CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   FLUENT (http://www.cfd-online.com/Forums/fluent/)
-   -   How to Create the Rotating Reference Frame of a MRF Problem in DM wrt to an Interface (http://www.cfd-online.com/Forums/fluent/101567-how-create-rotating-reference-frame-mrf-problem-dm-wrt-interface.html)

Zev Xavier May 8, 2012 01:03

How to Create the Rotating Reference Frame of a MRF Problem in DM wrt to an Interface
 
Hi


I am new to Fluent and am wanting to apply a Multiple Reference Frame model to my simple centrifugal pump geometry to analyse the flow behaviour within the pump. I am using an assembly of two components the first being a solid impeller and the second being the geometry of the wetted surface area within the pump housing and volute, please images belowhttp://photobucket.com/ZevXavier. I used SolidWorks for the generation of both components. My currect concern is how to create the multiple zones where two fluid zones are connected via an interface boundary so as to later define the rotating frame in Fluent. I am not sure how to created this in Design Modeler.


Although I am sure this step is rather simple for those already understanding how to create these multiple fluid zone boundary interfaces, It has proved rather challanging for me even after devoting a significant amout of time to understanding this step.


I appreciate any assistance in helping me understand this process.
__
Zev

Impeller: http://i1170.photobucket.com/albums/...r/impeller.png
Fluid Geometry
http://i1170.photobucket.com/albums/...vier/Fluid.png

sunflower May 8, 2012 03:59

Here is my input for your case.

If you go through the Fluent tutorial with MRF, you will have some idea.

If you only solve gas flow inside the pump ( I mean heat transfer will not be considered), the second geometry with fluid portion is enough.

You will need to create a cylinder volume which is slightly bigger than solid impeller in order to surround the impeller. We can call this zone as rotating zone. The rest of fluid portion is stationary zone. You need only define rotating frame for rotating zone.

The interface between rotating zone and stationary zone is treated as interior. You don't have to define anything for it.

Hope this helps.




[QUOTE=Zev Xavier;359841]Hi


I am new to Fluent and am wanting to apply a Multiple Reference Frame model to my simple centrifugal pump geometry to analyse the flow behaviour within the pump. I am using an assembly of two components the first being a solid impeller and the second being the geometry of the wetted surface area within the pump housing and volute, please images belowhttp://photobucket.com/ZevXavier. I used SolidWorks for the generation of both components. My currect concern is how to create the multiple zones where two fluid zones are connected via an interface boundary so as to later define the rotating frame in Fluent. I am not sure how to created this in Design Modeler.

felicemastronzo May 8, 2012 07:17

In design modeler you have to create a sketch and than, after you have freezed the geometry, with the command extrude you have to split the volume using the sketch. So you can obtain two separate volumes. Than you have to select the interface boundaries in order to be able in Fluent to create the interfaces.

F

Zev Xavier May 8, 2012 08:27

Hi Felice,
Thankyou for your reply. I am unsure however on the actual steps to take to select the interface boundaries. Do you just create named selection of the generated geometry faces, calling them "interface"?

(I will have to remember that freeze option, It has been a few years since I used ANSYS DM so I am a bit fuzzy currently)
__
Zev

Zev Xavier May 8, 2012 08:44

Thank you for your reply Sunflower. I followed your thought process and proceeded to simulate the fluid in my pump using just the two fluid regions (and no impeller). I have included images of the new geometry below hopefully my methodology seems suitable for this particular case.


From this I was able to apply an automatic mesh method and the interface between the two fluid zones was automatically detected and shown as a green dotted line (which was fantastic! So thank you for your advice). I then proceeded to open the mesh in Fluent, apply basic boundary conditions and the problem converged in under 300 iterations. I was then able to look at the velocity profile, which is provided below, and it appears to generally show what you would expect to occur.


This has given rise to a new question however wrt to the accuracy of the simulation. If I just set the simulation up like this with the fluid regions, and not the actual impeller itself, is it reasonable to assume the results would somewhat vary to those completed with an impeller? My final goal for this analysis will be to investigate the effects of impeller orientation wrt the distance between the blade tips and the sharpest point of the cutaway region of the pump. This particular analysis will look at how the impeller drives the fluid, and I will also be trying not to over constrain the simulation to obtained the best results with regard to this goal. To do this I would assume it would be much more efficient to work with a model which incorporates the impeller into the analysis, so it can simply be rotatined before each simulation rather than going back to the CAD program and creating a new fluid geometry for each orientation.


Do you, or anyone else, have any alternative suggestions to correctly define the interactions between multiple components in ANSYS?



Following this Analysis I created an assembly of three components: two fluid zones (as used above) and the impeller. When I attempted to mesh this assembly in the ANSYS Mechanical Application, no interface boundary between the fluid zones was automatically created. Not knowing how to specify this condition, I thought I would see how Fluent read the mesh file to see if perhaps it was ok. For this particular mesh, three separate Cell Zone Conditions were detected by Fluent. With this, I was not sure how to assign BC to the zones and was not sure if both the impeller and fluid immediately surrounding the impeller were both to be assigned as moving. After numerous simulation tests of various combinations of rotation/stationary boundary conditions were applied, nothing which seemed correct was obtained.


