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

Converting a 2Dmesh to axisymmetric

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

Like Tree8Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   February 23, 2009, 12:18
Default Hi everyone, i think i've n
  #41
Member
 
Etienne Lorriaux
Join Date: Mar 2009
Location: Compiegne, France
Posts: 43
Rep Power: 8
elorriaux is on a distinguished road
Hi everyone,

i think i've noticed an error in makeAxialMesh. Comparing a wedge realized with gmsh and another with makeAxialMesh, i've noticed that the wedge angle is 2.5, not 5.

Checking the code, i can see a scalar variable "angle" set to 2.5 in order to revolve -2.5 and +2.5, but i also see a 0.5 factor in the "factor" variable.

I think that the factor should be set to 1.0 or the angle to 5, am I wrong ?

Sincerely,

Etienne.
elorriaux is offline   Reply With Quote

Old   February 24, 2009, 09:03
Default Hi! Etienne convinced me on
  #42
Assistant Moderator
 
Bernhard Gschaider
Join Date: Mar 2009
Posts: 3,915
Rep Power: 40
gschaider will become famous soon enoughgschaider will become famous soon enough
Hi!

Etienne convinced me on the IRC that he is right (and I am wrong). The mistake is now corrected in the 1.4.1-version on the SVN. In the 1.5 version it was already corrected

Bernhard
__________________
Note: I don't use "Friend"-feature on this forum out of principle. Ah. And by the way: I'm not on Facebook either. So don't be offended if I don't accept your invitation/friend request
gschaider is offline   Reply With Quote

Old   February 24, 2009, 14:25
Default Hi everyone ! I've found an
  #43
Member
 
Etienne Lorriaux
Join Date: Mar 2009
Location: Compiegne, France
Posts: 43
Rep Power: 8
elorriaux is on a distinguished road
Hi everyone !

I've found another problem in makeAxialMesh ;) (sorry Bernhard to bother you ;)). This one is present in the 2 versions. But I think we have to discuss if we correct it or not.

In fact, makeAxialMesh does not revolve the mesh, it projects the mesh on wedge planes. I agree that the error is really small (depending on the radius of the problem), but it caused me great problems for coincidence with another mesh.

I've added 2 lines and modified one to solve the problem in 1.4.1, the same modif can be applied in the 1.5 version.

The question is : "should we consider this point as a modelization problem ?"

Regards, Etienne.
elorriaux is offline   Reply With Quote

Old   March 2, 2009, 15:33
Default Hello, I've modified the co
  #44
Member
 
Etienne Lorriaux
Join Date: Mar 2009
Location: Compiegne, France
Posts: 43
Rep Power: 8
elorriaux is on a distinguished road
Hello,

I've modified the code and added a revolve option. This change should be transparent for users who don't want this feature. The 2 versions 1.4.1 and 1.5 have been updated.

To activate it, add '-revolve' to the command line or change it in the dictionary if you use the rotationDict.

Check the output when running makeAxialMesh, you'll see 'Revolving nodes' or 'Projecting nodes'

Etienne.
elorriaux is offline   Reply With Quote

Old   March 13, 2009, 07:24
Default Just tried to compile makeAxia
  #45
egp
Senior Member
 
egp's Avatar
 
Eric Paterson
Join Date: Mar 2009
Location: Blacksburg, VA
Posts: 197
Blog Entries: 1
Rep Power: 9
egp is on a distinguished road
Just tried to compile makeAxialMesh on 1.5-dev. It is looking for repatchPolyTopoChanger.H, which was removed in 1.5-dev (I can't find it in src/dynamicMesh). Given that makeAxialMesh is distributed through the OpenFOAM-extend repository, I figured it would have been tested and fixed for the -dev versions. Anyone have a solution?

