try this ... i found some folded elementes near the horizontal edges on my blocking... fixed them... all went good
neewbie

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

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 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.

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.

In the attachment there is a sketch of the system. I didn't put anything between the two subdomains...

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...

How to find the boundary faces of a volume mesh?
 

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

Symmetry
 

lost.identity

Did you solve the problem with symmetry?

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

Thanks in advance

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

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?

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.

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

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).

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

Moody software....... The mind boggles with the implications of that :)

Design Modeler Fluid/Solid
 

What are the effects of defining the geometry as solid/fluid after importing from a external 3D modeling software? (see attached picture)

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).

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?