# [OpenFOAM] Calculating Lift and Drag in Paraview (paraFoam)

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 May 24, 2011, 23:11 Calculating Lift and Drag in Paraview (paraFoam) #1 Member   Scott Join Date: Sep 2009 Posts: 44 Rep Power: 13 Hi there, I have a body that I wish to extract the lift and drag forces for in Paraview. I assume that this can be achieved using the calculator but I cannot work it out. Could someone please give me some pointers on this. Basically I need to calculate the normals for each surface, then find the pressure on each surface in the components of X (or Y or Z, depending on if it is Drag, Lift or side force), then intergrate these values for the whole body to get the Force value. If someone has a procedure for something like this then please let me know! Thanks for your help, Scott kubashmuba and varun0505 like this.

 May 25, 2011, 03:49 #2 Member   Scott Join Date: Sep 2009 Posts: 44 Rep Power: 13 I found a solution: Extract Surfaces Generate Surface Normals Use the calculator to multiply pressure by the surface normals (Normals*p) This then prints the values in the data tab at the right in three columns, one for each normal direction. I then integrate these to get total forces on the area using Integrate Variables. Let me know if you see any problems with this approach! Cheers, Scott elmo555 likes this.

 July 18, 2011, 16:17 #3 New Member   Join Date: Aug 2010 Posts: 15 Rep Power: 12 Hey Scott, I am trying to do the same thing and am attempting your approach. I was just wondering if you've made any more progress since you posted. I'd like to collaborate with you if possible.

 July 18, 2011, 18:33 #4 New Member   Join Date: Aug 2010 Posts: 15 Rep Power: 12 Scott, Where (and how) do you calculate the area of each panel? I'm struggling finding a particularly good way of doing this. Right now I'm performing a similar calculation in Fortran, but I would prefer to do this in paraview.

 September 12, 2011, 11:28 #5 Member   Daniel Join Date: Apr 2010 Location: Manchester Posts: 30 Rep Power: 12 Any advances on this? Also, how would you go about including the effect of skin friction? I guess the wallShearStress post-pro function would be a start.

 January 3, 2014, 04:19 lift and drag coeffs in paraview #6 Member   Arash Mahboubidoust Join Date: Jun 2013 Location: Iran Posts: 57 Rep Power: 9 Hi How can I calculate lift and drag coefficient in paraview? I've run an oscillating airfoil with pitching motion.I've calculated lift and drag coefficient through libforces in controlDict, but the values ​​are wrong. I want to calculate them in paraview and plot them over the time or angle. Please tell me how to do this?

 March 27, 2014, 12:38 #7 Senior Member     Louis Gagnon Join Date: Mar 2009 Location: Stuttgart, Germany Posts: 304 Rep Power: 14 In 2D, you might want to try something like this in paraview on the surfaces you want to evaluate, 1. filter: generate surface normals (disable splitting, activate compute cell normals) 2. filter: calculator using something like this for moments : Normals_Y*p*yourDensity*(yourCoRx-16) + Normals_X*p*yourDensity*(yourCoRy-coordsY) replacing yourDensity and yourCoR* by appropriate values or simplify it to get forces 3. filter: integrate variables and look for the results of the integration in the table that appears in the end this procedure gives you sum_cells(P*rho*A*norm_y) I think this can be easily adapted to 3D. cheers Ruli, brucecumt, arashfluid and 2 others like this.

 April 16, 2014, 08:13 #8 Member   Daniel Join Date: Apr 2010 Location: Manchester Posts: 30 Rep Power: 12 I've had some success working with cell data (as opposed to point data) on 3D surface meshes, if it's of use: Cell area can be obtained using the Mesh Quality filter and the Area option. Use the Point Data to Cell Data on your pressure data. Then use Generate Surface Normals (may need to Extract Surface first) with the Compute Cell Nomals option enabled. Pop these into a calculator using the Cell Data mode and that should have you on the right track for the pressure side of things. arashfluid likes this.

