[Gaëtan47]

Dear all,

I took a look in the forum and tutos to find an answer to my problem but I didn't find it (so sorry if it is hidden somewhere).


Background: for my master thesis, I have to evaluate the lift and drag coefficient of 1 blade of a blade row coming from a steam turbine. I have experimental results and I should find the same using a CFD software. Sadly, after months of research, I don't get the same results. I hope I'll find help here


Details about the parameters: the experimental results have been obtained in a flux of steam with the following properties: density=0.33777kg/m3; steam velocity=100m/s;
Results found experimentally are force in drag direction (x) =2.16N and lift direction (y)= 1.25N ;


In order to reproduce this test from the blade profile, I have reproduced it in ansys. You can see the screenshot of the flow here:

https://drive.google.com/open?id=1mE...QIG_5Pf8YRpgrb


I have done a meshing, with an increased accuracy close to the blades. In order to create a wall function (y+), I have made an inflation using the first layer thickness, and then I have specified 10 layers. You can see the screenshots of mesh and configuration here (sorry for french ansys):

https://drive.google.com/open?id=1hK...x8THBJj2xMyab-

https://drive.google.com/open?id=1wd...pORLFBkHT6O_0t

I have played a lot with the first layer thickness, but I never had results closed to the expected ones.

[Gaëtan47]

To check the configuration, please check the following file:

https://drive.google.com/open?id=11E...tYvemwn6ZjR9qs


Basically I have chosen a SST solver, and I have selected and automatic wall function, with the option "fully turbulent" -> error might come from here since I have no idea what I should use... I haven't found the options in ANSYS HELP neither on internet...


Result (CFD post):
https://drive.google.com/open?id=1SL...3tp4taCssTIFfU

Finally in CFD post I can observe the flux. Velocity seems logic. However, I have tried to adjust the Eddy viscosity to have a transition in the wall function layer but I did not succeed to do this ( probably due to mistake in the meshing or configuration). The result I expected to reach is the one I've seen in this tutorial:

https://www.computationalfluiddynami...oundary-layer/

Also, the pressure seems weird to me. I have 1.3 bars from the inlet to the blade...is this logic? I think that I might have good result if I succeed to have 1 bar both at the inlet and outlet with a steam flow of 100m/s at the inlet, but here, it is like I have set a steam flux...


Finally, if I use force_x@blade I find 3.16N instead of 2.16N experimentally and force_y@blade I find 1.21N instead of 1.25N experimentally.

Those CFX results and far from the reality (especially in the x;drag direction) (y direction seems ok). That is why I am wondering about the front pressure....

[ghorrocks]

You do not appear to have the top and bottom faces as periodic boundaries. Is this what you intend?

Please attach your CCL or output file. Screen dumps of your setup are unreadable.

Your question is an FAQ: https://www.cfd-online.com/Wiki/Ansy..._inaccurate.3F

In this case I can see you mesh is way too coarse for accurate results. You are going to have to refine your mesh a lot more. But do it properly and do a mesh sensitivity check to determine what mesh you need - plot you important output parameters versus mesh size as you refine, and it should converge to more accurate values as your mesh goes finer.

[Gaëtan47]

(and the end of my original post (I don't know why I couldn't post all of it together...))




I have also provided the ANSYS files in "New blade.zip"

Everything mentioned above is there:

https://drive.google.com/drive/folde...iG?usp=sharing

Basically I am lost, I don't know what's wrong, so any advice would be a great help.

Also if somebody knows how to do it, I'm ready to buy the solution since I'm running out of time.... (not really the spirit of the forum I know but I'm desperate)


Thank you in advance for your help, please let me know if you want more details...

[ghorrocks]

I don't have time to go through your setup in detail.

Just post your output file as an attachment to the post. That is all we need to know for your setup.

My previous post linked to the FAQ and pointed out your mesh is definitely a problem. Have you looked into that at all?

