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

Connecting two fluid zones in Ansys Fluent 12

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

Like Tree4Likes
  • 1 Post By izumi11
  • 2 Post By PSYMN
  • 1 Post By hamiasmai

Reply
 
LinkBack Thread Tools Display Modes
Old   February 20, 2010, 01:46
Question Connecting two fluid zones in Ansys Fluent 12
  #1
New Member
 
Join Date: Feb 2010
Posts: 11
Rep Power: 6
izumi11 is on a distinguished road
Hello,
I have been struggling for awhile with this. My geometry is made of several fluid zones which are supposed to be connected. When I mesh with ansys, it creates walls and interior boundaries. I would like to remove the walls, but it seems I can't. Also I cannot change a wall b.c. into interior for some reason.
Your help is greatly appreciated.

Last edited by izumi11; February 22, 2010 at 02:43.
izumi11 is offline   Reply With Quote

Old   February 20, 2010, 02:04
Default
  #2
New Member
 
Join Date: Feb 2010
Posts: 11
Rep Power: 6
izumi11 is on a distinguished road
Also Ansys mesher computes all the contacts between bodies before creating the mesh, but this doesn't translate into interface b.c. I think one way to make it work would be to create named selections on each faces that are connected and defined them later as interface, but this takes a lot of work and there should be a way to do this automatically in my opinion.
Thanks in advance for the help ^^
izumi11 is offline   Reply With Quote

Old   February 23, 2010, 00:12
Default
  #3
New Member
 
M S
Join Date: Feb 2010
Posts: 2
Rep Power: 0
msen is on a distinguished road
What are your inlet conditions and how did you define your inlet geometry? You should be able to define an inlet boundary condition for each different fluid at the inlet. You do not have to connect them in this case.
msen is offline   Reply With Quote

Old   February 23, 2010, 06:13
Default
  #4
New Member
 
Join Date: Feb 2010
Posts: 11
Rep Power: 6
izumi11 is on a distinguished road
Hi thank you for your reply. My fluid is as follows :
-two inlets, one with hydrogen+h2o, one with air
-one outlet.
For the moment I am only interested in the flow so I am ok with a single species, single phase simulation.

The problem is I have spread the fluid into several different contiguous zones. Some of which are porous. Therefore I can't merge them at the cad level. Ansys should handle it. So the outlet and the inlets are in different zones.

What I get is the interface between inlet and outlet becomes a wall under Fluent and the continuity residual never decreases as a result (obviously) because the fluid can't escape.
There should be a way to automate this process. I can't prescribe every fluid interface since there is a large number of zones. I know that the mesher in workbench resolves contacts, but it seems it creates wall b.c. where it should be an interface. Is there a way to tell ansys that a contact between two fluids should be an interface whereas a contact between a fluid and a solid should be a wall?

Hope I was clear enough.
Thanks
izumi11 is offline   Reply With Quote

Old   February 24, 2010, 09:31
Default
  #5
New Member
 
Join Date: Feb 2010
Posts: 11
Rep Power: 6
izumi11 is on a distinguished road
Ok I think I get the problem. From the fluent perspective I should use fuse faces to merge the walls. Fluent will then create a new thread for the intersecting faces and I can set it to interior. The problem is fluent calculates face coincidence on a node by node basis, which means only conformal interfaces are merged. In my case faces were merged separately so this doesn't work.

I think there is a way in designmodeler to let the mesher know it should mesh contacting faces together, by using "shared topology". I couldn't get it to work though.

A third solution would be I guess to use virtual topologies in the mesher, but I am not sure that will work.
What's bothering me is that Ansys mechanical goes all the way to calculate every contact, but doesn't apply that to meshing fluid interfaces. I think the information is only used for mechanical contacts or FSI.
rgd likes this.