 February 12, 2016, 08:58 #9 New Member   Join Date: Jan 2016 Posts: 3 Rep Power: 7 Hello louisgag, could you please explain what do you mean by "yourCoR"? Thank you very much.

 February 12, 2016, 08:59 #10 Senior Member     Louis Gagnon Join Date: Mar 2009 Location: Stuttgart, Germany Posts: 304 Rep Power: 14 Center of Rotation Regards, -Louis

February 12, 2016, 09:00
#11
New Member

Join Date: Jan 2016
Posts: 3
Rep Power: 7
Quote:
 Originally Posted by louisgag replacing yourDensity and yourCoR* by appropriate values or simplify it to get forces cheers
Could you please explain what is "yourCoR"?
Thank you very much.

 February 12, 2016, 09:07 #12 New Member   Join Date: Jan 2016 Posts: 3 Rep Power: 7 Thank you for your quick reply. Another question if you don't mind, So, If my center of rotation is (0,0,0), Does this mean that CoRx=0, and CoRy=0? Sorry if the question is too simple, I am new to CFD.

 February 12, 2016, 09:10 #13 Senior Member     Louis Gagnon Join Date: Mar 2009 Location: Stuttgart, Germany Posts: 304 Rep Power: 14 Yes, that is correct. -Louis

October 24, 2016, 07:50
#14
Member

Emre
Join Date: Nov 2015
Location: Izmir, Turkey
Posts: 94
Rep Power: 7
Quote:
 Originally Posted by louisgag In 2D, you might want to try something like this in paraview on the surfaces you want to evaluate, 1. filter: generate surface normals (disable splitting, activate compute cell normals) 2. filter: calculator using something like this for moments : Normals_Y*p*yourDensity*(yourCoRx-16) + Normals_X*p*yourDensity*(yourCoRy-coordsY) replacing yourDensity and yourCoR* by appropriate values or simplify it to get forces 3. filter: integrate variables and look for the results of the integration in the table that appears in the end this procedure gives you sum_cells(P*rho*A*norm_y) I think this can be easily adapted to 3D. cheers
Hello and thank you very much. But after doing this I still can't see the drag force (Normal_X*p*1.16)

November 18, 2016, 10:20
#15
New Member

bruce
Join Date: May 2012
Posts: 12
Rep Power: 10
Quote:
 Originally Posted by louisgag In 2D, you might want to try something like this in paraview on the surfaces you want to evaluate, 1. filter: generate surface normals (disable splitting, activate compute cell normals) 2. filter: calculator using something like this for moments : Normals_Y*p*yourDensity*(yourCoRx-16) + Normals_X*p*yourDensity*(yourCoRy-coordsY) replacing yourDensity and yourCoR* by appropriate values or simplify it to get forces 3. filter: integrate variables and look for the results of the integration in the table that appears in the end this procedure gives you sum_cells(P*rho*A*norm_y) I think this can be easily adapted to 3D. cheers
Hi louisgag,
May I ask why it's 16 in your equation: Normals_Y*p*yourDensity*(yourCoRx-16) + Normals_X*p*yourDensity*(yourCoRy-coordsY) ?
Another quenstion is about the center of rotation in paraView. My understanding is that the center of the geometry will be the center of rotation. please correct me if I am wrong. It will be very appreciated if you can indicate how to get or display the coordinates of the center of rotation.
Thank you very much in advance!

 November 18, 2016, 10:42 #16 Senior Member     Louis Gagnon Join Date: Mar 2009 Location: Stuttgart, Germany Posts: 304 Rep Power: 14 Hi Bruce, I'm pretty sure that's a typo, and should read "coordsX" thanks for noting it I'll correct it. Regards, -Louis

 November 18, 2016, 22:34 #17 New Member   bruce Join Date: May 2012 Posts: 12 Rep Power: 10 Hi Louis, Thank you very much for your prompt reply. It's clear now. By the way, I found a way to get the center of rotation: simply click the Probe Location button in the tool bar and the 'Center' followed by three values in the Properties tab would be the Center of Rotation used in the equation. If you cannot find the Probe Location button in your tool bar, go to the main menu, then Fliters>Data Analysis>Probe Location, you will get the same thing. This may be very redundant for experienced ParaView user, but I think it should be helpful for newbie of ParaView, like me. Cheers, Bruce louisgag likes this.

