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

Moving PIPE

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   November 20, 2014, 06:16
Default
  #21
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,267
Rep Power: 136
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
1) Yes, the sliding interface is transient rotor stator.
2, 3) 1 and 2 are moving mesh domains (but stationary frame of reference). 3 is a stationary frame of reference with no moving mesh.
4) No, do not select any solid motion options. Use moving mesh on a solid domain. Do not use a rigid body model.
5) 1 and 2 have mesh deformation on.
6) interface 1 to 2 is stationary I think, if that does not work then TRS. 2 to 3 is TRS.
ghorrocks is offline   Reply With Quote

Old   November 20, 2014, 06:36
Default
  #22
Senior Member
 
Martin_Sz's Avatar
 
Marcin
Join Date: May 2014
Location: Poland, Swiebodzin
Posts: 225
Rep Power: 11
Martin_Sz is on a distinguished road
I have another question
Where do I finf frame of reference option ?
Best regards
Martin_Sz is offline   Reply With Quote

Old   November 20, 2014, 06:51
Default
  #23
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,267
Rep Power: 136
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
Frame of reference is where you choose either stationary or rotating. The default is stationary so leave it at the default for all domains.
ghorrocks is offline   Reply With Quote

Old   November 24, 2014, 02:22
Default
  #24
Senior Member
 
Martin_Sz's Avatar
 
Marcin
Join Date: May 2014
Location: Poland, Swiebodzin
Posts: 225
Rep Power: 11
Martin_Sz is on a distinguished road
Hello Glenn,
So I make simulation with idea which You wrote on the lasts posts and I have another problem.
On the solver only six steps go on and on the seventh error jump in with information
cNWDIST
At least one highly skewed element has been detected on a wall boundary, leading to unreliable near-wall distance calculation for the turbulent wall functions. The solver will continue to execute, but convergence and/or accuracy may be affected. Please consider improving the mesh quality. the coordinates of the element face are...

So what can I do at that moment to fix this error ??
Best regards
Martin_Sz is offline   Reply With Quote

Old   November 24, 2014, 05:22
Default
  #25
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,267
Rep Power: 136
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
This tells me you have got the mesh motion wrong.

Re-run the simulation saving a results file on each time step which includes the mesh. Then have a look at the time step before it crashes at the location it specifies. If you cannot work out what the problem is post an image of it on the forum.
ghorrocks is offline   Reply With Quote

Old   November 24, 2014, 05:36
Default
  #26
Senior Member
 
Martin_Sz's Avatar
 
Marcin
Join Date: May 2014
Location: Poland, Swiebodzin
Posts: 225
Rep Power: 11
Martin_Sz is on a distinguished road
I increase mesh quality and simulation goes on to the 14th step.
and crashes with element volume error.
The strangest thing is that. On the 14th step and other steps before I haven't got heat transfer on the tube (on moving area of the tube).
When I define moving interface on domain 2, i need to define wall velocity ??
Best regards
Martin_Sz is offline   Reply With Quote

Old   November 24, 2014, 05:46
Default
  #27
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,267
Rep Power: 136
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
The error has nothing to do with mesh quality. Have you done what I recommend in my last post?

The error is most probably due to the mesh motion settings you are using. You need to define a displacement function (versus time) and apply that to all the boundaries of the moving domain. If you miss a boundary you can get the error you got - and that includes interface boundaries so I bet you missed one of them.
ghorrocks is offline   Reply With Quote

Old   November 24, 2014, 06:03
Default
  #28
Senior Member
 
Martin_Sz's Avatar
 
Marcin
Join Date: May 2014
Location: Poland, Swiebodzin
Posts: 225
Rep Power: 11
Martin_Sz is on a distinguished road
So on the attachments I'm sending You what i define on interfaces of domains
Best regards
Attached Images
File Type: jpg exp1.jpg (23.1 KB, 9 views)
File Type: jpg interfaces.jpg (36.9 KB, 9 views)
File Type: jpg interfaces2.jpg (47.4 KB, 5 views)
Martin_Sz is offline   Reply With Quote

Old   November 24, 2014, 06:12
Default
  #29
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,267
Rep Power: 136
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
I cannot tell much about what is happening from the screen dumps. Please your CCL.

But even more important is the post I put up #25 about how to debug this. It should allow you to identify exactly what the problem is.
ghorrocks is offline   Reply With Quote

Old   November 24, 2014, 06:24
Default
  #30
Senior Member
 
Martin_Sz's Avatar
 
Marcin
Join Date: May 2014
Location: Poland, Swiebodzin
Posts: 225
Rep Power: 11
Martin_Sz is on a distinguished road
can You verify my defined interfaces which I send on the last post (attachments )
Best regards
Martin_Sz is offline   Reply With Quote

Old   November 24, 2014, 06:51
Default
  #31
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,267
Rep Power: 136
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
I said:

Quote:
I cannot tell much about what is happening from the screen dumps.
The next sentence meant to say: Please attach your CCL.

