[asifnafi]

Experiment Name : Flow over a wing with leading-edge rotation.
Analysis Type- External Flow analysis(Time Dependent Analysis)
Airfoil- NACA0024 (0.2m chord,0.6m span),
Leading-Edge Cylinder- 25mm dia,rotating at 400rad/s , 3820RPM clockwise.
freestream Velocity-5m/s
AOA-5 degree

Problem Details- i faced no problem regarding the setup.
When i started the simulation mesh generation finished properly no prb faced.
But after some iterations "High Mach Number Flow Exists" was shown in solver..ALSO the PRESSURE n VELOCITY plot was totally blue no changes there..
I have attached the main files. plz take a look

[Boris_M]

Hi Asif,

well the setup is very simple but also not correct. Here are some things you did wron:

1. You use the averaging approach for a cross flow which doesn't work as the velocities are averaged in circumferential direction. Meaning, if you have flow from left into the rotating region it is positive and if you have outflow to the right it is negative and the average will be zero.
You need to use the sliding mesh approach which is transient but since you are calculating it in transient, there will be no problem.

2. You computational domain is way too small for external aerodynamics.

3. You should apply more than just lift and drag force goals. For the calculation to be of good quality in airfoil aerodynamics use also pressure, velocity and density for example.

4. Your mesh is way to coarse for any good result. Yes you used adaptive refinement but based on a really bad mesh the gradients are wrong already so the refinement will be wrong also. FloEFD or SWFS is good with fewer cells compared to traditional CFD tools but this is just too few.
The gap between the rotating cylinder and the airfoil is not resolved at all.

5. You should use a 2D calculation if you don't require a 3D calculation. If you need a 3D calculation I guess you were planning to have a symmetry plane at z=0.

6. You didn't select any manual time step so the solver will probably run in µs steps automatically.

7. You specified Periodic refinement. Rather specify 2-3 refinements than periodic refinements.

A mesh in external aerodynamics should look somewhat like in the one image below and the computational domain from the side for a whole airplane with only the basic mesh shown (not the final mesh) looks like in the other image.

Boris

[asifnafi]

Thank you very much sir for ur help ).I had to go through many online tutorials and books to solve this problem(High mach). I used real wall angular motion option in solidworks and the results were very close to the experimental results(Moving surface boundary layer control).
Sir , I set downstream computational domain is as large as 10*chord.
also upper and lower domain 5*chord

3d with a good mesh takes a lot of time to solve so i used 2d simulation(Wind tunnel experiment was also 2d,both end of the wing was attached to the test section)

soon my group is going to take a project of building a low velocity wind tunnel(1-20m/s)..so i will have to use local rotating region for that simulation(3d).....I am very much scared of this "High Mach" problem nw. Sir would u please explain it a bit further to me why this "high mach" arising?? isn't meshing quality related to the accuracy of the result? why supersonic flow will be there cuz freestream velocity 5m/s also for circular motion v=omega*r ; my linear velocity of rotation around 10m/s so how supersonic flow is detected by solidworks?

many many thanks to u sir for ur reply. I thought nobody gonna help me cuz everyone got reply but i didn't get any..sir i would very much appreciate ur advises on this "high mach" problem for local rotating region. If possible please help me with some tutorials on this topic as well as how to generate a good mesh.
NB- sir i have access to solidworks 2014 only.sliding mesh is a 15 feature?

[Boris_M]

Hi Asif,

Yes, the computational domain should at least be 10 times the characteristic length if not even 20 times bigger.

Yes, especially with a small gap between the cylinder and the airfoil a good mesh can cause a lot of cells over a long distance.

I noticed I forgot to mention that you don't necessarily need the local rotation as it is a smooth cylinder surface. You can use the wall motion to get the Magnus effect.

Yes, a good mesh is important for good accuracy but you cannot do a bad initial mesh and just use the adaptive refinement as it refines the mesh based on the first solver results and if they are not accurate you basically create a finer mesh based on bad results.

The high Mach number problem you experience is most likely due to some cells that are too big in a small gap or sometimes it can happen that a cell is not so nice placed and you can search for that high Mach number region as explained here: http://www.cfd-online.com/Forums/flo...-impeller.html

It is usually just 1-2 cells that causes extreme flow and the values are growing. You can see that by looking at the dV/V value which is shown in the error message. It give the dV= volume the high Mach number appeared in the overall volume of the simulation V as a fraction so usually very small value as it is just 1-2 cells causing the issue.

If you send me your email address in a private message I can send you a help on how to create a good mesh in your case.