Last edited by izumi11; February 25, 2010 at 01:52.
izumi11 is offline   Reply With Quote

Old   March 25, 2010, 01:24
Thumbs up 2 fluids at different inlets
  #6
New Member
 
ankit
Join Date: Mar 2010
Posts: 3
Rep Power: 6
anga87610del is on a distinguished road
Sir, I am facing problem in having 2 different fluids at 2 inlets at different sections of my geometry(liquid water and air)fluent only shows an option for mixture ,is there any way out to specify these 2 liquids differently at the two inlets.I hope i have made my point clearly.
anga87610del is offline   Reply With Quote

Old   March 25, 2010, 02:18
Default
  #7
New Member
 
Join Date: Feb 2010
Posts: 11
Rep Power: 6
izumi11 is on a distinguished road
My problem was only about connecting the fluid zones in the mesher. In ansys I've solved it by using multi-body parts. I think your problem is different. I think you will need to do a multiphase simulation with some kind of interface tracking unless the liquids don't mix. Since I only use gases I only had to set the percentage of each species at each inlet so a simple mixture simulation was enough.
Hope that helps.
izumi11 is offline   Reply With Quote

Old   March 25, 2010, 02:53
Default
  #8
New Member
 
ankit
Join Date: Mar 2010
Posts: 3
Rep Power: 6
anga87610del is on a distinguished road
actually i only want know ..how u set different fluid at each inlet(as u may have done in ur case)...in multiphase it only gives phases to be set..how to set specific fluid at specific inlet...please help me out with procedure in ansys fluent ver. 6.3...as u may have done it in ur case.

Thanks
anga87610del is offline   Reply With Quote

Old   March 25, 2010, 03:11
Default
  #9
New Member
 
Join Date: Feb 2010
Posts: 11
Rep Power: 6
izumi11 is on a distinguished road
In my case it's a gas mixture so there is only one phase. I set the inlet as a mass flow inlet. In materials, I set the fluid as a mix of hydrogen, oxygen h2o and nitrogen. The in the inlet bc, species tab, I set hydrogen mass fraction to 1 for inlet 1 and oxygen mass fraction to 0.21 for inlet 2.
Now this is only a gas mix so it is not really multiphase, in your case since liquids are involved it might be more complicated.
best.
izumi11 is offline   Reply With Quote

Old   March 25, 2010, 03:47
Default
  #10
New Member
 
ankit
Join Date: Mar 2010
Posts: 3
Rep Power: 6
anga87610del is on a distinguished road
thanx..!!!!
anga87610del is offline   Reply With Quote

Old   May 14, 2010, 23:14
Default 2 fluids at different inlets
  #11
New Member
 
raj
Join Date: Feb 2010
Location: OKlahoma
Posts: 13
Rep Power: 6
sammyraj is on a distinguished road
Hi

I am facing same problem as anga87610del, I have to introduce two fluids( liquids) at two inlets and the geometry consists of two annular pipes in which inside pipes ends at the middle and fluid coming from it joins with the fluid coming from outside pipe and both go through a single outlet. Hope I made it clear.

Please suggest me a method to use and how to introduce two inlets especially and I have been trying to use VOF method but I am not sure I am in a correct way. and also my fluids does not mix.

anga87610del please let me know if you have found solution.


Thanks a lot..!!
sammyraj is offline   Reply With Quote

Old   July 18, 2010, 10:36
Default 2 inlets...
  #12
New Member
 
bilalmerei
Join Date: Mar 2010
Posts: 14
Rep Power: 6
bilalmerei is on a distinguished road
Hello everyone.
have you find the way to introduce 2 different velosity inlets?
still waiting for a solution i tried a lot of ways but it seems that i need help
bilalmerei is offline   Reply With Quote

Old   October 8, 2010, 12:10
Default My 2 cents...
  #13
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,650
Blog Entries: 1
Rep Power: 34
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
Sorry, there was a lot to follow here and I am not sure on the final status, but someone asked me to comment, so here i am...

