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

symmetry boundary conditions in cfx

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

Like Tree1Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   June 13, 2009, 08:53
Default
  #21
Senior Member
 
Matthias Voß
Join Date: Mar 2009
Location: Berlin, Germany
Posts: 446
Rep Power: 12
mvoss is on a distinguished road
Quote:
Originally Posted by neewbie View Post
okay... so no ANSYS CFX Mesh... sorry.
I´ve had the same problem with this kind of geometry (i am refering to your first post: no plane surface) and i found my mistake by checking the mesh-surface normals in CFX Post. The association at the small face in the center, forming the artificalltube later, was corrupt. Did you do a mesh check over dterminanentes an soone in ICEM?
neewbie
try this ... i found some folded elementes near the horizontal edges on my blocking... fixed them... all went good
neewbie
mvoss is offline   Reply With Quote

Old   June 14, 2009, 03:12
Default
  #22
Senior Member
 
Join Date: Apr 2009
Posts: 118
Rep Power: 9
lost.identity is on a distinguished road
Thanks. Sorry for all the questions but how do you actually check for folded elements in ICEM?


I've looked at the determinants, angles, warpage. I have some very small 2x2x2 determinats (of about 0.04) near the horizontal axis. But I don't know how you could tell whether they are folded? And how did you fix them?
lost.identity is offline   Reply With Quote

Old   June 14, 2009, 10:52
Default
  #23
Senior Member
 
Matthias Voß
Join Date: Mar 2009
Location: Berlin, Germany
Posts: 446
Rep Power: 12
mvoss is on a distinguished road
Quote:
Originally Posted by lost.identity View Post
Thanks. Sorry for all the questions but how do you actually check for folded elements in ICEM?


I've looked at the determinants, angles, warpage. I have some very small 2x2x2 determinats (of about 0.04) near the horizontal axis. But I don't know how you could tell whether they are folded? And how did you fix them?
hi
load the cfx5-mesh in post and examine the facenormals at the axis.
aslong as your are trying to simulate a 2D-symmetric geometry, you could also delete the "axis-face" and collapse the geometry back to the real model, wich means no "symmetry-face" but a real axis.

You would fix the bad elements by making shure that the face you project the surfaces on and the edges you project the lines on are the same. In other words, make shure the surface really ends up in the line on which you projected the blockingedges on, because sometimes, the surfaceenclosing lines and the pure lines of the imported geometry are not the same.
Try repear and build topology in the geometrytab.

neewbie
mvoss is offline   Reply With Quote

Old   June 14, 2009, 20:34
Default
  #24
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,411
Rep Power: 97
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
Hi,

Also keep in mind the fact that when you try to convince CFX to do a 2D axisymmetric simulation using a small angled wedge you have two competing requirements - You need the wedge angle small so it accurately represents the full revolved geometry but you need it large enough such that the mesh quality of the elements on the axis is not too bad. For some sensitive free surface flow simulations I could not go smaller than 5 degrees before I got convergence problems. But for general stuff you should be able to go much smaller than that.

Glenn Horrocks
ghorrocks is offline   Reply With Quote

Old   November 6, 2009, 08:29
Smile
  #25
New Member
 
Xue-Guan Song
Join Date: Mar 2009
Location: Busan, Korea
Posts: 14
Rep Power: 9
songxguan is on a distinguished road
ghorrocks is right,

anybody who want to simplify his/her 3D modelling to 2D one layer axi-symmetrical modelling should simulate a simple case to emphasize the understanding of the simplification.

in my case, first i used a 3.6deg one layer mesh, and cfx run it very well. however, when i tried to modified a little of the mesh, cfx couldn't run the .msh file again, it's said one symmetrical b.c. is not a real plane......
I tried many ways to resolve it, even build the 3D modelling and import it to icemcfd again, but unfortunately, it didn't work, always wrong mesh.

at last, i changed the 3.6deg to 7.2deg, it's very surprising, it's OK!......

so, what I want to say is: cfx also has wrong place sometimes, don't trust it all.

hope this will help somebody who's using one layer axi-symmetrical model.
songxguan is offline   Reply With Quote

Old   April 14, 2010, 17:42
Default
  #26
Senior Member
 
Joshua Counsil
Join Date: Jul 2009
Location: Halifax, Nova Scotia, Canada
Posts: 366
Rep Power: 10
Josh is on a distinguished road
I was having this same problem. Glenn's suggestion of changing the symmetry section in ICEM to two separate parts worked. I then created two symmetry boundary conditions in Pre and it worked.