Eric
egp is offline   Reply With Quote

Old   March 13, 2009, 07:46
Default Hello Eric, you're right, m
  #46
Member
 
Etienne Lorriaux
Join Date: Mar 2009
Location: Compiegne, France
Posts: 43
Rep Power: 8
elorriaux is on a distinguished road
Hello Eric,

you're right, makeAxialMesh does not compile with 1.5-dev because of slight divergences between the official release and the svn release.

I've searched quickly but I've not found a way to solve this problem easily.

Sincerely, Etienne.
elorriaux is offline   Reply With Quote

Old   March 16, 2009, 08:29
Default
  #47
Assistant Moderator
 
Bernhard Gschaider
Join Date: Mar 2009
Posts: 3,915
Rep Power: 40
gschaider will become famous soon enoughgschaider will become famous soon enough
Quote:
Originally Posted by egp View Post
Just tried to compile makeAxialMesh on 1.5-dev. It is looking for repatchPolyTopoChanger.H, which was removed in 1.5-dev (I can't find it in src/dynamicMesh). Given that makeAxialMesh is distributed through the OpenFOAM-extend repository, I figured it would have been tested and fixed for the -dev versions. Anyone have a solution?

Eric
The part of the extend outside of the dev-tree tries to be "version-agnostic". I havn't used makeAxialMesh for a long time and never with the dev. I'll have a look what a few #ifdefs can do to fix this

Bernhard
gschaider is offline   Reply With Quote

Old   April 29, 2009, 00:28
Default makeAxialMake and collapseEdges
  #48
New Member
 
Peter Johnston
Join Date: Mar 2009
Location: Brisbane, Queensland, Australia
Posts: 23
Rep Power: 8
prjohnston is on a distinguished road
Dear Bernhard,

I was able to download and compile the version of makeAxialMesh for OpenFOAM v1.5. It seems to run OK, but I am having trouble running the test case axialCavity. I think the problem is that I am unsure how to use the routines.

Firstly, I run blockMesh, then I run the command

makeAxialMesh -axis fixedWalls -wedge frontAndBack

This seems to give no errors, but writes the mesh to time 0.00125 (why?). In the same directory I run the command

collapseEdges 0.0001 175

(small length and large angle as suggested in the wiki) no small edges are collapsed, but this is looking in the time=0 directory. The new mesh is in the time=0.00125 directory. However, when I force collapseEdges to look at the time=0.00125 directory, I get 21 collapsed small edges, the results of which are written in the time=0.0025 directory (again why?).

Is the idea to copy the keep copying the files generated by makeAxialMesh and collapseEdges back into constant/polyMesh?

Thanks,

Peter
prjohnston is offline   Reply With Quote

Old   April 29, 2009, 14:00
Default
  #49
Assistant Moderator
 
Bernhard Gschaider
Join Date: Mar 2009
Posts: 3,915
Rep Power: 40
gschaider will become famous soon enoughgschaider will become famous soon enough
Quote:
Originally Posted by prjohnston View Post
Dear Bernhard,

I was able to download and compile the version of makeAxialMesh for OpenFOAM v1.5. It seems to run OK, but I am having trouble running the test case axialCavity. I think the problem is that I am unsure how to use the routines.

Firstly, I run blockMesh, then I run the command

makeAxialMesh -axis fixedWalls -wedge frontAndBack

This seems to give no errors, but writes the mesh to time 0.00125 (why?).
@why: this is a convention enforced by most mesh-utilities to protect you from accidentally overwriting the mesh in constant/polyMesh. Just set in the controlDict the startFrom to latestTime, do your things and in the end copy the mesh from the latest time-step to constant (and remove all other meshes). In other words: think of it as an undo-function for mesh-manipulation.

If you can do without undo: most mesh utilities have an option -overwrite ....

Quote:
Originally Posted by prjohnston View Post
In the same directory I run the command

collapseEdges 0.0001 175

(small length and large angle as suggested in the wiki) no small edges are collapsed, but this is looking in the time=0 directory. The new mesh is in the time=0.00125 directory. However, when I force collapseEdges to look at the time=0.00125 directory, I get 21 collapsed small edges, the results of which are written in the time=0.0025 directory (again why?).

