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

Discontinuous contour at interface

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

Reply
 
LinkBack Thread Tools Display Modes
Old   December 2, 2014, 23:20
Default Discontinuous contour at interface
  #1
Member
 
Sangwoo Kim
Join Date: Jul 2014
Location: Seoul, South Korea
Posts: 91
Rep Power: 3
swtbkim is on a distinguished road
Hi all.

I attached my simulation results.
As you can see, there is some unreasonable contour at interface.

Does anyone know about this phenomenon?


I used meshing tool, Pointwise
and GGI interface.

Thank you in advance.
Attached Images
File Type: png interface1.PNG (26.9 KB, 18 views)
File Type: png interface2.PNG (28.0 KB, 14 views)
File Type: jpg interface3.jpg (54.2 KB, 11 views)
__________________
Best regards
swtbkim is offline   Reply With Quote

Old   December 3, 2014, 01:11
Default
  #2
Senior Member
 
Join Date: Jun 2009
Posts: 294
Rep Power: 9
Opaque is on a distinguished road
What kind of domain interface ? Frame change model used ?

Can you show mesh density on both sides of the interfaces ?

Are you plotting hybrid, or conservative values ?
Opaque is offline   Reply With Quote

Old   December 3, 2014, 02:51
Default
  #3
Member
 
Sangwoo Kim
Join Date: Jul 2014
Location: Seoul, South Korea
Posts: 91
Rep Power: 3
swtbkim is on a distinguished road
Quote:
Originally Posted by Opaque View Post
What kind of domain interface ? Frame change model used ?

Can you show mesh density on both sides of the interfaces ?

Are you plotting hybrid, or conservative values ?

Thank you for reply!


I don't use frozen rotor or something; so frame does not change.
I have to make subdomain for momentum source, that is the reason why I made multi block grid and interface is needed.

Hybrid is used.
Actually I don't know about this option.. hybrid vs. conservative
Hybrid is default, and I just used it.

I attached about mesh.
Attached Images
File Type: jpg mesh.jpg (80.7 KB, 17 views)
File Type: jpg mesh2.jpg (92.1 KB, 16 views)
File Type: jpg mesh3.jpg (49.2 KB, 11 views)
__________________
Best regards
swtbkim is offline   Reply With Quote

Old   December 3, 2014, 05:47
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,809
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Which post processor did you draw this with?
ghorrocks is offline   Reply With Quote

Old   December 3, 2014, 06:10
Default
  #5
Senior Member
 
RicochetJ's Avatar
 
Mr CFD
Join Date: Jun 2012
Location: Britain
Posts: 289
Rep Power: 6
RicochetJ is on a distinguished road
Is the mesh adequate for your problem? I don't know the full details of your mesh, but it looks poorly formed.
RicochetJ is offline   Reply With Quote

Old   December 3, 2014, 06:18
Default
  #6
Member
 
Sangwoo Kim
Join Date: Jul 2014
Location: Seoul, South Korea
Posts: 91
Rep Power: 3
swtbkim is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
Which post processor did you draw this with?

All figures are drawn with CFD-POST.
__________________
Best regards
swtbkim is offline   Reply With Quote

Old   December 3, 2014, 06:29
Default
  #7
Member
 
Sangwoo Kim
Join Date: Jul 2014
Location: Seoul, South Korea
Posts: 91
Rep Power: 3
swtbkim is on a distinguished road
Quote:
Originally Posted by RicochetJ View Post
Is the mesh adequate for your problem? I don't know the full details of your mesh, but it looks poorly formed.

I agree with you..
This is one of several versions of mesh. Not well-made grid.

You mean, mesh quality is important in this case?
I thought that this is an issue about interpolation inside each grid cell, not mesh quality.


I attached view of mesh at large.
Flow is induced from left to right(i.e. from opening into pipe)
Opening is one block, and Inside the pipe is one block.
So the inlet of the pipe is specified as interface between two blocks.

And I made an inflation layer at that interface.
It's pretty weird treatment, but I thought it was not important.
Attached Images
File Type: jpg large view.jpg (97.9 KB, 20 views)
__________________
Best regards
swtbkim is offline   Reply With Quote

Old   December 3, 2014, 11:29
Default
  #8
Super Moderator
 
diamondx's Avatar
 
Ghazlani M. Ali
Join Date: May 2011
Location: Canada
Posts: 1,291
Blog Entries: 23
Rep Power: 20
diamondx will become famous soon enough
mesh quality is poor, extend your prism to other boundary at lest. I personnaly don't like transitions from 10 layers to 0 layer
__________________
Regards,
New to ICEM CFD, try this document --> http://goo.gl/G2gkE
Ali
diamondx is offline   Reply With Quote

Old   December 3, 2014, 12:07
Default
  #9
Senior Member
 
Thomas MADELEINE
Join Date: Oct 2014
Posts: 122
Rep Power: 2
Thomas MADELEINE is on a distinguished road
Just another question about the mesh...
Why did you use some inflation layout on the interface ?
In my point of view it is only usefull close to wall (with no slip option) to catch the layer (big gradient of the velocity in small area) so it should be on the walls but not on the interface.

