Hi,

I was wondering whether anyone has done experiments with testing a fan in a circular duct with a circular plate at the end to increase or decrease pressure within the tube that the fan has to work against.

I have this setup where I have taken the system from fully closed (i.e. pressure plate flush against the outlet of the duct to stop air escaping the outlet and load the system right up) to fulling open where the pressure plate is fully removed and the airflow is able to discharge freely into the room. In between these two extremes I have the pressure plate set at different setting from 2mm to 100mm between it and the outlet of the duct.

First I tried to model the fan for some time in CFX using an opening for the inlet (which I've modelled as a half dome to represent the air intake from the room where the tests are being done) and a mass flow outlet. Both these boundary conditions were recommended by the technicians at CFX. At the fully open load where there was no pressure plate, or the wider openings, say 100mm, the agreement with the experiments for the static pressure was good and the velocity wasn't bad, although a bit lower than the experiment. However for any readings say at 2, 5, 20 and 35mm distances the velocities are about 40% less than the experimental values and the pressures are way off. Particularly at 2mm where I am getting a static pressure reading of about 0.2Pa whereas in reality the experiment gives about 80Pa.

After much trial and error, going through the experimental results with a fine tooth comb, I tried modelling the pressure plate in the numerical model too, simulating it's distance away from the outlet for each case. This time I set the inlet as a mass flow inlet and the outlet as a static pressure outlet (entrain with zero turbulence gradient). Again the fully open case agreed well with the experimental values, but at the high pressure loadings the values were way off. This time the 2mm load gave 2000Pa and the velocities in all cases were about 30% less than the experimental.

It is a complex case as the fan is three dimensional and quite unlike any standard axial or centrifugal fan and I am trying to model a difficult physical situation. I have been playing around with increasing and decreasing the mass flow values. When I use 75% less mass flow at the inlet I get a static pressure of 122Pa and a velocity of 3.882m/s which is much closer to the experimental values of 81.37Pa and 2.68m/s. At 25% less mass flow I am getting 1100Pa and 1.363m/s. So the next thing I am going to try is incrementally lower values than 25% to try to match the experimental velocity and see if then I get agreement with the value of static pressure.

After this long explanation, the question I want to ask is whether anyone has experienced this before with this type of experimental setup. For some reason when the fan is loaded the system is seeing a lot less mass flow than is actually being produced and I suspect it is due to the back pressure causing airflow to go back out the inlet. However in CFX I thought an inlet did not allow two directional flow. In my solution I am not getting anything mentioning about CFX having to put a wall in to stop backflow. but somehow I am loosing mass flow in the system.

I am baffled and would really appreciate any input anyone might have.

Jenny

Hi Jenny,

Have you tried applying a total pressure inlet and static pressure outlet? How is the mass flow rate determined in the experiment? Are you sure you are comparing the same pressures?

-CycLone

Hi Cyclone,

Thank you for your reply.

The measurements I have taken in the experiment are the total and static pressure readings from pitot measurements taken 200mm from the outlet. From these values and the calibrated pitot tube I have calculated the dynamic pressure and thus volume flow and mass flows.

I'm definitely comparing the right pressures and have had several people (CFX engineers included) looking through my model. I haven't tried the boundary conditions you suggested, so will give this a go.

The latest thing I am going to try is modelling a different geometry for the inlet. Currently I have a dome shape in the front, but I seem to be losing too much mass flow in the system, so am just going to extend the duct as my inlet opening and see what affect this might have.

The only way I can simulate the correct pressures from the experiment are when I greatly reduce the mass flow in the system at the more loaded condition when the pressure plate is close to the opening.

Jenny

Have you compared the dynamic and static pressures at the same location as your pitot tube? When you estimate the mass flow from the pitot readings, do you assume a constant velocity profile?

-CycLone

Hi Cyclone,

Yes the pressures are being compared at a plane in exactly the same position where the pitot tube measurements were taken.

The velocity profile in the experimental results is asymmetric, so I have been using an area weighted average rather than just an arithmetic average.

I have tried the numerical model with a dome like shape at the inlet and also just an extension of the tube in case this was affecting the mass flow rate too dramatically. When I used a total pressure inlet and static pressure outlet my static pressure values were in the right ball park, but the mass flow and velocity were too low. When I use a mass flow inlet condition with a static pressure outlet then I get a really wonky pressure reading when the outlet is being choked by the pressure plate, but the velocities are more realistic. However I don't understand how the velocity still doesn't agree with the experimental value when I put in the mass flow value obtained from the experiment. This just shouldn't be possible since mass flow is directly proportional to the dynamic velocity.

I've got a CFX engineer currently investigating the problem, but we are all a bit stumped at the moment.

Thanks for your reply.

Jenny

Which velocity doesn't agree?

The problem may be with the experimental evaluation of mass flow rate. A single pitot tube measurement only tells you the velocity at a single point, but you need to integrate the velocity variation over the surface to get the mass flow. Assuming a velocity profile will add some error to this calculation. It also depends on the pitot tube being aligned with the flow and properly calibrated for the experimental Reynolds number. This is not to suggest that the simulation is right, just that experiment has errors too.

Also be careful comparing averaged data at a plane with a single point of data, such as your pitot tube measurement; these will not be the same. You should locate a point at the same location in space and probe the pressures at that point.

Finally, some degree of error is normally expected. These arise from a number of sources:

1. Modeling errors arise from assumptions about boundary conditions, missing features, simplifications (periodicity, symmetry, defeaturing), fluid properties and physical models (turbulence), 2. Numerical errors arise from grid resolution, grid quality, computer precision, numerical models, etc. 3. Solution errors arising from unconverged systems and computer precision.

Most of our discussion thus far has centered around the modeling errors, which are usually responsible for large discrepancies between simulation and test results. One common problem is the test set-up can be quite different from the simulation set-up, although it sounds like your modeling the test set-up, which is good.

If you are satisfied that the model closely matches the test, I would start to look at the other two sources of error. CFX is well proven in industry for these applications, so accurate results are attainable.

-CycLone

Thanks again for your reply.

The velocity at the plane where the pitot point readings were taken doesn't agree with the experimental. I have done some theoretical calcs and the mass flow rates are very similar to what I'm getting experimentally, plus I've gone through the experimental results with a fine tooth comb and recalibrated the pitot tube three times now. So I am as confident as I can be with the experimental data.

The pitot readings were not taken at a single point in either the experimental or the numerical work. I took 6 readings across the diameter of the tube in the vertical and horizontal, following the British Standard for fan flow analysis. I've integrated the velocity variation over the plane where the readings were taken to get the mass flow.

I'm going to try and run the model without the fan in it and see how this compares in case there is something fundamentally wrong with the setup, otherwise I'm almost out of ideas on how to get the static pressure, velocity and mass flow results for the numerical working ALL agreeing at the same time, with the experimental. If I get the pressure close then the velocity and mass flow are off, and vice versa.

Thanks again for your suggestions and advice.

Jenny

I wouldn't expect the answers to be exactly the same at all operating points. Assuming you are confident that you are comparing the same data and the boundary conditions and geometry are sufficiently similar, I would look into what is happening at the fan when the simulation deviates from the test results.

Also verify that your inlet turbulence level is reasonable.

Earlier you mentioned a loss of mass, can you please explain? If you applied a specified mass flow, the inlet flow should match this (note that if there is a pitch change, the mass per full revolution is conserved, the mass per pitch could be different).

-CycLone