2D rotating ellipse (domain interface??)
 

Hi,

I'm trying to model a 2D spinning ellipse. The model I'm using is a rectangle with 0.3m depth acting as "wind tunnel" and an extruded ellipse (separate mesh) with the same depth.

The ellipse is effectively touching both sides of the tunnel, how do I create an interface between the tunnel and the ellipse in order for it to rotate correctly?

So far I've been able to do a transient rotor stator using the 2 sides of the ellipse to effectively rotate the ball but it doesn't seem to effect the air flow at all, creating streamlines simply go through the ellipse model.

how can i tackle this?

Patrick

Can anyone push me in the right direction for this? Is the current setup valid for creating a domain interface between the two meshes or will I need to alter the mesh somehow?

to reiterate:
wind tunnel mesh has 6 faces
2D ellipse has 3 faces

Hi,

I cannot picture what you are describing. Can you draw a diagram?

Glenn Horrocks

Not at home currently so don't have the files but I created this in workbench quickly to model the problem.
http://img511.imageshack.us/img511/5188/93505141.jpg

Bear in mind that they are 2 separate meshes in my configuration.

Patrick

hi,
you have to model the ellipse inside a cylinder and define it as the rotating frame.
You will end up with 3 domains.

neewbie

Thanks for the reply.

Could you be more specific in regards to domain interfaces between these 3 domains (ellipse, cylinder, rectangle)?

Patrick

hi,

what you do is setting up a rotating frame which includes the ellipse.
Within the rotating frame you setup everything like you did.A solid/fluid-interface in an rotating frame.
Between the rotating and stationary frame you set up another interface.
Now you could set up the desired spin relatively.
I am not sure about the "windtunnel-walls" in the rotating frame but i think you should set them counterrotating within the rotating frame.Check out the manual on that.

neewbie

Right, I think I follow the general layout which can be seen in the image:

http://img21.imageshack.us/img21/674...oglecomcvy.jpg

My problem is which faces do I use for the sides in the domain-interfaces? I've read through countless pages in the manual, searched online and on this forum, tutorials that have domain-interfaces don't seem to work on this comp, so I can't figure out how to create the interface between ball-cyllinder and cyllinder-wall.

Here's my setup so far:
2D ball has 3 faces.. defined as solid domain, stationary
cyllinder has 3 faces.. defined as fluid domain, rotating
fluid-solid interface between the two.. using the outer faces (4) ??

wall has 6 faces.. defined as fluid domain, stationary
fluid-fluid interface between wall-cyllinder... faces?

I'm guessing it's probably something really simple that I'm missing?

Patrick

Hi,

You don't need to model the solid region (which I assume is the ellipse) if you are not modelling heat transfer. If this is the case then you will have two fluid regions, one stationary and one rotating connected by a GGI set to a transient rotor-stator.

Glenn Horrocks

hi,
like glenn said: if you donn´t need heattransfer, you don´t have to model the inner part of the ellipse.
so you will need one fluid-fluid interface for the transient rotor-stator-combination.
The walls will be treated as walls as usual.
Maybe i am wrong but you meshed e.g. the tunnel without the rotating frame, right?

neewbie

Ok, so I got rid of the solid domain which leaves me now with 2 domains (ellipse and cylinder have been combined as one domain).
Cyllinder is rotating
Wall is stationary
I've tried to create a transient rotor stator interface but I'm obviously using the wrong faces because I keep getting error about the 360 degree tolerance.

http://img16.imageshack.us/img16/9923/cfx.jpg

So I still don't understand which sides to define for the interface.

Patrick

hi,
why is there an ballright/ballleft? Where is the interface in the stationary domain?
You should end up with 7 faces for the tunnel (6 boundaryfaces and the interface(lookslike this is your cyllCIRCLE)) and 4 faces for the rotating domain (2 sideparts touching the tunnelwall, the surface of the ellipse and the interfacesurface which is congruent with the interface within the tunneldomain).

neewbie

ballleft and ballright refers to the ellipse sides. ballellipse refers to the ellipse surface, and cyllCIRCLE refers to the cyllinder surface.

Correct me if I'm wrong but this is the setup you're suggesting:
- cylinder + tunnel in one domain (stationary) - the whole cylinder mesh used as side1 for TRS interface
- ellipse in another domain (rotating) - the whole ellipse mesh used as side2 for TRS interface

With this setup though, how do I define the ellipse as a wall without overlapping with interface?

Patrick

hi,
I´m sorry but no.
The ellipse is included in the cylindric domain, which is the rotating domain. This domain in connected via an interface to the stationary one, the tunnel.
Two domains, one interface.
There is no ellipse-sidepart if setup like this.

neewbie

Frozen Rotor
 

Hi

If you want to model a rotating ellipse in a rectangular flow field. Then you ll have to create two domains. A cylinder (encompassing the Ellipse) and a rectangular flow field. The two domains would be joint by a froze rotor interface if it's a steady state simulation and transient rotor if the simulation is transient.

BOL

Tassi

Right, I understand the 2 domains 1 interface but like I said before, when defining the interface, I don't know which "face(s)" to use for side-1 and side-2 specifically so the solver keeps ending with errors.

I've defined as transient by the way.

Patrick

hi,
there shouldn't be any problem if you set up proper surface names and the meshes do not intersect.
Side 1 Rotating Domain Interface (Cylinder Surface);
Side 2 Stationary Domain Interface (Cylinder surface included within the Tunneldomain).
Which error do you get and when?

