Advice needed on <EXCEPTION> <DVP_1> (DYNA_NON_LINE)

hkboondoggle · 2020-06-29 06:13:27

Hi all,

I am trying to simulate an impact scenario with a ball travelling on negative z-axis direction and being about to collide on a static plate.

With the aid of konyaro, Johannes, mecour, and others (I really appreciate it guys!), I have set up the case which details can be found in the attached zip file.
It includes the .py script for geometry & mesh generation (.med too large), the .comm file and .log of the problematic Run case.

The following error happened as the Run Case was being launched:

.. __stg1_cmd9:1
# ------------------------------------------------------------------------------------------
# Commands No: 0012 Concept of the type: evol_noli
# ------------------------------------------------------------------------------------------
solver = DYNA_NON_LINE(MODELE=model1,
CHAM_MATER=fieldma0,
CONTACT=contact,
ETAT_INIT=_F(VITE=init_vel,
PRECISION=1.E-06,
CRITERE='RELATIF',),
INCREMENT=_F(LIST_INST=timeline,
PRECISION=1.E-06,),
SCHEMA_TEMPS=_F(SCHEMA='HHT',
ALPHA=-0.3,
MODI_EQUI='NON',
FORMULATION='DEPLACEMENT',
COEF_MASS_SHIFT=0.0,),
AMOR_RAYL_RIGI='TANGENTE',
METHODE='NEWTON',
NEWTON=_F(REAC_INCR=1,
MATRICE='TANGENTE',
REAC_ITER=1,
REAC_ITER_ELAS=0,
MATR_RIGI_SYME='NON',),
CONVERGENCE=_F(ITER_GLOB_MAXI=10,
ITER_GLOB_ELAS=25,
ARRET='OUI',),
SOLVEUR=_F(RENUM='AUTO',
NPREC=8,
ELIM_LAGR='LAGR2',
STOP_SINGULIER='OUI',
TYPE_RESOL='AUTO',
ACCELERATION='AUTO',
LOW_RANK_SEUIL=0.0,
PRETRAITEMENTS='AUTO',
POSTTRAITEMENTS='AUTO',
PCENT_PIVOT=20,
RESI_RELA=-1.0,
GESTION_MEMOIRE='AUTO',
FILTRAGE_MATRICE=-1.0,
MIXER_PRECISION='NON',
MATR_DISTRIBUEE='NON',
METHODE='MUMPS',),
MESURE=_F(TABLE='NON',),
ARCHIVAGE=_F(PRECISION=1.E-06,
CRITERE='RELATIF',),
INFO=1,)

Comme vous n'avez pas défini explicitement le comportement, tout le modèle est supposé élastique en petites perturbations.
Liste des comportements
Affecté sur 186954 éléments
Relation : ELAS
Déformation : PETIT
Nombre total de variables internes : 1
V1 : VIDE
Le système linéaire à résoudre a 734008 degrés de liberté:
- 734008 sont des degrés de liberté physiques
(ils sont portés
par 244274 noeuds du maillage)
- 0 sont les couples de paramètres de Lagrange associés
aux 0 relations linéaires dualisées.
La matrice est de taille 734008 équations.
Elle contient 31072249 termes non nuls si elle est symétrique et 61410490 termes non
nuls si elle n'est pas symétrique.
Soit un taux de remplissage de 0.011 %.
Lecture de l'état initial
Il n'y a pas d'état initial défini. On prend un état initial nul.
Le champ <DEPL> est initialisé a zéro
Le champ <SIEF_ELGA> est initialisé a zéro
Le champ <VARI_ELGA> est initialisé a zéro

!-----------------------------------------------------------------!
! <A> <ALGELINE7_20> !
! !
! On ne peut pas remplir la composante DX du noeud numéro N1 !
! pour le champ "&&NMETL2.CHAMP.CONV" !
! !
! !
! This is a warning. If you do not understand the meaning of this !
! warning, you can obtain unexpected results! !
!-----------------------------------------------------------------!

