[Wolfram]

Dear all,

i am simulating a mixed flow fan with a diameter of approx. 250mm, around 3100RPM, steady simulation, frozen rotor and k-epsilon turbulence model. The domains and boundaries are shown below:
https://www.bilder-upload.eu/bild-26...25032.jpg.html
I am comparing the simulation results with experimental results from our test bench. The fans inlet is installed at the test chamber, and the exhaust is at free air.

Here is the issue:
When i start the simulation with low volume flow rates (200m^3/hr) the simulation does not converge with a timestep of 1. Especially within the rotating region i can find high "MAX Residuals". After playing around with a higher timestep of around 30, the simulation starts converging and the pressure rise of 418Pa show a good matching with the performance curve. Using this converged solution for runs with a higher volume flow rate (1600m^3/hr), the simulation is also converging and the pressure rise with 36Pa is close to the test bench result. You can find the mentioned operation points as blue dots in the graph below.

When i start the simulation with high volume flow rates (1600m^3/hr) without the previous converged solution, the simulation is not converging at at. Especially within the rotating region the high "MAX Residuals" are not decreasing and the pressure rise 116Pa is far away from the test bench results. Interestingly the "not converged" solution with high "MAX Residuals" in the rotating region shows a good matching with the performance curve relating to the pressure rise for low volume flow rates (200m^3/hr).You can find the mentioned operation points as red dots in the graph below.
https://www.bilder-upload.eu/bild-23...26090.jpg.html

The flow pattern is different, too. With high volume flow rates the fluid velocity in the "not converged solution" is much high in the outer spans than in the "converged solutions". The bigger tip vortex for the "not converged" solution is shown below on the right side.


Here you can see the residuals with 1600m^3/hr for the "not converged" solution:
https://www.bilder-upload.eu/bild-e1...28098.jpg.html

Here you can see the residuals with 1600m^3/hr for the "converged" solution (same setup and mesh as above. The only difference are the inital values as discribes at the beginning of this post):
https://www.bilder-upload.eu/bild-b1...28200.jpg.html


I have tried tons of different meshes from 5 mio. elements to 70 mio elements. Furthermore als kinds of plausible boundaries and a huge range of domain sizes.

I would be really grateful for your advices to fix this issue.

Kind regards from germany

Wolfram

[ghorrocks]

You refer to images which were not attached.

Your question appears to be covered by this FAQ: https://www.cfd-online.com/Wiki/Ansy...gence_criteria

The FAQ lists things to try to obtain convergence.

It is quite normal for some flow rates to converge easily and some to be challenging. When the flow is attached and the device is running near design conditions the simulation should converge more easily. When you are off design conditions and there are recirculations and separations things are much more challenging. The only difference between these two conditions is the flow rate.

[Wolfram]

Dear ghorrocks,

the images should be available now.

I combed the forum before writing my post above, due to this i found your link several times and memorized it - i assume this is your attention . For sure went through it without success.

The design condition is around 1200m^3/hr. The convergence behaviour and head deviation in this operation point is the same as for the high volume flow rates around 1600m^3/hr. It becomes better the lower the volume flow rates regardless of design point.

I have simulated various impellers and tested them experimental - the pattern of increasing head deviation for high volume flow rates is repeatable. After converging the low volume flow rates and using them as initial values, the head is matching the performance curve of the test rig.

[ghorrocks]

Can you attach an image of your geometry and results for a few flow rates and your output file.

[Wolfram]

Dear ghorrocks,

i apologize for not uploading a picture of the geometry. It is a mixed-flow fan with 7 impeller blades and 13 guidewheel vanes.

The performance curve of the test rig (solid line) and the cfd results (dots & squares) are shown below. The blue dots are runs when a former "converged" solution was used as initial value. The red dots are run without these initial values.

Here you see the out file for converged run and low volume flow rates: https://www.bilder-upload.eu/bild-5d...62245.png.html
I call it "converged" when the MAX residuals within the rotating region are below 10^-4 because this is the only remarkable difference between the "converged" and the "not converged" solution, even if the head for both is equal for low volume flow rates. For higher volume flow rates the MAX residuals within the rotating region and the head deviation are connected.