[Gaëtan47]

Thank you for your answers. Actually I have figured out that the outlet was defined as "opening" instead of "outlet". I got better results but I have still a gap with the reality.

I will update the files in 8 hours (it's 1:40 am here..)

And no I haven't checked my mesh with the method that you have pointed out. I will definitly look into it tomorrow.

[Gaëtan47]

Hello,

I have made some major update.

The major problem I had was the type of outlet.


At first, the material used was defined with constant properties (molecular mass, density, dynamic viscosity). But I had still some deviation from the reality.


So I have tried to use steam properties from "Dry Steam,IAPWS IF97", with 650K as static temperature and 100m/s at the inlet.

The main problem is that I cannot set the inlet pressure neither the steam density (targets are 0.33777kg/m3 and 1bar). How can I fix those parameters?

Because with the current parameters I have a density of 1.55kg/m3 and a pressure of 3.6bars. This leads to supersonic flows and a non-converging calculation.

You can find attached pressure and density contour sreenshots.

result file (.out):

https://drive.google.com/file/d/1CrT...ew?usp=sharing


All the data are available at this location:
https://drive.google.com/drive/folde...Ji?usp=sharing


Thank you in advance fr your help.


PS: I know the meshing is not really accurate, but for the moment I keep this one in order to run calculation easily.

[Gaëtan47]

I have now better results (no more supersonic and strange streamlines), but still I have a density 2 times higher than what I'm looking for. Is it possible to change this density, keeping the static pressure and the inlet velocity (to 1bar and 100m/s)?

[Opaque]

May I ask which boundary condition you are using for the outlet? Average Pressure?

The solution may not have converged completely and you are seeing numerical artifacts not present in the solution of the equations.

[ghorrocks]

Opaque is right - the solution may not be fully converged. So ensure it is fully converged before you start drawing conclusions from it. Also check the boundary conditions are correct.

But I would add that your mesh is unlikely to be adequate to event capture general trends. You have only 1 inflation layer on several blades, a super-fine mesh at the end of the blade, your general mesh is far too coarse. You need to fix these problems before proceeding. Also, you have 4 elements in the z direction. Is this a 2D simulation? If so then use 1 element in the z direction with symmetry boundary conditions on the top and bottom.

[Gaëtan47]

For the outlet I'm using "outlet boundary" with static pressure=1bar.

I'm using 2D simulation so yes, I will remove the multiple mesh layers. But what do you mean by "symmetry boundary conditions on the top and bottom"? That I should do only 1 mesh and then symetry boundary in the CFX-pre will do the other face?

Ok, I will try to make a better mesh. But I have ran other simulations with multiple inflation layers (see attached screenshots): is this enough to take into account the boundary layer (y+)?


Also you can see on the attached pictures that now my simulation looks better. But I still have an higher density than what I want. Also I would like to avoid this pressure rise just after the inlet...

Since the density is still around 2 times higher than what I want, I have approximately 2 time the value wanted for the lift and drag force on the central blade.

Concerning the convergence, I have set it to 1e-5. Isn't it enough? (see screenshot). Or should I wait for the slope to disapear?

[Gaëtan47]

and the missing screenshots

[ghorrocks]

I have looked at your output file. I see lots of issues:
* You have a boundary "sides" which is adiabatic and free slip. This should probably be a symmetry boundary which is mathematically the same but numerically works better (as long as it is planar).
* You do not appear to have periodic boundaries on the top and bottom faces. This appears to be a major mistake.
* Why are you setting the body force averaging? Just leave it as default unless you have a good reason to change it.
* You are not using double precision. You probably will need double precision if you are using IAPWS.
* You have a very coarse mesh. But I have said that many times already
* You have table bounds warnings on many variables. You are going to have to check whether this is reasonable, and if so extend the table bounds on the material properties.
* You have materials "Steam 1", "Steam2", and then in your fluid definition you define material named "Steam 1" to use properties of "Steam2". While this is not an error, it is very bad practise to have confusing names and to mix them up like this. Makes debugging a nightmare. Change your material definitions to more descriptive names and your fluid definitions to something which is not confusing.