!----------------------------------------------------------------------------------------!
! <A> <MECANONLINE_2> !
! !
! Lors de la recopie du champ &&NMETL2.CHAMP.CONVER donné dans ETAT_INIT de la commande !
! STAT_NON_LINE vers le champ !
! &&NMCH1P.VITMOI, certaines composantes de &&NMCH1P.VITMOI !
! ont du être mises à zéro. !
! !
! Ce problème survient lorsque le champ donné !
! dans ETAT_INIT ne comporte !
! pas assez de composantes, on complète donc par des zéros. !
! !
! !
! This is a warning. If you do not understand the meaning of this !
! warning, you can obtain unexpected results! !
!----------------------------------------------------------------------------------------!

Le champ <VITE> est lu dans ETAT_INIT, par un champ donné explicitement
Le champ <ACCE> est initialisé a zéro
One considers an acceleration initial.
The initial state does not have acceleration given.
It is computed.

Filing of the initial state
Filing of the fields
Field stored DEPL at time 0.000000000000e+00 for the sequence number 0
Field stored SIEF_ELGA at time 0.000000000000e+00 for the sequence number 0
Field stored VARI_ELGA at time 0.000000000000e+00 for the sequence number 0
Field stored COMPORTEMENT at time 0.000000000000e+00 for the sequence number 0
Field stored VITE at time 0.000000000000e+00 for the sequence number 0
Field stored ACCE at time 0.000000000000e+00 for the sequence number 0
Field stored CONT_NOEU at time 0.000000000000e+00 for the sequence number 0
Il y a 0 points initialement en contact et 0 points exclus.
-----------------------------------------------------------------------------------------------------------------------------------------
Time of computation: 4.000000000000e-03
-----------------------------------------------------------------------------------------------------------------------------------------
| CONTACT | NEWTON | RESIDU | RESIDU | OPTION | CONTACT | CONTACT | CONTACT |
| BCL. GEOM. | ITERATION | RELATIF | ABSOLU | ASSEMBLAGE | NEWTON GENE | PRESSURE | CRITERE |
| ITERATION | | RESI_GLOB_RELA | RESI_GLOB_MAXI | | VARI. CONT. | ERROR | VALEUR |
-----------------------------------------------------------------------------------------------------------------------------------------
Traceback returned by pdbhelp:
[0] print_trace_
[1] utmess_core_
[2] utmess_
[3] assert_
[4] mmcaln_
[5] mmvppe_
[6] te0365_
[7] te0000_
[8] calcul_
[9] nmelcv_
[10] nmfocc_
[11] nmprta_
[12] nmpred_
[13] nmnewt_
[14] op0070_
[15] execop_
[16] expass_
[17] initaster_fonctions
[18] PyMethodDef_RawFastCallKeywords
[19] PyMethodDef_RawFastCallKeywords
[20] PyEval_EvalFrameDefault
[21] PyMethodDef_RawFastCallKeywords
[22] PyEval_EvalFrameDefault
[23] PyMethodDef_RawFastCallKeywords
[24] PyEval_EvalFrameDefault

!-----------------------------------------------------------------------------------------------!
! <EXCEPTION> <DVP_1> !
! !
! Program error. !
! !
! Condition not met: !
! ASTER_FALSE !
! File !
! /home/siavelis/PROJETS/aster/windows/build/codeaster-src/bibfor/cont_elem/mmcaln.F90, line 63 !
! !
! -------------------------------------------- !
! Contexte du message : !
! Option : CHAR_MECA_CONT !
! Type d'élément : COT6T6 !
! !
! Maillage : mesh !
! Maille : XXX !
! Type de maille : TRIA66 !
! Cette maille appartient aux groupes de mailles suivants !
! : !
! !
! Position du centre de gravité de la maille : !
! x=nan y=0.000000 z=0.000000 !
! !
! !
! !
! Il y a probablement une erreur dans la programmation. !
! Veuillez contacter votre assistance technique. !
!-----------------------------------------------------------------------------------------------!

