|
[Sponsors] |
[ANSYS Meshing] Contact surface generated betwwen surfaces not in contact |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
October 6, 2016, 08:27 |
Contact surface generated betwwen surfaces not in contact
|
#1 |
Senior Member
Manu Chakkingal
Join Date: Feb 2016
Location: Delft, Netherlands
Posts: 129
Rep Power: 10 |
Hello
I am planning to do a conjugate heat transfer problem with a lot of spheres in a box. As in figure one the spheres arent in contact while the inerfaces shows a contact region for it..This goes away when I make sphere small and none of the spheres are close. At present distance b/w two sphere is .005cm. Could some one comment on this? (Geometry creation and meshing in workbench)
__________________
Regards Manu |
|
October 6, 2016, 18:37 |
|
#2 |
Senior Member
Join Date: Apr 2014
Location: Melbourne
Posts: 584
Rep Power: 13 |
delete all the contact regions listed!
use named selection for any contacts! |
|
October 12, 2016, 07:53 |
|
#3 |
Senior Member
Paritosh Vasava
Join Date: Oct 2012
Location: Lappeenranta, Finland
Posts: 732
Rep Power: 22 |
Indeed this is bit difficult to handle. But I can think of two ways to fix this.
1. Right click on the 'contacts' and select 'Repair Overlapping Contact Regions'. This should help eliminate or highlight the faces that appear in more than one interfaces. The operation will also generate an extra set of interfaces, you can check them and decide if you want to keep or delete them. Another way is rather manual. (1) Rename the solid spheres as sphere1, sphere2.... and so on. (2) Delete all the interfaces. (3) Generate automatic contact regions. (4) Right click on 'Contacts' and you will see option for naming the interfaces according to body names. This will name the interfaces accordingly e.g. Bonded-fluid_To_Sphere1, Bonded-Sphere1_To_Sphere2 and so on. Now you can clearly see which intefaces and between fluids and which ones are between spheres. Are you using Design modeler or SpaceClaim for CAD? If you are using spaceclaim, then there is another way to do this. Last edited by vasava; October 12, 2016 at 08:07. Reason: add |
|
October 12, 2016, 07:54 |
|
#4 |
Senior Member
Manu Chakkingal
Join Date: Feb 2016
Location: Delft, Netherlands
Posts: 129
Rep Power: 10 |
Design modeler
__________________
Regards Manu |
|
October 12, 2016, 08:53 |
|
#5 |
Senior Member
Paritosh Vasava
Join Date: Oct 2012
Location: Lappeenranta, Finland
Posts: 732
Rep Power: 22 |
I have no experience with DM. You can try those two tricks and let us know how it went.
|
|
October 12, 2016, 08:55 |
|
#6 |
Senior Member
Manu Chakkingal
Join Date: Feb 2016
Location: Delft, Netherlands
Posts: 129
Rep Power: 10 |
the repair worked for me
__________________
Regards Manu |
|
October 27, 2019, 17:16 |
|
#7 |
New Member
Valera
Join Date: Dec 2018
Posts: 27
Rep Power: 7 |
I've faced with the same problem. The pipes of my heat exchanger aren't in contact, but contacts have been created.
I don't quite understand how you repared it. Can you, please, tell, how you've solved it? You just manually deleted them? My model includes only internal volume (i.e water, without metal cladding). So no regions should be created. Is there any way how avoid the automatically creating these contacts? Or I just have to delete them? |
|
November 12, 2019, 14:04 |
|
#8 |
Member
Joshua
Join Date: Aug 2014
Posts: 49
Rep Power: 11 |
The Ansys Workbench default is to automatically create contacts according to the default settings (whether or not you have a fluid or solid modeled is relevant to the contact creation tool).
You can change the default settings such that this doesn't happen in the future. For now, delete the auto-created contacts and then disable the creation of auto-contact generation selecting 'Connections' and disabling the 'auto-create on re-attach' option. This way, if you re-attach the geometry from Design Modeler the contacts won't auto recreate themselves. |
|
November 12, 2019, 14:32 |
|
#9 | |
New Member
Valera
Join Date: Dec 2018
Posts: 27
Rep Power: 7 |
Quote:
Thank you for your response! I've been waiting it so much!!! |
||
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
[ICEM] Problems with coedge curves and surfaces | tommymoose | ANSYS Meshing & Geometry | 6 | December 1, 2020 12:12 |
[ICEM] surface mesh merging problem | everest | ANSYS Meshing & Geometry | 44 | April 14, 2016 07:41 |
[snappyHexMesh] SHM not snapping to some surfaces | Swift | OpenFOAM Meshing & Mesh Conversion | 13 | January 4, 2016 02:56 |
[ICEM] How to generate sunstructured "all-tri patch-dependant" surface mesh in ICEM? | jash | ANSYS Meshing & Geometry | 19 | July 23, 2013 19:48 |
Dynamic mesh in Fluent to study tire in contact with road surface | lihuang | FLUENT | 10 | March 8, 2011 11:21 |