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

I see fluid solid interface on the setup domain although there is not one

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

Like Tree1Likes
  • 1 Post By recap2000

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   November 10, 2019, 06:11
Default I see fluid solid interface on the setup domain although there is not one
  #1
New Member
 
Tamer Ataol
Join Date: Nov 2019
Posts: 5
Rep Power: 6
recap2000 is on a distinguished road
Hi,


With ansys 18, fluid flow(cfx), I am doing two simulations for heat transfer as a result of fluid flow. The two simulations involve one cupe geometry and one hexagon geometry. Cube and hexagon has air inside of them. And on the faces I cut some piece and inserting ceramic. And there is one more part inside of this ceramic. Now this ceramic doesn't have any interface with the inside air because of this part inside of the ceramic. For the cube geometry I am seeing that there is only solid solid interface for the ceramic and for the hexagon there is fluid solid interface. And cube geometry simulation results are as expected and symmetric. But for hexagon it is very unsymmetric and wrong in my opinion. I am connecting this to the supposedly non happening fluid solid interface on the hexagon geometry. Where can I be wrong? I couldn't find the mistake. I checked the geometry and rebuild it. It seems fine. Can you help?
recap2000 is offline   Reply With Quote

Old   November 10, 2019, 16:30
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,830
Rep Power: 144
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
I am not sure exactly what you are asking, but it appears your interfaces are not set up correctly. The default generated interfaces should be checked in CFX-Pre to make sure they have the right surfaces in them. You can edit the surface list to make sure it is correct.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   November 15, 2019, 07:45
Default
  #3
New Member
 
Tamer Ataol
Join Date: Nov 2019
Posts: 5
Rep Power: 6
recap2000 is on a distinguished road
Hi,


Thank you for your answer. Let me explain more on the problem I have got. I have pentagon and hexagon structures. Both of them is problematic. I will post pictures of pentagon. You can see pentagon structure in the below pictueScreenshot from 2019-11-15 15-22-22.jpg The empty faces in the pentagon is filled with ceramic pieces that exactly fit. That is the ceramic completes the pentagon wall. Ceramic's inside face is boundary to aliminium heat sinks. There are five of them. Aside from these heat sinks, inside of the pentagon is filled with air completely. Now the problem is that air is not supposed to touch inside of ceramics. I checked the CAD file and this is the case. But, still in CFX-Pre, I see air-ceramic interface, that is to say fluid-solid interface on ceramics. You can see this in the second picture.



In the second picture there are only ceramic and its interfacesScreenshot from 2019-11-15 15-43-21.jpg. Green interface is solid-solid, which is as expected. But blue interfaces are fluid-solid. According to my symmetry there must not be any fluid-solid interface. I am assuming that there is something wrong with the way I mesh this geometry. I might be doing something wrong in the mesh settings. I tried to change size and adaptive options. But I cant find what could cause this in CFX. Do you have any suggestion to fix the problematic interface?
recap2000 is offline   Reply With Quote

Old   November 16, 2019, 05:21
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,830
Rep Power: 144
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
As I said in my previous post, if the default interfaces are wrong then edit them to correct them. Add or remove surfaces until they are correct.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   November 16, 2019, 10:38
Default
  #5
New Member
 
Tamer Ataol
Join Date: Nov 2019
Posts: 5
Rep Power: 6
recap2000 is on a distinguished road
Hi,


I tried what you said. But I cannot edit the default interface in anyways with (right click) edit or edit in command line options. When I delete the fluid solid interface a new interface with the same properties is created automatically and this is useless. What is the correct way to edit default interfaces under domains?
recap2000 is offline   Reply With Quote

Old   November 16, 2019, 12:37
Default
  #6
Senior Member
 
Join Date: Jun 2009
Posts: 1,860
Rep Power: 33
Opaque will become famous soon enough
How many mesh volumes do you have in your setup?

