|
[Sponsors] |
![]() |
![]() |
#1 |
New Member
Join Date: Oct 2012
Posts: 5
Rep Power: 13 ![]() |
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 CFX-Pre: (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 |
|
![]() |
![]() |
![]() |
![]() |
#2 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,816
Rep Power: 144 ![]() ![]() ![]() ![]() |
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.
|
|
![]() |
![]() |
![]() |
![]() |
#3 |
New Member
Join Date: Oct 2012
Posts: 5
Rep Power: 13 ![]() |
What do you mean by draw your functions on these line? do you mean select those lines as where the expression should be computed?
|
|
![]() |
![]() |
![]() |
![]() |
#4 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,816
Rep Power: 144 ![]() ![]() ![]() ![]() |
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. |
|
![]() |
![]() |
![]() |
![]() |
#5 |
Senior Member
Ovi
Join Date: Oct 2012
Location: Sydney, Australia
Posts: 166
Rep Power: 13 ![]() |
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 -
__________________
-- Mechanical Engineering Sydney, Australia Last edited by Crank-Shaft; December 7, 2012 at 20:09. Reason: Additional Information |
|
![]() |
![]() |
![]() |
![]() |
#6 | |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,816
Rep Power: 144 ![]() ![]() ![]() ![]() |
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:
|
||
![]() |
![]() |
![]() |
![]() |
#7 | |
Senior Member
Ovi
Join Date: Oct 2012
Location: Sydney, Australia
Posts: 166
Rep Power: 13 ![]() |
Quote:
Also, please share some ideas regarding the reattachment location.
__________________
-- Mechanical Engineering Sydney, Australia |
||
![]() |
![]() |
![]() |
![]() |
#8 |
Senior Member
Ovi
Join Date: Oct 2012
Location: Sydney, Australia
Posts: 166
Rep Power: 13 ![]() |
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 |
|
![]() |
![]() |
![]() |
![]() |
#9 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,816
Rep Power: 144 ![]() ![]() ![]() ![]() |
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.
|
|
![]() |
![]() |
![]() |
![]() |
#10 |
Senior Member
Ovi
Join Date: Oct 2012
Location: Sydney, Australia
Posts: 166
Rep Power: 13 ![]() |
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 |
|
![]() |
![]() |
![]() |
![]() |
#11 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,816
Rep Power: 144 ![]() ![]() ![]() ![]() |
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. |
|
![]() |
![]() |
![]() |
![]() |
#12 | |
Senior Member
Ovi
Join Date: Oct 2012
Location: Sydney, Australia
Posts: 166
Rep Power: 13 ![]() |
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 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. Thanks for your guidance Glenn.
__________________
-- Mechanical Engineering Sydney, Australia |
||
![]() |
![]() |
![]() |
![]() |
#13 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,816
Rep Power: 144 ![]() ![]() ![]() ![]() |
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?
|
|
![]() |
![]() |
![]() |
![]() |
#14 | |
Senior Member
Ovi
Join Date: Oct 2012
Location: Sydney, Australia
Posts: 166
Rep Power: 13 ![]() |
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.
__________________
-- Mechanical Engineering Sydney, Australia |
||
![]() |
![]() |
![]() |
![]() |
#15 |
Senior Member
Ovi
Join Date: Oct 2012
Location: Sydney, Australia
Posts: 166
Rep Power: 13 ![]() |
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.
__________________
-- Mechanical Engineering Sydney, Australia |
|
![]() |
![]() |
![]() |
![]() |
#16 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,816
Rep Power: 144 ![]() ![]() ![]() ![]() |
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.
|
|
![]() |
![]() |
![]() |
![]() |
#17 | |
Senior Member
Ovi
Join Date: Oct 2012
Location: Sydney, Australia
Posts: 166
Rep Power: 13 ![]() |
Quote:
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 |
||
![]() |
![]() |
![]() |
Tags |
cfx, coefficient of pressure, expression, post, pressure |
|
|
![]() |
||||
Thread | Thread Starter | Forum | Replies | Last Post |
Simulation of a single bubble with a VOF-method | Suzzn | CFX | 21 | January 29, 2018 00:58 |
Pressure Outlet Guage pressure | Mohsin | FLUENT | 36 | April 29, 2016 17:16 |
how to plot the pressure coefficient distribution along the foil of the wetted flow | super | OpenFOAM Running, Solving & CFD | 3 | December 19, 2012 15:03 |
pressure distribution in water flow, differences in icoFoam and COMSOL | deniggo | OpenFOAM Running, Solving & CFD | 14 | September 30, 2010 03:48 |
cavitation model pressure distribution | Rahmat Arazgaldy | FLUENT | 0 | July 17, 2006 07:45 |