Once again, I am in debt to Glenn.
Josh is offline   Reply With Quote

Old   June 18, 2010, 06:34
Default
  #27
New Member
 
Join Date: Jun 2010
Posts: 10
Rep Power: 8
caravell78 is on a distinguished road
In the attachment there is a sketch of the system. I didn't put anything between the two subdomains...
Attached Images
File Type: png Picture.png (2.3 KB, 48 views)
caravell78 is offline   Reply With Quote

Old   June 18, 2010, 06:54
Default
  #28
New Member
 
Join Date: Jun 2010
Posts: 10
Rep Power: 8
caravell78 is on a distinguished road
I understand what you said, and actually I used a Domain Interface, disabling the momentum transfer and enabling the mass flux. However,
the problem about flux unfortunately still remains...
caravell78 is offline   Reply With Quote

Old   July 2, 2010, 06:51
Question How to find the boundary faces of a volume mesh?
  #29
New Member
 
ankit
Join Date: Jul 2010
Posts: 1
Rep Power: 0
amazingankit123 is on a distinguished road
Hi, I am a newbie to ansys. I am using ANSYS v12.
I want to know the procedure to find boundary faces of a 3d volume mesh. I am doing tetrahedral meshing. I need to know the node numbers of all the triangular elements that will be created due to meshing on a geometry like a solid hemisphere to apply boundary conditions for convection.

Any help from this forum will be highly appreciated.

Thank you
Ankit
amazingankit123 is offline   Reply With Quote

Old   May 16, 2013, 08:19
Default Symmetry
  #30
New Member
 
Amod Panthee
Join Date: Apr 2013
Location: Nepal
Posts: 18
Rep Power: 5
amodpanthee is on a distinguished road
Quote:
Originally Posted by lost.identity View Post
So I've imported the mesh into CFX without any errors and set the inlet, outlet and wall BCs. Then I applied symmetry boundary conditions to the two side faces (they are in individual parts this time). But when I run the simulation I still get this error, even though the face is infact in a plane.
lost.identity

Did you solve the problem with symmetry?

I have similar problem......Can you explain what you did?

Thanks in advance
amodpanthee is offline   Reply With Quote

Old   May 16, 2013, 09:31
Default
  #31
Senior Member
 
OJ
Join Date: Apr 2012
Location: United Kindom
Posts: 475
Rep Power: 12
oj.bulmer will become famous soon enough
The answer lies infact in the error message - third option:

(3) Increase the value of the Solver Expert Parameter |
| 'vector parallel tolerance' (the default value is 1 deg.). |
| Note that the accuracy of the symmetry condition may decrease |
| as the tolerance is increased. This is because the tolerance |
| is the number of degrees that a mesh face normal is allowed |
| to deviate from the average normal for the entire face set.

Try increasing the expert parameter value of vector parallel tolerance to 5 or 10 or 15 etc... You should surely remove the error. Or, consider using free-slip boundary condition instead of symmetry.

