[warex]

Hello all,

I am a brand new user to CFD, this is my first attempt at a simulation in fact. I am using Solidworks 2009. I am looking to compare various different impellers in a centrifugal pump application. I was able to follow the tutorial with moderate sucess but i had a few questions/problems.

Here is my setup:

Inlet Boundary Condition: Environment pressure at 101325 Pa
Outlet Boundary Condition: Environment pressure at 101325 Pa
Global rotating reference frame: 210 rad/s (2000 rpm)
Fluid: Water
Walls: Pump housing walls set to Stator.

Goals:
Inlet Static Av. Pressure
Outlet Static Av. Pressure
Torque on Impeller
Surface Flow Rate Out
Equation goal = pressure drop (outlet press - inlet press)
Equation goal = efficiency of impeller (pressure drop*flow rate/angular vel/torque on impeller)

Results of goals:
Inlet Static Av. Pressure = 88687 Pa
Outlet Bulk Static Av. Pressure = 100573 Pa
Torque on Impeller = -0.1898 Nm
Surface Flow Rate Out = 0.005 m^3/s
Equation goal = pressure drop
Equation goal = efficiency of impeller = 1.58 = 158%

As you can see the efficiency is definitely wrong as you would assume it to never be above 1. I do not know if the values of torque or pressures are reasonable as I do not have much experience. The one thing I have done different than the tutorial is my inlet boundary condition is environmental pressure and not a flow rate. I felt that it was strange that you would feed a pump with external flow rate and I would rather evaluate the performance of the impeller with no external help.

I will be evaluating many different impeller geometries so utilizing efficiency as a performance metric would be very useful. I just want to make sure that my boundary conditions and goals are reasonable.

Thanks for everyone's help.

[warex]

Can anyone shed some light?

[Boris_M]

Hi warex,
if your model is more complex than the tutorial model and you use the outlet opening of the real pump and not a ring like opening as in the model you should use "bulk avg." for your goals as the massflow is also considered in the average not just the surface. You would notice the difference as soon as you have a non equally distribution of the velocity on the outlet.

But most important you have to define a volume flow rate for the inlet. This is the way the boundary conditions (BC) for the rotating regions work the most stable and accurate. You have to think of three different zones, the inlet non rotating zone, the rotating zone and the outlet non rotating zone. Each zone receives a flow rate inlet condition and a pressure outlet condition. You cannot control the BC of the rotating region, they are setup automatically with the definition of the feature rotating region. So the outlet of the inlet zone is pressure and the inlet of the rotating region is flow rate and these two are automatically connected.
I assume you want to record the pump curve and with that you can simply run several projects with predefined volume flow rates and get the corresponding pressure difference, efficiency etc.

Try this and it should work, let me know the results. I'm curious :-)

I hope this helps,
Boris

[warex]

Thanks Boris, my model isn't very different from the tutorial. It just has a different impeller but it still has the flow exiting around the circumference, rather than through a volute. I have been using the measurement ring as in the example to measure bulk average static pressure on the outlet.

I see your point on the inlet flow rate boundary condition, i needed to think it over to convince myself but i think i understand now. I have run different projects, as you suggested, with flow rates from 10 gpm to 100gpm in 10gpm increments with a constant 2,000rpm rotation of the impeller. First, I set the inlet volume flow rate and ran all of the projects. I graphed average static outlet pressure vs. flow rate and the graph wasn't what i expected. I expected a graph similar to a characteristic curve where head decreases as flow increases. My graph showed that pressure actually increased as flow increased. I decided to set the flow rate BC to the outlet rather than the inlet and that is when I got a much better graph. The pressure decreased as flow increased. However, my efficiencies were all still above 100% which cannot be accurate.

Here is an example of my goals output when I had the inlet BC set to 0.00315 m^3/s and outlet to environment pressure.
Goal Name
Unit
Value
Inlet Mass Flow
[kg/s]

3.146309726

Outlet Mass Flow
[kg/s]

-3.141098274

SG Av Static Pressure Inlet
[Pa]

87997.56573

SG Bulk Av Static Pressure Outlet
[Pa]

99085.58974

Impeller Torque
[N*m]

-0.26255882

SG Volume Flow Rate Outlet
[m^3/s]

-0.003148776

SG Volume Flow Rate Inlet
[m^3/s]

0.003154

Impeller Force Z Dir
[N]

34.44710258

Av Total Pressure Out
[Pa]

79060.6853

Pressure Drop
[Pa]

11088.02401

Flow out in GPM
[ ]

-49.87661429

Efficiency
[ ]

0.633213315

This looks reasonable, but when i do multiple different flow rates at the same RPM, they do not follow a trend I would expect. When i switched to the outlet flow BC then it started trending much better, but my efficiencies were way off.

As you can see i am still fairly confused

Thanks for the help.

