[sherifkadry]

Hello, I was hoping I could ask some turbo experts some questions. I am trying to compare some experimental 2 stage axial turbine data with a CFX model (experimental data was taken with 5 hole probes). I constructed a coarse and fine mesh, initially I want to do a steady-state run. Using the coarse mesh, I started by using the SST model, and after about 200 iterations my residual show an oscillating behaviour. I tried using the SSG RSM and the case converged at a specific shaft speed (3000 rpm). At lower shaft speeds the RSM model will observe the oscillatory behaviour. Is this oscillatory behaviour an indication of unsteadyness or something else? When trying the finer mesh, (2-3 times as many elements when compared to the coarse mesh) the SST still exhibits the oscillation, and the RSM models give me an error before the 1st iteration is complete with an overflow. I tried starting with SST and switching to RSM, but I still get an overflow 2 iterations after switching. Not sure why the fine mesh is failing this way. What model has been the most robust for you guys when it comes to turbomachinery?

Simulation info
Inlet BC: Total Pressure ~90kPa (abs)
Inlet BC: Total Temperature ~ 40 deg C
Outlet BC: Exit Static Pressure ~70 kPa
Stage Interface used is the CFX 'Stage' Option.

model picture:
http://i615.photobucket.com/albums/t...Screenshot.png

[Attesz]

Hi,
SST is a good start to model turbulence, and it's more robust. If you have convergence problems, it not caused by SST propably, but rather by the mesh. The transient phenomenons can be modeled with steady simulation too, you get an "averaged" flow field, mostly at surge. Are you "far" to surge? If yes, there is an other problem. I've done simulatons (compressor) with very coarse mesh, the results were very inaccurate, but it could converge.
Look at the settings once again, if everything is OK, check the mesh quality. Huge aspect ratios, low cell quality can cause divergence too.
Send some information about your cfx settings, interfaces, b.c.-s etc., and near pictures about your mesh. Send a picture about your mesh at the rotating blades near its wall (boundary layer mesh).

Regards,
Attesz

[Attesz]

Looking at your picture once again, I can't see it clearly, are you simulating a birotary(contra rotating) turbine? because the last blade's domain (which is rotating in general) has a long flow field behind...

[sherifkadry]

Originally Posted by Attesz

Hi,
SST is a good start to model turbulence, and it's more robust. If you have convergence problems, it not caused by SST propably, but rather by the mesh. The transient phenomenons can be modeled with steady simulation too, you get an "averaged" flow field, mostly at surge. Are you "far" to surge? If yes, there is an other problem. I've done simulatons (compressor) with very coarse mesh, the results were very inaccurate, but it could converge.
Look at the settings once again, if everything is OK, check the mesh quality. Huge aspect ratios, low cell quality can cause divergence too.
Send some information about your cfx settings, interfaces, b.c.-s etc., and near pictures about your mesh. Send a picture about your mesh at the rotating blades near its wall (boundary layer mesh).

Regards,
Attesz

Hey Attesz, I used ICEMCFD to create the mesh, and was told a mesh with no elements of quality <0.3 should be okay. Is this a fair assumption? I have about 15 points for the blade wall boundary layer. I willl send pictures of that as well. Here are some of my settings:
4 domains: S1, R1, S2, R2.
RPM (R1, R2): 3000 rpm (this changes but I would like to get 3000 rpm to converge)
Turbulence model: SST
Wall Function: Automatic
Heat Transfer = Total Energy Incl. Viscous work term.
No tip or wall clearences for S1,S2,R1,R2
Ref Pressure = 0 Pa
Inlet Pressure (total): 100.3 kPa
Inlet Total Temp: 41.09 deg C
Exit Pressure (Static): 73.1 kPa
1 blade instance was used for all domains. Number of blades:
S1 = 66
S2 = 66
R1 = 63
R2 = 63
Interface between S1-R1 = 'Stage' model
Interface between R1 - S2 = 'Stage' model
Interface between S2 = R2 = 'Stage' model
Rotational Periodicity for all domains S1,S2,R1,R2 (periodic high and periodic low)

All domains have shrouded blades.

Advection Scheme = High Resolution
Turbulence Numerics = High Resolution
Timescale control = Auto Timescale (I have tried applying a value but I still get oscillatory behaviour with the residuals)

Attesz, as for your comment about the large rotating exit plenum. No there is no counter-rotation. I'm basing my geometry on an experimental turbine which I have taken data for. The exit pressure is measured at point far from the second rotor and therefore I extended the domain to the location at which this exit pressure is measured. I thought this could have been a problem so I tried a test case with a very short exit plenum, and still I get the oscillatory behaviour. Thanks for your help, if you need any more details please let me know.

