Coefficient of Pressure Distribution
Hi, (0.5*Density*(areaAve(Velocity)@INLET)^2)I am working on a flow simulation over a sail. In order to validate my results I need to plot the coefficient of pressure distribution along the sails which I will compare to some experimental data. I've entered the following expression in CFXPre: (Pressure  areaAve(Pressure)@OUTLET)/ then when I go to CFX post and I want to plot tha expression, i need to specifi a location for the data series. Is there any way to create a line, or better a surface, exactly coincident with my geometry so that I can get the pressure distridution along that line or surface? I can create a straight line, but what I want is a line following the profile of my sail. Thank you. umberto 
Draw contours of x, y or z (or any function you like to generate other shapes) on the sail surface. Then draw your function on these contour lines.

What do you mean by draw your functions on these line? do you mean select those lines as where the expression should be computed?

Here's a more complete explanation:
* Create a contour object. Make its "Locations" the sail surface, and the "Variable" such that it creates contours on surface you wish to view  X, Y or Z; or a more complex function if you want it angled or curved or whatever. * Create a Polyline object. Method is "From Contour", and select the contour level you want. * You now have a line object you can do "stuff" with, plot your variable, export data, put vectors on it, anything you like. 
I encountered a related problem so I would like to share it on this thread. 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 

By the way, I think you will find areaAve(Density)@Inlet * areaAve(Velocity)@Inlet ^2 does not equal areaAve(Density*Velocity^2)@Inlet. Be careful how you write expressions like this  I suspect the second form is what you want, not the first.
Why are you using 0 reference pressure? This is just introducing numerical round off errors. Use a reference pressure representative of the static pressure in the domain to reduce round off. Total pressure is offset by the reference pressure, just as all other pressure quantities are. Quote:

Quote:
Also, please share some ideas regarding the reattachment location. 
Hey Glenn,
Yes thanks for that reminder about the areaAve(Velocity^2)@Inlet. I actually defined it correctly in the CFD Post expression but had a typo on the forum post. I now have to change the reference pressure and the gauge pressure so that my expression PressureReference Pressure or Total Pressure is valid in the numerator of my Cp expression. 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. Is it still possible to define a 0 gauge pressure at the outlet while avoiding the numerical rounding errors you mentioned? If the application uses Gauge Pressure = Total PressureReference Pressure then it should be acceptable and I will change the outlet BC values. Please share some suggestions on how to correct the issues with large Cp values. 
Can you explain what you are modelling? Or if you have already explained it post a link to the thread which explains it? You probably have explained it before but there are so many threads on the forum I cannot remember them all.

The flow domain represents an openflow with standard atmospheric air properties flowing over a backward facing ramp. The geometry is essentially a 2 m long tunnel with a 5 deg. leading ramp and 16 deg. trailing, backward ramp. The ramp is there to induce separation and also provide a benchmark test case, which will be compared to results after the application of vortex generators on the top. The side walls have been modelled as symmetric boundary conditions and the top face was treated as a zeroshear wall. The inlet is at 4.5 m/s with a 0 gauge pressure outlet.
My attempts at blocking and meshing the geometry is summarised in the forum thread  http://www.cfdonline.com/Forums/ans...generator.html Please let me know whether the geometry, the flow conditions and the overall aims are clear and I look forward to your reply. 
You forgot to mention the most important bit  the relevant nondimensional numbers. I will assume this flow is low Ma number (so incompressible) and moderate Re number (so fully turbulent, but with boundary layers of a significant thickness). I also assume the flow is at atmospheric pressure or close to it.
If my assumptions are correct then you should: * Set a reference pressure of atmospheric pressure * Set the outlet as 0 pressure, inlet as the desired velocity * I think a previous post then says the pressure range is 015Pa * Your post #5 is talking about pressure and skin friction coeffs. I would write these as: (pressure or wall shear at that point)/(0.5*FlowDensity*InletVelocity^2), and FlowDensity is set to the density you are using and InletVelocity to the flow velocity, and these CEL expressions used to set the fluid density and inlet velocity. Then you do not need to use callback functions to calculate these values. 
Quote:
Regarding the user expressions you wrote above, I can confirm that my new ones are very similar. The default reference value was 0 Pa for the domain pressure. When my Fluent results are exported into CFX Post I found a coefficient of pressure and skinfriction as result variables. When considering the mathematical definition as Cp=P_sP_ref/(0.5*rho*Vel^2) the Total Pressure variable in the results file should be already calculating the numerator. Hence, I have used this so far and it is matching my manual calculations. It is still fairly unclear what the differences are between each of the variables such as Total Pressure, Relative Total Pressure, Static Pressure, Relative Static Pressure and so on. For the Cf values I have been using Wall Shear X in the streamwise direction, since this matches my mean flow direction and is the only way I get a dataset with negative and positive results. My intention was to use these results and the streamwise velocity plots to determination separation points and reattachment lengths amongst other flow features. Thanks for your guidance Glenn. 
Total pressure and Static pressure are reported in CFX as gauge pressures, that is they are offset by the reference pressure. The Absolute pressure is exactly that  the absolute pressure with no reference pressure. I do not know what relative static/total pressure is  where is that coming from?

Quote:
I am not sure about the Relative pressures and will try not be too concerned with this. I will share some comparative plots here for further discussion. Thanks everyone for the input. 
4 Attachment(s)
Correction to previous quote  The Reynolds Number is 500 000. I conducted a very basic timestep and also boundary condition sensitivity study with this flow domain.
The optimal timestep was calculated with the Courant number of 1 and 0.5t Optimal represents Courant number of 0.5. The characteristic distance delta_x was taken from average cell size within the domain. The boundary condition characteristic Length and Turbulence Intensity were calculated based on the boundary layer thickness and these were set for the inlet and the pressure outlets. Attached images are available for discussion. I really need to try and interpret the results and would really appreciate if you can help draw some insights from this. Please ignore the title of the charts since they were not recently updated. 
The recommended approach is to use adaptive time stepping homing in on 35 coeff loops per iteration. Courant Number time stepping is not recommended as Courant number is not a fundamental parameter for an implicit CFD code like CFX.

Quote:
For the first 5070 timesteps the number of iterations are greater however, based on my limited knowledge this is to be expected. Please correct me if I am mistaken here. Another issue is the blocking and meshing of this geometry and the link is provided here  http://www.cfdonline.com/Forums/ans...generator.html 
Post cfx
Dear all. I am working on CFX axial compressor. I have completed my simulation but how may i get boundary layer details and complete compressor performance details via post cfx analysis. Kindly guide me.

Have you looked at the CFX tutorials and CFDPost tutorials? They show how to do most of the basic tasks. They are available on the ANSYS customer webpage.

All times are GMT 4. The time now is 05:19. 