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

reconstructPar --> fileName::stripInvalid() called for invalid fileName commandtouse

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

Like Tree5Likes
  • 1 Post By nimasam
  • 1 Post By nimasam
  • 3 Post By wyldckat

Reply
 
LinkBack Thread Tools Display Modes
Old   July 3, 2009, 11:15
Default reconstructPar --> fileName::stripInvalid() called for invalid fileName commandtouse
  #1
Member
 
Adam Donaldson
Join Date: Mar 2009
Location: Ottawa, Ontario, Canada
Posts: 37
Rep Power: 8
adona058 is on a distinguished road
I am attempting to set up my dual-core computer to use MPIRUN with a case that I am running.

I decomposed the file, ran MPIRUN without a problem, and the results are distributed within the Processor0 and Processor1 directories as expected. Note that I have run MANY parallel cases on a larger network cluster in the past, so I am familiar with the general process.

The problem I am encountering occurs when I attempt to use reconstructPar to reconstruct the results. The terminal output is as follows:

reconstructPar
/*---------------------------------------------------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 1.5.x |
| \\ / A nd | Web: http://www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
Exec : reconstructPar
Date : Jul 03 2009
Time : 11:02:57
Host : adona058-laptop
PID : 27442
Case : /home/adona058/OpenFOAM/adona058-1.5.x/run/taylorBubbleParallel
nProcs : 1

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

fileName::stripInvalid() called for invalid fileName commandtouse
For debug level (= 2) > 1 this is considered fatal
Aborted



I would appreciate it if someone could get back to me on why this is occuring. I can set the debug level to 0 to avoid it, but I would rather know that the program is executing correctly.

Thanks,

Adam
adona058 is offline   Reply With Quote

Old   July 3, 2009, 12:53
Default
  #2
Super Moderator
 
Mattijs Janssens
Join Date: Mar 2009
Posts: 1,416
Rep Power: 16
mattijs is on a distinguished road
you have an invalid named file somewhere. After stripping out the invalid characters it is 'commandtouse'.
mattijs is offline   Reply With Quote

Old   November 19, 2009, 12:46
Default
  #3
Senior Member
 
Steve Hansel
Join Date: Jun 2009
Location: Colorado, USA
Posts: 112
Rep Power: 8
hansel is on a distinguished road
Quote:
Originally Posted by mattijs View Post
you have an invalid named file somewhere. After stripping out the invalid characters it is 'commandtouse'.
I have the same problem and my file names aren't using any strange characters. Is there a length limit for the entire path and file name?
hansel is offline   Reply With Quote

Old   November 20, 2009, 03:21
Default
  #4
Senior Member
 
Mark Olesen
Join Date: Mar 2009
Location: http://olesenm.github.io/
Posts: 777
Rep Power: 18
olesen will become famous soon enough
Quote:
Originally Posted by hansel View Post
I have the same problem and my file names aren't using any strange characters. Is there a length limit for the entire path and file name?
The only real length limit would be INT_MAX, which likely isn't a problem (your filesystem will likely have problems first).

Could you post which file name is getting stripped, so we can reproduce the problem. For reference, here is what src/OpenFOAM/primitives/strings/fileName/fileNameI.H states:

Code:
inline bool Foam::fileName::valid(char c)
{
    return
    (
        !isspace(c)
     && c != '"'   // string quote
     && c != '\''  // string quote
    );
}
Thus whitespace and quotes are the only things it could (should) be complaining about.
olesen is offline   Reply With Quote

Old   November 20, 2009, 11:32
Default
  #5
Senior Member
 
Steve Hansel
Join Date: Jun 2009
Location: Colorado, USA
Posts: 112
Rep Power: 8
hansel is on a distinguished road
The filename it was working on was:
/storage/OpenFOAM_cases/lenz2_size_exp/len2_18in_tsr06_halftail

The error message would report the name but leave off the _halftail part.

Changing the name to /storage/OpenFOAM_cases/lenz2_size_exp/len2_18inht_tsr06 made the problem go away.

I'm pretty sure I didn't have any spaces in the name, but since I changed it I can't be 100% sure.

