The tutorials have a pump example that should match what you are trying to do.
Basic setup for this type of problem:
Add local rotation
Pressure opening on both ends to determine flow rate
If you want to try and find out what velocity it will rotate at, apply a mass flow for the inlet flow and then iterate the flow until you have zero torque On the blades.
If you need more than this, post a pic of what you are working with and where you are stuck exactly.
I would also suggest checking out the swx kb. Lots of good articles on rotation.
I read many articles on this forum but I could not find helpfull information. As my question are related to the subject "turbine in flow simulation" I have not created a new subject. My questions come after many try and for remind each calculation takes more than 10 hours.
I am a teacher in mechanics. I tried to simulate the behavior of the turbine of Kurt Schreckling. (only the turbine of the gas engine for model aircraft).
I first tried to calculate the physical parameters of the turbine manually :
- Hypotheses : C out = 160 m/s 75 000 tr/min To1= 873K s = 0.85 for distributor and 0.85 for wheel degree of reaction epsylon=0.5
qm =0.115 kg/s Rmoy = 26.5 mm U=208 m/s alpha2 = 53° beta2 = 0° alpha3 = 0° beta3=53°
1 -> inlet 2-> between distributor and wheel 3-> outlet
Calculations gave : Po1 = 1,5 bar Po2 = Po3 = 1.21 bar
To1=873 K To2=873 K To3 = 835 K
T1=862 K T2 = 843.5K T3 = 824,3 K
T2’ = 842.5 K
P1 = 1.43 bar P2 = 1.3 bar P3 = 1.149 bar
Rhô1 = 0.578 kg/m3 rhô2 = 0,537 kg/m3 rhô3 = 0,486 kg/m3
V1=156,7 m/s V2 = 260 m/s V3 = 156,7 m/s
W2 = 156,7 m/s W3 = 260 m/s
S1 = 1.27e-3m2 S2 = 1.36e-3m2 S3 = 1.51e-3m2
Secondly I did a model with flow simulation : The model take the profile of blades given by Schreckling on the average diameter. I simplify the model by drawing the same profile for all the radius.
for this I selected : internal analysis, unsteady flow 0.01 s by step 0.0001 s, global rotation frame = 7850 rad/s, fluid = air, laminare and turbulent, numb. 4 for mesh
Boundary conditions : inlet Po1= 150 000 Pa, T1=875 K
On outlet mass flow = 0.115 kg/s
Stator on fix part of the turbine real wall
I am giving now you the results which are disappointing for me :
- The results did not completely converge ( even for the mass flow it's OK)
- In my opinion I should see same total temperature from inlet to the wheel (875K)
Sharp decrease of the total temperature in the wheel
The same total temperature from the wheel to the oulet ( around 820 K)
This is not the case
The fluid temperature did not decrease enough. One dimensional model give T1 =875 K to T3 = 820 K
Model flow give T1=875 K to only 853 K
* In the end the torque on the shaft is only 0.01 N.m which give a output of 78 W.
On the hand model I should have an output of 5000 W which give a torque of 0.6 N.m
So my questions are :
- Are my boundary conditions OK?
- As I have an idea of the results is it possible to use them to increase the speed of convergence?(would help me to multiply try)
- How is it possible to evaluate the number of cells needed?
I was in touch with a man specialized in turbomachinery. But he did not know flow works. So could not help me on improving the flow works model. He advise me for rough estimation to simplify the model by deleting turbulence (possible in general settings) and viscosity.
Is it possible to delete viscosity and how?
So I followed these advises (I could not delete viscosity) but the results where even more disappointing. The calculation could not converge and the speed of gases was suppose to reach 1e11m/s.
How could I improve the models of the turbine (the first one and the simplified one) ?
Thanks in advance.
lots going on here
first, i'd check out the technical reference and solving engineering problems on rotating regions. i think your model is on the verge of being outside the scope of the rotating region method for flow simulation. you should be able to connect with a reseller to get confirmation from the developers.
for problem setup, the first thing i'd suggest is extending the tunnel that your turbine sits in, those BCs are too close to your area of interest. also, mass flow out is a no no. (see swx kb, help and other references) is there a way you can set it up differently?
also, is there a reason that you're working with a time dependent solution? in the technical refernecem you'll also find that rotation in transient is solved in a psuedo steady state manner anyways. i don't see time dependent componnets in your hand calcs. but those also could use a reference like wherey ou're marking p0...etc. knowing what your assumptions are would also be helpful to know whether you're comparing apples to apples.
