CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > CFX

2D rotating ellipse (domain interface??)

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree1Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   April 17, 2009, 09:51
Default
  #21
New Member
 
Erik Sandstroem
Join Date: Apr 2009
Posts: 11
Rep Power: 9
Kambusha is on a distinguished road
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
Kambusha is offline   Reply With Quote

Old   May 15, 2012, 05:58
Default
  #22
New Member
 
claudia
Join Date: Jan 2012
Posts: 11
Rep Power: 6
dclaudia85 is on a distinguished road
Hi everybody!
I'm trying to simulate something like this.

Quote:
Originally Posted by ghorrocks View Post
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
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

Last edited by dclaudia85; May 15, 2012 at 06:39.
dclaudia85 is offline   Reply With Quote

Old   May 15, 2012, 07:46
Default
  #23
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,638
Rep Power: 98
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
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.
ghorrocks is offline   Reply With Quote

Old   May 15, 2012, 07:55
Default
  #24
New Member
 
claudia
Join Date: Jan 2012
Posts: 11
Rep Power: 6
dclaudia85 is on a distinguished road
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
dclaudia85 is offline   Reply With Quote

Old   May 15, 2012, 19:24
Default
  #25
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,638
Rep Power: 98
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
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.
ghorrocks is offline   Reply With Quote

Old   May 16, 2012, 03:42
Default
  #26
New Member
 
claudia
Join Date: Jan 2012
Posts: 11
Rep Power: 6
dclaudia85 is on a distinguished road
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.
dclaudia85 is offline   Reply With Quote

Old   May 17, 2012, 04:23
Default
  #27
New Member
 
claudia
Join Date: Jan 2012
Posts: 11
Rep Power: 6
dclaudia85 is on a distinguished road
does anybody have any good idea to help me?
dclaudia85 is offline   Reply With Quote

Old   May 17, 2012, 06:07
Default
  #28
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,638
Rep Power: 98
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
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.
ghorrocks is offline   Reply With Quote

Old   May 17, 2012, 06:44
Default
  #29
New Member
 
claudia
Join Date: Jan 2012
Posts: 11
Rep Power: 6
dclaudia85 is on a distinguished road
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:

dclaudia85 is offline   Reply With Quote

Old   May 17, 2012, 07:00
Default
  #30
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,638
Rep Power: 98
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
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?
ghorrocks is offline   Reply With Quote

Old   May 17, 2012, 07:10
Default
  #31
New Member
 
claudia
Join Date: Jan 2012
Posts: 11
Rep Power: 6
dclaudia85 is on a distinguished road
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.
dclaudia85 is offline   Reply With Quote

Old   May 17, 2012, 07:13
Default
  #32
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,638
Rep Power: 98
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
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?
ghorrocks is offline   Reply With Quote

Old   May 17, 2012, 07:28
Default
  #33
New Member
 
claudia
Join Date: Jan 2012
Posts: 11
Rep Power: 6
dclaudia85 is on a distinguished road
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?

Last edited by dclaudia85; May 17, 2012 at 08:39.
dclaudia85 is offline   Reply With Quote

Old   May 17, 2012, 14:17
Default
  #34
New Member
 
claudia
Join Date: Jan 2012
Posts: 11
Rep Power: 6
dclaudia85 is on a distinguished road
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.
Attached Images
File Type: jpg Immagine3.jpg (93.9 KB, 11 views)
File Type: jpg Immagine4.jpg (96.9 KB, 7 views)
dclaudia85 is offline   Reply With Quote

Old   May 17, 2012, 18:55
Default
  #35
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,638
Rep Power: 98
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
Quote:
do you think I'm modeling the fsw process in the right way?
I don't know what you are trying to learn from this simulation, so cannot answer that.

Quote:
I managed to run a very simple simulation with a fluid moving toward a cylinder with an heat source on a boundary.
OK, so that shows that the heat is being convected away in a fluid domain, but what about in a solid domain?
ghorrocks is offline   Reply With Quote

Old   May 18, 2012, 04:56
Default
  #36
New Member
 
claudia
Join Date: Jan 2012
Posts: 11
Rep Power: 6
dclaudia85 is on a distinguished road
I'm much more interested in temperature in the workpiece. My problem was I could not see the wake in the fluid.
dclaudia85 is offline   Reply With Quote

Old   May 18, 2012, 07:47
Default
  #37
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,638
Rep Power: 98
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
CHT should work fine into the fluid, so a heat wake should form if the conditions are correct.
ghorrocks is offline   Reply With Quote

Old   May 18, 2012, 09:09
Default
  #38
New Member
 
claudia
Join Date: Jan 2012
Posts: 11
Rep Power: 6
dclaudia85 is on a distinguished road
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.
dclaudia85 is offline   Reply With Quote

Old   May 19, 2012, 07:10
Default
  #39
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,638
Rep Power: 98
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
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.
ghorrocks is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Concentric tube heat exchanger (Air-Water) Young CFX 5 October 6, 2008 23:17
CFX Solver Memory Error mike CFX 1 March 19, 2008 08:22
rotating domain in rotating domain, different axis Robert Stringer CFX 3 December 4, 2006 08:04
Convective Heat Transfer - Heat Exchanger Mark CFX 6 November 15, 2004 16:55
Replace periodic by inlet-outlet pair lego CFX 3 November 5, 2002 21:09


All times are GMT -4. The time now is 11:38.