Given this failed attempt I then though if I perhaps I make a separate thin walled segment in the CAD program I would be able to assign it as an interface boundary when meshing. This assembly consisting of four components (shown expanded below), was imported into ANSYS. After doing this however the assembly would not mesh, it did not come up with an error but appeared to stop working which I think was directly attributed to the thin walled part as I tried a few times so it was not just a random error.


Given my difficulty in overcoming this particular challenge, I welcome any suggestions which others in similar situations have yielded positive results.
Thanks again
__
Zev



Two Fluid Zone Image

http://i1170.photobucket.com/albums/...FluidZones.png







Velocity Profile of Two Fluid Zone Geometry


http://i1170.photobucket.com/albums/...r/velocity.png




Four Component Exploded Assembly with Thin Walled Interference Geometry
(0.001mm thick, with impeller diameter being 21mm for reference)
http://i1170.photobucket.com/albums/...mponents-1.png

felicemastronzo May 8, 2012 09:17

The freeze command is available in the upper command menu. Buy if you have already the 2 separate volumes, you just need to create two named selection on the two sides of the interface the names can be for example interface1 and interbace2). When you import the mesh in fluent, the software will recognises the two volumes and the two sides of the interfaces. In fluent under interface you can couple the two surfaces.

You need to modell also the impeller only if you will perform some thermical analysis.

F

Zev Xavier May 8, 2012 09:48

Thanks very much. I will keep that in mind and definitely give that method of naming interface1/interface2 a go tomorrow :).
__
Zev

sunflower May 8, 2012 21:48

Hi Zev,

You aim to study the effect of impeller geometry on gas flow surrounding it. Still, you don't have include solid impeller in your simulation domain. You can still use the two fluid zones (rotating zone and stationary zone).

Please keep in mind that when the impeller geometry is changed, geometry of rotating zone is also changed.

And how the impeller drives the flow is define through boundary condition and cell zone condition. It means you don't have to include solid impeller in simulation domain.

However, if you really want to include solid impeller in simulation domain, this approach with solid impeller can still work. But it makes the problem more complicated, and not necessary.


[QUOTE=Zev Xavier;359922]Thank you for your reply Sunflower. I followed your thought process and proceeded to simulate the fluid in my pump using just the two fluid regions (and no impeller). I have included images of the new geometry below – hopefully my methodology seems suitable for this particular case.

Zev Xavier May 9, 2012 17:39

Hi Sunflower,

I'm glad that I have the simulation correctly working with the two fluid zones, however I would like now to try and get the simulation to work with a solid impeller also, (as this project is a learning exercise and although the development of this model may be more complicated I think it will be more efficient overall when solving the impeller in various orientations). Do you know how I would go about this approach, or what sort of material I should be looking at to understand the set up?
__
Zev

sunflower May 10, 2012 01:52

Normally the interface boundary between two fluid zones, i.e., rotating zone and stationary zone, will not automatically created. You can define it in meshing by name selection. Even though you don't define it, you don't have to worry about it. When meshing is imported into Fluent, that interface will be automatically created, and defined as interior by default.

So you don't have to create the thin wall so called.

Now there are 3 cell zones, which are solid impeller, rotating fluid zone and stationary fluid zone. Have you tried defining both solid impeller and rotating fluid zone as rotating, and they share the same rotating speed and direction?

The other thing is define the boundary condition for the interface between solid impeller and rotating zone. You can define them as Moving wall, which is stationary relative to adjacent cell zone.

Have a try first and good luck.

[QUOTE=Zev Xavier;360175]Hi Sunflower,

I'm glad that I have the simulation correctly working with the two fluid zones, however I would like now to try and get the simulation to work with a solid imp[B]eller also, (as this project is a learning exercise and although the development of this model may be more complicated I think it will be more efficient overall when solving the impeller in various orientations). Do you know how I would go about this approach, or what sort of material I should be looking at to understand the set up?

PAMPS September 25, 2012 12:03

Importing/Creating Impeller Geometry in DM
 
Hi Zev,

I have an impeller to model in a Tank. At the end of the day I need to find the Power and torque of the impeller + shaft.
My intention to model only one "slice" (120) of the tank in order to simplify the model.
I have the impeller geometry in ACAD 3D, and in script files (sections and periphery line).
My problem is:
1. Create the impeller blade geometry in DM
2. Create the rotating domain with the same pitch and shape at periodic domain interfaces.

In adition I have studied several tutorials and some of them have a "stagefluidzone" behind the impeller. Do I need this feature?

Thank you for some guidance.

PAMPS

mrtkrs October 14, 2014 08:46

fan model
 
can someone add video how to make this anlsys because it is so complicated.thanks


All times are GMT -4. The time now is 12:54.