[Wolfram]

Dear all,

I am facing a physical not valid flow pattern - i think. When simulating a fan with really low flow rates (10m^3/hr), the entire upstream inlet domain in front of the impeller starts rotating. The flow enters inlet straight (in dependeny of the inlet BC) and the more iterations, the stronger the swirl becomes upstream. So it has to be induced by the impeller.
In front of the impeller you can find a small grid. The simulation is running with k-epsilon, frozen rotor and the following BC:
https://www.bilder-upload.eu/bild-2d...51403.jpg.html

Here you can see the swirling inlet:
https://www.bilder-upload.eu/bild-e0...51444.jpg.html

Switching to first order in advection scheme reduced the swirl remarkable, but is still persistent.

Due to the swirl directly in front of the impeller, the head is much to low in comparison to the performance curve. High volume flow rates show a good match regarding head with performance where the pre swirl does not occur.

I made an attempt with a porous media as inlet domain. To prevent any swirl, i set the permeability close to zero for theta direction. Surprisingly the head hits the performance curve really close for the entire operation range. But for sure i cannot rate other inlet geometries with this porous media. Here you can see the reduced swirl:
https://www.bilder-upload.eu/bild-72...53980.jpg.html


--> So is this pre-swirl for low volume flow rates a numerical phenomenon?


Kind regards

Wolfram

[Opaque]

Questions for thought:

1 - Are you using the Alternate Rotation Model? Otherwise, there will be numerical errors for axial flows in the stationary frame.

2 - Have you evaluated alternatives model to the Frozen Rotor approximation? Recall this is a major approximation.

3 - Using Upwind to obtain better results is a sign that something is wrong elsewhere. Upwind should only be used to obtain converged solutions to start cases which more accurate schemes when those cases do not converge from poor initial guesses. I will not trust an Upwind converged solution where there are velocity gradients.

4 - Have you contacted ANSYS CFX turbomachinery specialists for assistance?

[Gert-Jan]

- I would have made my inlet geometry significant larger.
- I think this can happen in real life, depending how the inlet close to the fan looks like. You mention a kind of grid. Can you show the exact geometry?
- is this the same geometry that was used in the test by the fan supplier? Or did he use an anti-rotation device?

[Wolfram]

Originally Posted by Opaque

Questions for thought:

1 - Are you using the Alternate Rotation Model? Otherwise, there will be numerical errors for axial flows in the stationary frame.

2 - Have you evaluated alternatives model to the Frozen Rotor approximation? Recall this is a major approximation.

3 - Using Upwind to obtain better results is a sign that something is wrong elsewhere. Upwind should only be used to obtain converged solutions to start cases which more accurate schemes when those cases do not converge from poor initial guesses. I will not trust an Upwind converged solution where there are velocity gradients.

4 - Have you contacted ANSYS CFX turbomachinery specialists for assistance?

1 - Alternate rotation model is applied

2 - Tried Mixing Stage as well, without huge change. The fan consists of one blade row (impeller only). The upstream grid is nearly axially symmetrical.

3 - Using upwind was just an attempt. In Autodesk CFD there is an option called "adv5_no_dtime_flag" for the advection scheme and the issue of rotating inlet was solved.

4 - I have not contacted the turbomachinery specialists for assistance. Is there a special site for this? I have found the general contact regarding their products and so on

[Wolfram]

Originally Posted by Gert-Jan

- I would have made my inlet geometry significant larger.
- I think this can happen in real life, depending how the inlet close to the fan looks like. You mention a kind of grid. Can you show the exact geometry?
- is this the same geometry that was used in the test by the fan supplier? Or did he use an anti-rotation device?

I have enlarged the inlet geometry and designed it is a cube. The swirl within the huge inlet decreased and is negligible. But the swirl in the duct upstream the impeller has not changed.

The grid consists of simple struts reaching from one side to the other as you can see in the picture posted above: https://www.bilder-upload.eu/bild-2d...51403.jpg.html
The main purpose of the grid is to shelter the user to stick finger inside the fan.

The simulated geometry and the geometry tested in our test bench is equal.