
[Sponsors] 
April 28, 2013, 03:55 
plot cp on airfoils

#1 
Senior Member
saeideh mohamadi
Join Date: Aug 2012
Posts: 229
Rep Power: 5 
hi everyone,
i wana plot the pressureCoeffs on NACA4412 airfoil, i resd in the forum that i can use PlotOnIntersectionCurves in paraview, my question is that, how can i use PlotOnIntersectionCurves in paraview? i don't know what normal i should use, x y or z ? i put my VTK file of the airfoil and the forceCoeffs on it in the following, would you please please give me some advice to use PlotOnIntersectionCurves? thank you very very much 

April 28, 2013, 07:53 
plot cp on airfoils

#2 
Senior Member
saeideh mohamadi
Join Date: Aug 2012
Posts: 229
Rep Power: 5 
hi musahossein and wyldckat
i am working on airfoils and i need to plot the "pressureCoeffs" on the airfoil. as you said i add these lines to my controlDict and i get the result with two format vtk and raw for the latestTime,i'll put them in attachment, how should i plot this result??? please help me wallPressure { type surfaces; functionObjectLibs ("libsampling.so"); surfaceFormat raw; // vtk; outputControl outputTime; interpolationScheme cellPoint; fields ( p ); surfaces ( airfoil_airfoil { type patch; patches ("airfoil.*"); interpolate true; triangulate false; } 

April 28, 2013, 09:36 
plot cp on airfoils

#3 
Senior Member
saeideh mohamadi
Join Date: Aug 2012
Posts: 229
Rep Power: 5 
hi Dear Foamers
anybody isn't here to say me how can i plot "pressureCoeffs" on a airfoil????? i am tired of looking for the answer of this question everywhere i found many way to plot this figure but none of didn't give me a final result. please please help me, thank you very much 

April 28, 2013, 12:28 

#4 
Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,253
Blog Entries: 34
Rep Power: 84 
Hi Saeideh Mohamadi,
I moved the second post from sampleDict and controlDict and the first one from the ParaView forum, because you've opened this new thread and it made more sense to keep these questions together.
Bruno
__________________
Last edited by wyldckat; April 28, 2013 at 12:33. Reason: more info on the moves 

April 29, 2013, 12:16 

#5  
Senior Member
saeideh mohamadi
Join Date: Aug 2012
Posts: 229
Rep Power: 5 
Quote:
i have a question from the figure that is resulted from "Plot On Intersection Curves" in the paraview, what is the value of x axis stand for? is it chord length? i mean your chord length is 2.5 that the x axis show us 2.5? i want comparison my result with experimental result, so i need to figure that "y axis" is "pressureCoeffs" and the "x axis" is e.g "x/chord" if the chord is along the x axis. thanks again for giving me advise dear wyldcka 

April 29, 2013, 17:28 

#6 
Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,253
Blog Entries: 34
Rep Power: 84 
Hi Saeideh Mohamadi,
Sorry, I forgot to mention that you can configure in the tab "Display", the values to be plotted on the graph. There you can choose what values to be used for X and what values to be used for Y. As for calculating specific values, such as the "x/chord", you'll need to first apply the filter "Calculator". In other words:
Best regards, Bruno
__________________


April 30, 2013, 09:43 

#7  
Senior Member
saeideh mohamadi
Join Date: Aug 2012
Posts: 229
Rep Power: 5 
Quote:
i read in a forum; the pressure value that openFoam gives us after finishing the analysis, is "p/rho" not only "p", is it right? now i have a question, as i solve the incompressible flow over an airfoil, so the pressure that i give after finishing the analysis is "gauge pressure", therefore the theoretical formula for cp that is " cp=(ppinf)/(0.5*rho*Uinlet^2) " is reduced for my analysis to " cp=(p guage)/(0.5*Uinlet^2) ? i mean that for using the calculator that is in the paraview, i should write " p/0.5*Uinlet^2" ? your answer really help me, thanks again Bruno. 

April 30, 2013, 17:52 

#8 
Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,253
Blog Entries: 34
Rep Power: 84 
Hi Saeideh,
Yes, in incompressible solvers the "p" field is actually "pressure/rho" and it is relative to the global pressure, so basically it is "pressure gauge / rho" as you wrote. And yes, it makes perfect sense the symbolic calculation you've made... although you forgot the parenthesis on the last equation: Code:
p/(0.5*Uinlet^2) Bruno
__________________


May 1, 2013, 12:09 

#9  
Senior Member
saeideh mohamadi
Join Date: Aug 2012
Posts: 229
Rep Power: 5 
Quote:


December 3, 2013, 10:21 
plot cp on airfoils

#10 
Member
Tobias Adam
Join Date: Oct 2013
Location: Siegen
Posts: 55
Rep Power: 3 
Hello
I tried to follow the instructions of this thread. Poorely I get an errormessage when I use Saeideh MohamadiŽs code for the wallPressure function. The Runtime Postprocessing code: Code:
wallPressure { type surfaces; functionObjectLibs ("libsampling.so"); surfaceFormat vtk; // raw; outputControl timeStep; outputInterval 2; interpolationScheme cellPoint; fields (p); surfaces (BLADE { type patch; patches ("BLADE"); interpolate true; triangulate false; } ); } Code:
> FOAM FATAL ERROR: More than one patch accessing the same transform but not of the same sign. patch:SYM1 transform:0 sign:1 current transforms:(1 0 0) From function Foam::label Foam::globalIndexAndTransform::addToTransformIndex ( const label, const label, const bool ) const in file lnInclude/globalIndexAndTransformI.H at line 240. FOAM exiting I get the same error message when I use foamToVTK. So I wonder how to get the surfaceinformation of the airfoil! My questions now are: 1. How can I make wallpressure work or anyhow get information of the surfacepressure, or if the next one is easier to solve 2. Is there another possibility to plot cp on airfoils Thank you very much Best regards Tobi Last edited by Tobias Adam; December 4, 2013 at 08:49. 

December 11, 2013, 11:05 
Next problem to be solved

#11 
Member
Tobias Adam
Join Date: Oct 2013
Location: Siegen
Posts: 55
Rep Power: 3 
Hey
I solved my problem as I did not do the steps with the VTKfile, but with my normal Foamfile. To be sure to get the data of the airfoil I only activated the meshregion "BLADE" in the meshregion window. I generated Values for cp with the calculator filter and did the Plot On Intersection Curves as described above. Poorely I still donŽt know how to rescale the xaxis, so that I get x/chordlength ( y/chordlength for my case). Furthermore IŽd like to plot the graphs for the suction and pressureside separately (in one diagram). Is there any possibility to do so? Best regards Tobi 

January 5, 2014, 16:38 

#12  
Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,253
Blog Entries: 34
Rep Power: 84 
Greetings Tobias,
Quote:
Bruno
__________________


January 15, 2014, 09:18 

#13 
Member
Tobias Adam
Join Date: Oct 2013
Location: Siegen
Posts: 55
Rep Power: 3 
Hello everyone :)
Thank you Bruno for your help! I still didnŽt achieve to seperate the two plots, but nevertheless the plot looks quite good. IŽve got one last question to this topic: Is there a possibility to get the data arrays, which are used for the plot, as coupled point data in a data sheet with two rows? One row for the cp and one for the y/chord? IŽd like to use it in a calculator program like excel to compare my cp values with values from older simulations. Thanks for your help! Best regard Tobias :) 

January 16, 2014, 15:57 

#14  
Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,253
Blog Entries: 34
Rep Power: 84 
Hi Tobias,
Quote:
Bruno
__________________


January 17, 2014, 08:18 

#15 
Member
Tobias Adam
Join Date: Oct 2013
Location: Siegen
Posts: 55
Rep Power: 3 
Hi Bruno,
Thanks again for your advice, it helped me a lot! IŽm sorry for making demands on your time! This problem was realy easy to solve! Kind regards, Tobi 

June 9, 2015, 11:37 

#16 
Senior Member
Hasan K.J.
Join Date: Dec 2011
Location: Bristol, United Kingdom
Posts: 181
Rep Power: 5 
Dear Bruno,
I am stuck in one such similar Cp problems, I want to calculate the Lift and Drag from Cp of my airfoil. But my airfoil is one single patch. is there anyway to spererate it into upper and lower patch ? and extract Cp Seperately for upper and lower surfaces. I cant do this in the meshing software since it is ICEM and it take association as one single patch. so the entire airfoil is one patch. I want to extract the data for upper and lower surface of the airfoil seperately, but when I do it using Surface Extract it comes in its own format and I am not able to isolate the upper and lower surface seperately for post processing Any suggestion, Thanks for your time and Effort, Hasan K.J
__________________
"Real knowledge is to know the extent of one's ignorance."  Confucius 

June 12, 2015, 18:12 

#17 
Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,253
Blog Entries: 34
Rep Power: 84 
Quick answer: Case running in serial, but Parallel run gives error post #9


Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
I want to plot residual U:  vahid.najafi  OpenFOAM PostProcessing  10  June 2, 2014 09:31 
How to plot xyY plot of certain nodes  maple2012  FLUENT  0  November 5, 2011 11:00 
multiple airfoils at once, are they affected?  kdrbrk  FLUENT  0  October 18, 2010 05:31 
graph plot  anindya  Main CFD Forum  2  September 17, 2003 12:00 
why can't I plot Y+ value?  Jiaying Xu  CDadapco  2  August 18, 2001 10:56 