This happened with 1.5dev, so you may not want to bother with it.
hansel is offline   Reply With Quote

Old   April 14, 2010, 10:35
Default Too long path name
  #6
Senior Member
 
Join Date: Apr 2010
Posts: 151
Rep Power: 7
flowris is on a distinguished road
Hansel, Olesen,


I also tried to run blockMesh on a very deeply nested set of files, and it got the same error. When i copied the folder to my desktop, I could run it.
flowris is offline   Reply With Quote

Old   April 14, 2010, 15:48
Default
  #7
Super Moderator
 
Mattijs Janssens
Join Date: Mar 2009
Posts: 1,416
Rep Power: 16
mattijs is on a distinguished road
Is this 16x on linux? We have not been able to reproduce the problem - do you have an example?
mattijs is offline   Reply With Quote

Old   April 15, 2010, 03:26
Default deeply nested
  #8
Senior Member
 
Join Date: Apr 2010
Posts: 151
Rep Power: 7
flowris is on a distinguished road
Goeiemorgen Mattijs,

I tried to run the interFoam tutorial by Hassan Hemida. The files can be downloaded from http://www.tfd.chalmers.se/~hani/kurser/OS_CFD_2007/. I nested everything very deeply in my file structure , namely in:

Documents/OpenFOAM\ info/Chalmers/interFoam/fillBottle/lamFillBottle/

However, some other minor difficulties occurred with these files. I had to change some names of parameters like gamma to alpha and pd to p in the system files. I also had to add files like constant/turbulenceProperties and constant/g. Is this because the tutorial was written for an older version of interFoam? I am using OpenFOAM-1.6.


Joris
flowris is offline   Reply With Quote

Old   April 15, 2010, 04:01
Default
  #9
Senior Member
 
Mark Olesen
Join Date: Mar 2009
Location: http://olesenm.github.io/
Posts: 777
Rep Power: 18
olesen will become famous soon enough
Quote:
Originally Posted by flowris View Post
I tried to run the interFoam tutorial by Hassan Hemida. The files can be downloaded from http://www.tfd.chalmers.se/~hani/kurser/OS_CFD_2007/. I nested everything very deeply in my file structure , namely in:

Documents/OpenFOAM\ info/Chalmers/interFoam/fillBottle/lamFillBottle/
Spaces in directory and file names are pure poison for OpenFOAM (and several other bits of Unix software). Try renaming to something without space/tab etc and see if that does the trick.
olesen is offline   Reply With Quote

Old   December 23, 2013, 11:40
Default
  #10
New Member
 
ahmad taheri
Join Date: Oct 2013
Posts: 4
Rep Power: 3
taheri.atp is on a distinguished road
hi
I have this problem too!
I can run blockMesh but when I want too see my mesh in ParaFOAM I get this answer:

fileName::stripInvalid() called for invalid fileName /home/ahmad/Desktop/tpfoch/system/fvSolution::solvers:U|k|epsilon)
For debug level (= 2) > 1 this is considered fatal

can you help me to solve this problem?
taheri.atp is offline   Reply With Quote

Old   December 25, 2013, 02:55
Default
  #11
Senior Member
 
Nima Sam
Join Date: Sep 2009
Location: Tehran, Iran
Posts: 1,124
Blog Entries: 1
Rep Power: 14
nimasam is on a distinguished road
Send a message via Yahoo to nimasam
Dear Ahmad

it return to files names usually, check that you have no extra space or unusual file name, another suggestion can be that you can copy your blockMeshDict into icoFoam/cavity , then run blockMesh and see whether it works or not
taheri.atp likes this.
__________________
Training Course on OpenFOAM at (http://www.isme.ir/)
My Weblog (http://openfoam.blogfa.com/)
nimasam is offline   Reply With Quote

Old   December 25, 2013, 03:11
Default
  #12
New Member
 
ahmad taheri
Join Date: Oct 2013
Posts: 4
Rep Power: 3
taheri.atp is on a distinguished road
Quote:
Originally Posted by nimasam View Post
Dear Ahmad

it return to files names usually, check that you have no extra space or unusual file name, another suggestion can be that you can copy your blockMeshDict into icoFoam/cavity , then run blockMesh and see whether it works or not
wow!
I copied blockMeshDict to cavity and it worked!!!!
what does it mean?!?!?!
taheri.atp is offline   Reply With Quote

Old   December 25, 2013, 03:18
Default
  #13
Senior Member
 
Nima Sam
Join Date: Sep 2009
Location: Tehran, Iran
Posts: 1,124
Blog Entries: 1
Rep Power: 14
nimasam is on a distinguished road
Send a message via Yahoo to nimasam
it means nothing, means you should create a new test case or find where the typo is,
as i said it usually returns to bad file name
taheri.atp likes this.
__________________
Training Course on OpenFOAM at (http://www.isme.ir/)
My Weblog (http://openfoam.blogfa.com/)
nimasam is offline   Reply With Quote

Old   December 25, 2013, 06:37
Default
  #14
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,516
Blog Entries: 34
Rep Power: 86
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
Greetings to all!