[Attesz]

Hi,

I used ICEMCFD to create the mesh, and was told a mesh with no elements of quality <0.3 should be okay. Is this a fair assumption? I have about 15 points for the blade wall boundary layer.

These values are good, but you can set 1 to quality when running smoothing iterations, at most you can't reach it.
The reference pressure is a general basic pressure, for example 101.3kPa (environment pressure). Your turbine working in vacuum? Your inlet pressure is relative low, and the outlet pressure from the turbine is above environment pressure too.

However, the problem with this large rotating plenum is that it's not physically real. The rotation of the flow develops around the blade, but behind that it's calming. If you set a domain rotating, the solver will give a tangential velocity component to the flow. It's physically exists only near the blades. Use an other Interface behind the second rotating domain, and set this passage not rotating, and you can set that as long as you need.

Try it, but I think, maybe there is some other problems too. I will think about it, but firstly send some picture about your b.l.mesh.

Good luck,
Attesz

[sherifkadry]

Mesh scenes:
http://i615.photobucket.com/albums/t.../Mesh/R1_1.png
http://i615.photobucket.com/albums/t...esh/R2_4-1.png
http://i615.photobucket.com/albums/t.../Mesh/R1_2.png
http://i615.photobucket.com/albums/t.../Mesh/R2_1.png
http://i615.photobucket.com/albums/t.../Mesh/R2_2.png
http://i615.photobucket.com/albums/t.../Mesh/R2_3.png

[sherifkadry]

Originally Posted by Attesz

Hi,



These values are good, but you can set 1 to quality when running smoothing iterations, at most you can't reach it.
The reference pressure is a general basic pressure, for example 101.3kPa (environment pressure). Your turbine working in vacuum? Your inlet pressure is relative low, and the outlet pressure from the turbine is above environment pressure too.

However, the problem with this large rotating plenum is that it's not physically real. The rotation of the flow develops around the blade, but behind that it's calming. If you set a domain rotating, the solver will give a tangential velocity component to the flow. It's physically exists only near the blades. Use an other Interface behind the second rotating domain, and set this passage not rotating, and you can set that as long as you need.

Try it, but I think, maybe there is some other problems too. I will think about it, but firstly send some picture about your b.l.mesh.

Good luck,
Attesz

Hey Attesz, Thanks for your help again, I put up some pictures of my mesh, I will try your suggestion once more. I wanted to clarify the pressure issue. The turbine is not running in a vaccum. I just do not like working with gauge pressures (-ve values). Thus when I say my inlet is 100 kPa, that is absolute not gauge. Is that okay? I thought it is. The turbine rig experimentally runs in a suction mode, i.e. a compressor downstream of exit is run to suck air through the turbine, therefore the pressures throughout the turbine are below the ambient pressure in the room. Thanks for your help I'm going to try a few things.
Cheers,

[Attesz]

Your mesh seems to be OK. Later some mesh sensitivity test, and yplus checking is recommened.

Now I understand your pressure settings. It's interesting, the compressor sucks the air through a turbine?

Setting ref.press to 0 you don't make a big mistake. But, If you set how I suggested you, you will get a little bit accurate result. The solver computes the values in 7 numbers (precision). If the ref.pressure is set to for example 1 bar, the other values will be computed in higher level of accuracy, because you have more "place" to store the numbers. It's very difficult to explain for me, sorry

For example:
You want to store 1211.4573 Pa gauge pressure in memory.
When you set the ref pressure to 101.3kPa, it needs 7 numbers in memory.
When you set the ref. pressure to 0 kPa, so you have to calculate with absolute pressure= 101300+1211.4573=102511.4573 Pa, it needs 10 numbers. To store it in memory, you have only 7 "place" so the last 3 number will be cutted: 102511.4 Pa! You lost precision! Maybe it is not important, but why not getting better results?

So, make an other interface behind the second rotating stage, and if you think so, set ref pressure to ambient or preferably to inlet absolute pressure.

Regards,
Attesz

[sherifkadry]

Originally Posted by Attesz

Your mesh seems to be OK. Later some mesh sensitivity test, and yplus checking is recommened.

Now I understand your pressure settings. It's interesting, the compressor sucks the air through a turbine?

Setting ref.press to 0 you don't make a big mistake. But, If you set how I suggested you, you will get a little bit accurate result. The solver computes the values in 7 numbers (precision). If the ref.pressure is set to for example 1 bar, the other values will be computed in higher level of accuracy, because you have more "place" to store the numbers. It's very difficult to explain for me, sorry

For example:
You want to store 1211.4573 Pa gauge pressure in memory.
When you set the ref pressure to 101.3kPa, it needs 7 numbers in memory.
When you set the ref. pressure to 0 kPa, so you have to calculate with absolute pressure= 101300+1211.4573=102511.4573 Pa, it needs 10 numbers. To store it in memory, you have only 7 "place" so the last 3 number will be cutted: 102511.4 Pa! You lost precision! Maybe it is not important, but why not getting better results?

