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

Error in probes functions!!!

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   October 12, 2017, 09:37
Default Error in probes functions!!!
  #1
Member
 
Jingxue Wang
Join Date: Sep 2017
Posts: 51
Rep Power: 5
Jingxue Wang is on a distinguished road
Dear all

I am doing a flat roof pressure simulation using LES. I want to observe the pressure in the front of the building.I found a method to use probes. So I add the following codes in controlDict:

Code:
functions
{#includeFunc probes}
And I also made a copy of /opt/openfoam4/etc/caseDicts/postProcessing/probes/probes to the systerm folder of my case. The codes in probes are the following:

probes:
Quote:
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object probes;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

probes
{

#includeEtc "caseDicts/postProcessing/probes/probes.cfg"

writeControl adjustableRunTime;

writeInterval 0.005;

fields ( p );
probeLocations
(
(7.7 0.4 3)
);



}
When I using simple at the terminal, the error happens:
--> FOAM FATAL ERROR:
Unknown functionEntry 'includeFunc' in "/home/olmati/OpenFOAM/olmati-3.0.1/run/Wangjingxue/Flatroof5/system/controlDict" near line 56

Valid functionEntries are :

7
(
inputMode
codeStream
include
calc
remove
includeIfPresent
includeEtc
)


From function functionEntry::execute(const word& functionName, dictionary& parentDict, Istream&)
in file db/dictionary/functionEntries/functionEntry/functionEntry.C at line 83.

FOAM exiting

Could somebody have some idea for this? Many thanks!
Jingxue Wang is offline   Reply With Quote

Old   October 12, 2017, 09:53
Default
  #2
Senior Member
 
Alexey Matveichev
Join Date: Aug 2011
Location: Nancy, France
Posts: 1,924
Rep Power: 35
alexeym has a spectacular aura aboutalexeym has a spectacular aura about
Send a message via Skype™ to alexeym
Hi,

In OpenFOAM 3.0.1 there is no includeFuncEntry (see https://github.com/OpenFOAM/OpenFOAM...unctionEntries). It appeared in version 4 (see https://github.com/OpenFOAM/OpenFOAM...unctionEntries).

So, guess, "some idea" would be "use OpenFOAM 4.x".
alexeym is offline   Reply With Quote

Old   October 12, 2017, 10:04
Default
  #3
Member
 
Jingxue Wang
Join Date: Sep 2017
Posts: 51
Rep Power: 5
Jingxue Wang is on a distinguished road
Quote:
Originally Posted by alexeym View Post
Hi,

In OpenFOAM 3.0.1 there is no includeFuncEntry (see https://github.com/OpenFOAM/OpenFOAM...unctionEntries). It appeared in version 4 (see https://github.com/OpenFOAM/OpenFOAM...unctionEntries).

So, guess, "some idea" would be "use OpenFOAM 4.x".
Hi,alexeym

Many thanks! My openfoam version is 3.0.
I am considering what method should I take to process probe even in Openfoam3.1.Do you have some idea?
I tried the #includeEtc, but the following error existed:

Create time
--> FOAM FATAL IO ERROR:
wrong token type - expected string, found on line 56 the word 'probes'

file: /home/olmati/OpenFOAM/olmati-3.0.1/run/Wangjingxue/Flatroof5/system/controlDict at line 56.

From function operator>>(Istream&, fileName&)
in file primitives/strings/fileName/fileNameIO.C at line 56.

FOAM exiting
Jingxue Wang is offline   Reply With Quote

Old   October 12, 2017, 17:54
Default
  #4
Senior Member
 
Alexey Matveichev
Join Date: Aug 2011
Location: Nancy, France
Posts: 1,924
Rep Power: 35
alexeym has a spectacular aura aboutalexeym has a spectacular aura about
Send a message via Skype™ to alexeym
Hi,

You can try other entries as well or you can just use search on the 3.0.x repository [1] to find out, how you can add probes function object to constrolDict in OpenFOAM 3.0.x.

[1] https://github.com/OpenFOAM/OpenFOAM...q=probes&type=
alexeym is offline   Reply With Quote

Old   October 12, 2017, 21:30
Default
  #5
Member
 
Jingxue Wang
Join Date: Sep 2017
Posts: 51
Rep Power: 5
Jingxue Wang is on a distinguished road
Quote:
Originally Posted by alexeym View Post
Hi,

You can try other entries as well or you can just use search on the 3.0.x repository [1] to find out, how you can add probes function object to constrolDict in OpenFOAM 3.0.x.

[1] https://github.com/OpenFOAM/OpenFOAM...q=probes&type=
hi,alexeym

I will try this.Many thanks for your help!
Jingxue Wang is offline   Reply With Quote

Old   November 25, 2017, 05:39
Default OpenFOAM 5.0: probes and contrlDict error
  #6
New Member
 
Luca Montagliani
Join Date: Nov 2017
Posts: 5
Rep Power: 5
luca_mon is on a distinguished road
Hello guys
I'm new to the forum.
I have this problem ... I have to run a two square tandem simulation and would like to evaluate downstream pressure fluctuations of the two cylinders through probes and probesDict.
When I start the simulation, however, the log file pulls me out of this error:

--> FOAM Warning :
From function virtual void Foam:robes::findElements(const Foam::fvMesh&)
in file probes/probes.C at line 119
Did not find location (0.15 0 0) in any cell. Skipping location.
--> FOAM Warning :
From function virtual void Foam:robes::findElements(const Foam::fvMesh&)
in file probes/probes.C at line 119
Did not find location (0.06 0 0) in any cell. Skipping location.
--> FOAM Warning :
From function virtual void Foam:robes::findElements(const Foam::fvMesh&)
in file probes/probes.C at line 119
Did not find location (1 0 0) in any cell. Skipping location.