Using the "converged" solution (head ~410Pa, RR MAX residuals <10^-4) as initial value for high volume flow rates results in the blue dots in the graphic above. Here you can see an out-file for high volume flow rates and the converged solution as initial value:

Here you can see an out-file for high volume flow rates without specificated initial values and the mentioned high MAX residuals within the rotating region (red dots in the graphic above):


You will notice in the out-files, that domains like inlet and outlet are of a different size. After i have noticed this pattern of high max residuals i have tried several domain sizes and BC's to find the cause but neither converge behaviour, nor head has changed for high volume flow rates.

[ghorrocks]

I see nothing obviously wrong. But some comments:

You have a lot of partitions (32) and a lot of domains (4). This means there are going to be lots of partition boundaries in this model. Try a run with less partitions, maybe 4 or 8 and run it overnight and see if that makes a difference to the convergence.

You are using auto time stepping. You should use "Edit run in progress" to change this to a physical time step after it has done the initial few iterations. Try to increase the time step as much as you can, keeping an eye on the residuals for signs that you have gone too big (oscillating residuals and/or divergence).

Keep in mind that frozen rotor simulations approximate the flow at the position the rotor is frozen at. If there is torque variation over the whole cycle you won't capture this unless you run multiple runs at different angular positions.

You have not posted an image of your geometry or some example results (eg vectors or blade surface pressure)

[Wolfram]

Dear ghorrocks,

the amount of partitions and domains are due to interpolating different initial values with different domains and so on new domains. But the discussed behaviour is unchanged for other runs - usually i use 3 domains (inlet - RR - outlet). The longest simulation was running for 54 hours, just to give a try but the results and convergence behaviour have not changed after the first 300 iterations.

I was of the opinion by scaling the auto time step do adjust the physical time step - but i will follow your advice for upcoming simulations.

I am aware of the dependency of the impeller positions for frozen-rotor simulations. It remained exactly the same for all runs, so this cannot cause the deviation.
Interestingly the torque matches our measurements with our engine test bench really well with an almost constant offset for the "converged" and the "not converged" solution.


As I mentioned before there are conspicuous differences in the flow pattern in the tip region of the impeller. Here are some pictures, i hope they are sufficient:

Contour of the static pressure, sectional side view of the tip region: https://www.bilder-upload.eu/bild-ba...73229.jpg.html
https://www.bilder-upload.eu/bild-6d...73566.jpg.html

Contour of the static pressure, with isovolume of vorticity, sectional side view of the tip region:
https://www.bilder-upload.eu/bild-63...73599.jpg.html


The difference in the pressure distribution of the "converged" and "not converged" solution influences the upstream velocity distribution in front of the impeller.
Counter of the velocity in front of the impeller, front view: https://www.bilder-upload.eu/bild-44...73782.png.html
Same as above, different view:
https://www.bilder-upload.eu/bild-4d...73995.png.html
Velocity distribution (vectors), sectional side view:https://www.bilder-upload.eu/bild-6e...74065.png.html

[ghorrocks]

Have you tried a transient simulation? These take a lot longer but are the often the only way to get tricky simulations to converge. Note this was mentioned in the FAQ I linked to at the beginning, it is a very standard method.

[Opaque]

Have you tried using a mixing plane (Stage model) instead of frozen rotor model (which I would not recommend)?

[ghorrocks]

Why don't you recommend the frozen rotor model?

[Wolfram]

Dear ghorrocks,

i have tried running it transient. With an adaptive timestep, controlled by a max Courant number of 5. The head is not "bouncy" anymore as in the steady simulations (it was fluctuating by +/- 2Pa, depending on timestep) but exaxtly in the same magnitude.

[ghorrocks]

So if you have obtained convergence now, then you have the result which your simulation results in. If the answer is not correct then you need to do a validation and verification exercise (which should be done for any simulation requiring accuracy anyway, as normal practice)

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

[Wolfram]

True.

The only thing i am wondering about are the different results of the simulations in dependency of the initial values. Not only the huge deviation of head, especially the different flow pattern within the senstive tip region of the impeller.

[ghorrocks]

Bifurcations are a feature of CFD. One of the many reasons CFD is interesting

Have a look at the two converged flows and check they look plausible. It is most likely they are, which implies this is a flow which can bifurcate depending on the initial condition. You will probably find the actual impeller can flip between the two states if you give it the right push in the right place.