[shezi266]

Hello Boris Sir ,
sir iam doing simulation on turbochrger compressor and i have a full turbochager ( compressor & turbine both)
here my questions are:
1: if iam doing simulation on single part , should i enclose the whole part in domain or just a single part on which iam going to find results.
2. i have solid works 14 and got the same problems as mach num and supersonic flow , i just created wizard and i haven't did any meshing , just it meshes automatically .


so please guide me , i will be very thank ful to you

[Boris_M]

Hi Shahzad,

1. If you want to only simulate one part and it is usually an internal simulation, then it often makes sense to also enclose that part. But it depends on what that part is and what you want to simulate. It should always represent the reality as close as possible. For example, if you want to simulate a water-cooled turbocharger housing and apply a heat source on the inside and a water flow in the cooling channel but also want to use the external natural convection, then the duct needs to be closed but you can run an external analysis. But if you want to only run a simulation on the turbocharger impeller (turbine or compressor) then I would suggest to run it internally similar to the tutorial model of the impeller.

2. As mentioned in the posts above, if the mesh is fine enough and there actually is no supersonic flow in the model in reality, then this might come from one single cell causing some issues. Simply switch to manual mesh settings in the global mesh settings and add one cell for the basic mesh in any of the three coordinate axis directions. For example, increase the Nx number of cells by 1 and try it again. This will cause the mesh to slightly shift and should usually fix that one cell as it will slightly move and the problem is gone.
If this is not the case, then try to add another cell in one of the other directions.

Regards,
Boris

[shezi266]

Thank you Sir for your response,
sir iam doing simulation on turbo compresor and just want to see the outlet pressure and temperature of compressor , i gave total pressure at inlet and mass flow at outlet at a certain rpm , as i increased rpm and mass flow that problem exists.
please let me know this will be internal analysis.

[shezi266]

sir boris,
what rotation type i have to use for this turbo compressor , local region or global region and averaging and sliding type is not included in my solid works 14

[Boris_M]

Hello Shahzad,

It is best to use a flow rate at the inlet and pressure at the outlet.
What is the flow rate and RPM this problem appears?

The sliding type of rotation should be available since SW 15, so you will not have that option. The local rotation is the averaging type of rotation. It was renamed to distinguish between sliding and averaging as both are local definitions.
It will depend on how your model looks like if you can use global or local. For example, if the model looks as rotational symmetric as the tutorial model on the impeller, then global works, but if you use the turbocharger volute for the outflow geometry, then you need to use local rotation.

Regards,
Boris

[shezi266]

hello sir,
sir i have attached the model picture on which iam working ,

actually iam following a research paper and want to find the pressure at outlet that's why i have provided pressure at inlet and mass flow rate at outlet. i gave environment pressure at inlet along with temperature. the values on which i faced problem of mach number and supersonic flow are 140219 rpm and 0.12 kg/s , before i gave 60000 rpm and 0.01 kg/s and got warning "the vortex crosses the pressure openings".
sir , now please tell me which type of rotation i should use as i have now switched to solid works 2016 . and also please tell me solution to get rid of these two problems


thank you.

[Boris_M]

Hello Shahzad,

I assume the inlet pressure you are looking for is the total pressure?
Then it will be most likely higher than the environment pressure, correct?
And since the mass conservation has to be fulfilled, it wouldn't matter if there is a mass inlet or outlet and the pressure will establish on the inlet and outlet as well.

There is no problem to define a static pressure of 1atm at the outlet and a mass flow rate at the inlet. The total pressure at the outlet and inlet will develop during the simulation and can be checked with surface goals. The mass flow at the inlet and outlet are the same due to the conservation of mass.

In fact, it is better to define it this way as the outlet mass flow rate at that turbocharger housing is equally distributed over the outlet surface and in reality, the flow profile looks different. If you suck the air out then you cause the profile to change and pressure near the outlet will also not be represented correctly in its distribution.
It also does not represent the reality, the turbocharger is meant to charge the engine by force and not the engine to suck it out of the turbocharger.

You either have to use sliding mesh or the averaging plane method if you use a turbocharger housing as not the whole geometry is rotating you cannot use global rotation. Both methods work and the difference is mostly that sliding mesh is transient.

As for the error message. Considering your RPM is ~140k and I am just assuming your outer diameter of the impeller is ~6cm, then the tangential velocity at the outer diameter is around 440m/s which is bigger than the speed of sound, which is roughly 335m/s at 10°C. So yes, this can certainly be true.
The previous RPM was less than half and the tangential velocity would therefore be ~188m/s.
These are just assumptions but you need to check if the results you get make physical sense, this is engineering work that still needs to be done by you and not just blindly trust the software. The software only does what you tell it to do and humans make mistakes such as accidentally adding an additional 0 to the RPM or mass flow rate or the wrong units etc.
So if in doubt, do a brief hand calculation the old fashion way to check if it is correct.