OJ
oj.bulmer is offline   Reply With Quote

Old   May 16, 2013, 09:59
Default
  #32
New Member
 
Amod Panthee
Join Date: Apr 2013
Location: Nepal
Posts: 18
Rep Power: 5
amodpanthee is on a distinguished road
Thanks oj.bulmer......I will check if it works or not .......Actually, I tried changing it to 5 earlier......but it didn't work in my case.....May be I should increase it more...... Does changing this default value to higher values cause any inaccuracy in simulation?
amodpanthee is offline   Reply With Quote

Old   May 16, 2013, 18:46
Default
  #33
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,411
Rep Power: 97
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
It absolutely does cause inaccuracy! This error message is telling you to go back to your mesh and fix up the symmetry surface and make it flat.There is a good reason why the tolerance is 1 degree.
ghorrocks is offline   Reply With Quote

Old   May 20, 2013, 13:47
Default
  #34
Senior Member
 
OJ
Join Date: Apr 2012
Location: United Kindom
Posts: 475
Rep Power: 12
oj.bulmer will become famous soon enough
Actually, this was the advice given to me by a CFX engineer. I once was troubled by the similar problem and couldn't get rid of this error. The mesh quality was alright and in side view it the symmetry surface looked flat, but even for 15 deg of the vector parallel tolerance, the error stayed. Amazingly, the identical mesh I did which was copied from the same mesh, was fine even within 1 deg of tolerance!

Ideally, you should keep it tight. But there are instances where, no matter what you do to the mesh, the error just doesn't go away. In those cases, either you can stare in despair at the screen, or you can use this getaway - provided the mesh on symmetry plane is fine enough and all the facets of cells on the symmetry are seen to be on the symmetry plane to the eye, when looked from sideways. At least this is what ANSYS guys suggest.

OJ
evan247 likes this.
oj.bulmer is offline   Reply With Quote

Old   May 20, 2013, 18:13
Default
  #35
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,411
Rep Power: 97
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
Your comment is correct - many times the deviation is in an unimportant part of the flow and will not affect things. But if it is in a critical part of the flow it will. It is a case of caveat emptor (http://en.wikipedia.org/wiki/Caveat_emptor).
ghorrocks is offline   Reply With Quote

Old   May 21, 2013, 05:16
Default
  #36
Senior Member
 
OJ
Join Date: Apr 2012
Location: United Kindom
Posts: 475
Rep Power: 12
oj.bulmer will become famous soon enough
Well I do appreciate your viewpoint, and I agree that this suggestion should be the last resort, and after being aware of the implications

But some funny experiences make me believe that sometimes, this error is a symptom of CFX's moodiness and has little to do with the mesh per se.

OJ
oj.bulmer is offline   Reply With Quote

Old   May 21, 2013, 19:21
Default
  #37
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,411
Rep Power: 97
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
Moody software....... The mind boggles with the implications of that
ghorrocks is offline   Reply With Quote

Old   May 22, 2013, 05:33
Default Design Modeler Fluid/Solid
  #38
New Member
 
Amod Panthee
Join Date: Apr 2013
Location: Nepal
Posts: 18
Rep Power: 5
amodpanthee is on a distinguished road
What are the effects of defining the geometry as solid/fluid after importing from a external 3D modeling software? (see attached picture)
Attached Images
File Type: jpg new.JPG (69.6 KB, 17 views)
amodpanthee is offline   Reply With Quote

Old   May 22, 2013, 05:58
Default
  #39
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,411
Rep Power: 97
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
All it does it to make the default domain in the CFX-Pre section solid or fluid. You can overwrite it if it is wrong (or you did not bother setting it).
ghorrocks is offline   Reply With Quote

Old   May 22, 2013, 06:00
Default
  #40
New Member
 
Amod Panthee
Join Date: Apr 2013
Location: Nepal
Posts: 18
Rep Power: 5
amodpanthee is on a distinguished road
While importing the solid geometry....I have defined the operation as "Add Frozen". What are the differences of defining operation as Add frozen or Add Material?
amodpanthee 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
CFX Boundary Conditions albert62 CFX 5 January 5, 2010 07:49
2D Airfoil - Dimensions & boundary conditions -CFX Santiago CFX 3 December 13, 2006 11:50
Help with boundary conditions Dan CFX 0 April 3, 2006 11:32
Water vapour condensation in CFX-5.7.1 hdj CFX 1 November 27, 2005 08:15
Trimmed cell and embedded refinement mesh conversion issues michele OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ... 2 July 15, 2005 04:15


All times are GMT -4. The time now is 21:11.