[SOLVED] Stress analysis on a symmetrical shaft

marcelo · 2019-10-30 20:09:27

Hi,

I'm having trouble setting my Aster_Study problem with respect to my model's attachment point (Fixed). Link: encurtador.com.br/hw237.

I am trying to reproduce the behavior of a bearing, but when I will analyze the deformation of the shaft, I see that the condition is not set correctly, mainly because it has a similar analysis as comparative (link: encurtador.com.br/fmuFW).

The difference to the analysis made in commercial software is the use of the '' Remote Displacement '' (link: encurtador.com.br/bBPU7) condition on the opposite side of the shaft symmetry condition. Could someone tell me if it is possible to use such condition in Aster_Study?

Initially I am doing a linear analysis, later I intend to do the nonlinear analysis and later the fatigue analysis.

.comm:

DEBUT(LANG='EN')

mesh = LIRE_MAILLAGE(FORMAT='MED',
                     UNITE=20)

model = AFFE_MODELE(AFFE=_F(MODELISATION=('3D', ),
                            PHENOMENE='MECANIQUE',
                            TOUT='OUI'),
                    MAILLAGE=mesh)

mater = DEFI_MATERIAU(ECRO_LINE=_F(D_SIGM_EPSI=0.0,
                                   SY=579.0),
                      ELAS=_F(E=210000.0,
                              NU=0.3,
                              RHO=7.85e-06))

fieldmat = AFFE_MATERIAU(AFFE=_F(MATER=(mater, ),
                                 TOUT='OUI'),
                         MAILLAGE=mesh)

Load = AFFE_CHAR_MECA(FORCE_FACE=_F(FY=18392.0,
                                    GROUP_MA=('Force', )),
                      MODELE=model)

Fixed = AFFE_CHAR_MECA(DDL_IMPO=_F(DX=0.0,
                                   DY=0.0,
                                   DZ=0.0,
                                   GROUP_MA=('Fixed', )),
                       MODELE=model)

g = AFFE_CHAR_MECA(MODELE=model,
                   PESANTEUR=_F(DIRECTION=(0.0, 0.0, -1.0),
                                GRAVITE=9.8066,
                                GROUP_MA=('Eixo', )))

Symmetry = AFFE_CHAR_MECA(DDL_IMPO=_F(DX=0.0,
                                      GROUP_MA=('Symmetry', )),
                          MODELE=model)

reslin = MECA_STATIQUE(CHAM_MATER=fieldmat,
                       EXCIT=(_F(CHARGE=Load),
                              _F(CHARGE=Fixed),
                              _F(CHARGE=g),
                              _F(CHARGE=Symmetry)),
                       MODELE=model)

reslin = CALC_CHAMP(reuse=reslin,
                    CONTRAINTE=('SIGM_NOEU', 'SIGM_ELNO'),
                    CRITERES=('SIEQ_NOEU', 'SIEQ_ELNO'),
                    FORCE=('REAC_NODA', ),
                    RESULTAT=reslin)

IMPR_RESU(FORMAT='MED',
          RESU=_F(INFO_MAILLAGE='OUI',
                  RESULTAT=reslin),
          UNITE=80)

FIN()

mesh: encurtador.com.br/pxDR9

Last edited by marcelo (2019-11-30 14:09:34)

dezsit · 2019-10-31 09:09:44

Hello,

I did not check your model, but if you want to achieve something like Remote displacement and Remote load, you should check LIAISON_SOLIDE and LIAISON_RBE3.