Boris

[shezi266]

Hello Sir Boris,

thank you for your help,
sir actually i assume that compressor takes air from atmosphere so i set environment pressure and temperature as inlet and mass flow rate at the outlet , now i want pressure ratio which is the pabs/ patm.

are these bcs correct?
i want absolute pressure at the outlet ,but there is no option of absolute pressure , Or the total pressure is the absolute pressure?

thanks

[Boris_M]

Hi Shahzad,

Not sure what you understand about absolute pressure but usually it means the pressure value not being the difference between environment pressure and the pressure at the inlet or outlet but being the pressure above absolute zero pressure.

P_total = P_static + P_dynamic + P_potential

P_total = P_static + 1/2*rho*v^2 + rho*g*h

where:
rho = density
v = velocity of the fluid
g = gravity (9.81 m/s^2)
h = height difference

P_static is the environment pressure, so at that elevation or the chamber it is measured at still air.

So the absolute pressure for the environment pressure is 1 atm (atmosphere) which is 1013,25 Pascal. So absolute is the difference from absolute vacuum to the environment pressure.

The absolute pressure from your outlet would be the pressure difference between zero pressure and the static pressure at the outlet.

Also see here:
https://en.wikipedia.org/wiki/Pressure_measurement

In turbomachinery, the pressure ratio is usually the total pressure after the compressor divided by the total pressure before the compressor. So in your case:

PR = P_total_outlet / P_total_inlet

Example here:
https://www.grc.nasa.gov/WWW/k-12/Vi...plane/epr.html

And this:
https://www.slideshare.net/Clutch007...d-supercharger

So your BCs are in theory correct, but not ideal. It's not that it won't work but you will cause an error due to the forced flow profile.

Boris

[shezi266]

hello sir,

You mentioned that your BCs in theory are correct but there will be errors.


so finally what should i do that there would be no error and and what boundary conditions should i use to find the desired pressure ratio for compressor.


Thanks

[Boris_M]

Hi Shahzad,

As I mentioned, the ideal boundary conditions are mass flow rate on the inlet at a specified RPM and static pressure at the outlet.
You can use surface goals on inlet and outlet to ask for any pressure, volume flow rate or other parameter and work with equation goals to set up the pressure ratio to be calculated right away.

Try if this works and the results match.

Regards,
Boris

[shezi266]

hello boris sir,
thank you sir , you helped me alot .

please can you tell me to set calaculation control options for my project?

should i use automatic mesh or manual mesh?

[Boris_M]

Automatic mesh works to some degree but if you move the slider to a high level it might cause a lot of cells on edges in the geometry which can be avoided with some smarter settings manually.
I usually prefer manual mesh settings to better define the mesh I want to have.
With some experience it usually takes a few minutes to get a good setting and maybe a few more minutes for any local mesh definition.

That depends on what rotational method you are using. If you use averaging, then there should be no settings in the calculation control options. If you do sliding mesh, then you should set the manual time step as well as specify the interval at which you want to save results.

Regards,
Boris

[shezi266]

hi boris sir ,
you helped me so much.


as iam following your techniques on my flow simulation, just please guide me about manual mesh settings , on what criteria these settings are to be set.


i used cells already set by software in x , y and z coordinates ,i just set refinement level to 2 . and i got warning " a vortex crosses the pressure opening " constantly on every flow rate values.




thanks

[shezi266]

hello boris sir

sir i set static pressure of 101325 kpa and 298 K at outlet of turbo compressor and mass flow rate at the inlet of compressor ,but iam unable to find the results as in research paper ,


sir please suggest me what to do now.

[Boris_M]

The vortex crosses pressure opening is appearing as your volute causes some separation I assume which has a vortex and if there is an inflow in an outflow pressure opening, it assumes that there is a vortex. If you extend the outlet with a duct to have the vortex fully inside the computational domain and therefore fully calculated in the model, then the error will vanish. This error might also only appear at the beginning of the simulation and vanish as the simulation progresses as the vortex gets smaller or vanishes.

I cannot help you with anything from your last post. You need to tell me more than just that the values are not in the paper.
I don't know what paper you have or what your values are nor do I know your model setup in detail.
If you need help, then you need to provide more information. Consider the point of view of the people that should help you. You have all the information but I only know your input and output parameters and RPM. I don't know the paper you have or the geometry and don't know your mesh. There are many reasons why the results might be wrong.
If the paper and the model are not confidential, then please provide more information.

FloEFD provides good results for turbochargers as there are many companies using it for such applications, so the reason you have wrong results are most likely from wrong settings.

Regards,
Boris