!-----------------------------------------------------------------!
! !
! FATAL ERROR detected in Code_Aster for Windows version !
! !
! If an ABNORMAL_ABORT occured, that is not reproductible !
! on official Linux version, or if you need some help to !
! understand the message above, please report issues at: !
! !
! support@simulease.com !
! !
!-----------------------------------------------------------------!

Could you please advice in dealing this problem?
Thanks!

I have attached the mesh info below FYI:

Attachments:
Case_Files.zip, Size: 13.4 KiB, Downloads: 339

hkboondoggle · 2020-07-03 09:40:59

Thinking that the problem might be caused by the stretching of the mesh, I have replace the whole mesh set up with an uniform setting shown below:

However, the same exception still occurs.
The comm, log & med files of this latest trial are attached FYI.

Last edited by hkboondoggle (2020-07-03 09:41:48)

Attachments:
Trial_2_Study_Files.zip, Size: 1.27 MiB, Downloads: 351

konyaro · 2020-07-08 08:49:38

Hello,
your case runs fine. It requires a lot of RAM as there are many nodes and you're using a direct solver. I guess that's the source of your problem. The Windows version doesn't depict the memory error messages. You should try to increase the amount of memory or reduce the size of the mesh.

In the attached files I switched to larger linear elements and changed a few things in your comm file: GROT_GDEP, contact, reuse for CALC_CHAMP, less steps as I don't want to wait for hours. It does converge well.

Konyaro

Attachments:
ball2.zip, Size: 427.24 KiB, Downloads: 357

hkboondoggle · 2020-07-17 06:52:22

Thanks Konyaro for your inspection.

I have shorten the calculation time from 10 to 3.24 (<DVP_1> would happen at 3.26), and the calculation does converge well.
Although the result is physically incorrect again with the ball re-bounces backward after the collision, whereas the reference I'm following [1] has the ball undergoes plastic deformation and stays attached to the substrate.

The material properties and initial velocity of the ball in my code-aster simulation follow the presented data in [1] and are the normalized with respect to the density of copper, the speed of sound, the diameter of the ball, and the room temperature.

After inspection, I found that the RELATION of behavior of DYNA_NON_LINE by default is 'ELASTIC'.
Thinking that this might be the reason of the discrepancy of the calculated result, I changed it to 'VMIS_JOHN_COOK'.
Other changes included halving the time increment to 5e-3, and enabling Deformation in CLAC_CHAMP.

Now it appears to be having trouble in convergence, as time increment automatically down-sizing itself to the order of -16 once the ball impacts the substrate & 'VMIS_JOHN_COOK' kicks into action, which ultimately leads to <MECANONLINE9_3>.
The comm, log & med files of this latest trial are attached FYI.

I also tried switching DEFORMATION of behavior of DYNA_NON_LINE from 'GROT_GDEP' to 'SIMO_MIEHE', as high strain rate deformation is expected upon the collision.
The calculation refused to launch and instantly gave out <F>_ABNORMAL_ABORT with EXECUTION_CODE_ASTER_EXIT_8627=0.

Any suggestions / ideas in handling the latest issue?

[1] T. Schmidt, F. Gärtner, H. Assadi, et al., "Development of a generalized parameter window for cold spray deposition", Acta Materialia, 2006, 54, pp 729-742.

Last edited by hkboondoggle (2020-07-17 06:55:10)

Attachments:
Case_Files.zip, Size: 635.26 KiB, Downloads: 344

hkboondoggle · 2020-07-29 08:53:52

Hello, could some one please help me out?

sameer21101970 · 2020-07-29 09:20:39

You may try below, hope it will work.

Apply Liasion Mail Command to ball & surface.
Apply Velocity or acceleration to ball.

