CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   ANSYS Meshing & Geometry (http://www.cfd-online.com/Forums/ansys-meshing/)
-   -   [ANSYS Meshing] Patch Conformal Tetrahedron Mesh failure ... (http://www.cfd-online.com/Forums/ansys-meshing/120419-patch-conformal-tetrahedron-mesh-failure.html)

sandy_1982 July 6, 2013 13:39

Patch Conformal Tetrahedron Mesh failure ...
 
hi friends ,

i have to do a fuel tank slosh study in CFX

i had the tank geometry in CATIA V5 which i have imported into DM as .igs

the fluid i have extracted by 'sewing' the many surfaces and keeping 'creat solid' as 'on'

out of the many operations (running into 100s of those ) that i have done in DM to finally come to the 'fluid' domain from the basic tank structural geometry - only two operations have shown a 'warning' regarding the surfaces on which these were being performed while sewing etc.

having mentioned all the above , following is where i stand in the MESHER :

Update 1 (5th July 2013)

In Meshing, I have gone for the Patch Conformal Tetrahedron Method

Meshing Parameters chosen by me :

Min Size = 1 mm

Max Face Size = 10mm

Max Size = 30mm

Growth Ratio = 1.2

Mininum Edge Length (MEL) = 3.3e-003mm (Output from S/W)

Defeaturing Parameters

Pinch Tolerance = 2.98e-003 mm (I’ve taken it as 90% of MEL)

Advacd. Mesh Based Defeaturing “On”

Defeaturing Tolerance = 0.5 mm (I’ve taken it as 50% Min Size)

What I observed is that the Mesher has no problem to model all the “edges”, it’s only during modeling of “faces” that the Mesher shows the below error

“Following surfaces could not be meshed with acceptable quality. Try different element size or Virtual Topology”

Also in the Design Modeler I have observed some surfaces are missing from the fluid that has been extracted (by sewing surfaces and forming a ‘solid’) , although it has volume and surface area both – could this be the cause of error ?


How to get the meshing done ?


Update 2 (6th July 2013)

1. i am able to highlight the 'Trouble Surfaces' in Ansys Mesher which turn green

2. i then create a virtual cell on that face and/or alter the global or face sizing parameters on this particular face

3. still i am getting the same error " following surfaces could not be meshed..."
following surface here means the same surface that i had detected in step 1 above

{ALSO i observed that the 'Trouble Surface' can change depending on the ' Min Size' global parameter. }

Please tell me if i am on the correct path , because still the issue remains that the mesher is not able to model all the 'faces' because of the 'Trouble surface(s)" present in the geometry


thanks & regards

Sandeep

adunne304 July 11, 2013 11:48

Have you tried breaking down the fluid volume into smaller volumes, then meshing each one one at a time? This will allow you to isolate where exactly on the surface the mesher is failing. It could be caused by thin slivers, or by continuous curved surfaces.
From this you can decide whether you need to rework the geometry, use a different CAD export format (IGES is generally pretty poor), or mesh the volume in different sections.

sandy_1982 July 11, 2013 12:48

[QUOTE=adunne304;439219]....tried breaking down the fluid volume into smaller volumes, then meshing each one one at a time? This will allow you to isolate where exactly on the surface the mesher is failing. It could be caused by thin slivers, or by continuous curved surfaces."


Thanks for replying Adrian :)

presently i am using virtual topology and/or local face sizing for the 'problem surfaces' [which i can see upon right clicking on the error message], what i found is that after i do 'preview surface mesh' a new surface shows up as a 'problem surface' which means that there are many such faces which need to be taken care of. Is this the correct approach to take ?

and i take your suggestion of slicing the volume into smaller ones , but i am really not sure now that it will turn out an efficient method for my geometry

regards

Sandeep

adunne304 July 12, 2013 04:13

I know that the mesher generally doesn't tell you much about why the mesh is failing, but I find that sometimes splitting the surface, or splitting the volume across the surface can help.
Try exporting the CAD geometry as parasolid instead of .igs.

sandy_1982 July 18, 2013 13:09

a query related to the tank sloshing problem
 
what i have is a multibody part , there are two parts [tank fluid domain in two parts] which are just adjacent to each other - two faces are overlapping.

when i preview the surface mesh i get mesh on both these overlapping faces but there is not any node to node connection ( i have non conformal mesh here)

MY DOUBT is how to correct this situation in the solver , is there any way by which we can make the mesh conformal using some setting in the solver CFX ? Please keep in view that Tank flushing and Sloshing being my ultimate aim !



thanks

Sandeep

adunne304 July 19, 2013 06:49

If you take the geometry into Design modeller, right click the two domains [bodies] in the tree and choose 'form new part', then when you bring the geometry into the mesher, they'll share on common face and have a conformal mesh.
You could also use a match control or connections from within the mesher either.
Otherwise, as you are, you can use a GGI in the solver.

sandy_1982 July 25, 2013 13:52

hi ,
sorry for delay in reply ....

1.cutting up the fluid domain in smaller pieces is helping

2. in all , i have three 'fluid pieces' that make up the whole tank , that means three bodies (and two interfaces) i have in the same part (multi-body part)

3. i am meshing each of these three 'pieces' one by one , replacing the trouble parts/features by simpler ones by necessary operations in DM

4. so far i have been able to mesh two out of the three 'pieces' individually , now my next step will be two have these two meshed together(by keeping these two un-supressed in DM) , also i wonder how the mesh at the interface will come ? i want a good node to node connectivity ..!

am i going right ?...else what could be the 'more correct' approach , considering for the moment that only these two 'pieces' form the whole fluid domain ?

thanks

Sandeep

adunne304 July 26, 2013 06:35

AsI said in my previous post, if you group these three bodies into the same part (by right clicking them in the tree and selecting 'form new part' in DesignModeler), they will come into the mesher as a single part.
This means that the node to node connectivity between the bodies in the mesh will be exact, i.e. conformal. When you bring this into the solver, the mesh will be all in one, without any need for grid interfaces.

sandy_1982 July 27, 2013 13:58

yes , i am progressing well ...

i am getting conformal mesh at the multi-body part interface

i observe that while generating mesh in this multibody part - mesh sizing , defeaturing tolerance , and pinch tolerance become important ,apart from virtual topology.

also , the settings (min. size , max. face size , max. size) that are applicable for a single body are applicable exactly , in case of the multi-body part also , except that the various tolerances (defeaturing , pinch) may need to be altered in the latter case .....thats how i am approaching step by step.

vasava July 29, 2013 02:27

Have you tried playing with 'Advanced Size Function'? It might help if your model has too many curved faces.

rgd August 24, 2014 00:04

Quote:

Originally Posted by sandy_1982 (Post 442348)
yes , i am progressing well ...

i am getting conformal mesh at the multi-body part interface

i observe that while generating mesh in this multibody part - mesh sizing , defeaturing tolerance , and pinch tolerance become important ,apart from virtual topology.

also , the settings (min. size , max. face size , max. size) that are applicable for a single body are applicable exactly , in case of the multi-body part also , except that the various tolerances (defeaturing , pinch) may need to be altered in the latter case .....thats how i am approaching step by step.

Hi Sandeep,

Which of these features u mentioned, fixed ur connection problem? I am currently facing the same problem.
Could u plz elaborate in more detail?

Thanks a lot in advance.

sandy_1982 September 9, 2014 09:30

@rgd : sorry for late revert...i have given my approach as clearly as was possible at that time (its been a long time since...) in my previous posts ....please read all of them once again and you will get an idea for your problem

best wishes
Sandeep


All times are GMT -4. The time now is 21:58.