plot cp on airfoils
3 Attachment(s)
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 
plot cp on airfoils
2 Attachment(s)
Quote:
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; } 
plot cp on airfoils
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:) 
1 Attachment(s)
Hi Saeideh Mohamadi,
I moved the second post from http://www.cfdonline.com/Forums/ope...ntroldict.html 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 
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:) 
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 
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. 
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 
Quote:

plot cp on airfoils
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 Code:
> FOAM FATAL ERROR: 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 
Next problem to be solved
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 
3 Attachment(s)
Greetings Tobias,
Quote:
Bruno 
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 :) 
Hi Tobias,
Quote:
Bruno 
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 
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 
Quick answer: http://www.cfdonline.com/Forums/ope...tml#post392721 post #9

Greetings to all!
I was asked this week via PM about how to open VTK files that were generated with sample. Since this post was referenced in the PM, I'll add the steps I've taken for diagnosing the problem so that all can access this information. When we sample data with sample or a sampling function object and if the data is saved in VTK format, e.g.: Code:
setFormat vtk; If we run the script "./Allrun" for that tutorial (make sure you're using your own copy of the original tutorial, see chapter 2 from the OpenFOAM User Guide), it will generate the folder: Code:
postProcessing/sets/1000/ Now, for saving the results to VTK, instead of raw, edit the file "system/sampleDict" and change the line: Code:
setFormat raw; Code:
setFormat vtk; Now run: Code:
sample latestTime Code:
paraview Then:
Best regards, Bruno 
Thank you Bruno.
It worked for me. :) Is there a way to see, in ParaView, the position of the gauges? Regards, Cristina 
1 Attachment(s)
Hi Cristina,
Quote:
If this isn't what you meant, please provide an image that shows what you're referring to. Best regards, Bruno 
All times are GMT 4. The time now is 12:45. 