1) At the geometry level, you can combine bodies into a multi body part (using the model tree at the top left of DM). This will cause the meshes to be conformal. Not combining bodies into a part will result in them meshing separately... You could then create named selections on each body face where it contacts its neighbor so that you can net up non-conformal interfaces in Fluent... I think there is even an automatic way to do this (similar to automatic contact detection) but I forget the exact steps...

2) At some point (in DM or ANSYS Meshing), you would need to create named selections. Personally, I like to do it in ANSYS Meshing because there are more options and you can't forget to turn on the setting that passes named selections. You would create these for the faces of the bodies (such as Inlet, Outlet, etc.) but you should also create them for the bodies themselves... If all your bodies are supposed to be same zone, just select them all with the body selection tool, right click and Create a Named Selection named Fluid. If some of your bodies are in a porous, solid or other region, you should select those separately and name them. This should take care of the zones, interfaces, etc.

3) as for the questions about how to specify which fluids are coming thru each inlet, how the mixing happens, etc... I am sure there are some Fluent tutorials about that or you could ask the question on the Fluent Solver Forum.
hamiasmai and mayank199325 like this.
PSYMN is offline   Reply With Quote

Old   October 9, 2011, 04:49
Default problem to define another flow in mass flow inlet B.C
  #14
New Member
 
amir
Join Date: Jan 2011
Posts: 10
Rep Power: 5
amirmohebbi is on a distinguished road
dear all
hi
I am new in fluent
how i can define all of my mesh zone stagnation air
and mass flow inlet another flow like that fuel
then i have to the mixing rate of them
please help me?
thanks for your attention
amir mohebbi
amirmohebbi is offline   Reply With Quote

Old   November 20, 2012, 04:03
Default
  #15
New Member
 
prishor p k
Join Date: Jul 2012
Posts: 29
Rep Power: 4
prishor is on a distinguished road
hi all,
i am doing a multiphase flow simulation in fluidized bed using fluent 6.3. i have to enter air and steam as mixture in material properties. how should i proceed to enter the mixture property as it is currently disabled in material panel. i am doing the simulation without species transport.

please help me.

thanks and regards,

prishor p k
prishor is offline   Reply With Quote

Old   June 14, 2013, 23:29
Default
  #16
New Member
 
Mahboobe Mahdavi
Join Date: Mar 2013
Posts: 22
Rep Power: 3
Mahboobe365 is on a distinguished road
Hi all,I have the same problem one of the zones is vapor and one of them is porous with liquid. my problem is that the common line btweeb two zones is velocity inlet for example the water escapes from liquid zone come to vapor zones. But when i use multy parts in ansys , The lines will be defined az wall and i cant define velocity for them . Can you help me? pleasee
Mahboobe365 is offline   Reply With Quote

Old   December 2, 2013, 08:43
Default
  #17
New Member
 
Musty
Join Date: Oct 2013
Posts: 7
Rep Power: 3
mustafa-uslu is on a distinguished road
Quote:
Originally Posted by PSYMN View Post
Sorry, there was a lot to follow here and I am not sure on the final status, but someone asked me to comment, so here i am...

1) At the geometry level, you can combine bodies into a multi body part (using the model tree at the top left of DM). This will cause the meshes to be conformal. Not combining bodies into a part will result in them meshing separately... You could then create named selections on each body face where it contacts its neighbor so that you can net up non-conformal interfaces in Fluent... I think there is even an automatic way to do this (similar to automatic contact detection) but I forget the exact steps...

2) At some point (in DM or ANSYS Meshing), you would need to create named selections. Personally, I like to do it in ANSYS Meshing because there are more options and you can't forget to turn on the setting that passes named selections. You would create these for the faces of the bodies (such as Inlet, Outlet, etc.) but you should also create them for the bodies themselves... If all your bodies are supposed to be same zone, just select them all with the body selection tool, right click and Create a Named Selection named Fluid. If some of your bodies are in a porous, solid or other region, you should select those separately and name them. This should take care of the zones, interfaces, etc.