There, the flow will have to pass through multiple cells from one domain to another.

However I am not sure of all of this but I have never saw this problem before using this method...

I hope this can help.
Regards,
Thomas MADELEINE
Thomas MADELEINE is offline   Reply With Quote

Old   December 3, 2014, 12:27
Default
  #10
Senior Member
 
Join Date: Jun 2009
Posts: 294
Rep Power: 9
Opaque is on a distinguished road
Could you share the same plot using Conservative values ?

You should probably have a look at the documentation about what Hybrid values are, and the known issues with them. Interpret what they are in the context of the mesh you have shown plus the fact that it may be coarse, mismatched and the fact that interpolation must be used to create the plot.

I did not understand the reasoning for creating an interface. Definitely, the fact that you need a subdomain to include sources is not enough reason to justify an interface. Subdomains do not have to cover all of the domain.

If your physics is the same everywhere (except for the source), and there is no frame change, they only reason left for an interface is that you meshed the volumes separately, the faces do not match at those common surfaces; therefore, you must manually stitch them.
Opaque is offline   Reply With Quote

Old   December 3, 2014, 17:49
Default
  #11
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,809
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Have you had a look at the non-overlap fraction? Does the velocity field look correct in the area? The GGI might not be joining these faces together properly and so these bits of the mesh might not be connected. This should be seen in the non-overlap fraction and a obvious kink in the velocity field.
ghorrocks is offline   Reply With Quote

Old   December 3, 2014, 22:28
Default
  #12
Member
 
Sangwoo Kim
Join Date: Jul 2014
Location: Seoul, South Korea
Posts: 91
Rep Power: 3
swtbkim is on a distinguished road
Quote:
Originally Posted by Thomas MADELEINE View Post
Just another question about the mesh...
Why did you use some inflation layout on the interface ?
In my point of view it is only usefull close to wall (with no slip option) to catch the layer (big gradient of the velocity in small area) so it should be on the walls but not on the interface.

There, the flow will have to pass through multiple cells from one domain to another.

However I am not sure of all of this but I have never saw this problem before using this method...

I hope this can help.
Regards,
Thomas MADELEINE


It was just my curiosity that there is also a big gradient of velocity at the inlet of pipe, so if there is an inflation, then it may increase the accuracy or not?
__________________
Best regards
swtbkim is offline   Reply With Quote

Old   December 3, 2014, 22:29
Default
  #13
Member
 
Sangwoo Kim
Join Date: Jul 2014
Location: Seoul, South Korea
Posts: 91
Rep Power: 3
swtbkim is on a distinguished road
Quote:
Originally Posted by diamondx View Post
mesh quality is poor, extend your prism to other boundary at lest. I personnaly don't like transitions from 10 layers to 0 layer
You mean, make inflation at all walls?
__________________
Best regards
swtbkim is offline   Reply With Quote

Old   December 3, 2014, 22:40
Default
  #14
Member
 
Sangwoo Kim
Join Date: Jul 2014
Location: Seoul, South Korea
Posts: 91
Rep Power: 3
swtbkim is on a distinguished road
Quote:
Originally Posted by Opaque View Post
Could you share the same plot using Conservative values ?

You should probably have a look at the documentation about what Hybrid values are, and the known issues with them. Interpret what they are in the context of the mesh you have shown plus the fact that it may be coarse, mismatched and the fact that interpolation must be used to create the plot.

I did not understand the reasoning for creating an interface. Definitely, the fact that you need a subdomain to include sources is not enough reason to justify an interface. Subdomains do not have to cover all of the domain.

If your physics is the same everywhere (except for the source), and there is no frame change, they only reason left for an interface is that you meshed the volumes separately, the faces do not match at those common surfaces; therefore, you must manually stitch them.


Thank you. I'm going to check the hybrid value issue.

Then, interfaces are always exactly matched to each other??
How can it be done automatically?


first image is conservative values
blue region became red(..)


second and third image are about another mesh. It is also not good, but not that much than previous mesh.
Grid cell is not matched, GGI interfaces are used, and discontinuous contour is made.
How can I fix this??
Should I make exactly matched surface mesh at interface?
Attached Images
File Type: jpg 1.jpg (19.2 KB, 10 views)
File Type: jpg 2.jpg (21.0 KB, 11 views)
File Type: jpg 3.jpg (65.0 KB, 12 views)
__________________
Best regards
swtbkim is offline   Reply With Quote

Old   December 3, 2014, 22:49
Default
  #15
Member
 
Sangwoo Kim
Join Date: Jul 2014
Location: Seoul, South Korea
Posts: 91
Rep Power: 3
swtbkim is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
Have you had a look at the non-overlap fraction? Does the velocity field look correct in the area? The GGI might not be joining these faces together properly and so these bits of the mesh might not be connected. This should be seen in the non-overlap fraction and a obvious kink in the velocity field.

