It's an internal analysis with a local rotating region and without cavitation. I am using inlet volume flow and outlet total pressure BCs.
have you already looked through the other posts about this? almost always this is related to setup and not following recommendations about the rotating region. have you already seen the recommendations in the kb and the solving engineering problems document?
can you elaborate on your setup. what inlet and outlet conditions are you using?
finally, you mentioned some very specific parameters that you're looking at, what do other parameters look like? velocity, pressure...etc do they look like they are trending to what you expect? if you make a change like rotation speed..etc, does it trend in the right direction? this could indicate a difference between physical and simulation.
there are verification problems in the tech reference that show how the software has been validated so i would guess setup or mesh.
Yes, I have been browsing this forum a lot and read about proper setup and rotating region in multiple sources. However, the sources have not provided uniform information. In one case two official support technicians have given recommendations that are in total contradiction against eachother.
I am using inlet volume flow and outler total pressure.The other parameters look completely normal. There are no abnormal changes in pressure or velocity and the outlet volume flow (goal) matches inlet volume flow (BC). Torque and inlet pressure are the only weird ones. The torque goal contains all impeller surfaces in contact with liquid.
Every single source I've searched information from has had a different answer to the rotating region. Some say it should be between the chamber wall and the impeller, others say it should reach inside the chamber wall. The official support technician of SolidWorks told me the rotating region should not go outside the impeller at all, instead it should be like in this picture. It was the first shape that actually gave some sensible results and made the simulation converge. When the region was outside the impeller, small glitch points where the velocity suddenly jumps to supersonic speeds were constantly appearing. With this shape the pressure drop and torque are too high though.
The performance of pumps is often staten in relation to volume flow. For example we want to find the efficiency and pressure drop at different volume flows, like 5 l/s, 15 l/s, 25 l/s etc. I have ran the simulation with varying volume flow and the direction of change in outcome values is correct; when volume flow is increased, pressure drop decreases and efficiency increases. Just as expected. That would imply the setup is not the problem, wouldn't it?
The last one we did we followed the recommendations from the solving eng problems and kb and it worked pretty well. In that case the rotating region was sunk into the walls of the volume and appropriate stators applied.
Inlet flow and pressure outlet seem like the appropriate setup. Total pressure I'm not sure about, generally I've seen static.
If you question the answer from your var, have them contact the developers.
The other option is to post your model and what you are comparing against and a list of your assumptions and approximations made.
In this case, due to 3-dimensionally twisting and widening spiral shape, it is impossible to sink the rotating region inside the chamber walls while making it uniform, axially symmetric and not intersecting with the inlet channel.
I have used both total and static pressure, they give the same outcome. What's the practical difference with these two boundary conditions?
The vars have been forwarding my questions to developers.
I uploaded my model here now. Here are a couple of values from actual measurements:
Volume flow 0.015 m3/s --> Inlet pressure = 200 kPa, Outlet pressure = 390 kPa, Power = 7 kW, Efficiency = 70%
Volume flow 0.025 m3/s --> Inlet pressure = 200 kPa, Outlet pressure = 420 kPa, Power = 5.5 kW, Efficiency = 64%
The difference in pressure should be around 200 kPa, but in my simulations it always goes up to 400 kPa (regardless of how much the boundary condition pressure is). The motor power (torque * rad/s) is also too big by an equal relative amount.
CFD.zip 3.3 MB
Rotating regions are difficult. I'd just like to point out one assumption that may be affecting the results.
In a rotating region, the assumption is that the pressure is the same all the way around the circumference of the rotating region. This can be a problem when you have an opening at one end of the pump. It can also be a problem if there is geometry which is close to the rotating blades. This assumption can highly affect the accuracy of your results.
Unfortunately, the way to get around this is to have something called a "moving mesh" which Flow doesn't have yet.
With this assumption in mind, your best bet is to create a rotating region which covers the entire impeller like the one attached.
All the best,
Impeller 35112.SLDPRT.zip 792.5 KB
I'm not sure I understand your first comment about the shape of the region, are you sure you aren't overthinking it? Even if it falls into open space, what is ok. Same with overlapping faces, deal with them with stators.
Regarding total vs static pressure, generally static but really doesn't matter as much since the pressure difference will be what stays constant relative to your set pressure at the outlet.
Regarding the comparison, can you give more details about the testing setup? Is the model exactly the same as physical? Orientation the same? Materials the same..etc?