[Boris_M]

Hi warex,
since you are unsing SWFS the first time it would make sense to test your calculations on models that already have been measured, so existing pumps where the pump curve is known and you can validate with them.
The thing with expectations is, they can be wrong.
I know of several companies using SWFS or FloEFD in the pump industry and get great results also with cavitation. This is why I would recommend you to test it on an existing product and compare with known results better than expectations.

I hope you understand. One would expect bumblebees should not be able to fly, but we all know they do :-)

So please try to confirm your calculation on an existing model first and you should see it matches the results very good. It's hard to guess whats wrong from writing here and if that test doesn't work, kontakt your support and let them help you.

Boris

[warex]

I understand, thanks for the advice i'll have to try to get my hands on some existing data. I'll figure it out eventually, this is just a side project anyway so i won't have too much time to work on it. Thanks for all your help!

[ihadi]

hi all

I want to simulate pump impeller,to
can help me anyone,by sending me any tutorial

then i want to adding Fluid-structure interaction into simulating.

thank you for help me.

for.learn@yahoo.com

[Boris_M]

Hello ihadi,

the tutorials for such a case come with the software and there is not much fluid-structure interaction you can do. FloEFD/SW Flow Simulation is a CFD code, no FEM is provided by the developers of that code. There are some interfaces to FEM codes to provide the pressure and temperature loads but there is no feedback from deformed geometry to CFD that you can use directly and create some loop in simulation automatically.

Boris

[ihadi]

hi Boris

I've been working in this field.
But this time I used this method to analyze a pump as close to reality.

Unfortunately I do not have access to Ansys Training Center.

please if you have any filese or linkes send to this Email.
new Email address: for.learning@ymail.com

[Boris_M]

Hi ihadi,

I think you are in the wrong forum. This is about FloEFD/SW Flow Simulation and TloTHERM, not ANSYS products.

Boris

[abbas_madraswala]

Hi,

I want to perform CFD analysis of centrifugal pump in Swx Flow Simulation. I have the actual pump testing curve (Volume flow rate vs head) and the pump CAD model. I have define the set up as per above settings but many times I got an error "Solver Abnormally terminated". Some times it got solved but I observe that the volume flow rate, static pressure value at inlet and outlet, and torque values were very high. Also the flow was leaving from pump from both the ends i.e. inlet and outlet.

Kindly help me out and suggest how should I define the problem.
Thank you for the help in advance.

[Boris_M]

Hi Abbas,

How did you apply the boundary conditions on inlet and outlet, what type of conditions are they, pressure or flow.
Also does your rotating region basically block the whole flow field or is there a gap between it and the housing for example in which flow can pass without going through the rotating region?

Boris

[abbas_madraswala]

Hi Boris,

I have applied Volume flow rate at inlet and Environment pressure at outlet. Please refer to the attached image for rotating region. I have marked the rotating region in green colour.

[Boris_M]

Hi Abbas,

there are a few improvements you can do on the rotating region. On the bottom side of the impeller (rotor) you don't need an rotating region in the fluid if there is no geometry that is rotating through the fluid. If it is just the flat surface without anything sticking out of it like a blade or rib that would drive the fluid in any way, you can have the rotating region go inside the solid and simply define the rotor surfaces that are not covered or just partially covered in the rotating region as a rotating wall so the fluid is only driven by the wall friction of the rotating wall. That only works on circular or cylindrical surfaces that do not have any extrusion at local spots. on the rotating disc.
For example you take a music CD as a rotating disc. All the surfaces of the CD can be used as rotating surfaces as only the wall friction will drive the fluid to rotate near the wall, there is no extrusion like a fan blase or like a nail that is sticking through the CD that is out of the rotation centrer and at some local spots. If there is a rib that is circular and is rotational symetric going around the center as its own center then also just the rotating wall is enough, you don't need a rotating region.

But if you have like a nail or a block or like a impeller blade sticking out of the CD then you need to have them inside a rotating region. If they are only on the top surface of te CD then the rotating region can end inside the CD plane (not at the surface but inside the solid) and the back side can be used with the rotating wall.

The reason for that is that you should use at least three cells between the solid and the rotating region surface and then again between the surface of the rotating region and the next solid. So at least 6 cells in the fluid whereas this is not necessary for a rotating wall. These minimum 3 cells are necessary as there is a hidden boundary condition applied by FloEFD automatically to provide the interface from fluid leaving the non rotating region into the rotating region. So similar as if you apply an outlet boundary condition on the outside of the rotating region and an inlet boundary condition on the inside for the flow coming into the rotating region (RRF). After the flow enters the RRF it need a few cells to react on any geometry to flow around them in some way. Therefore you need at least 3 cells to get good results.
Now with your very thin distance between the RRF and the rotor like on the front face of the cylindrical face on the bottom of the rotor (in -x direction) or on the thin distance on the curved top surface that covers the impeller flow region (see red arrows), there would be a very fine mesh necessary. I'll try to produce some images that will explain it a little bit better in another post.


