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

Overset mesh error.

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

Reply
 
LinkBack Thread Tools Display Modes
Old   February 28, 2013, 15:00
Unhappy Overset mesh error.
  #1
Member
 
Arun Krishnan.L.H
Join Date: Jan 2013
Posts: 75
Rep Power: 5
arun7328 is on a distinguished road
Hi all

I am trying to create an overset mesh for a problem of cylinder falling into water. I did the mesh and when i initialize i get the error "found inactive faces in region background.Could be due to too coarse or fine. I have made sure that the region of overlap has the same mesh size and has more than 4-5 cells.

Can anyone please help me out with the error?

The cells in the outer of the overset mesh is of 0.1 m and that in the background symmetry plane is of 0.125 m. I have attached the mesh and status diagram..

Please tell me what i should check. I have tried to change the sizes and check but still i get the same error.

Regards
Arun
Attached Images
File Type: jpg overset mesh.jpg (55.7 KB, 116 views)
File Type: jpg cell status.jpg (88.8 KB, 118 views)
arun7328 is offline   Reply With Quote

Old   February 28, 2013, 15:15
Unhappy
  #2
Member
 
Arun Krishnan.L.H
Join Date: Jan 2013
Posts: 75
Rep Power: 5
arun7328 is on a distinguished road
just to add this is my cell status..the picture is better...

Pls give me a tip if you know how to get this right..
arun7328 is offline   Reply With Quote

Old   February 28, 2013, 23:47
Default
  #3
Senior Member
 
KHB
Join Date: Aug 2010
Location: Singapore
Posts: 109
Rep Power: 7
lava12005 is on a distinguished road
Hi,

It seems from your Overset cell status the background value is 1 (red coloured) which means in-active and it shouln't be that way I suppose?
Maybe you should check whether you are assigning the correct overset boundary type to the correct boundary?
Or have you created the Overset Interface between the 2 domain?
lava12005 is offline   Reply With Quote

Old   March 1, 2013, 04:28
Default
  #4
Member
 
Arun Krishnan.L.H
Join Date: Jan 2013
Posts: 75
Rep Power: 5
arun7328 is on a distinguished road
I have created the overset interphase between the two and when i try to initialize the interface it fails. Now with changing the mesh values of the 2 regions i have got to another error which says "failed to cut a hole..could be a problem with overlap"..but how to check this overlap..I have left enoung cells in the overlap region of both boundaries.

thanks
arun
arun7328 is offline   Reply With Quote

Old   March 1, 2013, 14:41
Default
  #5
Member
 
Melih MeriÁ
Join Date: Apr 2011
Posts: 34
Rep Power: 7
grad@itu is on a distinguished road
if you want, you can send your file to me.. i would like to see..
grad@itu is offline   Reply With Quote

Old   March 1, 2013, 19:34
Default
  #6
Member
 
Arun Krishnan.L.H
Join Date: Jan 2013
Posts: 75
Rep Power: 5
arun7328 is on a distinguished road
ya sure ..i got it running now but after some time it displays an error the mesh might be too coarse or fine. Can i put it in the drop box? how can i share it with u?..my id is arun7328@gmail.com..if you gimme ur id i can share it with u...

Thanks a lot
Regards
Arun
arun7328 is offline   Reply With Quote

Old   March 3, 2013, 17:24
Default
  #7
Member
 
Arun Krishnan.L.H
Join Date: Jan 2013
Posts: 75
Rep Power: 5
arun7328 is on a distinguished road
Quote:
Originally Posted by grad@itu View Post
if you want, you can send your file to me.. i would like to see..
how should i send the file?..I have got it running but after some time it gives the same error, that the mesh is coarse of fine..I am not able to figure out why because i have made sure that the overset does not cross boundary region and also the mesh sizes even during movement is comparable. The physics is happening correctly now.

Regards
Arun
arun7328 is offline   Reply With Quote

Old   January 20, 2014, 22:19
Default
  #8
New Member
 
phanh
Join Date: Feb 2011
Posts: 20
Rep Power: 7
phanh is on a distinguished road
Quote:
Originally Posted by arun7328 View Post
how should i send the file?..I have got it running but after some time it gives the same error, that the mesh is coarse of fine..I am not able to figure out why because i have made sure that the overset does not cross boundary region and also the mesh sizes even during movement is comparable. The physics is happening correctly now.

Regards
Arun
Hi Arun,

Did you solve your problem? I have the similar error message. could you give me some advises for this issue?

