Help needed: Calculation Error, "SPACER"
- Tom Krivec
- Topic Author
- Offline
- New Member
-
Less
More
- Posts: 12
- Thank you received: 0
17 years 2 weeks ago #1913
by Tom Krivec
Help needed: Calculation Error, "SPACER" was created by Tom Krivec
Hi,
at calculation of a spacer part with some load applied as pressure with SALOME-MECA stand alone package (SALOME 3.2.6, CODE ASTER 9.1) I get the following error message. Any help out there ??? The *hdf, *com, etc. files are attached. Thanks in advance!
<F> <FACTOR_20> !
! !
! !
! -> Matrice non factorisable : !
! Le pivot est presque nul à la ligne 2087 pour le noeud NJB et !
! la composante DX. !
! Pour information, le nombre de décimales perdues est de 15. !
! !
! -> Conseil & Risque : !
! Il s'agit peut etre d'un mouvement de corps rigide mal bloqué. !
! Vérifiez les conditions aux limites. !
! Si vous faites du contact, il ne faut pas que la !
! structure ne "tienne" que par le contact. !
! !
! !
! !
! Cette erreur est fatale. Le code s'arrete.
at calculation of a spacer part with some load applied as pressure with SALOME-MECA stand alone package (SALOME 3.2.6, CODE ASTER 9.1) I get the following error message. Any help out there ??? The *hdf, *com, etc. files are attached. Thanks in advance!
<F> <FACTOR_20> !
! !
! !
! -> Matrice non factorisable : !
! Le pivot est presque nul à la ligne 2087 pour le noeud NJB et !
! la composante DX. !
! Pour information, le nombre de décimales perdues est de 15. !
! !
! -> Conseil & Risque : !
! Il s'agit peut etre d'un mouvement de corps rigide mal bloqué. !
! Vérifiez les conditions aux limites. !
! Si vous faites du contact, il ne faut pas que la !
! structure ne "tienne" que par le contact. !
! !
! !
! !
! Cette erreur est fatale. Le code s'arrete.
- Tom Krivec
- Topic Author
- Offline
- New Member
-
Less
More
- Posts: 12
- Thank you received: 0
17 years 2 weeks ago #1914
by Tom Krivec
Replied by Tom Krivec on topic Re:Help needed: Calculation Error, "SPACER"
Hi again,
attached there are the message *.txt files and the *comm file.
I understand that there is a problem with the matrix, but do not know how to solve it...
bye, Tom
attached there are the message *.txt files and the *comm file.
I understand that there is a problem with the matrix, but do not know how to solve it...
bye, Tom
Attachment ab_v3_cut.gz not found
- Claus
-
- Offline
- Moderator
-
Less
More
- Posts: 670
- Thank you received: 34
17 years 2 weeks ago #1915
by Claus
Code_Aster release : STA11.4 on OpenSUSE 12.3 64 bits - EDF/Intel version
Replied by Claus on topic Re:Help needed: Calculation Error, "SPACER"
If you'll allow me to take a wild guess: did you make sure you 'secured' your holding point to all axes i.e dx/dy/dz - the error indicates that theres a pivot-point around dx at *something* 2087 - go back and make sure you've set dx/dy/dz to 0 - again, my French is almost nonexistent so I'm probably wrong 
Code_Aster release : STA11.4 on OpenSUSE 12.3 64 bits - EDF/Intel version
- Joël Cugnoni
-
- Offline
- Moderator
-
17 years 2 weeks ago #1917
by Joël Cugnoni
Joël Cugnoni - a.k.a admin
www.caelinux.com
Replied by Joël Cugnoni on topic Re:Help needed: Calculation Error, "SPACER"
You are right: this message means that the stiffness matrix cannot be factorized due to a zero pivot (=singular matrix).
In other terms, there is a "rigid body" motion in your model. The message also says that it is along the X direction (DOF = DX).
As Claus advised, check your boundary conditions: in 3D you should block all the six rigid body motions (3 translations and 3 rotations).
In other terms, there is a "rigid body" motion in your model. The message also says that it is along the X direction (DOF = DX).
As Claus advised, check your boundary conditions: in 3D you should block all the six rigid body motions (3 translations and 3 rotations).