You will find below my answers and questions.
first, i'd check out the technical reference and solving engineering problems on rotating regions. i think your model is on the verge of being outside the scope of the rotating region method for flow simulation. you should be able to connect with a reseller to get confirmation from the developers. I will try to get this confirmation from SW.
for problem setup, the first thing i'd suggest is extending the tunnel that your turbine sits in, those BCs are too close to your area of interest.
I agree. As I mentionned a calculation takes more than 10hours. So I tried to reduce the number of cells to the minium.
I will change.
also, mass flow out is a no no. (see swx kb, help and other references) is there a way you can set it up differently?
Sorry I don’t understand ‘no no’??
I did research on internet and in the forum. How can we have an access to the swx kb, technical reference ?
also, is there a reason that you're working with a time dependent solution?
I use transcient option because I use flow tutorial as a reference. And for the calculation of a centrifugal compressor, they use transcient option. So I will change to steady option.
in the technical refernecem you'll also find that rotation in transient is solved in a psuedo steady state manner anyways. i don't see time dependent componnets in your hand calcs. but those also could use a reference like wherey ou're marking p0...etc. knowing what your assumptions are would also be helpful to know whether you're comparing apples to apples.
Po… is stagnation pressure. I think in english speaking countries they noted it Pi…
And I will remind questions:
Is it possible to decrease the time of calculation as I have an idea of the results? Ex the calculation starts with outlet temp. of 273 K. It seems to me, if the calculation starts with an outlet temp. of 700K, the calculation could take maybe less time.
According to you, is it possible to remove the viscosity of a fluid?(In order to simplify the model).
"no no" > not recommended practice.
technical reference > it is in the flow simulation installation directory. lang > english > docs.
swx kb > customerportal.solidworks.com, create an account, register your serial number
Po > understood that Po is stagnation pressure. same designation here in usa/canada. The point i'm trying to make is i'm not sure where your equations are coming from, or how they are laid out or what their assumptions are. part of the issue with comparing simulation to hand calculations is confirming that they are equivalent. this can only be done by knowing the assumptions for both..etc.
decrease the calculation time > steady state will help. but rotating regions does take time and most likely if this is a reasonable problem for flow, you're going to need more cells than you think. regarding your comment about temperature, this is related to steady state. if you choose initial conditions close to the final, it will converge quicker. with transient, you have to choose the appropriate initial conditions for the transient solution.
remove the viscosity > i don't know what you mean here.
technical reference >
I did not know this document interesting document but also complex. Because of the use of a lot of specific vocabulary.
swx kb >
Unfortunately, with my serial number I do not have access to the knowledge base. It’s a shame.
I try to give you the expected answer below.
I started with the data from the book.
After a first calculation the book fixed the following :
Mass flow qm =0.115 kg/s and output speed C out = 160 m/s needed for thrust.
75 000 tr/min and (average radius) Rmoy = 26.5 mm => U=208 m/s
In the book they choose a reaction turbine with degree of reaction epsylon=0.5 Tmax = 875 K
By experience they fixed alpha2 = 53° or 37° dependent on the convention (American or European)
For the calculations I use equation of ideal gas (Pv=rT, T^γ. P^1-γ=cste)
With γ = 1.33 and Cp = 1147 J/(kg.K)
I suppose isentropic expansion with an isentropic efficiency of ηs = 0.85 for distributor and 0.85 for wheel
Equation linking P… to Po… And Euler Equation : wi = U2V2u-U3V3u
The idea was I do first calculation manually . Then I create a model of the turbine, introduce conditions found at the exit of the combustion chamber. The turbine turn at 75000 tr/min and check the power output, torque on the shaft. In the end compare hand calculation of temp, pressure, velocity of gas with the flow sim calculation. In order to check If I am able to build such a model.
remove the viscosity >
If I am not wrong, the flow simulation solve the navier stockes equations. The model of the fluid is a newtonian fluid where ” μ is a scalar constant of proportionality, the shear viscosity of the fluid”(from wikipedia).
In the hand calculations I don’t use viscosity except maybe when I use isentropic efficiency ηs.
So if it would be possible to use a fluid without viscosity, it would maybe simplify the equations and calculations and help to get estimation close to reality even if it’s not exact(avoid meaningless results like P or speed 10^11). This was a suggestion.