This will ensure your ball remain stick to the surface and you can study deformation.

hkboondoggle · 2020-07-31 09:25:00

Hello sameer, thank you for your reply.
May I ask a few questions about the 'Liaison_Mail' approach:

1. I was bumped with the following problem when trying out 'Liaison_Mail'. Can you please explain what the matter is?

.. __stg1_cmd6:1
# ------------------------------------------------------------------------------------------
# Commands No: 0009 Concept of the type: char_meca
# ------------------------------------------------------------------------------------------
BC_Fix = AFFE_CHAR_MECA(MODELE=model1,
DDL_IMPO=_F(GROUP_NO=('Substrate_Bottom', ),
DX=0.0,
DY=0.0,
DZ=0.0,),
LIAISON_MAIL=_F(GROUP_MA_MAIT=('Substrate_Top', ),
GROUP_MA_ESCL=('Particle_Face', ),
TYPE_RACCORD='MASSIF',
ELIM_MULT='NON',),
VERI_NORM='OUI',
DOUBLE_LAGRANGE='OUI',
INFO=1,)

!-----------------------------------------------------------------------------!
! <EXCEPTION> <CALCULEL4_55> !
! !
! Pas de mailles Ã projeter ou en correspondance. !
! !
! Dans le cas de l'utilisation de AFFE_CHAR_MECA / LIAISON_MAIL, les mailles !
! maÃ®tres !
! doivent avoir la mÃªme dimension que l'espace de modÃ©lisation : !
! - mailles volumiques pour un modÃ¨le 3D !
! - mailles !
! surfaciques pour un modÃ¨le 2D !
!-----------------------------------------------------------------------------!

!-----------------------------------------------------------------!
! !
! FATAL ERROR detected in Code_Aster for Windows version !
! !
! If an ABNORMAL_ABORT occured, that is not reproductible !
! on official Linux version, or if you need some help to !
! understand the message above, please report issues at: !
! !
! support@simulease.com !
! !
!-----------------------------------------------------------------!
Destruction of the concept BC_Fix.
<S> ERREUR UTILISATEUR RECUPEREE PAR LE SUPERVISEUR

2. Would you please elaborate on your suggestion "Apply Velocity or acceleration to ball" ? 'Cause I have already set the initial velocity of the ball in the following command:

init_vel = CREA_CHAMP(TYPE_CHAM='NOEU_DEPL_R',
OPERATION='AFFE',
MODELE=model1,
AFFE=_F(GROUP_NO=('Particle_Solid', ),
NOM_CMP=('DX', 'DY', 'DZ'),
VALE=(0.0, 0.0, -1.765),),
INFO=1,)

solver = DYNA_NON_LINE(MODELE=model1,
CHAM_MATER=fieldma0,
CONTACT=contact,
COMPORTEMENT=_F( ... ),
ETAT_INIT=_F(VITE=init_vel,
PRECISION=1.E-06,
CRITERE='RELATIF',),
INCREMENT=_F( ... ),
SCHEMA_TEMPS=_F( ... ),
SOLVEUR=_F( ... ),
AMOR_RAYL_RIGI='TANGENTE',
METHODE='NEWTON',
NEWTON=_F( ... ),
CONVERGENCE=_F( ... ),
MESURE=_F(TABLE='NON',),
ARCHIVAGE=_F( ... ),
INFO=1,)

3. How does setting up 'Liaison_Mail' help tackling the convergence issue of 'DYNA_NON_LINE' with 'VMIS_JOHN_COOK' enabled?

Thanks again!

Last edited by hkboondoggle (2020-07-31 09:25:30)

sameer21101970 · 2020-07-31 11:17:12

odÃ©lisation : !
! - mailles volumiques pour un modÃ¨le 3D !
! - mailles !
! surfaciques pour un modÃ¨le 2D

odelization:!
! - voluminal meshes for a 3D model!
! - stitches!
! surface for a 2D model

GROUP_MA_MAIT WILL BE 3D VOLUME
AND SELECT GROUP_NO_ESCL = 2D SURFACE

sameer21101970 · 2020-07-31 16:38:39

i hv tested, it is working under your given material law.

hkboondoggle · 2020-08-03 08:03:44

sameer, would you mind sharing the details of your test run?