So, make an other interface behind the second rotating stage, and if you think so, set ref pressure to ambient or preferably to inlet absolute pressure.

Regards,
Attesz

Hey Attesz, tried creating a fixed exit plenum and placing the boundary conditions like you've stated however I still get the oscillatory behaviour, here is a picture of the residuals. I'm going to look at the mesh now. Thanks.

http://i615.photobucket.com/albums/t.../residuals.png

[ghorrocks]

This is very common behaviour. Here is some tips.

http://www.cfd-online.com/Wiki/Ansys...gence_criteria

[Attesz]

Hi,

your residuals are oscillating. RMS=Root Main Square, this is an average difference between the discretizated equation and the real euqation for example moments. If it is oscillating, it doesn't means, that your results are oscillating!
Monitor some other points, for example mass flow and imbalances. You can do that in CFX solver tab, clicking on "New monitor" and setting the quantity and the place where you want to monitor. If these values are not oscillating, but RMS do, there is no problem! For example, at supersonic flows, the oscillation of RMS residuals is very common, as Glenn said.

Attesz

[ghorrocks]

Attesz' answer is correct but only part of the answer. The link I posted has a much more complete discussion and has a number of approaches to try depending on the situation.

[Attesz]

Of course, as Glenn said, read that in wiki, and in help. It's more complicated than I've written it, but it's worth to do while simulation is running.

Good luck,
Attesz

[sherifkadry]

Originally Posted by Attesz

Hi,

your residuals are oscillating. RMS=Root Main Square, this is an average difference between the discretizated equation and the real euqation for example moments. If it is oscillating, it doesn't means, that your results are oscillating!
Monitor some other points, for example mass flow and imbalances. You can do that in CFX solver tab, clicking on "New monitor" and setting the quantity and the place where you want to monitor. If these values are not oscillating, but RMS do, there is no problem! For example, at supersonic flows, the oscillation of RMS residuals is very common, as Glenn said.

Attesz

Hey Attesz,
I have actually monitored my inlet and outlet massflows and they do not oscillate. But does this mean my solution is converged? I don't think so. But then again I'm an experimentalist messing around with CFD. Another thing I noticed if I change my advection schemes' blend factor from 1.0 to 0.8 say to try to reduce the oscillation as the wiki recommends, my exit massflow changes by about 0.5% which is quite a change, why is this occuring? As far as I understand 0.8 means a mixture of first order and second order advection whereas 1.0 means second order? Anyway, I'll look further into improving my model Thanks again.

[Attesz]

Originally Posted by sherifkadry

Hey Attesz,
I have actually monitored my inlet and outlet massflows and they do not oscillate. But does this mean my solution is converged? I don't think so. But then again I'm an experimentalist messing around with CFD. Another thing I noticed if I change my advection schemes' blend factor from 1.0 to 0.8 say to try to reduce the oscillation as the wiki recommends, my exit massflow changes by about 0.5% which is quite a change, why is this occuring? As far as I understand 0.8 means a mixture of first order and second order advection whereas 1.0 means second order? Anyway, I'll look further into improving my model Thanks again.

Yes, this doesn't mean that your simulation is converged! There are a lot of aspect to check the convergence. For example residuals under 10^-5 or above etc. But if your mass flows, pressures etc are costants during a lot of iteration (100-200), you are close to convergence (of course, it doesn't means, that your results are correct, you should validate). The specified blend factor is a correction for the first order upwind sheme, it corrects this inaccuracies. If you decrease this factor from 1 to 0.8, your results will be a little bit inaccurate, so tha change of massflow can be occured by this.
Generally if your residuals are under 10^-5 or preferably under 10^-6 and your results are constants for 200 iteration (of course in steady simulation!), than you are close to a converged solution. After that you should do a mesh sensitivity check, an yplus check (if important) and validate your result. Thats all

Have a nice day,
Attesz

[michaelsinaga]

Hi, Im currently simulating the rotor of an axial turbine with 80000 rpm rotational speed. I have mass flow rate and total temperature as inlet B.C. and static pressure at the outlet. The problem is there is so much differences between properties at results and properties from theoretical approach. Even the velocity is increasing. Can anybody tell me what is wrong with my system ? The system, B.C., and results are attached. Thanks.

p.s. i have no issues in achieving 1e-6 rms residual.domainsetup.png

setup.PNG[ATTACH]Velocityl.png[/ATTACH]

[ghorrocks]

FAQ: https://www.cfd-online.com/Wiki/Ansy..._inaccurate.3F