Is the idea to copy the keep copying the files generated by makeAxialMesh and collapseEdges back into constant/polyMesh?
Yep. See above

Bernhard
gschaider is offline   Reply With Quote

Old   May 15, 2009, 14:15
Default
  #50
Member
 
Mihir
Join Date: Mar 2009
Posts: 40
Rep Power: 8
mihir1310 is on a distinguished road
Quote:
Originally Posted by egp View Post
Just tried to compile makeAxialMesh on 1.5-dev. It is looking for repatchPolyTopoChanger.H, which was removed in 1.5-dev (I can't find it in src/dynamicMesh). Given that makeAxialMesh is distributed through the OpenFOAM-extend repository, I figured it would have been tested and fixed for the -dev versions. Anyone have a solution?

Eric
Quote:
Originally Posted by elorriaux View Post
Hello Eric,

you're right, makeAxialMesh does not compile with 1.5-dev because of slight divergences between the official release and the svn release.

I've searched quickly but I've not found a way to solve this problem easily.

Sincerely, Etienne.
Quote:
Originally Posted by prjohnston View Post
Dear Bernhard,

I was able to download and compile the version of makeAxialMesh for OpenFOAM v1.5. It seems to run OK, but I am having trouble running the test case axialCavity. I think the problem is that I am unsure how to use the routines.


Thanks,

Peter
Hey , how did you compile makeaxialmesh in 1.5 ??? I encountered the same problem as Eric & Etienne . Did you find a way out ??
mihir1310 is offline   Reply With Quote

Old   May 17, 2009, 22:00
Default
  #51
New Member
 
Peter Johnston
Join Date: Mar 2009
Location: Brisbane, Queensland, Australia
Posts: 23
Rep Power: 8
prjohnston is on a distinguished road
I simply used the standard v1.5 and not v1.5-dev. I did not need to do anything special. However, I guess that is not much use to you. Sorry.

Regards,

Peter.
prjohnston is offline   Reply With Quote

Old   May 19, 2009, 17:52
Default
  #52
Assistant Moderator
 
Bernhard Gschaider
Join Date: Mar 2009
Posts: 3,915
Rep Power: 40
gschaider will become famous soon enoughgschaider will become famous soon enough
Quote:
Originally Posted by mihir1310 View Post
Hey , how did you compile makeaxialmesh in 1.5 ??? I encountered the same problem as Eric & Etienne . Did you find a way out ??
Which version of the sources are you using. I tried the last one from the SVN and successfully compiled them with 1.5.x and 1.5-dev (the dev has to be younger than approx 2 mths)

Bernhard
gschaider is offline   Reply With Quote

Old   May 20, 2009, 13:52
Default
  #53
Member
 
Mihir
Join Date: Mar 2009
Posts: 40
Rep Power: 8
mihir1310 is on a distinguished road
[/QUOTE]

Quote:
Originally Posted by gschaider View Post
Which version of the sources are you using. I tried the last one from the SVN and successfully compiled them with 1.5.x and 1.5-dev (the dev has to be younger than approx 2 mths)

Bernhard

All right , i i used the latest from the SVN . It compiled successfullyy . But what is the command . If the use the command: makeAxialMesh . . axis frontAndBackPlanes as in 1.4 , it doesnt not work .. What are the arguments that have to be specified ?