[Gaëtan47]

* sides changed from wall to symetry -> working

*I still don't understand what are periodic boundaries: you mean at the top and bottom face of the inlet!? Or periodicity of the blades? Is this a meshing parameter or a configuration parameter? I'll try to understand more tomorrow about this.

*set as default now

*double precision on

*coarse meshing, I know but I'm afraid to have very slow computing if I reduce the size of the elements...

*bounds extended: main problem was due to high mach number, but now it's ok

*names changed


With those changes, I find exactly 2 times my target: lift and drag forces are 2 times higher than the experimental data.... This probably comes from the density which is also 2 times higher. Do you have an idea on how I can devide the density per 2?

I'll upload the new files tomorrow.


Thanks a lot.

[ghorrocks]

You have a reference pressure of 1 [bar] and the outlet is set to 1 [bar] relative pressure. That means the outlet is set to 2 bar absolute. Did you intend this?

You should also change it so the outlet is 0 bar relative pressure and the reference pressure is the absolute pressure of the outlet. This will reduce round off errors and improve convergence (although the effect may not be noticeable in all cases).

[Gaëtan47]

Hello,

I have restarted from scratch to improve it.

I have made a symetrical part then I made a linear repetition.

In the mesh control, I have defined each sides as "symetry" for each parts.

I have let the meshing automatic to have an organized mesh (I can refine it later, but for the moment I want to have quick calculation...).

From this I have a problem: I cannot define the thickness of the first layer (y+) anymore (see screenshot). When I try to select one surface, it doesn't work. If I select one volume it says "actif -> no, unvalid method". Do you have an idea why?
Cause now, I cannot implement a well defined wall function...


Concerning the result, I find now a much faster and accurate convergence with the solver, and approximatly the same force on each blades. But with those symetry boundaries, am I not suppose to find exactly the same flow around each blades? You can see on the screenshot a discontinuity on the eddy viscosity contour. Is this ok or this might create a wrong calculation?

[Gaëtan47]

edit:

it's OK now for the continuity, just needed a proper use of the contact function in the meshing and a proper setting of the interfaces.

But I still cannot use the frist layer thickness definition...

[ghorrocks]

But with those symetry boundaries, am I not suppose to find exactly the same flow around each blades?

You have used a coarse mesh. You will not get accurate results on a coarse mesh.

[Gaëtan47]

What do you mean exactly by coarse mesh? Do you refer to element size? Or mostly organization of it?

I did a run with smaller element size (see attached pictures).

Is it accurate or do I need smaller elements?

Indeed the convergence looks better...

I have now a result which is 20% away from the reality concerning lift and drag forces, but I have a proportional deviation lift/drag which is good.


Do you have an idea on how I could set an inflation to set up the boudary layer?

[ghorrocks]

Until you get inflation layers onto it mesh refinement is pointless. Once you have sorted the inflation layers you will need to determine:
* What first element size you require
* How thick an inflation layer you require
* How big the bulk mesh needs to be.

You determine this through a sensitivity analysis. Do a simulation, get a result and extract your key performance parameters - in your case probably lift and drag.

Then refine the mesh by a significant amount. This would normally mean halving the element edge length, so for a 2D quad mesh you will get approximately 4 times the number of elements. Then repeat the simulation, get a result get your lift and drag.

Compare the lift and drag from the first mesh to the second. If they are the same to within a tolerance you are happy with then your mesh is acceptable. If there is variation in the two results then you need to refine the mesh further (that will be 16 times more elements than the initial mesh), and keep going until the results converge.

You should also do a similar sensitivity analysis on convergence tolerance and time step size (if transient).

You will find this process will often mean you need to run very large meshes. That is why CFD is run on supercomputers.