'Cause I have managed to get 'Liaison_Mail' implemented in my latest trial, but it is still giving out <MECANONLINE9_3> under 'VMIS_JOHN_COOK'.

Also, switching DEFORMATION of behavior of DYNA_NON_LINE from 'GROT_GDEP' to 'SIMO_MIEHE' still instantly leads to <F>_ABNORMAL_ABORT with EXECUTION_CODE_ASTER_EXIT_8627=0.

Attachments:
stderr_command_salome.log, Size: 446.85 KiB, Downloads: 390

sameer21101970 · 2020-08-03 12:36:34

Whether you hv made changes to your geometry. No gap between ball and striking face.

hkboondoggle · 2020-08-25 04:17:41

Hi sameer, sorry for the late replay. The lock down of the campus screws up my work flow.

I have re-done the geometry & meshing based on your recommendation (as shown in attached figure below). However, it is now reporting an issue in "DEFI_CONTACT":

!--------------------------------------------------------------------------------------------------------------------!
! <EXCEPTION> <CONTACT2_13> !
! !
! Contact methods with a grid. !
! The contact zone number 1 contains 1 nodes common to surfaces Masters and slaves. !
! Check the !
! definition of your contact surfaces or inform one of key words SANS_NOEUD/SANS_GROUP_NO/SANS_MAILLE/SANS_GROUP_MA. !
!--------------------------------------------------------------------------------------------------------------------!

I tried adding this additional settings in "DEFI_CONTACT":
SANS_GROUP_NO=('Particle_Face', )

But then it led to another fatal error when initializing the "DYNA_NON_LINE":

.. __stg1_cmd9:1
# ------------------------------------------------------------------------------------------
# Commands No: 0012 Concept of the type: evol_noli
# ------------------------------------------------------------------------------------------
solver = DYNA_NON_LINE(MODELE=model1,
CHAM_MATER=fieldma0,
CONTACT=contact,
COMPORTEMENT=_F(TOUT='OUI',
RELATION='VMIS_JOHN_COOK',
DEFORMATION='SIMO_MIEHE',
RESI_CPLAN_RELA=1.E-06,
RESI_INTE_RELA=1.E-06,
ITER_INTE_MAXI=20,
ITER_CPLAN_MAXI=1,
SYME_MATR_TANG='OUI',
PARM_THETA=1.0,),
ETAT_INIT=_F(VITE=init_vel,
PRECISION=1.E-06,
CRITERE='RELATIF',),
INCREMENT=_F(LIST_INST=timeline,
PRECISION=1.E-06,),
SCHEMA_TEMPS=_F(SCHEMA='HHT',
ALPHA=-0.6,
MODI_EQUI='NON',
FORMULATION='DEPLACEMENT',
COEF_MASS_SHIFT=0.0,),
SOLVEUR=_F(METHODE='MUMPS',
RENUM='AUTO',
NPREC=8,
ELIM_LAGR='LAGR2',
STOP_SINGULIER='OUI',
TYPE_RESOL='AUTO',
ACCELERATION='AUTO',
LOW_RANK_SEUIL=0.0,
PRETRAITEMENTS='AUTO',
POSTTRAITEMENTS='AUTO',
PCENT_PIVOT=20,
RESI_RELA=-1.0,
GESTION_MEMOIRE='AUTO',
FILTRAGE_MATRICE=-1.0,
MIXER_PRECISION='NON',
MATR_DISTRIBUEE='NON',),
AMOR_RAYL_RIGI='TANGENTE',
METHODE='NEWTON',
NEWTON=_F(REAC_INCR=1,
MATRICE='TANGENTE',
REAC_ITER=1,
REAC_ITER_ELAS=0,
MATR_RIGI_SYME='NON',),
CONVERGENCE=_F(ITER_GLOB_MAXI=10,
ITER_GLOB_ELAS=25,
ARRET='OUI',),
MESURE=_F(TABLE='NON',),
ARCHIVAGE=_F(PRECISION=1.E-06,
CRITERE='RELATIF',),
INFO=1,)
../../../bibc/supervis/aster_module.c 2343 : Echec lors de la creation du comportement (lccree/create) !
EXECUTION_CODE_ASTER_EXIT_4830=0
<INFO> Code_Aster run ended, diagnostic : <F>_ABNORMAL_ABORT

