[Optimization to blades]

hello user! I try to find out a way to get fan characteristic curve that includes efficiency. For that purpose I used Ansys Fluent and FLOEFD programs. My question in here is that both of the programs work properly to get volume flowrate-pressure charts. (I use pressure inlet-pressure outlet and rotating region or frame motion for the impeller) However while getting efficieny curve there must be decrease after peak efficiency. But in simulations efficiency increases up to a certain point and then it goes on at a level that is close to pick point even though pressure is increased.

Is there any solution for that problem ? Thank you to read...

[zacko]

Any convergence issues where you except the Efficiency to drop?

[Optimization to blades]

Actually I was using FLOEFD to get the result quiickly at first and then compared it with Ansys Fluent. The results are quite similar. The maximum pressure that the fan can handle with is approximately 1800 Pa. And the maximum efficiency that fan reaches at first is around 1100-1200 Pa. After that even though the pressure increased the efficiency is close to peak efficiency till 1700 Pa...

[zacko]

Again, any convergence issues? Can you share a photo of your CFD domain? How about the meshes for fluent and FLOEFD, do they differ largely?
Do you have any experimental data that proves that the Efficiency drops after 1100-1200 Pa? Maybe the fan efficiency curve is flat and does not have such a steep drop as you expect it to be

[zacko]

Also, can you share the reulsting plots of pressure over flow rate and efficiency over Flow rate?

[Optimization to blades]

I had no convergence issues. Actually from the basic mesh structure to the fine one I tried in Ansys. Results are not changing that much. (I did mesh based on y+ criteria once). However I don't have a data done in real life to prove it. I am going to have it in a month... Maybe as you said it is possible to have such data but when I looked at the graphs of centrifugal fans, I haven't seen such a case. That was the reason why I interrogate and became suspicious about it... I would gladly share the results with you.

[Optimization to blades]

[IMG]file:///C:/Users/melih/Desktop/ec.png[/IMG]

[zacko]

The uplaod of your iamge didn't work.
To uplaod directly into your thread, scroll down to "Manage Attachments". Then chosse your file and click on "Upload".

[Optimization to blades]

here is the curve. And thanks again for your interest on this problem
https://i.im.ge/2024/05/21/Ku8m1m.ec.png

[zacko]

Thanks for the curves.
So, there are somewhere about 34 simulations that you have conducted.
This is really much - and I don't believe it is needed to calculate the whole curve in such detail.
You can save a lot of computational time and resources. Maybe 7-10 Points max. should do the job.
The issues here is, that many points look like outlier.

Can you share an image of your CFD domain?
Do you simulate fan and volute?
Do you have extended inlet and outlet piping?
Have you looked into the streamlines? Are there any areas of big vortices?
You said, that the mesh was okay without any convergence issues.
How strict did you set your convergence? RMS 1e-6? or RMS 1e-4?

[Gerry Kan]

Dear Melih:

Looking at your curves, aside from the plateau in pump efficiency at lower flow rates, I think you are on the right track.

Am I correct to assume that you performed a rotating reference frame simulation (i.e., rotating pump blades) to calculate the head rise at each fixed volumetric flow rate / RPM. Judging from the noise in your results, I suspect (though not with 100% certainty) that you simply took the result at the end of the simulation (either after a certain point of time or at a certain blade orientation). I don't think this is enough.

What you need to do, is to perform each run until an oscillatory steady state has been reached because the outlet pressure (and by extension the volumetric flow rate) varies depending the impeller position. Then you take the mean outlet pressure and volumetric over last impeller revolution. You should get the characteristic curves in the shape you are looking for.

To determine whether you your simulation has reached this oscillatory steady state do this you need to look at the outlet pressure as a function of time. As initial guess, the pump should have displaced at least 3 to 4 times of its volume before this happens. That is why low RPM runs take much longer, because each impeller revolution took longer (in time) to complete.

Hope that helps, Gerry.

PS - As Daniel suggested, you don't need so many simulations; a few RPMs will do. I imagine you ended up running so many because you were not seeing the results you expected.

[Optimization to blades]

Hello Daniel. Thanks a lot for your reply again and actually I did many analyses as I wanted to find out the transition of pressure-volume flowrate and efficiency at critical points. This analyse done by FLOEFD but I did the same in Ansys also by using the model together with case. Results are similar at similar working conditions. That's why I just used FLOEFD for the curves but for detailed study I am going to continue using ANSYS.
I uploaded a photo of the model I created in Fluent. But this is a simple one again.(Without y+ consideration) However I also applied y+ in meshes and results didn't change that much. The photo I am going to upload is a simple one. Other fine meshed model is not available at the moment. But simply ı uploaded a model of fan here that analyzed in Ansys.

https://im.ge/i/Kdb874


As convergence criteria I set it up to 1e-4 in ANSYS. I am going to solve it again to share the voritces with you. And actally soon I am going to test the fan in real conditions. After getting the results I am going to share it with you to compare it with results and discuss about possible reasons of differences but it will take approximately 3 weeks if everything is going as it is planned.

[Optimization to blades]

Hello Gerry. Thanks a lot for your interest in my post. What I did is that I applied rotating frame model at constant RPM and at inlet and outlet I defined pressure. I took average volume flowrate at outlet. Static pressure equals to the athmospheric pressure at inlet and at outlet for free delivery. And then increased the outlet pressure or visa versa decreased the pressure at the inlet while rotation is constant at 2900 RPM.
Thank you Gerry for your answer.

[zacko]

Can you also share a photo where we can see the fan blades and the volute channel e.g. Volute tongue?

[Optimization to blades]

Yes I can show them. Here the links;
https://im.ge/i/Volute.K76eP8
https://im.ge/i/Volute-face-hidden.K7NMkh
https://im.ge/i/inlet.K764n9
https://im.ge/i/impeller.K76GqX
https://im.ge/i/imp-2.K76nxK

here I hide one of the face in volute to show you. Normally it is full. Either case(volute), impeller and inlet are defined as fluid body in fluent.. Thats why they are not empty as it is seen in hidden faced volute. The meshed (simple) body is seen in the link below.

https://im.ge/i/resim-2024-05-27-132919947.K7NuLC


here is the model created in solidworks... The actual one is this one that I converted that model to ansys;
https://im.ge/i/resim-2024-05-27-133451582.K7Ndkf

[zacko]

This mesh is not good. It is extremely course. You need to spend much more time on meshing and especially on refinement close to the wall.
With this mesh, the results won't be accurate.