I don't know what is nonoverlap fraction. I'm going to study about it..
When I make contour of it, all I see is this image.
Blue one is edges of whole domain; opening boundary condition quite far from pipe.


Mean flow looks good and reasonable.
Attached Images
File Type: png non.PNG (11.8 KB, 7 views)
__________________
Best regards
swtbkim is offline   Reply With Quote

Old   December 3, 2014, 23:12
Default
  #16
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,809
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Nonoverlap fraction applies to interface boundaries and is the proportion of the element face which does not overlap with an element on the other side of the interface. If you see a high nonoverlap fraction in a region of GGI which should be part of the mesh connection then you have a problem with your GGI interface as it has not correctly identified faces on either side of the boundary to match up.

This can occur on GGI interfaces when you have either big changes in mesh size over the interface, or high aspect ratio elements at the interface. In both these cases the default GGI settings do occasionally miss elements on interfaces.

You have now shown that when you use a mesh with an aspect ratio closer to 1 the interface works properly. You have high aspect ratio elements on the interface you first posted as you put inflation mesh on the interface boundary faces so I suspect you are getting this non-overlap problem.
ghorrocks is offline   Reply With Quote

Old   December 4, 2014, 01:53
Default
  #17
Member
 
Sangwoo Kim
Join Date: Jul 2014
Location: Seoul, South Korea
Posts: 91
Rep Power: 3
swtbkim is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
Nonoverlap fraction applies to interface boundaries and is the proportion of the element face which does not overlap with an element on the other side of the interface. If you see a high nonoverlap fraction in a region of GGI which should be part of the mesh connection then you have a problem with your GGI interface as it has not correctly identified faces on either side of the boundary to match up.

This can occur on GGI interfaces when you have either big changes in mesh size over the interface, or high aspect ratio elements at the interface. In both these cases the default GGI settings do occasionally miss elements on interfaces.

You have now shown that when you use a mesh with an aspect ratio closer to 1 the interface works properly. You have high aspect ratio elements on the interface you first posted as you put inflation mesh on the interface boundary faces so I suspect you are getting this non-overlap problem.


Thank you for careful reply, Glenn.

Then, do you think that interface I secondary posted is good enough?
But there is a discontinuous region yet.
You just meant that this is not about non-overlap fraction issue, but another one?
__________________
Best regards
swtbkim is offline   Reply With Quote

Old   December 4, 2014, 04:53
Default
  #18
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,809
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
You are never going to get a perfectly continuous contour at a GGI. The contour drawing gizmo inside CFD-Post only draws contours based on the values inside that domain, so it cannot do continuous contours across GGI interfaces as that spans multiple domains. The best you can do is get contours which are close. Your post #14 has contours which are close enough that I suspect the GGI is working correctly, but post #1 and #3 show contours which clearly are wrong and therefore are likely to have the non-overlap problem.
ghorrocks is offline   Reply With Quote

Old   December 4, 2014, 05:40
Default
  #19
Member
 
Sangwoo Kim
Join Date: Jul 2014
Location: Seoul, South Korea
Posts: 91
Rep Power: 3
swtbkim is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
You are never going to get a perfectly continuous contour at a GGI. The contour drawing gizmo inside CFD-Post only draws contours based on the values inside that domain, so it cannot do continuous contours across GGI interfaces as that spans multiple domains. The best you can do is get contours which are close. Your post #14 has contours which are close enough that I suspect the GGI is working correctly, but post #1 and #3 show contours which clearly are wrong and therefore are likely to have the non-overlap problem.

Then it is a limitation of CFD-POST and I should satisfy with it, and make finer grid if I want more smooth contour.



Thank you all very much
__________________
Best regards
swtbkim is offline   Reply With Quote

Old   December 4, 2014, 07:41
Default
  #20
Member
 
davide basso
Join Date: Jan 2012
Posts: 47
Rep Power: 5
rolloblues is on a distinguished road
Quote:
Originally Posted by swtbkim View Post
make finer grid if I want more smooth contour.
I will reiterate what other members correctly already pointed out:
I'm afraid that a finer mesh won't resolve your problems.
You should re-think your meshing approach without growing prisms from the interface.
rolloblues 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
Wind turbine simulation Saturn CFX 34 October 16, 2014 05:27
sliding mesh problem in CFX Saima CFX 35 May 12, 2014 20:28
Question about heat transfer coefficient setting for CFX Anna Tian CFX 1 June 16, 2013 06:28
Error finding variable "THERMX" sunilpatil CFX 8 April 26, 2013 07:00
RPM in Wind Turbine Pankaj CFX 9 November 23, 2009 05:05


All times are GMT -4. The time now is 16:53.