BR.
dezsit

marcelo · 2019-11-03 19:01:47

Hello,

I tried the LIAISON_RBE3 function, apparently it fits the case I commented, but I am getting errors. I don't know if I'm using the function incorrectly. I attached the files so if possible take a look.

error:

   !!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!
   ! <S> Exception user raised but not interceptee.                                 !
   ! The bases are fermees.                                                         !
   ! Type of the exception: error                                                   !
   !                                                                                !
   !  Erreur utilisateur:                                                           !
   !     On cherche ? imposer une condition aux limites sur le ddl DRY du noeud N8. !
   !     Mais ce noeud ne porte pas ce ddl.                                         !
   !                                                                                !
   !     Conseils :                                                                 !
   !      - v?rifiez le mod?le et les conditions aux limites :                      !
   !         - le noeud incrimin? fait-il partie du mod?le ?                        !
   !         - le noeud porte-t-il le ddl que l'on cherche ? contraindre ?          !
   !!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!

Case: encurtador.com.br/gsvJU

EDIT1: I believe the error is related to the node that I 'forced' into geometry. Because when I tried to add a node to the mesh and run the case... I was given the orphan node error, not belonging to the mesh. When I saw the geometry, I saw that this node I had inserted (at 0,0,0) was in the center of one element and not at the junction of both.

Last edited by marcelo (2019-11-03 19:20:50)

jeanpierreaubry · 2019-11-04 08:01:52

hello

the message is very clear
in 3D elements rotational DOF are not supported
and this is basic in finite element analysis

jean pierre aubry

marcelo · 2019-11-04 13:14:00

jeanpierreaubry wrote:

the message is very clear

Yes, the message from the .mess file is clear. However, I don't know what is wrong or what I should adjust to avoid the mistake...
I made my adjustments based on work I read in the forum.

EDI1: 3D has 6 DOF (3 of translation and 3 of rotation).

Last edited by marcelo (2019-11-04 13:27:41)

jeanpierreaubry · 2019-11-04 15:34:43

without the message file it is impossible to tell what is happening

marcelo · 2019-11-04 18:15:25

jeanpierreaubry wrote:

without the message file it is impossible to tell what is happening

.mess, .comm and .med: encurtador.com.br/gsvJU (Google Drive link)

EDI1: The Fixed condition is not necessary (I unintentionally added it to MECA_STATIQUE, as I had created it only to be able to use it for testing), but... removing it, the same error happens.

Last edited by marcelo (2019-11-04 20:13:43)

dezsit · 2019-11-04 21:34:07

Hi,

I did not check your case deeply, only the message file, but as JeanPierre said, it is clear: 3D solid does not have rotational DOF (it is not aster specific, 3D solid does not have rotational dof in any common mechanical fea package!) so you should remove the '-DRY-DRZ' from yout DDL_ESCL definition. A second thing related to the orphan node: yes aster does not able to handle orphan nodes. But as it was discussed many times, you can define a 0D element on your orphan node, and use a DIS_T or DIS_TR modelisation, depending on your needs, and attach a zero stiffness spring to this 0D element (AFFE_CARA_ELEM -> K_T_D_N or K_TR_D_N or whatever, again depending on the problem you modeling). So you have to provide stiffness for every node, even if it is zero stiffness.

BR,
dezsit.

marcelo · 2019-11-05 18:46:24

dezsit wrote:

3D solid does not have rotational DOF (it is not aster specific, 3D solid does not have rotational dof in any common mechanical fea package!) so you should remove the '-DRY-DRZ' from yout DDL_ESCL definition.

Yes, I know.
I'm just trying to reproduce what I did in commercial software, and the problem, I believe, is precisely trying to reproduce the condition of Remote Displacement (I'll leave this image out of curiosity: encurtador.com.br/lmC23 - pay attention to 6 DOF). Or is it the condition of symmetry?

dezsit wrote:

...and use a DIS_T or DIS_TR modelisation, depending on your needs, and attach a zero stiffness spring to this 0D element (AFFE_CARA_ELEM -> K_T_D_N or K_TR_D_N or whatever, again depending on the problem you modeling).

Yes, on the node I created I added the condition of DIS_TR (6 DOF), but apparently something is wrong. And I made that node not 'orphaned' but in the center of the face.