Last edited by mihir1310; May 20, 2009 at 15:17.
mihir1310 is offline   Reply With Quote

Old   May 20, 2009, 16:10
Default
  #54
Member
 
David P. Schmidt
Join Date: Mar 2009
Posts: 70
Rep Power: 8
schmidt_d is on a distinguished road
Mihir,

Take a look in cd $WM_PROJECT_USER_DIR/applications/MakeAxialMesh for the TestCases directory. Look at how the parameters are now passed to makeAxialMesh through the rotation dictionary:
system/rotationDict
schmidt_d is offline   Reply With Quote

Old   August 30, 2009, 13:33
Default
  #55
New Member
 
Emanuele Leoni
Join Date: Apr 2009
Posts: 13
Rep Power: 8
lions85 is on a distinguished road
Hi,
I hope this is the right post.
I'm trying to use makeaxialmesh but I found some difficulties.
I have this 2d mesh (1 cell thick) converted from a 2d fluent mesh using fluentofoam, with the axis edge named axis and the opposite edge (the one that has to be splitted in two edges) named wall.
In the terminal I went into the folder of the case and I gave this command:
makeAxialMesh axis wall
and I get this error:
Create time

Create mesh for time = 0

#0 Foam::error:rintStack(Foam::Ostream&) in "/home/lions85/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libOpenFOAM.so"
#1 Foam::sigSegv::sigSegvHandler(int) in "/home/lions85/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libOpenFOAM.so"
#2 ?? in "/lib/libc.so.6"
#3 std::basic_string<char, std::char_traits<char>, std::allocator<char> >::basic_string(std::string const&) in "/home/lions85/OpenFOAM/ThirdParty/gcc-4.3.1/platforms/linux64/lib64/libstdc++.so.6"
#4 main in "/home/lions85/OpenFOAM/lions85-1.5/applications/bin/linux64GccDPOpt/makeAxialMesh"
#5 __libc_start_main in "/lib/libc.so.6"
#6 _start in "/home/lions85/OpenFOAM/lions85-1.5/applications/bin/linux64GccDPOpt/makeAxialMesh"
Segmentation fault


Probably I'm making a mistake, but I can not find it simply.
Is someone able to help me?
Thank you very much
EManuele
lions85 is offline   Reply With Quote

Old   August 30, 2009, 13:47
Default
  #56
Member
 
Mihir
Join Date: Mar 2009
Posts: 40
Rep Power: 8
mihir1310 is on a distinguished road
Quote:
Originally Posted by lions85 View Post
Hi,
I hope this is the right post.
I'm trying to use makeaxialmesh but I found some difficulties.
I have this 2d mesh (1 cell thick) converted from a 2d fluent mesh using fluentofoam, with the axis edge named axis and the opposite edge (the one that has to be splitted in two edges) named wall.
In the terminal I went into the folder of the case and I gave this command:
makeAxialMesh axis wall
and I get this error:



Probably I'm making a mistake, but I can not find it simply.
Is someone able to help me?
Thank you very much
EManuele
Well Id name it frontAndBackPlanes

makeAxialMesh axis frontAndBackPlanes
mihir1310 is offline   Reply With Quote

Old   August 30, 2009, 15:30
Default
  #57
New Member
 
Emanuele Leoni
Join Date: Apr 2009
Posts: 13
Rep Power: 8
lions85 is on a distinguished road
Sorry,
may you explain it better?? I didn't understand very well.
Anyway i tried with the command

makeAxialMesh axis frontAndBackPlanes

and i got

Create time

Create mesh for time = 0

#0 Foam::error:rintStack(Foam::Ostream&) in "/home/lions85/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libOpenFOAM.so"
#1 Foam::sigSegv::sigSegvHandler(int) in "/home/lions85/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libOpenFOAM.so"
#2 ?? in "/lib/libc.so.6"
#3 std::basic_string<char, std::char_traits<char>, std::allocator<char> >::basic_string(std::string const&) in "/home/lions85/OpenFOAM/ThirdParty/gcc-4.3.1/platforms/linux64/lib64/libstdc++.so.6"
#4 main in "/home/lions85/OpenFOAM/lions85-1.5/applications/bin/linux64GccDPOpt/makeAxialMesh"
#5 __libc_start_main in "/lib/libc.so.6"
#6 _start in "/home/lions85/OpenFOAM/lions85-1.5/applications/bin/linux64GccDPOpt/makeAxialMesh"
Segmentation fault

