Fluent Drag and Lift monitors
Is there a way in fluent I am able to see the lift and drag forces that are produced in my CFD?
I know I can monitor cl and cd, but I want the X and Y forces. I can calculate L and D using the coefficient values, but I want to directly compare my results to an experiment (which gives me the force in newtons). The reason why I want the L and D values is because I am not 100% sure what area to use since my model is quite complex (Racing car). Is it the frontal projected area or planform or something else? Any help is greatly appreciated. EDIT: nvm I found it, its under Results, Reports, Forces if anyone else is interested 
Hello Shyam88, I understand that your geometry for the race car may be quite complicated however, for most bluff bodies the frontal area or projected area is used. This is relevant to the pressure coefficient and will allow you to find the pressure drag. The viscous coefficient, Cd is also the skinfriction coefficient if I am not mistaken and this will be relevant to the exposed external surface area of the car.
Regarding the comparison of the experimental data with the Fluent Simulations, I know you can use the reports item in the menu and generate force reports. This gives the pressure drag force and friction drag force. However, I don't really know how to monitor them for each iteration in a steadystate or for each timestep in transient case. My 2 Cents. 
I have been using the projected frontal area as my reference area, just needed to confirm. Regarding the monitor for drag and lift force, its no problem, I can just see the force report after I get convergence which is enough. I dont really need to monitor after each iteration.
Thanks crankshaft 
I have been using the projected frontal area as my reference area, just needed to confirm. Regarding the monitor for drag and lift force, its no problem, I can just see the force report after I get convergence which is enough. I dont really need to monitor after each iteration.
Thanks crankshaft 
Glad I could help.
Since we are on the subject of drag calculation I would like to discuss an additional concept. Do you have a clear understanding of how Fluent or any similar Computational Code calculates the pressure drag values? The pressure is a scalar field and after each iteration of an implicit solver we expect a value at each of the cells within the flow domain. For a given bluff body, it is possible to use this pressure field fore and aft of the body and integrate along the respective surfaces to find the resulting normal forces. The net force resulting from this is essentially the drag if I am not mistaken. Can anyone please provide some further information on how CFD codes actually implement drag force calculations or direct me to some additional educational material? 
Quote:

That makes a lot of sense LuckyTran. Thanks for sharing your knowledge. Since the normal direction vectors to the surface are simply being scaled with the scalar, I think it is easy to transform that with a dot product and report the loads in a particular direction. I am not clear on how this incorporates the surface areas of the body ?

Quote:
Quote:
I tried to only include the most important steps but actually there is another hidden step. When calculating the actual force, the reference pressure specified in the reference values is subtracted from the absolute pressure. This is to reduce roundoff error since the local gage pressure is usually much smaller magnitude in comparison to the absolute static pressure. An easy way to think of it is this: Fluent integrates the gage pressure to calculate the pressure force and not the absolute pressure. It's not actually the gage pressure that's being integrated (since the operating pressure and reference pressure are specified separately). However, with default settings the reference pressure and operating pressure are both 0. 
Make this in Referance values window in Fluent.
Area = 1 Density = 2 Velocity= 1 so the equation Cd=1/2*ro*A*V^2 becomes Cd= Drag and lift equation is CL = Lift 
What is the effect on the Fluent Drag Force results when the reference area is left at 1 m^2?
I am beginning to think that the reference value should reflect the surface area of the object of interest. However, if I am analysing the total drag, I am not sure whether the area should be the frontal or the surface area since skin friction coefficient and pressure coefficient both contribute to this total value. Please share some ideas and I look forward to any suggestions you may have. 
Briefly, Cd and CL are only coefficients that they dont have any effect on TOTAL DRAG OR LIFT. You can take any value for referance area in FLUENT. Fluent just use an equation for Cd and CL
Cd = Drag / (0.5*density*Area*V^2) The frontol area, density and the referance velocity are all up to your choice. 
Thanks for your response Emre. I understand that when we manually calculate a particular value for the Cd, Cf or Cp the area is altered to represent the respective formulae. If the reference area is defined as frontal area, I think it will be valid for calculation of the pressure drag and ultimately, the average pressure coefficient however, it is impractical to change the reference values and run the entire simulation again for Cf.
If the area is not as significant as I expected, how are the forces or shear stress values calculated? Are they simply using the respective wall areas for these values? Currently, there are three different methods I am trying  1) Load Fluent case files into CFD Post and then drawing a longitudinal line on the wall. This is used as a location and the Cf, Cp, total pressure, wall shear and y+ are plotted on this. I am concerned however, that these values and their average wouldn't really be equivalent to the actual forces on the entire body in 3D. 2) Use the Forces_x due to pressure, viscosity and total drag from the Fluent Force results panel. Enter these values into spreadsheet and perform all calculations based on my own definition. This is very slow and inefficient. 3) Same as 2) however, values are extracted from CFD Post rather than Fluent directly. Please share your thoughts and provide some feedback on these techniques. 
Recently, I imported the results into CFD Post in ANSYS 14.0. The Coefficient of Pressure and SkinFriction Coefficient were defined in CFX Post using the following expressions 
Total Pressure/(0.5*DensityFreeStream*VelocityFreeStream^2) Wall Shear/(0.5*DensityFreeStream*VelocityFreeStream^2) where, the denominator contains the areaAve(Density)@Inlet and areaAve(velocity)@Inlet respectively. These are the problems I have encountered when trying to plot these as scalar variables on wallbased polylines 

Emre,
I have tried what you have mentioned with the Density, Velocity and area and I have also found that the Forces and Cp, Cf values are all equal. This shows that the calculations are proceeding as expected. I now have to change the reference pressure and the gauge pressure so that my expression PressureReference Pressure is valid. The main problem is that when the Reference Pressure is defined as atmospheric with a value of 101325 Pa, the outlet definition of gauge pressure of 0 Pa leads to unrealistic Cd values >> 1. I don't really think changing the outlet boundary conditions to 101325 Pa would help since they are specified as gauge pressure, which obviously is the difference between the absolute and atmospheric or reference. Please share some suggestions on how to correct this. 
All times are GMT 4. The time now is 09:14. 