Location: Shiraz
Posts: 86
Rep Power: 6
amin144 is on a distinguished road
Hi dear Bruno
Thanks again
I swear GOD I'm not a confused man ( the way you think )
I know what I'm saying

The viscoelastic solver exist in 1.5 dev like 1.6 ext
My problem is using the boundary condition "timeVaryingUniform" not using solver
I appreciat if you can upload me a case using this kind of boundary condition
amin144 is offline   Reply With Quote

Old   August 9, 2012, 10:50
Default
  #7
Senior Member
 
bigphil's Avatar
 
Philip Cardiff
Join Date: Mar 2009
Location: Dublin,Ireland
Posts: 565
Rep Power: 19
bigphil will become famous soon enoughbigphil will become famous soon enough
Quote:
Originally Posted by amin144 View Post
gradientInternalCoeffs cannot be called for a genericFvPatchField (actual type timeVaryingUniform)
on patch inlet of field p in file "/home/amin/OpenFOAM/amin-1.5-dev/run/cavity/0/p"
You are probably trying to solve for a field with a generic boundary condition.

From function genericFvPatchField<Type>::gradientInternalCoeffs( ) const
in file fields/fvPatchFields/basic/generic/genericFvPatchField.C at line 692.

FOAM exiting
Hi Amin,

this errors essentially means that the solver can't find the timeVaryingUniform boundary condition.

In OpenFOAM-1.6-ext, there doesn't seem to be a boundary condition called "timeVaryingUniform".

If you check in the directory $FOAM_SRC/finiteVolume/fields/fvPatchFields/derived, you can see the time varying boundary conditions, they are:
timeVaryingFlowRateInletVelocity
timeVaryingMappedTotalPressure
timeVaryingUniformTotalPressure
timeVaryingMappedFixedValue
timeVaryingUniformFixedValue
timeVaryingMappedPressureDirectedInletVelocity
timeVaryingUniformInletOutlet

Maybe you mean to use one of these?

Best regards,
Philip
amin144 likes this.
bigphil is offline   Reply With Quote

Old   August 9, 2012, 18:38
Default
  #8
Member
 
Amin Shariat KHah
Join Date: Apr 2011
Location: Shiraz
Posts: 86
Rep Power: 6
amin144 is on a distinguished road
Hi dear philip
Thanks for your quick reply

I have used timeVaryingUniformFixedValue but it doesn't work

maybe ma data file is not correct or maybe I should add any library to solver and recompile it
I'm confused
amin144 is offline   Reply With Quote

Old   August 9, 2012, 19:23
Default
  #9
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,258
Blog Entries: 34
Rep Power: 84
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
Hi Amin,

You're lucky I had a 1.5-dev build in my machine. I've taken a look at the first case you provided and the modified version is attached.

Changes:
  • I had to fix "wallup" as "Wallup" in the files at the "0" folder.
  • Saw the list of possible BCs by running this command (1.5-dev is really old... the "bananas" trick didn't work ):
    Code:
    tree $FOAM_SRC/finiteVolume/fields/fvPatchFields
  • Switched to "timeVaryingUniformFixedValue" in the file "0/p".
  • icoFoam started complaining about missing info. To be in compliance with the complaints, I ended up with:
    Code:
    inlet
    {
         type timeVaryingUniformFixedValue;
         outOfBounds clamp;
         fileName "inlet.dat";
         value uniform 1e5 ;
    }
  • Also had to modify "inlet.dat" to something more... compliant:
    Code:
    (
     (0.0 1.0)
     (0.01 5 )
     (0.02 10)
     (0.03 20)
     (0.07  100)
    );
Have fun trying to make this work, because with me, icoFoam just blasted the Courant number out of the ballpark...

Best regards,
Bruno
Attached Files
File Type: gz testCaseTVU_mod.tar.gz (67.5 KB, 8 views)
amin144 likes this.
wyldckat is offline   Reply With Quote

Old   August 10, 2012, 13:18
Default
  #10
Member
 
Amin Shariat KHah
Join Date: Apr 2011
Location: Shiraz
Posts: 86
Rep Power: 6
amin144 is on a distinguished road
oh!
What a nice and great favor from you
Thanks dear Bruno

I wish I can help others in future in this forum
Atthaching cases is a good job because someone else who have problem like me can solve his/her problem very very quickly
amin144 is offline   Reply With Quote

Old   August 10, 2012, 13:35
Default
  #11
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,258
Blog Entries: 34
Rep Power: 84
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
Quote:
Originally Posted by amin144 View Post
Atthaching cases is a good job because someone else who have problem like me can solve his/her problem very very quickly
Or they'll simply go deeper into trouble... of not knowing what they're doing
wyldckat is offline   Reply With Quote

Old   August 11, 2012, 05:05
Default
  #12
Member
 
Amin Shariat KHah
Join Date: Apr 2011
Location: Shiraz
Posts: 86
Rep Power: 6
amin144 is on a distinguished road

But there isn't any known and clear reference to understanding deeply
maybe trial and error is a way for learning OF
It would be nice and great work if there be a extended and expanded user guide which is summarize of threads in forum
amin144 is offline   Reply With Quote

Old   August 11, 2012, 06:09
Default
  #13
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,258
Blog Entries: 34
Rep Power: 84
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
Quote:
Originally Posted by amin144 View Post
It would be nice and great work if there be a extended and expanded user guide which is summarize of threads in forum
Yes it would be great work... and a lot of work... and a lot of time! And very... veeeery tedious

Nonetheless, there are at least 2 places where you or anyone else can do this kind of information collection and cataloguing:
And as you can see from my signature link, my focus here at the forum has been of cataloguing the installation methods and some other details...
wyldckat is offline   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
UDF compiling problem Wouter Fluent UDF and Scheme Programming 6 June 6, 2012 04:43
Problem Importing Geometry ProE to CFX fatb0y CFX 3 January 14, 2012 20:42
Convergence Problem icoFoam steady flow over an airfoil Lucas OpenFOAM Running, Solving & CFD 5 February 18, 2011 13:46
natural convection problem for a CHT problem Se-Hee CFX 2 June 10, 2007 06:29
Adiabatic and Rotating wall (Convection problem) ParodDav CFX 5 April 29, 2007 19:13


All times are GMT -4. The time now is 19:06.