# Coefficient of Pressure Distribution

 Register Blogs Members List Search Today's Posts Mark Forums Read

 December 1, 2012, 10:12 Coefficient of Pressure Distribution #1 New Member   Join Date: Oct 2012 Posts: 5 Rep Power: 6 Hi, 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 CFX-Pre: (Pressure - areaAve(Pressure)@OUTLET)/(0.5*Density*(areaAve(Velocity)@INLET)^2) 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

 December 1, 2012, 15:48 #2 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 13,196 Rep Power: 102 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.

 December 1, 2012, 18:35 #3 New Member   Join Date: Oct 2012 Posts: 5 Rep Power: 6 What do you mean by draw your functions on these line? do you mean select those lines as where the expression should be computed?

 December 2, 2012, 18:06 #4 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 13,196 Rep Power: 102 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. k.vafiadis likes this.

 December 7, 2012, 20:57 #5 Senior Member     Ovi Join Date: Oct 2012 Location: Sydney, Australia Posts: 150 Rep Power: 6 I encountered a related problem so I would like to share it on this thread. The Coefficient of Pressure and Skin-Friction 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 wall-based polylines - I need to use the Static Pressure values relative to ambient or atmospheric. My Reference domain pressure is 0 Pa and the Absolute Pressure is quoted as 101325 Pa in CFX however, I need to implement the expression P_static-P_ambient. Does the Total Pressure variable provide for this? Since the global range of values is 0-15 Pa I imagined this to be a relative to the ambient conditions. Can you please suggest an alternative? The Cf values were expected to help identify the location of separation and reattachment as the stream-wise velocity vector changes direction. However, the when using the above formula on several simulations involving steady state in addition to various transient settings, the value never falls below 0. I was only able to produce this when choosing Wall Shear X as the main numerator. Can you please provide some guidance on how to implement this and what I may be doing wrong? Appreciate all the comments guys and girls. __________________ -- Mechanical Engineering Sydney, Australia Last edited by Crank-Shaft; December 7, 2012 at 21:09. Reason: Additional Information

December 8, 2012, 05:57
#6
Super Moderator

Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 13,196
Rep Power: 102
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:
 Since the global range of values is 0-15 Pa I imagined this to be a relative to the ambient conditions. Can you please suggest an alternative?
I do not understand this question. Can you explain it a bit more clearly?

December 8, 2012, 07:13
#7
Senior Member

Ovi
Join Date: Oct 2012
Location: Sydney, Australia
Posts: 150
Rep Power: 6
Quote:
 Originally Posted by ghorrocks 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. I do not understand this question. Can you explain it a bit more clearly?
Well I initially had the outlet pressure as 0 Pa and this is why I left the Reference Pressure as 0. I think I will retry the simulation with 101325 Pa as the reference pressure, representing ambient or atmospheric conditions. I was also concerned that setting the Pressure values to the relatively high non-zero values would lead to unrealistically high Cp values however, does it make sense if I rewrite the numerator as Pressure-Reference Pressure or Total Pressure-Reference Pressure? In the above quote I thought that since the Total Pressure values were relatively small in magnitude they already represented the difference between the static and reference pressure.

Also, please share some ideas regarding the reattachment location.
__________________
--
Mechanical Engineering
Sydney, Australia

 December 9, 2012, 01:38 #8 Senior Member     Ovi Join Date: Oct 2012 Location: Sydney, Australia Posts: 150 Rep Power: 6 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 Pressure-Reference 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 Pressure-Reference 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. __________________ -- Mechanical Engineering Sydney, Australia

 December 9, 2012, 05:42 #9 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 13,196 Rep Power: 102 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.

 December 12, 2012, 19:40 #10 Senior Member     Ovi Join Date: Oct 2012 Location: Sydney, Australia Posts: 150 Rep Power: 6 The flow domain represents an open-flow 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 zero-shear 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.cfd-online.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. __________________ -- Mechanical Engineering Sydney, Australia

 December 13, 2012, 06:49 #11 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 13,196 Rep Power: 102 You forgot to mention the most important bit - the relevant non-dimensional 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 0-15Pa * 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.