Any suggestions / ideas in handling the latest issue? Thanks!
As usual, the comm, log & med files of this latest trial are attached FYI.

Attachments:
Case_File_20200824.zip, Size: 237.24 KiB, Downloads: 329

sameer21101970 · 2020-08-25 07:49:05

!
! The contact zone number 1 contains 1 nodes common to surfaces Masters and slaves. !
! Check the

You have to correct your groups - surface selection.

do group selection in geometry.
ball surface.
rectangular top surface.

check attachment

Attachments:
Compound_Mesh_1.med, Size: 152.2 KiB, Downloads: 372

sameer21101970 · 2020-08-25 07:50:32

refer attachment

Attachments:
RunCase_1.comm, Size: 3.36 KiB, Downloads: 393

marco.mueller · 2020-09-01 14:43:23

Have you tried to alternate DEFORMATION='SIMO_MIEHE', i. e. GROT_GDEP.

I've just read SIMO_MIEHE may not be applicable to your material model.

Last edited by marco.mueller (2020-09-02 07:28:00)

hkboondoggle · 2020-09-04 03:14:33

@sammer: Thanks for sharing the your reference case! It did converge nicely. I am trying to replicate the settings to my existing study for having a finer mesh resolution on the substrate surface, though it turns out having issue of singular matrix (the comm, log & med files are attached FYI). Would you mind giving it a look? Thanks!

@mueller: Thanks for your input! I did try out "GROT_GDEP" which successfully launched the calculation. Do you mean that whether "SIMO_MIEHE" is applicable or not depends on the settings of "DEFI_MATERIAU"?

Attachments:
Case_settings_2020.09.03.zip, Size: 241.97 KiB, Downloads: 319

hkboondoggle · 2020-09-28 07:05:35

Hello, could some one please help me out?

As stated in my previous post, I am facing issue of singular matrix whenever repeating the calculation using a finer mesh.
The mesh is entirely NetGen 1D-2D-3D, and has no coincident nodes / elements. I have included the dump of mesh info FYI.

The comm, log & med files are attached in my previous post above.
I am running code aster version 14.4.0 on Windows-10-10.0.17134-SP0.

Many thanks.

Attachments:
Mesh_Info.txt, Size: 3.68 KiB, Downloads: 433

hkboondoggle · 2020-10-15 04:32:09

Grateful if anyone can assist.

After detail reviewing of the calculation log, one of the possible cause of the singularity matrix problem is identified with the following error prompt during the setup of adhesion relationship in AFFE_CHAR_MECA:

CrÃ©ation du fichier au format MED 3.3.1.

!------------------------------------------------------------------------------!
! <A> <CALCULEL5_49> !
! !
! LIAISON_MAIL: !
! The linear relation intended to eliminate the slave node N10 is a tautology !
! because the mesh Master in with !
! respect to this node has this same node in its connectivity. !
! It is thus not written. !
! !
! !
! This is a warning. If you do not understand the meaning of this !
! warning, you can obtain unexpected results! !
!------------------------------------------------------------------------------!

Node N10 appears to be the initial contact point where the bottom of the ball meets with the top surface of the substrate at T = 0. Is this a problem mesh creation? And if so, how should this be solved?