Since this is a frequently asked question, I've added to the FAQ: http://openfoamwiki.net/index.php/FA..._invalid.22.3F

Best regards,
Bruno
maybee, chinafly and taheri.atp like this.
wyldckat is offline   Reply With Quote

Old   June 7, 2014, 12:06
Default stripInvalid() with patch names
  #15
New Member
 
Dominik Pöltl
Join Date: Jul 2013
Location: Hamburg
Posts: 14
Rep Power: 4
Yeru is on a distinguished road
Hi foamers,

in order to get familiar with OF and especially groovyBC, I'm currently trying to get a case of 2 cyclically linked patches to work (according to this example in the wiki).

Here's where the relation to this thread comes in:
simpleFoam stops after having calculated u in the first timestep (after startTime) with this:
Code:
word::stripInvalid() called for word p_Rect0front
    For debug level (= 2) > 1 this is considered fatal
What's p_Rect0front?
There are <PatchName>_front and <PatchName>_back for every patch in the inlet and outlet.
In my 0/p-file, in order to use groovyBC, I defined:
Code:
boundaryField{
[...]
innerRect0_front
{
    type        groovyBC;
    variables       "p_Rect0back{innerRect0_back}=sum(p*mag(Sf()))/sum(mag(Sf()));    p_Rect0front=sum(p*mag(Sf()))/sum(mag(Sf()));    f_relax=0.5;";
    valueExpression "(p_Rect0front + f_relax*(p_Rect0back - p_Rect0front))";
    value        $internalField;
    }
    innerRect0_back
    {
        type            zeroGradient;
    }
The problem will not be any special characters or length of the variables, since the wiki example uses
Code:
p_int22
, so including numbers and an underscore.

Any ideas?
Yeru is offline   Reply With Quote

Old   June 7, 2014, 17:42
Default
  #16
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,516
Blog Entries: 34
Rep Power: 86
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
Greetings Dominik,

I've Googled just now for:
Code:
site:www.cfd-online.com stripInvalid groovyBC
and found this post by Bernhard from 2012: Problem: Defining a linear scalar BC with groovyBC post #2

Essentially you cannot have spaces inside the variables expressions, otherwise they'll count as part of the variable names. This is essentially exemplified in the wiki page section you indicated, where not a single space is present in the variables expressions!

And if you're wondering why this is still a problem since 2012, it's probably because no one has taken the time to report this on the bug tracker for swak4Foam/groovyBC .

Best regards,
Bruno
wyldckat is offline   Reply With Quote

Old   June 8, 2014, 05:24
Default stripInvalid() with patch names - SOLVED
  #17
New Member
 
Dominik Pöltl
Join Date: Jul 2013
Location: Hamburg
Posts: 14
Rep Power: 4
Yeru is on a distinguished road
Dear Bruno,

thanks a lot! It's sufficiently working now.
I'm sorry for stirring this up when a simple "google it" is the answer.
Anyway, thanks again,

Dominik
Yeru is offline   Reply With Quote

Old   June 2, 2015, 02:29
Default Problem while converting .msh to openFoam
  #18
New Member
 
Mayur Bhandari
Join Date: May 2015
Posts: 8
Rep Power: 2
bmayurm is on a distinguished road
I am using command fluentMeshToFoam to convert .msh fluent mesh (from ICEM) to openfoam format.
The error is same above
for debug level (= 2) 1 this is considered fatal aborted (core dumped).
Please help. I'm New in this
bmayurm is offline   Reply With Quote

Old   June 12, 2015, 18:47
Default
  #19
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,516
Blog Entries: 34
Rep Power: 86
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
Quote:
Originally Posted by bmayurm View Post
Please help. I'm New in this
Not enough information. Please follow the instructions given on this thread: How to give enough info to get help
wyldckat is offline   Reply With Quote

Reply

Tags
commandtouse, filename, reconstructpar, stripinvalid

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
reconstructParMesh not working with an axisymetric case francesco OpenFOAM Bugs 4 May 8, 2009 05:49


All times are GMT -4. The time now is 23:59.