CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ...

Converting meshes that includes interfaces

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

Reply
 
LinkBack Thread Tools Display Modes
Old   June 8, 2006, 05:29
Default When I try to read this file,
  #21
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,763
Rep Power: 21
hjasak will become famous soon enough
When I try to read this file, Fluent says: Error: Cannot change interface1 to interior because there is only one adjacent cell thread.

Your mesh is broken.

Hrv
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   June 8, 2006, 05:32
Default ... but Uncle Hrv has fixed it
  #22
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,763
Rep Power: 21
hjasak will become famous soon enough
... but Uncle Hrv has fixed it for you (at least I think so). You will get an E-mail soon,

Hrv
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   June 8, 2006, 07:13
Default Thanks. Did not know you co
  #23
ham
Member
 
Marcus Hammar
Join Date: Mar 2009
Posts: 33
Rep Power: 8
ham is on a distinguished road
Thanks.

Did not know you could convert .cas files.

What did you do?
Did you do anything in gambit?

I thought I had to run splitMesh after the mesh was converted, but I cant find a faceSetDict anywhere?
If a splitMesh is not necessary, what should i use as boundary conditions on the "interface1" and "interface2"?
I thougt interior, but?

Thanx again...
/M
ham is offline   Reply With Quote

Old   June 8, 2006, 09:19
Default Read it into Fluent, dealt wit
  #24
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,763
Rep Power: 21
hjasak will become famous soon enough
Read it into Fluent, dealt with the error there and wrote out the case file - this one converted fine.

Hrv
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   June 8, 2006, 09:32
Default Oh, nice. So what about spl
  #25
ham
Member
 
Marcus Hammar
Join Date: Mar 2009
Posts: 33
Rep Power: 8
ham is on a distinguished road
Oh, nice.

So what about splitMesh then? unnecessary?
faceSetDict?

ham
ham is offline   Reply With Quote

Old   June 12, 2006, 02:43
Default Hi again. A few questions:
  #26
ham
Member
 
Marcus Hammar
Join Date: Mar 2009
Posts: 33
Rep Power: 8
ham is on a distinguished road
Hi again.
A few questions:

How did you "deal with the error"?

In OpenFAOM, what bc:s should I choose for the interior boundary? "Interior" does not exist.

Thank you

/marcus
ham is offline   Reply With Quote

Old   January 5, 2007, 08:26
Default Marcus, Any luck with your e
  #27
Member
 
Radu Mustata
Join Date: Mar 2009
Location: Zaragoza, Spain
Posts: 96
Rep Power: 8
r2d2 is on a distinguished road
Marcus,
Any luck with your enquiry? I have the same sort of problem.(interface with non-conforming mesh either side of it, .msh file) fluentMeshToFoam will create an "internal boundary" and write it down in the boundary file. How can I get rid of it...cause I gather that one does not have to specify bcs on that...
Cheers,
Radu
r2d2 is offline   Reply With Quote

Old   January 8, 2007, 07:42
Default Hello again, I went a bit fu
  #28
Member
 
Radu Mustata
Join Date: Mar 2009
Location: Zaragoza, Spain
Posts: 96
Rep Power: 8
r2d2 is on a distinguished road
Hello again,
I went a bit further with the topic but I got stuck again. I will try to summarize what Ive done and I would appreciate any suggestion from you guys.
The case is a simple 2-D mesh, elbow like. I generated the mesh with Gambit, and I have defined two interfaces (interface1 & 2) having "non-conforming" hex meshes either side.
I ran fluentMeshToFoam, and this produced a "default Faces" in the boundary file and a couple of faceSets representing those two interfaces (after renaming them as internal in the .msh Gambit file).
Then I use the "createPatch" utility to create patches for these interfaces. createPatchDict reads:
patches
(

{
name interf2;
type patch;

constructFrom set;

set interface2;
}

{
name interf1;
type patch;

constructFrom set;

set interface1;
}
So now I have two new patches in the newly created boundary instead of those "defaultFaces" .
The next step I thought the reasonable was to use "stitchMesh" and there is where I got stuck. Although everything seems to be fine after createPatch (in paraFoam that is), as in the patches face eacho other and have the same area, the message of stitchMesh (with some debug flags on in controlDict) reads:

Exec : stitchMesh . pitzDaily interf2 interf1
Date : Jan 08 2007
Time : 11:46:47
Host : marte
PID : 14270
Root : /home/radu/OpenFOAM/radu-1.3/run/oodles
Case : pitzDaily
Nprocs : 1
Create time

Create mesh for time = 0

void polyMesh::initMesh() : calculating faceCells
Coupling patches interf2 and interf1
Resulting (internal) faces will be in faceZone interf2interf1CutFaceZone

Note: the overall area covered by both patches should be identical ("integral" interface).
If this is not the case use the -partial option

Adding point and face zones
Sliding interface object couple :
master face zone: 0
slave face zone: 1
void Foam::slidingInterface::calcAttachedAddressing() const for object couple : Calculating zone face-cell addressing.
void Foam::slidingInterface::calcAttachedAddressing() const for object couple : Finished calculating zone face-cell addressing.
Reading all current volfields
bool slidingInterface::projectPoints() : for object couple : Projecting slave points onto master surface.
Number of hits in point projection: 10 out of 10 points.
bool slidingInterface::projectPoints() for object couple : Adjusting point projection for integral match: done.
Number of adjusted points in projection: 0
... projection OK.
... point merge OK.
Number of merged master points: 10
Number of adjusted slave points: 0
Processing slave edges
.+ .+ .+ ....+ mmmm.....+ mmmm+ .....+ mmmm.....+ mmmm.....+ mmmm.....+ mmmm+ ....+ mmmm.....+ mmmm
bool slidingInterface::projectPoints() for object couple : Finished projecting points. Topology = (Detached interface) changing.
void slidingInterface::coupleInterface(polyTopoChange& ref) : Coupling sliding interface couple