3) as for the questions about how to specify which fluids are coming thru each inlet, how the mixing happens, etc... I am sure there are some Fluent tutorials about that or you could ask the question on the Fluent Solver Forum.

Awsome answer. I had the similar problem but solve it after reading your comment. Thanks very much
mustafa-uslu is offline   Reply With Quote

Old   February 21, 2014, 02:21
Default Thanks and Help and Thanks
  #18
New Member
 
Hami Asma'i
Join Date: Jan 2014
Location: Tronoh, Perak, Malaysia
Posts: 5
Rep Power: 2
hamiasmai is on a distinguished road
Quote:
Originally Posted by PSYMN View Post
Sorry, there was a lot to follow here and I am not sure on the final status, but someone asked me to comment, so here i am...

1) At the geometry level, you can combine bodies into a multi body part (using the model tree at the top left of DM). This will cause the meshes to be conformal. Not combining bodies into a part will result in them meshing separately... You could then create named selections on each body face where it contacts its neighbor so that you can net up non-conformal interfaces in Fluent... I think there is even an automatic way to do this (similar to automatic contact detection) but I forget the exact steps...

2) At some point (in DM or ANSYS Meshing), you would need to create named selections. Personally, I like to do it in ANSYS Meshing because there are more options and you can't forget to turn on the setting that passes named selections. You would create these for the faces of the bodies (such as Inlet, Outlet, etc.) but you should also create them for the bodies themselves... If all your bodies are supposed to be same zone, just select them all with the body selection tool, right click and Create a Named Selection named Fluid. If some of your bodies are in a porous, solid or other region, you should select those separately and name them. This should take care of the zones, interfaces, etc.

3) as for the questions about how to specify which fluids are coming thru each inlet, how the mixing happens, etc... I am sure there are some Fluent tutorials about that or you could ask the question on the Fluent Solver Forum.
I am new and this really helpful! Kudos.
May I add one question: How to make dissolution phenomena between 2 phases? (preferebly tiny solid particles + liquid)

Thank you in advance.
Paskal likes this.
hamiasmai is offline   Reply With Quote

Old   October 15, 2014, 11:50
Default Mesh connection
  #19
New Member
 
Join Date: Jun 2014
Posts: 3
Rep Power: 2
landerfwc is on a distinguished road
Hi, I had similiar problem and I have successfully solved it by supressing automatically created contact regions in Ansys meshing. Then, to connect the meshes I created a Mesh connection on appropriate edges.
landerfwc is offline   Reply With Quote

Old   October 20, 2014, 12:17
Default
  #20
New Member
 
Bill Wang
Join Date: Aug 2014
Posts: 20
Rep Power: 2
6863523 is on a distinguished road
Quote:
Originally Posted by landerfwc View Post
Hi, I had similiar problem and I have successfully solved it by supressing automatically created contact regions in Ansys meshing. Then, to connect the meshes I created a Mesh connection on appropriate edges.
Hi, I am facing a similar problem.
I want to do the simulation of evaporation. There are two regions, one is water vapor, the other is wick saturated with liquid water. the evaporation is supposed to occur at the contact line between wick and vapor.
Need i specify the boundary type? Which kind? Interface? wall? porous-jump?
Thank you. Any suggestions would be appreciated. My email is: 815719752@qq.com
6863523 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
Exporting ANSYS mesh to FLUENT peksen FLUENT 0 July 6, 2007 10:33
Ansys and Fluent..HELP ME Francesco FLUENT 6 March 23, 2007 01:45
ANSYS file into Fluent Liaquat FLUENT 4 April 17, 2006 10:32
Creating fluid zone within Fluent Suresh Main CFD Forum 1 November 25, 2002 07:36
Inputs for porous zones in FLUENT Roel van Os Main CFD Forum 1 September 1, 1998 12:41


All times are GMT -4. The time now is 12:55.