DEBUT(LANG='EN')

mesh = LIRE_MAILLAGE(FORMAT='MED',
                     UNITE=2)

mesh0 = CREA_MAILLAGE(CREA_POI1=_F(GROUP_NO=('Node', ),
                                   NOM_GROUP_MA=('Node', )),
                      MAILLAGE=mesh)

model = AFFE_MODELE(AFFE=(_F(MODELISATION=('3D', ),
                             PHENOMENE='MECANIQUE',
                             TOUT='OUI'),
                          _F(GROUP_MA=('Node', ),
                             MODELISATION=('DIS_TR', ),
                             PHENOMENE='MECANIQUE')),
                    MAILLAGE=mesh0)

mater = DEFI_MATERIAU(ECRO_LINE=_F(D_SIGM_EPSI=0.0,
                                   SY=579.0),
                      ELAS=_F(E=210000.0,
                              NU=0.3,
                              RHO=7.85e-06))

fieldmat = AFFE_MATERIAU(AFFE=_F(MATER=(mater, ),
                                 TOUT='OUI'),
                         MAILLAGE=mesh0)

Load = AFFE_CHAR_MECA(FORCE_FACE=_F(FY=18392.0,
                                    GROUP_MA=('Force', )),
                      MODELE=model)

g = AFFE_CHAR_MECA(MODELE=model,
                   PESANTEUR=_F(DIRECTION=(0.0, 0.0, -1.0),
                                GRAVITE=9.8066,
                                GROUP_MA=('Eixo', )))

Symmetry = AFFE_CHAR_MECA(DDL_IMPO=_F(DX=0.0,
                                      GROUP_MA=('Symmetry', )),
                          MODELE=model)

Remote = AFFE_CHAR_MECA(LIAISON_RBE3=_F(COEF_ESCL=(1.0, ),
                                        DDL_ESCL=('DX-DY-DZ-DRY-DRZ', ),
                                        DDL_MAIT=('DX', 'DY', 'DZ', 'DRY', 'DRZ'),
                                        GROUP_NO_ESCL=('Remote', ),
                                        GROUP_NO_MAIT=('Node', )),
                        MODELE=model)

reslin = MECA_STATIQUE(CHAM_MATER=fieldmat,
                       EXCIT=(_F(CHARGE=Load),
                              _F(CHARGE=g),
                              _F(CHARGE=Symmetry),
                              _F(CHARGE=Remote)),
                       MODELE=model)

reslin = CALC_CHAMP(reuse=reslin,
                    CONTRAINTE=('SIGM_NOEU', 'SIGM_ELNO'),
                    CRITERES=('SIEQ_NOEU', 'SIEQ_ELNO'),
                    FORCE=('REAC_NODA', ),
                    RESULTAT=reslin)

IMPR_RESU(FORMAT='MED',
          RESU=_F(INFO_MAILLAGE='OUI',
                  RESULTAT=reslin),
          UNITE=80)

FIN()

Last edited by marcelo (2019-11-05 18:49:04)

marcelo · 2019-11-14 22:33:25

Can anybody help me?

RichardS · 2019-11-15 09:39:25

Hi marcelo,
it seems you are still missing the AFFE_CARA_ELEM command to assign the structural element properties (spring stiffness) of your DIS_TR elements.

Best,
Richard

P.s.: What you could also do is to run a quick analysis on SimScale (free) with a similar setup and check the log file, there you can see exactly how the command file is built and you can use this information for your file. For example this project could be helpful: https://www. simscale.com/projects/rszoeke/pinned_bar_example/

marcelo · 2019-11-20 20:01:25

RichardS wrote:

For example this project could be helpful: https://www. simscale.com/projects/rszoeke/pinned_bar_example/

Thank you Richards for the answer.

I tried to reproduce the example case in Aster_Study but unfortunately I am trying similar errors to the ones I had previously. In this particular case he has been giving errors related to orphan nodes. I have tried every strategy I know and none have actually been effective. In SimScale there is a function that creates this node (CALC_MESH_UTILS), but this function does not exist in AsterStudy, so I tried to use the same strategy I was using for my problem, using Salome's own mesh solver.
Honestly, I don't know what to do anymore, I've been studying and haven't been able to find the solution to my problem.

