[Turbomachine]

Dear All,

I am modelling the NASA 67 transonic rotor case in steady state conditions. Unfortunately the solutions usually do not converge, and I have run out of ideas why. During the solution it often appears that: 'a wall has been placed to the inlet and /or outlet boundary to prevent fluid from flowing in...'. This raises the question whether the problem is with the boundary conditions. These are the following:

inlet total pressure profile: 85-101 kPa
inlet total temperature profile: 288K
outlet average static pressure 1.195atm (0.05 blend factor)
SST turbulence model

Direction of rotations is correct.

I am trying to vary the back pressure to get characteristic. The back pressure information is found from the paper by Strazisar page 34:

http://ntrs.nasa.gov/archive/nasa/ca...1990001929.pdf

There was one occasion when I could get convergence which was for 1.195 atm back pressure with k-e turbulence model only. However the pressure should be varies on a much broader range to get the characteristic.

Does anyone have any suggestions about what the problem might be?

Thank you very much

[Josh]

I'm probably oversimplifying this, but your inlet pressure value is lower than your outlet value, so naturally the flow from the inlet is not going to exit through the outlet. The overflow error is associated with backflow.

[michael_owen]

Yeah, what he said.

[Turbomachine]

Thank you for the replies. From previous data the choking condition for this fan should be at approx. 93000Pa back pressure. From this point the back pressure increases up to the stall point which is at approx 130000 Pa back pressure.

Do you think it is evident that if I have a higher static pressure at the outlet, some flow will evidently reverse into the passage? It is close to the boundary layer perhaps?

This is the result I got recently @ 1.195atm back pressure.



The shock is close to the trailing edge so it should be somewhere around peak efficiency point I suppose.

[Josh]

Originally Posted by Turbomachine

Do you think it is evident that if I have a higher static pressure at the outlet, some flow will evidently reverse into the passage?

Yes. A fluid wants to flow to the lowest possible pressure region.

[Turbomachine]

Thank you Josh! Does it mean that I should 'live with this' phenomenon or is there a solution? I also placed the inlet and outlet further away but if has no affect on the area that the solver blocks to avoid recirculating flow.

[Josh]

How far upstream/downstream did you place your inlet and outlet? Your test section looks very small. Where in the report did you get your conditions from? Did you average the values from Table 3?

I'm not really an internal aerodynamics guy, so I can only help you a little bit.

[michael_owen]

My apologies; when I first read the OP I completely clanked on te fact that it's a rotating machine; of course the flow can go from low pressure to high pressure. The fan is doing work on it.

Your problem could be caused by many things. First, you have pressure-pressure boundaries, which is sensitive to the initial guess. Second, your inlet and outlet are close to the blades; the flow field is being artificially truncated by the boundary condition, causing the artificial walls to be erected where te solution wants to back flow. You will likely need a better initial condition, better boundary conditions, farther boundary conditions, or some combination of all three.

To diagnose this a bit better, post process the flow field from a non-convergent solution as well as the residuals. See where the residuals are high and why, and where the flow field is trying to backflow at the boundary and try to assess if it is likely that the flow would be reversed there. If it is, either fix the boundary conditions or move them.

One option that will remove the artificial walls would be to use openings instead of inlets or outlets. However, there is no guarantee that the flow field that results will be physical I the inlets and outlets are poorly placed (i.e. too close).

[Attesz]

To diagnose this a bit better, post process the flow field from a non-convergent solution as well as the residuals. See where the residuals are high and why...

To do this, check the corresponding radio box in the output controls tab ,and set Output residuals to All. It is really very useful, i'm using it in my compressor simulations, which is similar to yours a bit.

Anyway, you have not shared with us all the informations about your simulation. First, the pic in your post is the whole domain? Do you use only one rotating frame, or do you have interfaces also? Do you use Total Energy model? SST would be propably better, it is strange that you get converged only with k-E model. Maybe you can paste here the corresponding section of an .out file. Choke condition means that your pressure ratio is low; in this case it should not be backflow from outlet, because it occurs usually near choke, or above the operation point. Send pictures about your mesh as well if you can. What about yplus, and your number of inflation layers? When using the k-E model the resolving of the boundary layer can be critical.

Attila

[mm.abdollahzadeh]

dear all

I am trying to model the same rotor with fluent. my domain is extended enough ( i think). i have tested almost everything but i can not obtain the correct pressure ratio for the design mass flow rate. i am using standard k-w turbulance model with 1% of turbulent intensity and 0.0001 turbulant length scale. I have tested both pressre based solver and density based solver. i have tested also diffrent combinations for inlet and outlet boundary condition. for inlet mass flow inlet or pressure inlet and at outlet pressre outlet with/without targeting the massflow rate and radial equilburim activated.
i will be thankful to recive your recomandations.