Best regards
phanh is offline   Reply With Quote

Old   January 21, 2014, 05:13
Default
  #9
Member
 
Arun Krishnan.L.H
Join Date: Jan 2013
Posts: 75
Rep Power: 5
arun7328 is on a distinguished road
Hi.

Yes I solved the problem. Not sure what you are facing though. The problem with my model was that the mesh sizes on the boundary of the overset and the background were not the same. They have to exactly similar. In my case overset boundary was 0.1m and back ground was 0.125. I changed both to 0.1 and it worked.

Hope it works for you, if not explain yours and we shall see what to do.

Regards
Arun
arun7328 is offline   Reply With Quote

Old   January 22, 2014, 09:58
Default
  #10
New Member
 
phanh
Join Date: Feb 2011
Posts: 20
Rep Power: 7
phanh is on a distinguished road
Hi Arun,

Thank you for taking your time. I also solved my problem.

Best regards
phanh is offline   Reply With Quote

Old   May 1, 2014, 18:11
Default
  #11
New Member
 
Join Date: Mar 2012
Posts: 8
Rep Power: 6
EnronZhang is on a distinguished road
Hi Arun,

I have the similar problem as you had before. Just wondering that the mesh sizes of overset and back ground should be exactly the same, does it mean the volume mesh or the surface remesh? Because I have made the volume meshes in the same sizes for both region, but it still did not work.

Many thanks.
Enron

Quote:
Originally Posted by arun7328 View Post
Hi.

Yes I solved the problem. Not sure what you are facing though. The problem with my model was that the mesh sizes on the boundary of the overset and the background were not the same. They have to exactly similar. In my case overset boundary was 0.1m and back ground was 0.125. I changed both to 0.1 and it worked.

Hope it works for you, if not explain yours and we shall see what to do.

Regards
Arun
EnronZhang is offline   Reply With Quote

Old   May 2, 2014, 04:32
Default
  #12
Member
 
Arun Krishnan.L.H
Join Date: Jan 2013
Posts: 75
Rep Power: 5
arun7328 is on a distinguished road
Dear Zhang,

Its the volume meshes. What is the error message you are getting? Are you able to initialise the interface.

Regards
Arun
arun7328 is offline   Reply With Quote

Old   July 9, 2015, 17:04
Default
  #13
New Member
 
Join Date: May 2012
Posts: 1
Rep Power: 0
dhaval is on a distinguished road
I am running into same issue. In my case, background mesh has prism layers on the boundaries. When overset mesh enters into this prism layers, I get the error message. May be it is because prism mesh is smaller?

Background mesh size: 1.25 mm
Size of first prim layer in background mesh: 0.77 mm
Overset mesh size: 1 mm

I am not sure if the error message (mesh is either too small or too coarse) is due to two surfaces coming too close or because of size difference. I run another simulation with following sizes and it run without any problem (background: 1.45, prism: 0.85, overset: 1)
dhaval is offline   Reply With Quote

Old   July 16, 2015, 08:33
Default
  #14
Senior Member
 
Gajendra Gulgulia
Join Date: Apr 2013
Location: India
Posts: 113
Rep Power: 5
ggulgulia is on a distinguished road
Hi Everybody

From the images posted above, it was obvious that the cells were not intersecting properly. The best method to avoid this is to use mesh size in the Background Region nearly 1.5 times the mesh size in the Overset Region.
ggulgulia is offline   Reply With Quote

Old   April 6, 2016, 09:42
Default
  #15
New Member
 
lailai
Join Date: Jul 2015
Posts: 4
Rep Power: 2
withwolf is on a distinguished road
I'm facing the same problem. It turns out that I forgot to set the overset interface interpolation option to "linear".
withwolf 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
error compiling modified applications yvyan OpenFOAM Programming & Development 21 March 1, 2016 05:53
Compiling dynamicTopoFvMesh for OpenFOAM 2.1.x Saxwax OpenFOAM Installation 25 November 29, 2013 06:34
How to install CGNS under windows xp? lzgwhy Main CFD Forum 1 January 11, 2011 19:44
checking the system setup and Qt version vivek070176 OpenFOAM Installation 22 June 1, 2010 12:34
attach/detach (valve opening/closing) phsieh2005 OpenFOAM Running, Solving & CFD 2 March 21, 2009 06:18


All times are GMT -4. The time now is 19:30.