ControlDict looks like this:
...
functions
{
#include "forceCoeffs"
#include "forceCoeffs2"
#includeFunc probes
}
CheckMesh says geometry it's OK.
Thanks again for the help you give me.
luca_mon is offline   Reply With Quote

Old   November 25, 2017, 08:18
Default
  #7
Senior Member
 
Alexey Matveichev
Join Date: Aug 2011
Location: Nancy, France
Posts: 1,924
Rep Power: 35
alexeym has a spectacular aura aboutalexeym has a spectacular aura about
Send a message via Skype™ to alexeym
Hi,

In simple case there are two possibilities:

1. You made mistake with probe coordinates. Could you post checkMesh output?

2. Due to mesh cells distribution, these three probes happened to be in between cells. So you just need to move them a little bit, i.e. try 0.149 instead of 0.15.
alexeym is offline   Reply With Quote

Old   November 25, 2017, 10:11
Default
  #8
New Member
 
Luca Montagliani
Join Date: Nov 2017
Posts: 5
Rep Power: 5
luca_mon is on a distinguished road
Quote:
Originally Posted by alexeym View Post
Hi,

In simple case there are two possibilities:

1. You made mistake with probe coordinates. Could you post checkMesh output?

2. Due to mesh cells distribution, these three probes happened to be in between cells. So you just need to move them a little bit, i.e. try 0.149 instead of 0.15.
Hi alexeym, thanks for the reply.
1) The checkMesh output is:
Create time

Create polyMesh for time = 0

Time = 0

Mesh stats
points: 230736
internal points: 0
faces: 458704
internal faces: 227966
cells: 114445
faces per cell: 6
boundary patches: 5
point zones: 0
face zones: 0
cell zones: 1

Overall number of cells of each type:
hexahedra: 114445
prisms: 0
wedges: 0
pyramids: 0
tet wedges: 0
tetrahedra: 0
polyhedra: 0

Checking topology...
Boundary definition OK.
Cell to face addressing OK.
Point usage OK.
Upper triangular ordering OK.
Face vertices OK.
Number of regions: 1 (OK).

Checking patch topology for multiply connected surfaces...
Patch Faces Points Surface topology
Left&Right 228890 230736 ok (non-closed singly connected)
Out 1429 2860 ok (non-closed singly connected)
In 187 376 ok (non-closed singly connected)
Body1 116 232 ok (non-closed singly connected)
Body2 116 232 ok (non-closed singly connected)

Checking geometry...
Overall domain bounding box (-1 -1 0.05) (3 1 0.1)
Mesh has 2 geometric (non-empty/wedge) directions (1 1 0)
Mesh has 2 solution (non-empty) directions (1 1 0)
All edges aligned with or perpendicular to non-empty directions.
Boundary openness (1.86406e-18 6.11543e-19 7.76693e-20) OK.
Max cell openness = 1.66152e-16 OK.
Max aspect ratio = 5.08653 OK.
Minimum face area = 2.2091e-05. Maximum face area = 0.0011521. Face area magnitudes OK.
Min volume = 1.10455e-06. Max volume = 2.65467e-05. Total volume = 0.398. Cell volumes OK.
Mesh non-orthogonality Max: 0 average: 0
Non-orthogonality check OK.
Face pyramids OK.
Max skewness = 4.3599e-13 OK.
Coupled point location match (average 0) OK.

Mesh OK.

End
2) I also tried the second option but it continues to give the same type of error.
luca_mon is offline   Reply With Quote

Old   November 25, 2017, 10:14
Default
  #9
Senior Member
 
Alexey Matveichev
Join Date: Aug 2011
Location: Nancy, France
Posts: 1,924
Rep Power: 35
alexeym has a spectacular aura aboutalexeym has a spectacular aura about
Send a message via Skype™ to alexeym
Your mesh z is in range [0.05, 0.1], so it is not surprising, that probes with z=0 are outside of the domain and are skipped.
alexeym is offline   Reply With Quote

Old   November 25, 2017, 10:21
Default
  #10
New Member
 
Luca Montagliani
Join Date: Nov 2017
Posts: 5
Rep Power: 5
luca_mon is on a distinguished road
Quote:
Originally Posted by alexeym View Post
Your mesh z is in range [0.05, 0.1], so it is not surprising, that probes with z=0 are outside of the domain and are skipped.
Thanks a lot!!!!!
Now is run
luca_mon is offline   Reply With Quote

Reply

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
How to solve the boundary layer without wall functions? WhiteW OpenFOAM Running, Solving & CFD 4 January 20, 2020 05:55
Wall functions ivan-s Main CFD Forum 0 August 25, 2014 13:35
[Commercial meshers] CCM+ Mesh Conversion Ingenieur OpenFOAM Meshing & Mesh Conversion 17 February 2, 2014 10:34
field functions - table crevoise STAR-CCM+ 3 March 26, 2013 10:37
probes function not working in Openfoam 2.1.1 nandiganavishal OpenFOAM 7 July 26, 2012 12:06


All times are GMT -4. The time now is 17:28.