I have attached my study (link: https: //drive.google.com/open?id=1xo-Pb8ZUOtNAQtHJcuBEpR25E253TaQL .mess; .comm and .med files) in case anyone wants to analyze and contribute.

Last edited by marcelo (2019-11-20 20:02:46)

konyaro · 2019-11-23 14:40:12

Hello Marcelo,
As RichardS said you didn't define an AFFE_CARA_ELEM. I modified your files in order to make them run. I changed your connections with a simple LIAISON_SOLIDE which is closer to a "rigid remote displacement".

There are many posts concerning an equivalent remote displacement with Code_Aster, for instance:
- https://code-aster.org/forum2/viewtopic.php?id=23018
- https://code-aster.org/forum2/viewtopic … 534#p50534
- Nice tutorial written by Claus: http caelinux.org/wiki/index.php/Contrib:Claws/Code_Aster/10_x_cases/torque

In your case it's quite easy because the displacements are small. In case of large displacements there are some issues if you link the remote point to the geometry with POU_D_T_GD:
- https://code-aster.org/forum2/viewtopic.php?id=21253
A new beam element should be available someday:
- https://code-aster.org/forum2/viewtopic.php?id=23652

Good luck,

Konyaro

p.s. Why don't you insert your attachments directly in your posts? I guess more people would help you. Most of the time I can't open your files, especially your "encurtador" ones.

Attachments:
rem_disp.zip, Size: 1.82 MiB, Downloads: 388

marcelo · 2019-11-25 13:21:19

konyaro wrote:

p.s. Why don't you insert your attachments directly in your posts? I guess more people would help you. Most of the time I can't open your files, especially your "encurtador" ones.

Hi Konyaro,

I can't attach to the forum because the vast majority of times I've tried 'very large file size' errors.

About the modifications you made, fortunately I was able to access the .comm file, but unfortunately the .med file could not be accessed, it presented error when I tried to import it.
So I can understand the changes that were made to the case, but I can't see the changes made to the mesh.
EDIT1: I was able to imitate your steps in my case. The results are somewhat distant from those presented in SimScale (where the idea of reproducing them came from), especially when the deformation is analyzed (SimScale max_D: 0.000096m; Aster_Study max_D: 0.001665). However, positive since I managed to run the case.

Did you even analyze my shaft case?

Last edited by marcelo (2019-11-25 14:45:42)

konyaro · 2019-11-25 13:28:16

I just changed the names of the groups:

Mesh Marcelo

Last edited by konyaro (2019-11-25 13:29:03)

Attachments:
Mesh_Marcelo.png, Size: 35.91 KiB, Downloads: 1,450

marcelo · 2019-11-25 14:26:24

konyaro wrote:

I just changed the names of the groups

Yes, it coincided that we put the message in the thread at the same time, I added an EDIT in the previous message.

EDIT1: I was able to imitate your steps in my case. The results are somewhat distant from those presented in SimScale (where the idea of reproducing them came from), especially when the deformation is analyzed (SimScale max_D: 0.000096m; Aster_Study max_D: 0.001665). However, positive since I managed to run the case.

Do you believe that by following these steps I will be able to solve my shaft case?

EDIT1: Using LIAISON_RBE3 also get similar results to those presented by LIAISON_SOLID.

Last edited by marcelo (2019-11-25 14:45:59)

marcelo · 2019-11-25 18:53:57

Hi,

I tried to reproduce what I had done in the bar, and it had worked, in the shaft.
Unfortunately, a series of errors appeared... which I understood to be from the mesh, but which I honestly don't think was badly done.

Because the mesh file is large, I put it in Google Drive: https:// drive.google.com/open?id=1acwcKCu2r4Ydmug13LB8A4NtzHJ6hYwP (Fixed region = Bearing)

The .mess and .comm files are then attached.
Who can help, I would be very grateful.