Moreover, there seems to be other hiccups in the mesh I am using.
This is reflected by the multiple (5 times) warnings during AFFE_MODELE:

!----------------------------------------------------------------------------------------!
! <A> <MODELE1_63> !
! !
! - > the mesh M155 carries an edge finite element, but it does not border !
! any element having" a rigidity". !
! !
! - > Risks & !
! advices: !
! That can involve problems of" null pivot" at the time of the resolution. !
! If the resolution of the linear systems does !
! not pose problems, you !
! can be unaware of this message. !
! If not, check the definition of model (AFFE_MODELE) by avoiding the use !
! !
! of operand TOUT='OUI'. !
! !
! !
! This is a warning. If you do not understand the meaning of this !
! warning, you can obtain unexpected results! !
!----------------------------------------------------------------------------------------!

What does this error suppose to mean?
Mesh elements in question (M155 ~ M159) locate at -x edge of the top surface of the substrate.
The whole mesh has no duplicating edge or mesh element.

hkboondoggle · 2020-10-19 03:12:52

I tried to avoid the issue of identical node at the initial contact point where the bottom of the ball meets with the top surface of the substrate through the following steps:

1.) Individually create the mesh of ball and particle respectively

2.) Ensure no existence of duplicating node or mesh element within each individual mesh.

3.) Create groups of node / surface / volume under each individual mesh with their corresponding geometries.

4.) Create a compound mesh from the individual meshes, enable the option "Create groups from input objects", and disable "Merge coincident nodes and elements".

While the error prompt of <A> <CALCULEL5_49> under LIAISON_MAIL no longer occur, the calculation is still plagued by the convergence issue where the time increment kept on decreasing and finally trigger the following:

!-----------------------------------------------------------------------------------!
! <EXCEPTION> <ADAPTATION_11> !
! !
! The value of the time step selected 1.862645169939e-13 is lower than PAS_MINI. !
!-----------------------------------------------------------------------------------!

!-----------------------------------------------------------------!
! !
! FATAL ERROR detected in Code_Aster for Windows version !
! !
! If an ABNORMAL_ABORT occured, that is not reproductible !
! on official Linux version, or if you need some help to !
! understand the message above, please report issues at: !
! !
! support@simulease.com !
! !
!-----------------------------------------------------------------!

Any suggestions / ideas in handling the latest issue? Thanks!
As usual, the comm, log & med files of this latest trial are attached FYI.

@sammer: Would you mind showing me the details of the meshing procedure in your reference case?

Attachments:
Case_Files_20201019.zip, Size: 784.26 KiB, Downloads: 342

sameer21101970 · 2020-10-19 07:47:34

I think you are doing 1 common mistake.

You have to uncheck one window as shown in attachment while Meshing - build Compound -
"" Merge Coincident Nodes & Elements """ Uncheck this window while building compound mesh.

refer attachment

Attachments:
Screenshot from 2020-10-19 12-16-00.png, Size: 56.91 KiB, Downloads: 248

hkboondoggle · 2020-10-20 02:16:48

Hello Sameer, thanks for your reply.

However, your suggestion is exactly what I did as in my previous description:

4.) ... and disable "Merge coincident nodes and elements".

So right now, I'm unsure if the latest convergence issue is in fact mesh related or not.

Did you also used compound mesh as well in the reference case you shared on 08/25?

I notice that the mesh size of the substrate is larger than that of the ball in the reference case. Does this factor plays a role in the convergence of the calculation?

Last edited by hkboondoggle (2020-10-20 08:14:47)

sameer21101970 · 2020-10-20 07:22:35

if i am not wrong, the slave surface has to be fine mesh then master.

i will go through your zip file and reply later.

give some time.

sameer21101970 · 2020-10-21 08:20:07

It is converging, do below.

Make Sphere (ball)Mesh Fine.
Reduce Time Step to 100

Last edited by sameer21101970 (2020-10-21 08:31:32)

hkboondoggle · 2020-10-22 08:40:49

Sorry Sameer, but I have to try out your latest suggestion at a later time.
My office desktop, where Code_Aster is installed, is now show BSOD issues. (Thanks Microsoft)

Could you please explain the reason why slave surface mesh has to be finer then that of master?

