CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > SU2

an error when Paraview try to input flow.vtk

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

Reply
 
LinkBack Thread Tools Display Modes
Old   January 28, 2013, 08:24
Default an error when Paraview try to input flow.vtk
  #1
Senior Member
 
Cean
Join Date: Feb 2010
Posts: 128
Rep Power: 7
shirazbj is on a distinguished road
Hi,

I am playing with TestCases\rotating\open_rotor.

When input flow.vtk with Paraview, I got an error sasying Error reading assii dat.

I opened the vtk file and saw the lookup_table for scalars mac_number like this:
-1.#IND000000000

Is this the problem?

Regards

Cean
Attached Images
File Type: jpg vtkerr.JPG (23.6 KB, 11 views)
File Type: jpg sca.JPG (22.0 KB, 11 views)
shirazbj is offline   Reply With Quote

Old   January 29, 2013, 00:34
Default
  #2
Senior Member
 
Cean
Join Date: Feb 2010
Posts: 128
Rep Power: 7
shirazbj is on a distinguished road
Just tried another testcase, and found its output to the terminal also have the -1.#IND00 value.

no wonder the VTK will have the same value.
Attached Images
File Type: gif ind.GIF (16.4 KB, 10 views)
shirazbj is offline   Reply With Quote

Old   January 29, 2013, 15:23
Default
  #3
Super Moderator
 
Thomas D. Economon
Join Date: Jan 2013
Location: Stanford, CA
Posts: 260
Rep Power: 5
economon is on a distinguished road
Thanks for trying the code and letting us know about issues with Paraview. A couple of thoughts:

1. What type of machine/OS are you using?

2. While the open rotor case is provided with the code (it is a little older, maybe out of date), I would recommend trying the rotating NACA 0012 which is simpler. If you try to view the output in Paraview with this case does it work? What about the transonic NACA 0012 case (not rotating)?

It could be something related to the Paraview file writer that is specific to rotating cases, so please let us know if you can isolate it with a few tests.
economon is offline   Reply With Quote

Old   January 29, 2013, 21:04
Default
  #4
Senior Member
 
Cean
Join Date: Feb 2010
Posts: 128
Rep Power: 7
shirazbj is on a distinguished road
Hi Thomas,

It's only the Mach number has this problem for this open rotor case. But from my second post using another test case, I realised the simulation is generating this data and output to screen.

I googled "1.#QNAN00000000" and found out it's the way "printf" deal with a huge number. So something is sort of divided by zero.

I am using win7-32b. I compiled the source with gcc for win and can now trace the program now. I found in output_structure.cpp when caculate Mach number:
Code:
                WriteInOutputFile(geometry, solution_container[FLOW_SOL], ConsVar_file, "Mach_Number", scalar,  0, "GetMach", config);
In WriteInOutputFile sub,
Code:
                if (!incompressible) {
                      mach_number = sqrt(solution_container->node[iPoint]->GetVelocity2())/solution_container->node[iPoint]->GetSoundSpeed();
                }
the value of SoundSpeed() in my case is ZERO. The program can save a few times but give up at the end.

Here should be a compressible calculation, but I give a very low mach number in cfg file.

Just wondering is "bool" value of "incompressible" set in CFG file? Which one? The solver is a compressible one, where to let it deal with incompressible case?

Regards

Cean
shirazbj is offline   Reply With Quote

Old   February 1, 2013, 03:17
Default
  #5
Super Moderator
 
Thomas D. Economon
Join Date: Jan 2013
Location: Stanford, CA
Posts: 260
Rep Power: 5
economon is on a distinguished road
I can confirm with some of my own tests that there is something odd happening in the Paraview output for rotating frame simulations. We will look into this issue, but in the meantime, do you have access to Tecplot (or another package that can read Tecplot ascii files)? These output files seem to be working just fine for rotating frame problems.

Lastly, yes, SU2 can indeed handle incompressible cases by using an artificial compressibility method. Please see some of the included test cases or other posts where this is discussed: the config options and required inputs are somewhat different for these cases. In general, an incompressible simulation can be run using the following option:

%
% Incompressible flow using artificial compressibility (NO, YES)
INCOMPRESSIBLE_FORMULATION= YES
economon is offline   Reply With Quote

Old   February 1, 2013, 03:45
Default
  #6
Senior Member
 
Cean
Join Date: Feb 2010
Posts: 128
Rep Power: 7
shirazbj is on a distinguished road
If I set FULLMG=YES with MGLEVEL= 2, i'll get zero velocity and zero sound speed. No matert if I output Tecplot or Paraview data.

Last edited by shirazbj; February 1, 2013 at 06:10.
shirazbj 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
paraview ignores SPACING in STRUCTURED_POINTS vtk data? jaffar ParaView 0 November 27, 2012 10:36
Newbie: Install ParaView 3.81 on OF-1.6-ext/OpenSuse 11.2? lentschi OpenFOAM Installation 1 March 9, 2011 03:32
Paraview not found fusij OpenFOAM Installation 2 January 1, 2011 21:44
Distributed ParaView and PV3FoamReader micalil OpenFOAM Paraview & paraFoam 4 July 1, 2010 05:09
paraFoam reader for OpenFOAM 1.6 smart OpenFOAM Installation 13 November 16, 2009 22:41


All times are GMT -4. The time now is 01:58.