CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > ANSYS Meshing & Geometry

[ANSYS Meshing] Patch Conformal Tetrahedron Mesh failure ...

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

Reply
 
LinkBack Thread Tools Display Modes
Old   July 6, 2013, 13:39
Default Patch Conformal Tetrahedron Mesh failure ...
  #1
Member
 
Sandeep
Join Date: Oct 2012
Location: India
Posts: 51
Rep Power: 4
sandy_1982 is on a distinguished road
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
sandy_1982 is offline   Reply With Quote

Old   July 11, 2013, 11:48
Default
  #2
New Member
 
Adrian
Join Date: Jul 2013
Location: Dublin
Posts: 21
Rep Power: 5
adunne304 is on a distinguished road
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.
__________________
www.idacireland.com
adunne304 is offline   Reply With Quote

Old   July 11, 2013, 12:48
Default
  #3
Member
 
Sandeep
Join Date: Oct 2012
Location: India
Posts: 51
Rep Power: 4
sandy_1982 is on a distinguished road
[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
sandy_1982 is offline   Reply With Quote

Old   July 12, 2013, 04:13
Default
  #4
New Member
 
Adrian
Join Date: Jul 2013
Location: Dublin
Posts: 21
Rep Power: 5
adunne304 is on a distinguished road
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.
__________________
www.idacireland.com
adunne304 is offline   Reply With Quote

Old   July 18, 2013, 13:09
Default a query related to the tank sloshing problem
  #5
Member
 
Sandeep
Join Date: Oct 2012
Location: India
Posts: 51
Rep Power: 4
sandy_1982 is on a distinguished road
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
sandy_1982 is offline   Reply With Quote

Old   July 19, 2013, 06:49
Default
  #6
New Member
 
Adrian
Join Date: Jul 2013
Location: Dublin
Posts: 21
Rep Power: 5
adunne304 is on a distinguished road
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.
__________________
www.idacireland.com
adunne304 is offline   Reply With Quote

Old   July 25, 2013, 13:52
Default
  #7
Member
 
Sandeep
Join Date: Oct 2012
Location: India
Posts: 51
Rep Power: 4
sandy_1982 is on a distinguished road
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
sandy_1982 is offline   Reply With Quote

Old   July 26, 2013, 06:35
Default
  #8
New Member
 
Adrian
Join Date: Jul 2013
Location: Dublin
Posts: 21
Rep Power: 5
adunne304 is on a distinguished road
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.
__________________
www.idacireland.com
adunne304 is offline   Reply With Quote

Old   July 27, 2013, 13:58
Default
  #9
Member
 
Sandeep
Join Date: Oct 2012
Location: India
Posts: 51
Rep Power: 4
sandy_1982 is on a distinguished road
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.
sandy_1982 is offline   Reply With Quote

Old   July 29, 2013, 02:27
Default
  #10
Senior Member
 
Paritosh Vasava
Join Date: Oct 2012
Location: Lappeenranta, Finland
Posts: 545
Rep Power: 12
vasava will become famous soon enough
Have you tried playing with 'Advanced Size Function'? It might help if your model has too many curved faces.
vasava is offline   Reply With Quote

Old   August 24, 2014, 00:04
Smile
  #11
rgd
New Member
 
Join Date: Dec 2012
Posts: 23
Rep Power: 4
rgd is on a distinguished road
Quote:
Originally Posted by sandy_1982 View Post
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.
rgd is offline   Reply With Quote

Old   September 9, 2014, 09:30
Default
  #12
Member
 
Sandeep
Join Date: Oct 2012
Location: India
Posts: 51
Rep Power: 4
sandy_1982 is on a distinguished road
@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
sandy_1982 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
failed 1 mesh checks (gmsh) appa Open Source Meshers: Gmsh, Netgen, CGNS, ... 2 July 30, 2015 17:09
[ICEM] Problem making structured mesh on a surface froztbear ANSYS Meshing & Geometry 4 November 10, 2011 09:52
StarToFoam error Kart OpenFOAM Meshing & Mesh Conversion 1 February 4, 2010 05:38
fluent add additional zones for the mesh file SSL FLUENT 2 January 26, 2008 12:55
Icemcfd 11: Loss of mesh from surface mesh option? Joe CFX 2 March 26, 2007 18:10


All times are GMT -4. The time now is 19:48.