CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   Having a few problems in simulating a rotating impeller (http://www.cfd-online.com/Forums/cfx/82895-having-few-problems-simulating-rotating-impeller.html)

ajinsan December 8, 2010 13:59

Having a few problems in simulating a rotating impeller
 
Hello,

i'm studying mechanical & process engineering in germany.
I am working on my bachelor thesis for about 6 weeks now. In my university there was no stuff like simulation softwares , so everything about cfx was absolutely new to me.


In these past 6 weeks i learned a lot about cfx and its theoretical backgrounds. This forum was a great help, and i’m very grateful for this community.


Now i am reaching a point, where i cant finish my works without somebodys helps. So I try this way, maybe someone here could support me.
First I need a confirmation for my works, wheter it is right or wrong. Secondly i would like to provide some questions about things which arent comprehensible for me.


1.)
The attached picture shows the fluid model i have designed in design modeler using the enclosure function. I have seprated the model into two stationary and one rotating domain.
The impeller doesnt exist as solid. While the rotating domain is set up with a angular velocity, the „Wall_rotating_frame“ is setting to „Counter Wall“.
Following BCs are adjust in this simulation:


Inlet :
massflow; turbulence option zero gradient

Outlet:
Opening ; opening pressure and dirn 0 Pa; turbulence option zero gradient

GGI Interfaces @ contact areas:
general connection; frozen rotor; pitch change automatic


It is a single phase, steady state simulation with a reference pressure of 0 atm using shear stress transport (as i read its the best option).
The massflow and the angular velocity oft the impeller are known values, which i gather from a experimental test. Also the pressure drop is known.



I want to know the following results:
- The force in fluid direction which affects the impeller
- The torque at the impeller


Does this work?????

2.) In post processor the streamline rotates in the wrong direction althoug i define a positive angular velocity, so i must set up a negative value.
Thereafter everythings working fine and the streamline goes into the right direction with an apparently realistic course.



Just dont get it, doesnt the rotation be subject to the right hand rule???


Im sorry for grammatical and spelling mistakes.
Hope sbdy can help me. I still have two months to finish my thesis.




http://img811.imageshack.us/img811/8636/fluidmodel.jpg

ajinsan :):):):):):):)

joey2007 December 8, 2010 14:50

I am not really an expert on turbo machinery simulation. However I will comment a bit on your setup.

  • The combination of massflow boundary with pressure boundary should be good solution.
  • Frozen rotor means that you model the geometry stationary and the influence of the rotation by rotational forces. It depends on the physics if these assumptions give reasonable results. Subsequently it is not resonable to just describbe the setup and then ask if it is right. The answer depends on the setup and the "real" physics of your application. So description of the latter is also required.
May be the others can comment a bit more.

Allow me some additional remarks: IMHO Neither it can be expected from a bachelor student to know this stuff nor it is healthy to work in while the short time of a bachelor thesis without any support by a experienced advisor. So my recommendation for your future master thesis seek better advisors who can explain you the stuff you can not know from your lectures.

saravana December 9, 2010 04:11

Rotating Impeller
 
Hi Ajinsan,

Welcome you to the field of simulation.
As, I have been working with similar Impeller simulation for some time, I think i can help you to some extent.

1. If you apply "Counter rotating wall" condition to a rotating domain wall, then those walls will be considered as stationary one. So just have a cross check over there.

2. opening pressure and dirn 0 Pa: This boundary condition need to be checked again. Because in general Impeller pump produces some considerable perssure depend upon the application. So 0 Pa seems to be bit unrealistic. The problem of rotation in the opposite direction may also be because of this!.

3. If you have considered the complete Impeller model in CFX you can give pitch change option as None.

4. Force and Torque can be calculated very easily using CEL commands with proper surface selection.

Best wishes.

Saravana

Hutaru December 9, 2010 04:48

Need information
 
where the right place and the right site to get any tutorials of ANSYS CFD, particularly in Ship RESISTANCE???

Max Efficiency December 9, 2010 05:55

You are right with the direction of rotation: Your thumb of your right hand is showing in the positive direction of z-axis (rotation axis). Your curved fingers then shows the positive direction of rotation. Don't forget: the impellers of blades in pumps etc. are often backwards curved. Keep that in mind when using right hand rule.
And don't forget: in Post you normally analyse the relative velocity components. They are showing in the other direction (compared to absolute velocity components).

And please be careful: Within a rotating domain the velocity-setting "counter-rotating" for wall-boundary means, that this wall is a stationary wall without any rotation. You need this options for walls in a rotating domain, that are still standing in reality (for example walls that belong to the casing).

ajinsan December 9, 2010 18:15

Thanks everybody for replying. :):):)

As the Inlet-Domain and Outlet-Domain are stationary domains, i thought i always would have to apply the "counter rotating wall" condition for those walls?!?!

I already changed the outlet boundary condition. now it is 2 bar.
In my simulation I defined some input parameters for inlet and angulary velocity.

Inlet: 50 l/min , 40 l/min , 30 l/min, 20 l/min
Outlet: 2 bar @ every design point
Angular Velocity: real values which depend on volume flow (Expression:massFlow/997[kg*m^-3]*60[s*min^-1]*1000[l*m^-3]*number of revolutions[rev*l^-1])

The mesh consists of 400 000 elements. The contact areas (ggi interfaces) are adjust at 100 relevance.
The solver runs 300 iterations per design point.