Thank you
Emanuele

P.S. consider that i have my boundary edges that I created with gambit and then I have two other boundaries created during the conversion from fluent to foam and one of this is named automatically FrontAndBackPlanes
lions85 is offline   Reply With Quote

Old   August 30, 2009, 16:16
Default
  #58
Member
 
Mihir
Join Date: Mar 2009
Posts: 40
Rep Power: 8
mihir1310 is on a distinguished road
Quote:
Originally Posted by lions85 View Post
Sorry,
may you explain it better?? I didn't understand very well.
Anyway i tried with the command

makeAxialMesh axis frontAndBackPlanes

and i got

Create time

Create mesh for time = 0

#0 Foam::error:rintStack(Foam::Ostream&) in "/home/lions85/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libOpenFOAM.so"
#1 Foam::sigSegv::sigSegvHandler(int) in "/home/lions85/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libOpenFOAM.so"
#2 ?? in "/lib/libc.so.6"
#3 std::basic_string<char, std::char_traits<char>, std::allocator<char> >::basic_string(std::string const&) in "/home/lions85/OpenFOAM/ThirdParty/gcc-4.3.1/platforms/linux64/lib64/libstdc++.so.6"
#4 main in "/home/lions85/OpenFOAM/lions85-1.5/applications/bin/linux64GccDPOpt/makeAxialMesh"
#5 __libc_start_main in "/lib/libc.so.6"
#6 _start in "/home/lions85/OpenFOAM/lions85-1.5/applications/bin/linux64GccDPOpt/makeAxialMesh"
Segmentation fault

Thank you
Emanuele

P.S. consider that i have my boundary edges that I created with gambit and then I have two other boundaries created during the conversion from fluent to foam and one of this is named automatically FrontAndBackPlanes
this is a 'segmentation violation (sigSegv)' problem caused by faulty memory allocation problem . I dont know how to deal with it compleely , but you can read this for more info http://openfoamwiki.net/index.php/HowTo_debugging
mihir1310 is offline   Reply With Quote

Old   August 31, 2009, 13:32
Default
  #59
Assistant Moderator
 
Bernhard Gschaider
Join Date: Mar 2009
Posts: 3,915
Rep Power: 40
gschaider will become famous soon enoughgschaider will become famous soon enough
Quote:
Originally Posted by mihir1310 View Post
this is a 'segmentation violation (sigSegv)' problem caused by faulty memory allocation problem . I dont know how to deal with it compleely , but you can read this for more info http://openfoamwiki.net/index.php/HowTo_debugging
I don't remember exactly where, but I've seen that error somewhere. The strange thing is that your stack-trace indicates the string-classes. Have you got an entry libs and or functionObjects in you controlDict. If yes: disable it. (But there's only a 20% chance that this is the problem)

The other thing: is there any other application that you successfully compiled before? Is your version of OF a downloaded binary or self-compiled? Because I remotely remember having seen a similar stack-trace in a previous discussion and it was a compilation problem or something like that

Bernhard
gschaider is offline   Reply With Quote

Old   October 27, 2009, 12:45
Default
  #60
Member
 
Hai Yu
Join Date: Mar 2009
Location: OvgU, Magdeburg
Posts: 65
Rep Power: 8
yuhai is on a distinguished road
Hi, dear all,
I tried to revolve (select withMesh option)my face in Gambit, and I can only get a volumn, but the mesh is not created in the volumn.
Does anybody know the answer?


sorry, I am away from the topic.
yuhai 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
Converting RANS solver into LES Chiara Main CFD Forum 5 February 19, 2009 10:36
converting user-coding in V4 Karl Mehler CD-adapco 0 September 28, 2008 15:48
Converting objects shuo OpenFOAM 1 November 6, 2006 17:51
Converting 2D mesh to 3D Farooq FLUENT 1 August 7, 2003 05:03
Converting from tecplot to gmv format Charles Crosby Main CFD Forum 0 May 7, 2003 15:02


All times are GMT -4. The time now is 12:53.