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

Problem with modelling contact in ansys fluent 12.1

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

Reply
 
LinkBack Thread Tools Display Modes
Old   August 14, 2010, 14:29
Default Problem with modelling contact in ansys fluent 12.1
  #1
New Member
 
Join Date: Jul 2010
Posts: 23
Rep Power: 6
mak86 is on a distinguished road
Hi,
I am modelling a 3 zone problem (2 Solid zones and one fluid).
It is consisted of a steel die that is in contact with an aluminium tube which contains a fluid. The die is heated up and as a result the temperature of the tube and fluid goes up.
I am using Ansys 12.1 and I have imported the model from solidworks to ansys workbench fluent.
In the meshing cell the contacts between solids and fluid are defined(automatically) but in the setup cell(fluent), when I try to set the BCs for the contact surfaces to coupled, there is no coupled choice.
I have checked the contacts(at Meshing) several times and everything seems to be ok.
What is the problem?
Thanks
mak86 is offline   Reply With Quote

Old   August 14, 2010, 22:35
Default
  #2
Senior Member
 
xrs333
Join Date: Aug 2010
Posts: 125
Rep Power: 7
xrs333 is on a distinguished road
The interface between two cell zones -- steel die-alum & alum-fluid -- should be set as the type of wall. On read into fluent, a shadow wall will be created automatically for those two-sided walls repectively. If there is no type of 'wall' in your mesher, just assign any type for the interface, and then change to wall type in fluent.by the way, the situation what you called 'contact' is usually referred to as 'conjugated' heat transfer.
xrs333 is offline   Reply With Quote

Old   August 15, 2010, 01:39
Default
  #3
New Member
 
Join Date: Jul 2010
Posts: 23
Rep Power: 6
mak86 is on a distinguished road
Quote:
Originally Posted by xrs333 View Post
The interface between two cell zones -- steel die-alum & alum-fluid -- should be set as the type of wall. On read into fluent, a shadow wall will be created automatically for those two-sided walls repectively. If there is no type of 'wall' in your mesher, just assign any type for the interface, and then change to wall type in fluent.
Dear xrs333,
Thanks for your reply
I know about the shadow walls and I had set the interface type to wall but I think the problem is caused by this:
I have imported the files from solidworks, infact it is a 3 part assembley (at this step) so each part has its own walls. After importing the geometry the contacts are automatically recognized by Ansys Meshing module but fluent does not recognize them as contacts.
So what should I do now?
Thanks for reminding me about the true name, but I used contact because I thought the origin of the problem is in the Meshing cell (defining contacts between parts).
Thanks again for your reply.
mak86 is offline   Reply With Quote

Old   August 15, 2010, 02:26
Default
  #4
Senior Member
 
xrs333
Join Date: Aug 2010
Posts: 125
Rep Power: 7
xrs333 is on a distinguished road
I guess that the mesh of the wall pair of the contact is non-conformal, that is the nodes on two side do not coincide. Non-conformal interface can be used whether or not non-conformal is the mesh. Try to follow these steps: 1>change the boundary type of the walls on both side of the contact to interface. 2>go to mesh interface panel to define a mesh interface for each contact surface pair with coupled wall option checked.
xrs333 is offline   Reply With Quote

Old   August 15, 2010, 05:33
Default
  #5
New Member
 
Join Date: Jul 2010
Posts: 23
Rep Power: 6
mak86 is on a distinguished road
Thanks alot.
mak86 is offline   Reply With Quote

Old   August 16, 2010, 04:20
Default
  #6
New Member
 
Join Date: Jul 2010
Posts: 23
Rep Power: 6
mak86 is on a distinguished road
I tried your solution and it worked but what it will be a little confusing for models with too many parts and contact surfaces.
Is there a better solution?
I mean the Mesher recognizes the contacts but that is ignored by fluent.
What can be done about this?
thanks
mak86 is offline   Reply With Quote

Old   August 16, 2010, 08:24
Default
  #7
Senior Member
 
xrs333
Join Date: Aug 2010
Posts: 125
Rep Power: 7
xrs333 is on a distinguished road
I use Gambit, but the idea is similar. I usually create the geometry as a whole solid body for all parts, then split it with surfaces into original shape, remember keep 'connected' between different part, and then assign wall boundary type for the interface of the contact parts. These walls will be recognized as 'two-sided wall' because they have cell zone adjacent on both side.
xrs333 is offline   Reply With Quote