How many mesh volumes are listed under the solid domain? 1 or more?
Opaque is offline   Reply With Quote

Old   November 16, 2019, 13:40
Default
  #7
New Member
 
Tamer Ataol
Join Date: Nov 2019
Posts: 5
Rep Power: 6
recap2000 is on a distinguished road
I have 33931 mesh elements and more than one element for solid domains.
recap2000 is offline   Reply With Quote

Old   November 20, 2019, 05:55
Default
  #8
New Member
 
Tamer Ataol
Join Date: Nov 2019
Posts: 5
Rep Power: 6
recap2000 is on a distinguished road
I solved the problem. In case someone else encounters this type of problem you can try this: In the meshing windows choose body selection tool and ctrl+click on the bodies with wrong contacts. Right click and click on show contacts of the selected bodies. If you are sure that these contacts should not exist then right click and delete those contacts on the left menu. Then mesh and in the default interfaces you wont see wrong interfaces.
Xun likes this.
recap2000 is offline   Reply With Quote

Old   November 10, 2021, 19:22
Default
  #9
New Member
 
Kevin Jones
Join Date: Feb 2011
Posts: 17
Rep Power: 15
jones007 is on a distinguished road
I have a different but related problem. I have a multi-block domain created in SolidWorks and imported into the Ansys mesher. Most of the connections that it automatically generated seemed correct, but a few had extra faces. Those were easily fixed. If I manually look through them, they all seem correct, although sometimes they indicate faces are in contact with each other when they only share an edge. I left these, but I'm not sure if I should.

The real problem shows up when I run the case. All but one of the fluid-fluid interfaces seem OK, but on one, fluid does not appear to be able to traverse the interface. Streamlines appear to artificially deflect such that they are parallel to the interface, even though they should pass through it.

in CFX-pre I have been digging through the mesh volume and surface database, and was able to add a missing to one of the volumes - the face where the error occurred, but re-running the solution, it appears to have the same problem, so I think I am either trying to fix the problem in the wrong place, or the fix I am trying is superficial.

If anyone has run into a similar problem or knows of a thread where it is perhaps already addressed, the help would be much appreciated.
jones007 is offline   Reply With Quote

Old   November 10, 2021, 22:11
Default
  #10
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,830
Rep Power: 144
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
Note that when you add faces to an interface you have to do it at the interface object level, not the interface boundary in the domain level.

You should be able to manually add a few faces easily to an interface to fix it up. Do you know why you are finding that difficult?

In the output file and the results file there is a variable "non-overlap fraction". This shows which bits of the interface do no have a matching pair. This can be useful to debug the interfaces.

Another point: In ANSYS Mesh you can define named selections which in some cases can make defining interfaces easier. But this does not work well when adjacent domains share a common face as the named selection only gets put on one side.

Final point : In cases where getting the faces correct is really tricky I import the mesh into ICEM and sort it out there. In ICEM you can edit everything, group surfaces together and split them up; even down to individual element faces.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   November 11, 2021, 13:05
Default
  #11
New Member
 
Kevin Jones
Join Date: Feb 2011
Posts: 17
Rep Power: 15
jones007 is on a distinguished road
Thanks for the quick response. I suppose I'm a bit of a newbie on multi-block meshes. In all my earlier attempts, the mesher seemed to create all of the face-to-face connections correctly, and I really didn't have to fiddle with anything to get it working right. This is the first case where things didn't automatically get set up right leading to clearly non-physical results.

The interface that is failing is a spot where a large block has a cylindrical cavity cut in it, and then two cylinders are fit into the cavity, where the outer face of both cylinders share the same face of the cylindrical cavity. The interface between one of the cylinders works and the other does not.

I looked at the non-overlapping area fractions. On one side it is around 6e-6, and on the other about 0.375, so probably reflecting the problem.

Update: I just tried splitting the outer block into 2 parts such that it matched the 2 inner parts. Now the non-overlapping areas are both down around 1e-7. Looks like the issue was have faces on two blocks sharing a common face on a second block.

Last edited by jones007; November 11, 2021 at 14:45.
jones007 is offline   Reply With Quote

Reply

Tags
ansys cfx 18, fluid-solid coupling

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
CFD analaysis of Pelton turbine amodpanthee CFX 31 April 19, 2018 18:02
Periodic Pressure drop cfd_begin CFX 10 May 25, 2017 07:09
Centrifugal fan-reverse flow in outlet lesds to a mass in flow field xiexing CFX 3 March 29, 2017 10:00
Problem in setting Boundary Condition Madhatter92 CFX 12 January 12, 2016 04:39
No results for solid domain Gary Holland CFX 10 March 13, 2009 03:30


All times are GMT -4. The time now is 12:19.