In addition, I made new experiences.
I tried to simplify the model by calculating the distributor and the wheel separately.
For distributor I found the results fit quite well the manually calculation.
BC : Po1=150000 Pa T1=862 K mesh level : 6
On exit qm=0.115 kg/s
The speed on the exit is a bit slower 245 m/s against 260 m/s. but for me such a results are OK.
For the wheel the results are worse.
BC : on inlet qm = 0.115 kg/s with a whirl w = 7850 rad/s these are the theoretical values
T3= 843,5 K P3 = 130000 Pa
On exit environnement pressure mesh level : 6
Results strange because close to the exit the fluid rotate fast suddently without reason and accelerate to 343 m/s . The flow should be near axial.
The diagram of total temperature seems not bad.
But the value of torque is close to 0.
In yellow values not in accordance with theory.
hi frederic, i would suggest breaking this down into smaller elements and getting them to correlate before attempting your full assembly. i highly suspect that you will need a MUCH higher cell count to get accurate results (see my comments on a recent airfoil post). and as i mentioned previous, i think you're really on the edge of what flow simulation can do. without access to solidworks technical support and the KB to learn what you need for setting up rotating problems including the recommended meshing processes this is going to be a pretty difficult problem to work through as your first flow simulation problem. the other thing that i would recommend is finding an example with known calculations and physical results to compare to your flow simulation problem. part of the issue could be that your calculations are too simple for flow and that is where the discrepency lies. IE, flow is right, your calcs are wrong. there are a lot of things to consider here. in the long run, I think if you could better understand how the individual blades work, and then the stacks of blades and you can get reasonable answers, you will probably know a lot about your structure.
another thing i just thought about is that there could be some issues here on reporting. agian there are a couple of great articles on this in the KB but it is important that all surfaces are "closed" when reporting torque or forces. otherwise your results will be incorrect.
hi frederic, i would suggest breaking this down into smaller elements and getting them to correlate before attempting your full assembly. i highly suspect that you will need a MUCH higher cell count to get accurate results (see my comments on a recent airfoil post).
I tried to do so. For example, I try to simulate all the turbine (distrib+ wheel) with mesh level 6. I saw close to 900 000 cells+ partial cells. And after few iterations, the calculation diverge strongly 10^11! When I see this I stop the calculation since it can run many days… But this could mean the model is not OK (assembly).
and as i mentioned previously, i think you're really on the edge of what flow simulation can do. without access to solidworks technical support and the KB to learn what you need for setting up rotating problems including the recommended meshing processes this is going to be a pretty difficult problem to work through as your first flow simulation problem.
I know that’s the reason why I try to get a support on the forum. With the resaler of SW, it’s difficult to have contact by phone. You have to send mail to an address such education@.... And you only get short answers with few words which are not helpfull. I would be happy if they could confirm me if the problem can be solved or not.
The best would be to be in touch with someone who have done such calculation with flow simulation. After discussions, In field of turbomachinery, flow simulation is not known.
the other thing that i would recommend is finding an example with known calculations and physical results to compare to your flow simulation problem. part of the issue could be that your calculations are too simple for flow and that is where the discrepency lies. IE, flow is right, your calcs are wrong. there are a lot of things to consider here. in the long run, I think if you could better understand how the individual blades work, and then the stacks of blades and you can get reasonable answers, you will probably know a lot about your structure.
That was the reason of the choice of this turbine. I bought the book with technical features, drawings. It's not easy to find an example of a turbine with so much information on a turbine which I am sure it runs.
I would like to find info on a small turbine running with water (incompressible fluid)=>more simple model. I will look for.
another thing I just thought about is that there could be some issues here on reporting. agian there are a couple of great articles on this in the KB but it is important that all surfaces are "closed" when reporting torque or forces. otherwise your results will be incorrect.
For info I select surface goal, click the wheel,filter, select (remove outer and keep outer surfaces and surfaces in contact with fluid).
I will check again the geometry or, maybe better, rebuild the model.
What is more disappointing for me is that with the same boundary conditions, I can get 2 different results. For example, at the beginning I got torque with value more than 1Nm.
And after so many trials, I cannot see coherence in the behavior of the software. Maybe a clue showing a problem with the geometry.