Joël Cugnoni - a.k.a admin
www.caelinux.com
- Tom Krivec
- Topic Author
- Offline
- New Member
-
Less
More
- Posts: 12
- Thank you received: 0
17 years 2 weeks ago #1919
by Tom Krivec
Replied by Tom Krivec on topic Re:Help needed: Calculation Error, "SPACER"
Thanks for your replies,
when creating the calculation case with the wizzard, the dedicated support surface (or alternatively one single node) is fixed in dx,dy,dz. In addition a small surface is loaded with the "pres" operator. This leads to the described error message.
When the *.comm file is edited manually and at affe_char_meca -> ddl_impo additionally all rotations drx, dry, drz are locked the result is the following:
"aucun noeud ne connait le ddl: DRX"
which means as far as I (and Google translator) understand that a drx DOF is not known for the specified node ...
Meanwhile I alternatively also tried to mesh the geometry not with the SALOME meshing tool but with Gmsh (*.unv mesh format). Then I imported the mesh into SALOME MECA, created an ASTER case and started the calculation ... unfortunately with the same result.
CU Tom
when creating the calculation case with the wizzard, the dedicated support surface (or alternatively one single node) is fixed in dx,dy,dz. In addition a small surface is loaded with the "pres" operator. This leads to the described error message.
When the *.comm file is edited manually and at affe_char_meca -> ddl_impo additionally all rotations drx, dry, drz are locked the result is the following:
"aucun noeud ne connait le ddl: DRX"
which means as far as I (and Google translator) understand that a drx DOF is not known for the specified node ...
Meanwhile I alternatively also tried to mesh the geometry not with the SALOME meshing tool but with Gmsh (*.unv mesh format). Then I imported the mesh into SALOME MECA, created an ASTER case and started the calculation ... unfortunately with the same result.
CU Tom
- Joël Cugnoni
-
- Offline
- Moderator
-
17 years 2 weeks ago #1922
by Joël Cugnoni
Joël Cugnoni - a.k.a admin
www.caelinux.com
Replied by Joël Cugnoni on topic Re:Help needed: Calculation Error, "SPACER"
Hello,
I have looked at the attached files:
it appear that you have only ONE node in the "fix" group and that you only impose the DX & DZ displacements to zero... This means that you will always have 6-2=4 Rigid body motions in your system.
To be sure to remove all these rigid DOF:
- you cannot use DRX,DRY,DRZ because solid FE do not have rotationnal DOFS
- you can use the simple "3-2-1" rule: on one node A, you contrain 3 translations; on another node B you constraint 2 translations and finally on the last one C you block on translation only => this makes 6 blocked DOFS => no rigid body motion & no overconstraint. You just need to choose the right DOFS to constrain all rotations:
for example if the segment AB is along X direction and AC is along Y direction, you should impose the following DOFS:
on A: DX,DY,DZ
on B: DY,DZ
on C: DZ
- or you can clamp a surface (clamping several nodes => more that 6 DOFS are blocked => hyperstatics, but this is not a problem in FE)
I hope that it will help you solve the problem.
Joël
I have looked at the attached files:
it appear that you have only ONE node in the "fix" group and that you only impose the DX & DZ displacements to zero... This means that you will always have 6-2=4 Rigid body motions in your system.
To be sure to remove all these rigid DOF:
- you cannot use DRX,DRY,DRZ because solid FE do not have rotationnal DOFS
- you can use the simple "3-2-1" rule: on one node A, you contrain 3 translations; on another node B you constraint 2 translations and finally on the last one C you block on translation only => this makes 6 blocked DOFS => no rigid body motion & no overconstraint. You just need to choose the right DOFS to constrain all rotations:
for example if the segment AB is along X direction and AC is along Y direction, you should impose the following DOFS:
on A: DX,DY,DZ
on B: DY,DZ
on C: DZ
- or you can clamp a surface (clamping several nodes => more that 6 DOFS are blocked => hyperstatics, but this is not a problem in FE)
I hope that it will help you solve the problem.
Joël
Joël Cugnoni - a.k.a admin
www.caelinux.com
Moderators: catux
Time to create page: 0.139 seconds