[Wolfram]

Originally Posted by ghorrocks

Bifurcations are a feature of CFD. One of the many reasons CFD is interesting

Have a look at the two converged flows and check they look plausible. It is most likely they are, which implies this is a flow which can bifurcate depending on the initial condition. You will probably find the actual impeller can flip between the two states if you give it the right push in the right place.

Although your answer does not solve my issue, it keeps at least my motivation high

[Opaque]

Originally Posted by ghorrocks

Why don't you recommend the frozen rotor model?

Taken from the ANSYS CFX documentation

The Frozen Rotor model must be used for non-axisymmetric flow domains, such as impeller/volute, turbine/draft tube, propeller/ship and scroll/volute cases. It can also be used for axial compressors and turbines. The Frozen Rotor model has the advantages of being robust, using less computer resources than the other frame change models, and being well suited for high blade counts.

The drawbacks of the model include inadequate prediction of physics for local flow values and sensitivity of the results to the relative position of the rotor and stator for tightly coupled components.

There are cases where it can be completely wrong, and only a clear understanding of the physics will let you notice the problem.

My 2 cents

[Opaque]

Originally Posted by Wolfram

... When i start the simulation with low volume flow rates (200m^3/hr) the simulation does not converge with a timestep of 1. Especially within the rotating region i can find high "MAX Residuals". After playing around with a higher timestep of around 30, the simulation starts converging and the pressure rise of 418Pa show a good matching with the performance curve.

What kind of timestep option are you using?

• Physical Timescale?
  Automatic Timescale with a Timescale Factor ?
  Local Timestep Factor ?

[Wolfram]

I am using Automatic Timescale with a Timescale Factor

[Opaque]

From the thread, I can conclude you are happy with the converged results (despite the problem to obtain them); however, you are very concerned on the difficulty of converging the high flow rate cases starting from rough guesses (no use of previous lower flow rates).

If the high flow rate cases are stuck at higher residuals than other cases, it is a good idea to locate these high residuals, and find out any correlation with flow conditions/mesh quality in such region.

Under Output Control/Results Files, activate the output of equation residuals. Run the case, and post-process.

In the post-processor, create a point and use Variable Maximum instead of XYZ method, and select the residual for the equation of interest. You should obtain at least one symbol at the location of interest. Then, the tough part is to understand if there is a correlation.

On the auto timescale option, the computed value is very conservative and sometimes must be scaled up to accelerate convergence (as you have done); however, at some value, the convergence may start to suffer and you should reduce it a bit.

Aside, having a CFD solution that is path dependent is not unheard of; however, it is important to know which of the obtained solutions is stable (not all are).

[Wolfram]

Originally Posted by Opaque

From the thread, I can conclude you are happy with the converged results (despite the problem to obtain them); however, you are very concerned on the difficulty of converging the high flow rate cases starting from rough guesses (no use of previous lower flow rates).

If the high flow rate cases are stuck at higher residuals than other cases, it is a good idea to locate these high residuals, and find out any correlation with flow conditions/mesh quality in such region.

Under Output Control/Results Files, activate the output of equation residuals. Run the case, and post-process.

In the post-processor, create a point and use Variable Maximum instead of XYZ method, and select the residual for the equation of interest. You should obtain at least one symbol at the location of interest. Then, the tough part is to understand if there is a correlation.

On the auto timescale option, the computed value is very conservative and sometimes must be scaled up to accelerate convergence (as you have done); however, at some value, the convergence may start to suffer and you should reduce it a bit.

Aside, having a CFD solution that is path dependent is not unheard of; however, it is important to know which of the obtained solutions is stable (not all are).

I found the location of high residuals with the help of isovolume - i hope this is also feasable. The cells of high residuals are located in the tip region and the path of the well known "tip vortex". In post #7 i have uploaded several pictures of this region and the related differences in the flow pattern between the converged and not converged solution depending on the initial values.
In the "not converged" solution with the huge deviation of head compared to the test bench, the tip vortex is stronger. I hope with the pictures you are able to retrace my verbal descrition - if not please let me know.

I have not found a correlation between this behaviour and the mesh. Several mesh densities in the gap and inflation layer options were used and the influence was negligibly small.