December 13, 2012, 22:28
#12
Senior Member

Ovi
Join Date: Oct 2012
Location: Sydney, Australia
Posts: 150
Rep Power: 6
Quote:
 Originally Posted by ghorrocks You forgot to mention the most important bit - the relevant non-dimensional 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 0-15Pa * 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.
Yeah sorry that was fairly stupid indeed. The Reynolds number calculated for the domain was Re_x=80 000 based on the length ahead of the inlet ramp. The Mach number is definitely < 0.2-0.3 and the incompressible fluid assumptions were applied. The energy equations were not used in the solution since isothermal conditions were assumed.

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 skin-friction as result variables. When considering the mathematical definition as Cp=P_s-P_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 stream-wise 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.

__________________
--
Mechanical Engineering
Sydney, Australia

 December 14, 2012, 05:30 #13 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 13,196 Rep Power: 102 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?

December 15, 2012, 01:01
#14
Senior Member

Ovi
Join Date: Oct 2012
Location: Sydney, Australia
Posts: 150
Rep Power: 6
Quote:
 Originally Posted by ghorrocks 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?
Yes the gauge pressure is exactly what I need and I have been using to to generate all the graphical plots so far. The wall shear stress seems to have x,y,z directional components and I have used the stream-wise direction and normalised x-axis velocity for Cf.

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.
__________________
--
Mechanical Engineering
Sydney, Australia

December 17, 2012, 04:39
#15
Senior Member

Ovi
Join Date: Oct 2012
Location: Sydney, Australia
Posts: 150
Rep Power: 6
Correction to previous quote - The Reynolds Number is 500 000. I conducted a very basic time-step and also boundary condition sensitivity study with this flow domain.

The optimal time-step 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.
Attached Images
 Reattachment comparison.jpg (36.0 KB, 61 views) Cf Comparison.jpg (38.4 KB, 50 views) Cp comparison.jpg (35.8 KB, 51 views) y+ Comparison.jpg (33.2 KB, 34 views)
__________________
--
Mechanical Engineering
Sydney, Australia

 December 17, 2012, 05:36 #16 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 13,196 Rep Power: 102 The recommended approach is to use adaptive time stepping homing in on 3-5 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.

December 18, 2012, 19:59
#17
Senior Member

Ovi
Join Date: Oct 2012
Location: Sydney, Australia
Posts: 150
Rep Power: 6
Quote:
 Originally Posted by ghorrocks The recommended approach is to use adaptive time stepping homing in on 3-5 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.
Well the Post-processing was done in CFX however, the results were extracted from Fluent using a implicit, SIMPLE coupling algorithm with all transport variables discretised with 2nd order approximation. I remember that you mentioned the adaptive time-stepping previously however, my simulation converges within 20-30 iterations for each time-step, which I believe is reasonably good for this solver.

For the first 50-70 time-steps 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.cfd-online.com/Forums/ans...generator.html
__________________
--
Mechanical Engineering
Sydney, Australia

 January 4, 2017, 07:12 Post cfx #18 New Member   Umer Sohail Join Date: Dec 2016 Posts: 2 Rep Power: 0 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.

 January 4, 2017, 18:21 #19 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 13,196 Rep Power: 102 Have you looked at the CFX tutorials and CFD-Post tutorials? They show how to do most of the basic tasks. They are available on the ANSYS customer webpage.

 Tags cfx, coefficient of pressure, expression, post, pressure

 Thread Tools 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 On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post Mohsin FLUENT 36 April 29, 2016 17:16 super OpenFOAM Running, Solving & CFD 3 December 19, 2012 16:03 deniggo OpenFOAM Running, Solving & CFD 14 September 30, 2010 03:48 Suzzn CFX 18 October 2, 2009 04:18 Rahmat Arazgaldy FLUENT 0 July 17, 2006 07:45

All times are GMT -4. The time now is 05:40.