I created an additional cylinder for the tunnel domain. Then for domain-interface I've used the cylinder surface in rotating domain and the cylinder surface in tunnel domain like this:
http://img185.imageshack.us/img185/6...ninterface.jpg

Using trans-rotor-stator, I get the following error:

| ERROR #001100279 has occurred in subroutine ErrAction. |
| Message: |
| For domain interface "Domain Interface 1" the pitch angle ratio o- |
| f 1.0000000E+00 does not match the area ratio of 2.- |
| 0120964E+00.

Yours stuck,
Patrick

Hi,

This simulation is a basic application of rotating frames of reference and really is not that hard when you understand the basics. However, explaining what to do on a forum is difficult. Have a look at the tutorial examples which come with CFX using rotating frames of reference, I think there is an axial flow turbine example.

In fact whenever you do a new type of simulation you should look at relevant tutorial examples first to see the basics of how to set it up.

Glenn Horrocks

Hi Erik
Agree with Glenn you can get a better idea after looking in tutorial. Also try using the following settings for you interface
Frame Change/mixing Model : Frozen-Rotor
Rotational Offset : 0 deg
Pitch Change: None
Mesh connection method : GGI

Hope this helps

Hi,

Problem was I couldn't open the tutorials to see how the interfaces had been done. Either way, I managed to get it work - these are my settings for the interface:
side 1: domain - ellipse; cylinder surface
side 2: domain - tunnel; cylinder surface
Type: GGI
Frame Change: Transient Rotor-Stator
Transformation Type: None
Pitch Change: Automatic

Thanks everyone for helping out!

Patrick

Hi everybody!
I'm trying to simulate something like this.

If I have to consider also heat transfer in my model then I have to include the rotating solid domain. Am I right? and how can I define the interfaces?


Claudia

No. You model the solid domain ONLY if you require the temperature distribution in the solid. If you are modelling temperature in the fluid but know the condition of the solid then you do not need to model the solid.

Thank you. I just wanted to be sure.
Unfortuntely I have still problems interfacing the two fluid domains: the stationary one and the rotating one.
I created a fluid/fludid interface between them, with frozen rotor frame change.
Now which boundary condition am I supposed to set in domain interface side 1 and domain interface side2 in terms of wall velocity?
I must specify that the stationary fluid has a traversing velocity as inlet boundary condition.


Claudia

If the interface has no gaps then you do not need to set any boundary condition. Have a look at the tutorials for how to set up rotating machinery simulations.

Sorry but I've already looked at all the tutorials, I'll check again.
I give you a better explanation of the problem:
I'm trying to simulate the Friction Stir Welding process. I'm using an Eulerian Method with the workpiece modeled as a fluid that moves towards a rotanting cylinder (the tool) and the heat generation due to friction between them.

does anybody have any good idea to help me?

Unless you give us some idea of what you are modelling I cannot help you. That is why I did not bother replying. I am not an expert at friction stir welding and I have no idea of how you propose to model it. So please post a drawing of what you propose and a clear description.

Thank you Glenn. I'm sorry. I'll give you a better explanation.

The model consists of a cylindrical steel tool which is rotating, it's plunged into the rectangular workpiece and then moved along the weld line.
There are three ways to analyse this process: eulerian, lagrangian or ALE approach.
I'm using the first one. So a give a translational velocity at inlet of the workpiece and the velocity of the material adjacent to the rotating tool is assumed to be equal to the tool's rotational speed. I think I managed to give this boundary conditions. The problem is when I have to insert the heat flux at the tool/workpiece interface. I've calculated it through analitical expressions assuming sticking conditions.

http://imageshack.us/photo/my-images...magineymn.jpg/

I should obtain in post processing a temperature contour like this but my contours ara concentric and I think they're not influenced by the translational motion:

http://ars.els-cdn.com/content/image...000679-gr8.jpg

I understand now. In fact I was part of a team which looked at friction welding of steering racks (for automotive stuff) years ago so I know a little about this process.

What version of CFX are you using? I think convection of heat in solids due to motion of the body was only put in V14. If you are using an earlier version it will not include convection and I suspect that could end up with concentric heat profiles.

Alternately, what causes the asymmetric heat in the images? Isn't there a bit of tool deflection, uneven melting and other stuff resulting in uneven heat generation?

I'm using version 13.So you're telling me that I can't see a wake behind the tool in terms of temperature contour?

In that image they consider heat generated by viscous dissipation.
The asymmetric temperature contour should be caused by the rotating motion; they consider also an angle between the tool and the workpiece.

They might have introduced this in V13. It is simple to check, just put a hot spot in a solid body and move it and see what happens. Do you see a hot wake behidn the tool?

I created a solid cylinder with a heat flux on a boundary interfaced with a fluid. On the tool side I can see the wake. On the fluid side I don't.
Maybe I make always the same mistake.

Apart from the specific boundary conditions do you think I'm modeling the fsw process in the right way?

I managed to run a very simple simulation with a fluid moving toward a cylinder with an heat source on a boundary.

That's the result. I can see the wake.
Now I have to find out what's wrong when I plunge the cylinder in the fluid domain.

:) I don't know what you are trying to learn from this simulation, so cannot answer that.

OK, so that shows that the heat is being convected away in a fluid domain, but what about in a solid domain?

I'm much more interested in temperature in the workpiece. My problem was I could not see the wake in the fluid.

CHT should work fine into the fluid, so a heat wake should form if the conditions are correct.

Yes my problem are definetely the conditions because I'm running more simulations and when I insert heat transfer coefficient on the other surfaces of the workpiece (to simulate the convective heat transfer with air) the wake disappear.

The obvious conclusion is your convective BC is wrong. I suspect it results in almost no heat transfer and therefore no heat wake. Check you HTC and temperatures.