(I can post also my case if you want to check)

Regards
Mahdi

[ghorrocks]

my domain is extended enough ( i think)

When people say things like that they are almost always wrong. You need to do a sensitivity analysis to be sure your domain is long enough. If your results look realistic but have significant error then this is the sort of check you need to do to get it accurate.

While you are at it, do a sensitivity analysis on mesh density and convergence tolerance.

[mm.abdollahzadeh]

Originally Posted by ghorrocks

When people say things like that they are almost always wrong. You need to do a sensitivity analysis to be sure your domain is long enough. If your results look realistic but have significant error then this is the sort of check you need to do to get it accurate.

While you are at it, do a sensitivity analysis on mesh density and convergence tolerance.

Thanks for your kind answer ghorrocks

I will for sure do the sensitvity analysis. acctually i am working with the grid that is on stansford university website. but at the moment i have some douts about the soliution procdure (as its my first case on rotors) .
i have seen that some guys are usingnot a extended geomtry in a way that inlet and outlet are placed in a position that experimental values of pressure and temperure and etc are avilable. but in my case geomtry is extended ( suppuse that it is enough). then i have just the pressure ratio and mass flow rate and temperate and pressure at inlet and some how the tempretaure at outlet.
Tin=288.2
Pin=101325
Tout=345.84
P.R=1.64
Massflow=33.25
number of blade=22

at the moment the temperature is not convergaing with density based solver ( and i have the warning related to "Temperature limited" )
but with pressure based solver everything is converging

the problem is that for both cases the pressure ratio is small maximum 1.5
and with mass flow is correct ( as i am using target mass flow rate)

i dont know exactly but i thinck there should be sth beyond grid (in fact my spanwise Mach number distrubition is not even similar to the correct results)

[ghorrocks]

Your questions are now relevant to the solver, and you are using Fluent. This is the CFX forum, so you will get better answers on the Fluent forum.

[mm.abdollahzadeh]

Originally Posted by ghorrocks

Your questions are now relevant to the solver, and you are using Fluent. This is the CFX forum, so you will get better answers on the Fluent forum.

Thank you for reminding

unfortunately, there is not a topic related to this subject

[ghorrocks]

Then start a new thread on the Fluent forum.

http://www.cfd-online.com/Forums/fluent/

[sivakumar]

Hi Josh,
Thanks for your reply,
As I mentioned before, I am simulating axial flow fan. the results looks wrong.
the simulation results shows inlet has higher pressure than outlet pressure.
I am giving some more details about my case.
I have attached the initial condition files, please have a look and give me your suggestions and idea for my problem.

I am sorry guys, I am openFoam user, however its general issue that is why I am posting here.

thanks,
Sivakumar

[Josh]

You should post this on the OpenFOAM forums or the general CFD forum (http://www.cfd-online.com/Forums/main/) since it does not pertain to CFX. I'm not an OpenFOAM user, so I don't know how to interpret those files.

Regardless, did you try everything suggested by the previous posts, e.g., extending the domain, trying different meshes, etc.?

[sainath.s@tdps.co.in]

The best possible way to simulate an axial fan is to use standard( AMCA/BSI). Try to develop a test rig of based on these standards and do the measurements at those specified locations in the standard.

Everything should work out then.. Example

At fans inlet, it is necessary to have a bell type opening and as the flow proceeds through the fan, a flow straighner must be employed.

Unless you follow a standard procedure, it will be difficult for you to validate your results with experimental one.

[sivakumar]

Hi Sainath,
Thank you for your reply, Unfortunately I didnt add bell mouth and flow smoother.
I have seen in the BS848, they have employed the flow smoother.

I hope the existing situation is reasonably fine. but the problem is i am getting less pressure at outlet than inlet.

now I am extending the domain, redoing the simulation.

do you have any suggestion for further implementation.

Thanks,
Sivakumar

[MUSohail]

Dear Josh and All
As earlier i mentioned that i am trying to do Transient simulation of rotor 67 to get pressure changes from blade to blade from 0 rpm to 16043 rpm where it flow becomes steady too..
I uses total time steps to 1 sec and time interval to 0.001 sec. Whereas at rotor domain i selected automatic static pressure and temperature with cartesian velocity 0, 0 and 1m/s (on z axis).

But when i run, back flow becomes 100% and error occurs..
How may i do unsteady simulation..