 December 24, 2016, 06:34 Mesh Quality working? #18 New Member   Join Date: Sep 2014 Posts: 5 Rep Power: 8 I'm trying to apply the methods in this thread to 3D data from a car inside a "wind tunnel" but I have some questions. My coordinate system is Z in the direction of flow, Y up and X is the right hand vector when facing the flow. - Wouldn't the drag force in Newtons be given by p*cell area*Normals_Z? I see that density is being suggested in the formula but I don't understand why, isn't force equal to pressure times area? - I have tried using the Mesh Quality filter to get the area of a surface in a cell, but this doesn't seem to be giving me the result I expected. Here's my setup: Capture.PNG In case the snapshot doesn't work, in text form, my filters are: 1. Simulation Run Data coming from OpenFOAM 2. ExtractSurface 3. GenerateSurfaceNormals (Splitting disabled, Filed Association=Cell Data) 4. ExtractCellsByRegion (to only extract faces of the object in the wind tunnel, not the boundaries of the computation, i.e. not the wind tunnel walls) 5. Mesh Quality (Triangle Quality Measure=Area, Quad Quality Measure=Area, Filed Association=Cell Data). This adds a Quality column to the data set which I would have expected to be the area of the triangle or quad in the cell 6. Calculator with formula p*Quality*Normals_Z (Attribute Mode=Cell Data) 7. IntegrateVariables (Field Association=Cell Data) The result of the integration is incorrect. If I look at the integration of Quality, I would have expected to find the total area of the object but it gives me 0.0716 for a car, way too low. As if just to nag me, on top of that the IntegrateVariables added a column named Area (I don't know why and how this appears) and that area seems perfectly reasonable at 27 m2 for a car, so somehow it managed to calculate this for me. Any idea of what is going wrong with the Mesh Quality filter? Has anybody had any luck computing all forces in Newtons? I'm so close...

 December 26, 2016, 05:41 Figured it out #19 New Member   Join Date: Sep 2014 Posts: 5 Rep Power: 8 My mistake. For some reason I thought the Integrate Variables filter was only doing the sum of all rows, when instead it multiplies each row by the measure of the cell, which is the surface area in my case, when summing. So the Mesh Quality filter is unnecessary, and the formula p*Normals_Z is all that is needed in the Calculator before integrating which will multiply by the area of each cell under the hood. One can easily see the Integration multiplying by the surface by modifying the formula in the calculator to be 1 (constant). The integration of 1 gives the total area, not the number of cells. Just a noob error on my part. LThomes and Alejandro_Dominguez like this.

 January 9, 2017, 09:22 #20 Senior Member     Louis Gagnon Join Date: Mar 2009 Location: Stuttgart, Germany Posts: 304 Rep Power: 14 Hi kubashmuba, Thanks for posting the answer to your question, it might help other people. Depending on the solver you use, the "pressure" that OpenFOAM returns may actually be pressure divided by density (I think this holds for every incompressible flow solver in OF). Thus, the density multiplier. Regards, -Louis

 Thread Tools Search this Thread Search this Thread: Advanced Search Display Modes Linear Mode

 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 OffTrackbacks are Off Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post CoolHersheys OpenFOAM Post-Processing 3 October 10, 2018 10:11 mechy SU2 7 January 9, 2017 06:18 Mike_star OpenFOAM Programming & Development 1 April 4, 2016 12:16 [OpenFOAM] Display lift and Drag in paraview SamerAli ParaView 1 May 16, 2013 13:51 morteza08 FLUENT 4 December 13, 2012 16:34

All times are GMT -4. The time now is 11:47.

 Contact Us - CFD Online - Privacy Statement - Top