But even better: if you do the images I said in post #25 I think we will be able to identify the problem straight away.
ghorrocks is offline   Reply With Quote

Old   November 24, 2014, 08:06
Default
  #32
Senior Member
 
Martin_Sz's Avatar
 
Marcin
Join Date: May 2014
Location: Poland, Swiebodzin
Posts: 225
Rep Power: 11
Martin_Sz is on a distinguished road
I'm sending a ccl of the simulation
Best regards
Attached Files
File Type: txt ccl.txt (13.6 KB, 10 views)
Martin_Sz is offline   Reply With Quote

Old   November 24, 2014, 08:11
Default
  #33
Senior Member
 
Martin_Sz's Avatar
 
Marcin
Join Date: May 2014
Location: Poland, Swiebodzin
Posts: 225
Rep Power: 11
Martin_Sz is on a distinguished road
I change mesh deformation to initial boudaries on subdomain option
Then 13 steps go on and on the 14th pop up an error (attachment)
Best regards
Attached Files
File Type: txt ccl2 error.txt (950 Bytes, 3 views)
Martin_Sz is offline   Reply With Quote

Old   November 24, 2014, 18:25
Default
  #34
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,267
Rep Power: 136
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
As I thought - you have not defined the mesh motion parameters on many boundary surfaces on mesh movement domains.

Boundaries which need it are:
kostka subdom Side 2
subdomena Default

Also the Walek domain (which appears to be your solid) looks like it has no mesh deformation. You need to use mesh deformation on this domain as well.
ghorrocks is offline   Reply With Quote

Old   November 25, 2014, 02:34
Default
  #35
Senior Member
 
Martin_Sz's Avatar
 
Marcin
Join Date: May 2014
Location: Poland, Swiebodzin
Posts: 225
Rep Power: 11
Martin_Sz is on a distinguished road
Hello Glenn,
Thanks for reply
Where can I change on solid domain mesh deformation ??
I dont see this option on solid domain (attachment)
Best regards
Attached Images
File Type: jpg solid deformation.jpg (73.0 KB, 6 views)
Martin_Sz is offline   Reply With Quote

Old   November 25, 2014, 05:07
Default
  #36
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,267
Rep Power: 136
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
What version of CFX are you using?
ghorrocks is offline   Reply With Quote

Old   November 25, 2014, 05:17
Default
  #37
Senior Member
 
Martin_Sz's Avatar
 
Marcin
Join Date: May 2014
Location: Poland, Swiebodzin
Posts: 225
Rep Power: 11
Martin_Sz is on a distinguished road
v15
And I have another question.
On Your schematic which domain is moving 1 or 2 ??
Martin_Sz is offline   Reply With Quote

Old   November 25, 2014, 06:52
Default
  #38
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,267
Rep Power: 136
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
1 and 2 are stationary frame of reference, moving mesh domains.

OK, good. V15 is the only version which supports motion in solid domains. I am pretty sure you can do moving mesh on solid domains. You might need to edit the CCL to do this, rather than doing it in CFX-Pre. Copy the format used in your moving mesh fluid domain.
ghorrocks is offline   Reply With Quote

Old   November 25, 2014, 08:47
Default
  #39
Senior Member
 
Martin_Sz's Avatar
 
Marcin
Join Date: May 2014
Location: Poland, Swiebodzin
Posts: 225
Rep Power: 11
Martin_Sz is on a distinguished road
So for the first time solution goes on.
And I have interesting results.
Interface between walek and subdomain go on the direction which I defined in mesh motion but solid domain on the end of simulation is on the start position. Only interfaces walek-subdomena with empty area inside goes on.
I dont know what to define mesh deformation on solid. ccl copy paste from fluid domain doesnt work. What can I do ??
Best regards
Martin_Sz is offline   Reply With Quote

Old   November 25, 2014, 18:27
Default
  #40
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,267
Rep Power: 136
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
Actually, you might need to use the solid motion options for the solid domain. Have you tried that?
ghorrocks is offline   Reply With Quote

Reply

Tags
cfx, mesh deformation, solid motion

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
simple open ended pipe flow with moving piston lmarf88 ANSYS 1 November 22, 2013 22:12
moving sphere in a pipe sajeesh FLUENT 1 February 25, 2013 09:35
Help needed in modelling/meshing a body moving in a pipe which is driven by a fluid hareshram.n ANSYS 0 March 19, 2010 03:23
Terrible Mistake In Fluid Dynamics History Abhi Main CFD Forum 12 July 8, 2002 10:11
fluid flow fundas ram Main CFD Forum 5 June 17, 2000 22:31


All times are GMT -4. The time now is 12:51.