Something is not clear in my mind regarding BC
with Total pressure : on a lid (outlet for ex) I fix Po (stagnation pressure) and Temperature.
with Static pressure : on a lid (outlet for ex) I fix P (pressure) and Temperature.
with Environment Pressure : on a lid (inlet) I fix Po(stagnation pressure) and Temperature.
On a lid (outlet) I fix P (pressure) and Temperature.
Am I right? What is the interest of environment pressure?
The option “pressure potential” is not clear. What does it mean?
You previously mentionned that the mass flow as boudary condition is not recommended .
Based on your experience, and what you understand from the problem.
what kind of boundary conditions could you suggest me?
Hi Frederic, I'm suggesting breaking Down this problem even further. For example just one fin, no rotation. I think part of the issue is that you're trying to get used to flow simulation on a diffcult problem with a lot of variables. So when it doesn't work, you're not sure if it is your setup, expectations or the software. The software has been validated for many types of problems. By breaking down the problem, you can test the individual elements to make sure they work until you get to the full model. For example I see the fin on their own, rotating cylinder and just the chamber inlet and outlet flow as easily calculatable.
To get a better idea if this will work in flow, someone is going to need your reference material and the model. Having done this for almost 9 years now, I would need to run a bunch of tests and probably consult the developers to confirm its validity with flow. But honestly I can't comment on bcs because I haven't seen your model other than pictures and don't have enoug information a out the application. With an edu license you are kind of stuck. Your instructor could connect with a reseller on your behalf but all the prerequisite work ived described would be necessary. This also includes confirming in the references suggested that your problem meets the needs for rotation.
At hawk ridge, if you wanted to send it to us, we could take a look, but it will take some time with our current customer work load.
Thanks for the proposition. For the moment I will continue to work on the model. I think I am on the good way.
After studies on some parts of the turbine, I worked on the study of the all turbine. I changed the geometry a little and the BCs. Put mass flow on inlet and total pressure on the outlet.
It was necessary for me to learn and work on the optimization of the meshing.
All the calculations converge. The results are not far from hand calculation.
Not easy to compare since it’s difficult for me to set precisely the temp and the pressure on the inlet.
For 824K on inlet, I get 0.482 Nm .
The temp should be 862.5K which would give a torque of around 0.6Nm (ideal model).
For me what is strange is that when I set environnement pressure on the outlet (instaed of total pressure) , the calculation quickly sharply diverge.
Are you surprised by such behavior ? Could you please explain me what difference between setting up of env. pressure and total pressure? (if it's easy).
Environmental pressure should be defined in the help. When it is an inlet it is total pressure, when it is an outlet it is static pressure. There are a couple of good articles on it in the kb. Basically it helps with problems that recirculate at the bc.
As for not converging properly, I don't think it is expected or unexpected unless you've chosen a bc that isn't correct. Either type or value.
I’m working on wind turbine blade flow simulation, I had read all your conversation with Jared, actually I have the same your problem of torque. Hand calculation shows much higher torque than simulation even with optimized mesh. Please note my input is only air velocity towered the blade and the blade is stationary, i.e not rotating with ambient pressure and temperature.
My question is what did you do to improve your results to get higher torque?
And did you run the simulation for stationary turbine to get 0.482 Nm?
sounds like your problem is significantly different, i'd recommend making your own thread for your problem.
i would suggest adding some info about what the application is, what your hand calcs were, what you setup in sim and what your boundary conditions are and what your mesh actually looks like.
the other thing to note is you should look at the continuity of your problem. torque might be wrong but it could be the way you're reading it in the software. do the rest of the values and flow field look correct?
I have a wind turbine blade as shown in the image. Hand calculations means the wind turbine specifications were all information of dimensions, torque and power are available from the manufactures. After drawing the blade the boundary condition were air velocity in y-direction, turbulent intensity and turbulent length. This flowing air will generate torque around y-axis trying to rotate the blade the same like Frederic turbine. Mesh used is around half million of partial cells and 2.3 million of fluid cells in 3-dimention decreases in size near the geometry as shown in the second image. The simulation is of 500 iteration steady state and convergent.
Ideal torque is around 10000 Nm for one blade
Simulation torque results around 90 Nm for one blade
take a look at this thread: https://forum.solidworks.com/thread/70713?tstart=0
my first thought is your comp domain is wayy too small.
i'd recommend starting with something like a simple plate to get your confidence in the software and the way that you're outputting results. then you can move to your full model.