Boris

[Boris_M]

Ok, sorry for my low artistic capabilities

Below you'll find two sketches on which I will explain in more detail what is what. The top of the models are the section views of the model which is shown with the black dashed line in the top view of the model below. That makes it easier to show how the rotating region and the rotating walls are applied.

Model 1:
This is the plain disc where the red lines (also in the other images red) are the rotating wall boundary condition. Here you don't need any rotating region because only the moving wall is basically pulling the fluid with it due to the friction.

Model 2:
Here you see an extrusion outside the center. Since it is outside the center and therefore rotaing around the center, it will need a rotating refion (yellow frame) and will not work with the rotating wall approach (red line) only. But you can see I left a larger distance between the object and the block for 3 cells you could say. Lets assume there would easily fit 3 cells to the left of it and to the top and there is more enough space to the right. I can move it closer to the block but then the cells need to be smaller and that would cause more cells in the whole model and hence more CPU time to solve it which we want to avoid as long as the flow is resolved enough by the mesh.

Model 3:
This model has a ring as you can see from the top view and is therefore perfectly fine with just rotating walls as it goes around the whole disc and the rotatinal center is in the center of the ring.

Model 3:
This comes closes to your impeller if you consider the blocks the blades in your impeller. You can see that I use the RRF (yellow) only around the blades and it ends also like in Model 2 inside the disc. All the other faces of the disc that are also rotating are covered with a rotating wall contidion. You don't have to split the surface to only select the part that is red until it contacts the RRF, if the rotating wall has the same rotational velocity as the RRF, the relative velocity to the RRF is 0 and therefore rotate with the same velocity also in the simulation.
In this model you can see how I saved a lot of cells by not going ouside the top and bottom walls of the disc with the RRF which would need 3 cells between the bottom and top surface and the RRF surface and we assume that the gap between the discs are resolved with more than 3 cells to resolve the flow so here we have min 3 cells too and we only need to make sure there are min 3 cells to the left and right of the blocks from block to RRF.
Now if you also have an shaft going along the rotational axis (green dash) then that is of course rotational and centric with the rotatinal axis and therefore also only needs the rotating wall and not a RRF as in your model on the bottom side of the impeller.

So summarized: Keep the RRF simple and not to many dents and cuts and ribs and if possible inside the material if the other side of the material can be used as rotating wall. For example the top of your rotaing region (in positive x-axis) is movig into the impeller again which is not necessary if not some geometry that is a stator would come in from the top and would cut into the RRF.

I hope that makes it clear.
Your boundary conditions are good and you should try to deactivate the maximum travels in the calculation controls as such rotating simulation might experience some flow out of the model in both ends for some time as long as the calculation is converging but that should vanish over time. But if the maximum travels is activated it might stop the calculation before it is converged. However it should not stop with abnormally terminated. In such a case check what the maximum/minimum velcitied, pressures and temperatures are. Maybe there is somewhere a cell fraction that causes the results to go crazy and then it aborts the calculation abnormally. Usually there should be a result file called r_abnorm.fld which you can load manually and have a look at the extreme values and where they are. It helps to deactivate the interpolation to see the exact value of each cell. These crazy cells would be red and right next to them they would be blue because the values are so much higher or if so much lower, the red blue would be the other way around.

I hope this helps.

Boris

[abbas_madraswala]

Hi Boris,

Thanks for providing such a good explanation about the rotating region. This has cleared my doubt about real wall boundary condition also. I will make the changes accordingly and try it.
Thanks for the help.

[abbas_madraswala]

Hi Boris,

I made the changes as you mentioned above and it got solved without giving any error.
Below are the results which I have got:

SG Av Static Pressure 1: [Pa] -1022579.18
SG Volume Flow Rate 1: [m^3/h] 30.0000
SG Av Static Pressure 2: [Pa] 101325.00
SG Volume Flow Rate 2: [m^3/h] -32.7014
SG Torque (X) 1: [N*m] -64.490

As per the experimental result For flow rate of 30 m^3/h, the head should be 130 m.

Here the pressure difference and torque value is high. Also the volume flow rate at inlet is little higher than the inlet flow rate.
Let me know your feedback on this and any suggestion required to get the required output.
Thanks

[Boris_M]

Hi Abbas,

I guess the 2.7 m^3/h difference in the flow rate comes from a not yet converged solution. I cannot tell for sure as I don't have the convergence plot, criteria and delta.
For the head you expect I cannot tell. If I'm not mistaken you currently have around 104 m. If the mesh is not good enough it might result in deviations but I cannot judge on that.

Boris

[abbas_madraswala]

Hi Boris,

All the goals had converged. I have attached a snapshot of the goal plot. please find the attachment.

[Boris_M]

Hmmm... looks good from the convergence. Sorry but I cannot tell what it is here. I suggest you contact your support team to have a look at the model. They should be able to find out what the issue is.

Sorry,
Boris