Hi, I am running an unsteady, incompressible 3D study of a sewage pump (single screw or spiral type blade, basically a single blade). I am using a segregated solver, a time step of 10 degrees and the fluid is water. I have specified a pressure at the outlet of 400000pa (40m) and a pressure at the inlet of 0pa. I am using a sliding mesh simulation and my rotational speed is 305rad/s (approximate 3000rpm). It is not run as periodic. However, when I run this problem, flow seems to be entering thru the pressure outlet and exiting through the pressure inlet. The mass flow rate and velocity vectors show this. I checked that the blade is rotating in the correct direction (!!!!) and it is. I am still on the first couple of revolutions, but should this problem still exist? I can understand that it may seem logical to the sofware to specifiy that the flow is moving from the high pressur to low pressure in the beginning, but shouldn't it figure out soon what is going on?? Has anyone experienced this problem when working on a pump or other device? Has anyone any idea?? All help appreciated. Jack.

(1). If the fluid is considered incompressible, then, all you can do is to specify a pressure somewhere at a point. Is that right? (2). At the inlet, you specify the pressure at 0.0 PA. Is that vacuum? (3). Can you specify the inlet velocity? (or mass flow rate)

HI John,

Yes, you specify the pressure at the surface or face which is the inlet. The pressure is set uniform to whatever you specify at this face. It is the static pressure. A pressure of 0 at inlet and 400000pa at outlet simply gives a pressure difference...?? No?? I mean, I could just as easily specify the pressure at inlet as 100000 and add 100000 to the outlet pressure. I could specify the mass flow rate at the inlet, yes, would fluent then calculate the pressure at inlet and outlet?? I guess it should. I had no problems with this procedure in the 2D analysis. Why do you recommend using the mass flow rate rather than the pressure as the boundary condition?? Thanks for your help John, Jack.

(1). I was just trying to point out that the problem you were having could be related to the boundary condition specification. (2). Now, if the rotor is not moving , do you still use the same condition? (3). Or if the exit pressure is such that the mass flow rate is zero, then, what are you going to do? (4). I am just trying to see whether there's something wrong with the boundary conditions. (5). Well, if it works for the 2-D, then it should also work for the 3-D. (check the user's guide or the tutorials for the boundary conditions, and make sure that everything's consistent)

It may be an error in the Fluent post-processor. I posted a message about a similar problem a while ago and got no repsonse. Plots of relative and absolute velocity vectors in a rotating problems appeared to be incorrect, i.e. some showed flow in the wrong direction and were not consistent. Have you compared relative and absolute velocity vectors and contour plots?

Hi, the pressure drop for starting case is too large. You must specify O Pa at the pressure outlet and check the direction of flow. If the direction is correct you will increase the pressure at outlet. The outlet pressure you must increase step by step, the pressure increment is based on a models, convergency, discretiztion scheme, etc. And the second note, is the efficiency of your spiral blade enough? Best Regards Pavel

Thank you Pavel,

I will try this. I recieved an email this morning saying that my problem may be due to Numerical stall....It was suggested to try using mass flow rates as my boundary conditions rather than pressure...similar to John C. Chiens suggestion. When you say that the pressure increment is based on models, convergence, discretization, etc., what do you mean? I choose a pressure increase with regard to these? HOw do I do this? Also, in experimetal work, the pump is capable of pumping fluid upto a pressure of 7 bar at the speed I am using in the model...so yes, it's effiency is o.k. Thanks for your help.

Sometimes you can set the final pressure by two steps and sometimes during ten steps. The pressure increment you must find by test. The second way is to use the mass flow rate, but the convergency is slower than pressure b.condition. All task with rotational fluids show a sensitivity on opposite pressure. Very often you can see the opposite direction of flow a you don't change the direction of increase on unrealistic speed rotation ! The large pressure drop influences very strong the direction of flow. I thing that two way are possible: 1. increase the pressure step by step, 2. use the patch of velocity (maybe axial only) for correction of flow direction.

As you can see the experimental comparison is very useful. :~)

Best Regards Pavel

Have you check the sizes of delivery and suction side(i.e pipe size)or connections.