Old   February 20, 2011, 01:08
Exclamation
  #8
New Member
 
jhthoh
Join Date: Feb 2011
Posts: 11
Rep Power: 6
jhthoh is on a distinguished road
Sorry for disturb, can i ask how about 2 zone prob? 1 fluid and 1 solid.
I m doing on car drag coefficient simulation in ANSYS 12.0 Fluent. Do i need to set the car body boundary to interface?
jhthoh is offline   Reply With Quote

Old   February 20, 2011, 11:27
Default
  #9
New Member
 
Edd
Join Date: Nov 2010
Posts: 3
Rep Power: 6
eddiejohn is on a distinguished road
mac86,

I am working on a similar model where i have heat transfer between two solids then a cooling flow over the surface.

I can get each zone to talk to each other by changing walls to interfaces then coupling the wall. This provides a good plot of heat transfer. However when the contours for velocity are plotted, there is no zero velocity boundary layer where the flow passes over the solid, which isnt right.

I would be gratefull for any more experienced users ideas how to overcome this?

Kind regards,

John
eddiejohn is offline   Reply With Quote

Old   July 23, 2012, 07:58
Default
  #10
New Member
 
Join Date: Jul 2012
Posts: 5
Rep Power: 4
nipunkothare is on a distinguished road
hey i`m making a design of 4 tubes- fluid solid solid fluid.
the walls were not getting coupled automatically in fluent
their were no coupled or wall boundaries formed.only interiors.
so i named each surface in the mshr and applied mesh interface in fluent for each coupling(3').
finally i got those boundaries in the boundary condition as interface and 6 walls +3 shadows ( which is as expected) but still i`m getting a calculation error.


can anyone please confirm if it is a coupling error : error in line 199, store still has data
nipunkothare is offline   Reply With Quote

Old   June 14, 2013, 23:42
Default
  #11
New Member
 
Mahboobe Mahdavi
Join Date: Mar 2013
Posts: 22
Rep Power: 4
Mahboobe365 is on a distinguished road
i have the same problem,can you explain about mesh interface in fluent?
Mahboobe365 is offline   Reply With Quote

Old   November 16, 2013, 13:57
Default
  #12
New Member
 
satish
Join Date: Nov 2013
Posts: 2
Rep Power: 0
satishverma is on a distinguished road
while genetaring a wall inside a duct
there is automaticaly a wall shadow is generated in the fluent, which is not desired.
if you have any idea to this problem please share it i will be very thankful.
satishverma is offline   Reply With Quote

Old   December 3, 2013, 21:26
Default Creating a wall shadow from mesh
  #13
New Member
 
Alex
Join Date: Dec 2013
Posts: 1
Rep Power: 0
AlexT is on a distinguished road
Hey, if someone is interested i solved this issue in the following way:

Fluent recognizes automatically the shadow coupling when the mesh is appropriate, this is, when mesh nodes are aligned.

I tried the creating interface option but this didnt work out to good for me because fluent didnt correctly assign the boundary conditions and created some ficticious extra boundaries.

The solution was to go to the mesh and solve it from there. From what i understand , the mesh was not topologically connected, so this nodes were independent. So, at least in ansys workbench, there is an option to connect mesh, called mesh connection, in the connection tab. This should solve at least some issues.

I think that pinch control also solves mesh tolerance problems, but that is more advanced and from my experience more troublesome to use.

Hope it works,
AlexT is offline   Reply With Quote

Old   December 4, 2014, 00:48
Default
  #14
New Member
 
Jeremy Harvey
Join Date: Dec 2014
Posts: 1
Rep Power: 0
jpharvey is on a distinguished road
Your problem is that you need conformal meshes across the different regions. This link should explain how to accomplish this:

https://www.sharcnet.ca/Software/Flu...esh_Parts.html
jpharvey 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
FLUENT results to ANSYS Jin Yan FLUENT 2 April 28, 2011 11:22
few quesions on ANSYS ICEMCFD and FLUENT Prakash.Paudel ANSYS 0 August 12, 2010 12:07
problem of running parallel Fluent on linux cluster ivanbuz FLUENT 11 March 10, 2010 16:13
Ansys to aquire FLUENT Michael Bo Hansen CFX 74 February 24, 2006 21:42
import Fluent data&case to ANSYS Vlad S FLUENT 0 April 2, 2003 05:49


All times are GMT -4. The time now is 21:29.