Also, I find your suggestion of reducing time steps surprising. Because I thought have a smaller time increment could aid the calculation in achieving convergence. Am I mistaken, or just this concept is not applicable in this calculation?

sameer21101970 · 2020-10-22 10:08:26

i had done with your 10000 time step....it shown material law failure.
so with 100...it was smooth...

regarding convergence,,,,,define as finer the mesh more accurate the results....there is a limit to fineness.

#1 2020-06-29 06:13:27

Advice needed on <EXCEPTION> <DVP_1> (DYNA_NON_LINE)

#2 2020-07-03 09:40:59

Re: Advice needed on <EXCEPTION> <DVP_1> (DYNA_NON_LINE)

#3 2020-07-08 08:49:38

Re: Advice needed on <EXCEPTION> <DVP_1> (DYNA_NON_LINE)

#4 2020-07-17 06:52:22

Re: Advice needed on <EXCEPTION> <DVP_1> (DYNA_NON_LINE)

#5 2020-07-29 08:53:52

Re: Advice needed on <EXCEPTION> <DVP_1> (DYNA_NON_LINE)

#6 2020-07-29 09:20:39

Re: Advice needed on <EXCEPTION> <DVP_1> (DYNA_NON_LINE)

#7 2020-07-31 09:25:00

Re: Advice needed on <EXCEPTION> <DVP_1> (DYNA_NON_LINE)

#8 2020-07-31 11:17:12

Re: Advice needed on <EXCEPTION> <DVP_1> (DYNA_NON_LINE)

#9 2020-07-31 16:38:39

Re: Advice needed on <EXCEPTION> <DVP_1> (DYNA_NON_LINE)

#10 2020-08-03 08:03:44

Re: Advice needed on <EXCEPTION> <DVP_1> (DYNA_NON_LINE)

#11 2020-08-03 12:36:34

Re: Advice needed on <EXCEPTION> <DVP_1> (DYNA_NON_LINE)

#12 2020-08-25 04:17:41

Re: Advice needed on <EXCEPTION> <DVP_1> (DYNA_NON_LINE)

#13 2020-08-25 07:49:05

Re: Advice needed on <EXCEPTION> <DVP_1> (DYNA_NON_LINE)

#14 2020-08-25 07:50:32

Re: Advice needed on <EXCEPTION> <DVP_1> (DYNA_NON_LINE)

#15 2020-09-01 14:43:23

Re: Advice needed on <EXCEPTION> <DVP_1> (DYNA_NON_LINE)

#16 2020-09-04 03:14:33

Re: Advice needed on <EXCEPTION> <DVP_1> (DYNA_NON_LINE)

#17 2020-09-28 07:05:35

Re: Advice needed on <EXCEPTION> <DVP_1> (DYNA_NON_LINE)

#18 2020-10-15 04:32:09

Re: Advice needed on <EXCEPTION> <DVP_1> (DYNA_NON_LINE)

#19 2020-10-19 03:12:52

Re: Advice needed on <EXCEPTION> <DVP_1> (DYNA_NON_LINE)

#20 2020-10-19 07:47:34

Re: Advice needed on <EXCEPTION> <DVP_1> (DYNA_NON_LINE)

#21 2020-10-20 02:16:48

Re: Advice needed on <EXCEPTION> <DVP_1> (DYNA_NON_LINE)

#22 2020-10-20 07:22:35

Re: Advice needed on <EXCEPTION> <DVP_1> (DYNA_NON_LINE)

#23 2020-10-21 08:20:07

Re: Advice needed on <EXCEPTION> <DVP_1> (DYNA_NON_LINE)

#24 2020-10-22 08:40:49

Re: Advice needed on <EXCEPTION> <DVP_1> (DYNA_NON_LINE)

#25 2020-10-22 10:08:26

Re: Advice needed on <EXCEPTION> <DVP_1> (DYNA_NON_LINE)

Board footer