Processing slave edges
.+ n-n-uuuun-n-n-n-n-un-n-n-n-
.+ uun-n-n-n-n-n-un-n-n-n-n-uu
.+ n-n-un-n-n-n-n-uuuun-n-n-n-
....+ n-un-un-n-uun-uuun-uuuun-u
.....+ n-n-n-n-n-n-n-uuuuun-n-n-n-n-n-n-n-n-n-n-n-un-un-un-un-un-uun-
+ un-n-n-un-u
.....+ n-uuuuuun-n-n-n-n-un-un-un-un-un-un-un-n-n-n-n-n-n-n-n-
.....+ n-n-n-n-n-n-n-uuuuuun-n-n-n-n-n-n-n-n-n-n-n-n-un-un-un-un-un-un-un-
.....+ n-uuuuuun-n-n-n-n-n-n-n-un-un-un-un-un-un-un-n-n-n-n-n-n-n-n-n-n-n-
.....+ n-n-n-n-uuuuuun-n-n-n-n-n-n-n-n-n-un-un-un-un-un-un-un-
+ un-n-un-n-u
....+ uuuuun-uun-un-un-un-un-un-
.....+ uuuuun-n-n-n-n-n-n-n-uun-un-un-un-un-un-n-n-n-n-n-n-n-n-n-n-n-
Enriched patch support OK. Slave faces: 4 Master faces: 20
local: 4(0 2 26 24) one side: 0 other side: 19
local: 4(2 3 27 26) one side: 0 other side: 18
local: 4(3 4 28 27) one side: 0 other side: 17
local: 4(4 5 29 28) one side: 0 other side: 16
local: 4(5 6 30 29) one side: 0 other side: 15
Finished face 0
local: 4(6 7 31 30) one side: 1 other side: 14
local: 4(7 8 32 31) one side: 1 other side: 13
local: 4(8 9 33 32) one side: 1 other side: 12
local: 4(9 10 34 33) one side: 1 other side: 11
local: 4(10 11 35 34) one side: 1 other side: 10
Finished face 1
local: 4(11 12 36 35) one side: 2 other side: 9
local: 4(12 13 37 36) one side: 2 other side: 8
local: 4(13 14 38 37) one side: 2 other side: 7
local: 4(14 15 39 38) one side: 2 other side: 6
local: 4(15 16 40 39) one side: 2 other side: 5
Finished face 2
local: 4(1 25 44 20) one side: 3 other side: 0
local: 4(44 43 19 20) one side: 3 other side: 1
local: 4(43 42 18 19) one side: 3 other side: 2
local: 4(42 41 17 18) one side: 3 other side: 3
local: 4(41 40 16 17) one side: 3 other side: 4
Finished face 3
Finished face 4
Finished face 5
Finished face 6
Finished face 7
Finished face 8
Finished face 9
Finished face 10
Finished face 11
Finished face 12
Finished face 13
Finished face 14
Finished face 15
Finished face 16
Finished face 17
Finished face 18
Finished face 19
Finished face 20
Finished face 21
Finished face 22
Finished face 23
Number of orphaned faces: master = 0 out of 20 slave = 4 out of 4


--> FOAM FATAL ERROR : Face 3327 reduced to less than 3 points. Topological/cutting error B.
Old face: 2(0 884) new face: 2(0 884)

From function void slidingInterface::coupleInterface(polyTopoChange& ref) const
in file slidingInterface/coupleSlidingInterface.C at line 1664.

FOAM aborting

Foam::error::printStack(Foam:stream&)
Foam::error::abort()
Foam::slidingInterface::coupleInterface(Foam::poly TopoChange&) const
Foam::slidingInterface::setRefinement(Foam::polyTo poChange&) const
Foam::polyTopoChanger::topoChangeRequest() const
Foam::polyTopoChanger::changeMesh()
stitchMesh [0x805524f]
__libc_start_main
__gxx_personality_v0
Aborted

Can anyone help.
Thanx in advance,
Radu
r2d2 is offline   Reply With Quote

Old   January 8, 2007, 09:04
Default I know this one: check the two
  #29
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,763
Rep Power: 21
hjasak will become famous soon enough
I know this one: check the two bits of the mesh and you will find they share vertices. This is not allowed: the two pieces should be TOPOLOGICALLY separate.

Not sure how to fix it in Gambit - in short, you have to make sure that the master and slave surface do not use the same vertices.

Hrv
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   January 8, 2007, 09:58
Default Yes, yes...I thought so as wel
  #30
Member
 
Radu Mustata
Join Date: Mar 2009
Location: Zaragoza, Spain
Posts: 96
Rep Power: 8
r2d2 is on a distinguished road
Yes, yes...I thought so as well. That is when I
compared to what Ive done before with blockMesh, those patches being built from double nodes...so as you say, topologically separate. Im not a gambit specialist, I only thought of it as a front end to OF. Now, although I dont like it, it seems I should be paying more atention to Gambit.
Cheers anyway,
Radu
r2d2 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
Several problems with the mesh conversion utility when converting the meshes from Gridgen su_junwei OpenFOAM Meshing & Mesh Conversion 2 July 26, 2008 23:58
meshes interfaces 2 ? amine CFX 0 March 7, 2008 14:59
Converting Gambit Neutral Meshes plmauk OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ... 2 July 20, 2007 07:08
Converting Gambit Neutral Meshes gschaider OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ... 1 May 12, 2005 12:13


All times are GMT -4. The time now is 11:27.