Last edited by marcelo (2019-11-25 19:16:54)

Attachments:
Shaft.zip, Size: 10.05 KiB, Downloads: 386

konyaro · 2019-11-27 20:21:13

Hello,
be careful with your boundary conditions, you must fix DRX and DRY, not DRZ. Attached the modified comm file.

Konyaro

Attachments:
modified.comm, Size: 2.71 KiB, Downloads: 399

marcelo · 2019-11-28 13:55:52

konyaro wrote:

be careful with your boundary conditions, you must fix DRX and DRY, not DRZ.

Hi Konyaro,

I did what you recommended and it worked. Thank you very much.

Last edited by marcelo (2019-11-29 13:51:39)

marcelo · 2019-11-29 13:54:16

Konyaro,

See the result of the analysis in both software. Of course there is no better... far from it, but the results presented by Code_Aster, to my understanding, are inferior and maybe, I'm not sure, could be the responsibility of the boundary condition, what do you think?

EDIT1: I also attached the .mess file.

Attachments:
Results.zip, Size: 429.46 KiB, Downloads: 447

konyaro · 2019-11-30 10:51:28

What do you mean by "inferior" ? I see different values due probably to a different applied force. Be careful, the FORCE_FACE is a pressure so you must divide the desired force by the area of the surface.

marcelo · 2019-11-30 14:09:14

konyaro wrote:

Be careful, the FORCE_FACE is a pressure so you must divide the desired force by the area of the surface.

True, I had forgotten that.

I made the modifications and the values are now close, not ''equal''... but I didn't do the mesh convergence test.

Thank you very much for your attention.

#1 2019-10-30 20:09:27

[SOLVED] Stress analysis on a symmetrical shaft

#2 2019-10-31 09:09:44

Re: [SOLVED] Stress analysis on a symmetrical shaft

#3 2019-11-03 19:01:47

Re: [SOLVED] Stress analysis on a symmetrical shaft

#4 2019-11-04 08:01:52

Re: [SOLVED] Stress analysis on a symmetrical shaft

#5 2019-11-04 13:14:00

Re: [SOLVED] Stress analysis on a symmetrical shaft

#6 2019-11-04 15:34:43

Re: [SOLVED] Stress analysis on a symmetrical shaft

#7 2019-11-04 18:15:25

Re: [SOLVED] Stress analysis on a symmetrical shaft

#8 2019-11-04 21:34:07

Re: [SOLVED] Stress analysis on a symmetrical shaft

#9 2019-11-05 18:46:24

Re: [SOLVED] Stress analysis on a symmetrical shaft

#10 2019-11-14 22:33:25

Re: [SOLVED] Stress analysis on a symmetrical shaft

#11 2019-11-15 09:39:25

Re: [SOLVED] Stress analysis on a symmetrical shaft

#12 2019-11-20 20:01:25

Re: [SOLVED] Stress analysis on a symmetrical shaft

#13 2019-11-23 14:40:12

Re: [SOLVED] Stress analysis on a symmetrical shaft

#14 2019-11-25 13:21:19

Re: [SOLVED] Stress analysis on a symmetrical shaft

#15 2019-11-25 13:28:16

Re: [SOLVED] Stress analysis on a symmetrical shaft

#16 2019-11-25 14:26:24

Re: [SOLVED] Stress analysis on a symmetrical shaft

#17 2019-11-25 18:53:57

Re: [SOLVED] Stress analysis on a symmetrical shaft

#18 2019-11-27 20:21:13

Re: [SOLVED] Stress analysis on a symmetrical shaft

#19 2019-11-28 13:55:52

Re: [SOLVED] Stress analysis on a symmetrical shaft

#20 2019-11-29 13:54:16

Re: [SOLVED] Stress analysis on a symmetrical shaft

#21 2019-11-30 10:51:28

Re: [SOLVED] Stress analysis on a symmetrical shaft

#22 2019-11-30 14:09:14

Re: [SOLVED] Stress analysis on a symmetrical shaft

Board footer