The results seems correct to me. The streamlines rotates in the right direction and in a realistic whirl. Showing vectors on the impeller provides arrows in the rotation direction.


Though I am thinking I am on the right way, I am insecure because of the display of the streamlines. I dont know which display options are right.
I took the velocity streamlines on stn frame (hybrid) as i think it is posting the right running of the streamlines.

Now I believe it is not right because conservative results shows more realistiv flow. Is it because hybrid let them streamlines interrupt at walls because of the wall boundarie conditions (velocity= 0)? I have read the definition of hybrid and conservative in the help before, but it would be great if somebody could confirm my thoughts.


For my goal it is not important wheter the results on the impeller (force, torque) are highly accurate or not , because I just need trends for comparing two models.


Thank you all for your help.
I caught a cold yesterday and I am feeling very sick, so I am really sorry for spelling and grammatical mistakes or when something is incromprehensible.

ajinsan :):):)

Turbomachine December 15, 2010 05:30

Hi,

firstly, as for the boundary conditions, you have to set the inlet and outlet as stationary. However as soon as we are talking about he rotor it is defined in a rotating reference frame, hence the counterrotating adjustment for the shroud it appropriate.

secondly, im am not sure why you are working with an opening type outlet. This is not a proper boundary condition for an impeller, because it allows reverse flow to occur. I would recommend setting an outlet type condition intead. If the flow solver crashes because of reversed flow at the outlet, try moving the boundaries further away instead.

thirdly, i think you should reconsider the boundary conditions you are using. Recently, you have changed the outlet pressure from 0 to 2 bars which is a huge change. It the impeller is runnign at low speeds you can still get surprisingly good convergence, but the results will be far away from the reality. To put it in another way, you can get nice colourful plot, steamlines etc., but the significant data i.e pressure ratio, efficiency will be completely false. You must also get an accurate work input value to get correct results.

suggestions: try to determine the outlet pressure of the inlet first at design point with 1D calculations. Hint: use the TE and LE angles and the mass flow rate. Check the velocity triangles and Euler's pump equation. Your may also have to write a few program lines to iterate. Only then go about doing the simulation.

archeoptyrx December 3, 2015 10:45

Hi,

I have some question related to this. Say I have a rotating domain Rotating at 100RPM. One side of the domain has to rotate at 1000 RPM. So I should specify wall velocity of 1000RPM at that wall right ?

Or Should I have to specify 900RPM to that wall (as the domain itself is rotating at 100RPM) ? .

I am confused on how CFX takes in the boundary conditions.

Kindly assist.

kjetil December 3, 2015 13:00

Couldn't you just say that both of them are rotating? The rotation is set for domain motion.

archeoptyrx December 3, 2015 13:56

The model i have has two surfaces rotating at different speeds. I can assume the stationary domain and specify two different wall motions. Wall _A = 1000 RPM and Wall _B = 100RPM.

I am confused how will be the boundary condition for a rotating domain. Say the domain rotates at 100 RPM. Wall_ B = Counter rotating wall. Wall_ A ?

Thanks
archep

ghorrocks December 3, 2015 16:57

The domain rotation should be at the speed required so the mesh sweeps out the correct geometry. For instance if you have a rotor with blade passages you need to set the rotation speed of the domain to the rotor speed.

But rotating walls can be modelled using tangential velocity boundary conditions. You do not set the speed of a rotating domain to a wall speed as the mesh does not sweep out any required geometry if it is just a rotating wall.

I don't know if that makes things clearer but there is a lot of confusion between wall speed and rotating domain speed.

archeoptyrx February 4, 2016 15:06

Quote:

Originally Posted by ghorrocks (Post 576112)
The domain rotation should be at the speed required so the mesh sweeps out the correct geometry. For instance if you have a rotor with blade passages you need to set the rotation speed of the domain to the rotor speed.

But rotating walls can be modelled using tangential velocity boundary conditions. You do not set the speed of a rotating domain to a wall speed as the mesh does not sweep out any required geometry if it is just a rotating wall.

I don't know if that makes things clearer but there is a lot of confusion between wall speed and rotating domain speed.


Hi Glenn,

Ok. To make my question clear.

Say I have a rectangular domain. Right wall is rotating at 100RPM. Left wall is rotating at -100RPM. There are two ways to specify the boundary condition now.

1. Define domain as stationary. Then add two boundaries to this domain with 100 RPM and -100 RPM . This is perfect.

2. Define domain as rotating with 100RPM (right wall speed). Then define only one wall boundary with -100RPM . This is where I am stuck. Is this wall boundary to be -100RPM or 0RPM .

Thanks
Archep

ghorrocks February 4, 2016 17:10

Option 1 is much preferred, if tangential wall velocity is applicable.

If you really want to implement option 2 then you have a rotating domain at 100rpm. Then the right wall has zero velocity in the rotating frame of reference, and the other wall will need to have a tangential velocity of -200rpm in the rotating frame of reference.


All times are GMT -4. The time now is 04:32.