Welcome to the forums. Please post in English or French.

You are not logged in.

## #1 2008-08-02 15:53:06

JMB365
Member
Registered: 2008-01-19
Posts: 781

### [RESOLU] 3D model with rigid bar elements and a point mass

[RESOLU]
[RESOLVED]

Hello,

(The "text" diagrams below are best viewed in a fixed-width font of your browser...)

In an attempt at a linear static analysis, I am trying to model a box (20mm cube) with rigid bar elements attached to one face.  One end of the rigid bars is to be attached to each node on a face of the cube while the other ends of the rigid bars meet at a point mass.  The cube is meshed with quad tetrahedral elements using Salome 3.2.9.  The opposite face of the cube is fixed.
______
|      |
Fixed | Cube |-----o -> Force
face  |______|    (m)

The "o" represents the point mass (m) to which a force is applied.  The point mass is to be connected to one face of the cube by numerous rigid bar elements (one of which is represented by dashes).  A force(s) is to be applied to the point mass.  Also since there are many nodes on the face I would like to know if I can create the rigid bar elements in Salome 3.2.9 (or Code-Aster 9.2) without tediously clicking (or typing) each one using a "grouping" method perhaps?  I think I should use M_T_DN of DISCRET (Discrete element) in AFFE_CHAR_ELEM (pg 37/52 of U4.42.01-I) for the point mass.

I have tried LIAISON_GROUP but get:

!----------------------------------------------------------------------------!
! <F> <MODELISA3_12>                                                         !
!   Mot clé LIAISON_GROUP : les mots clés GROUP_NO_1 et GROUP_NO_2 à mettre  !
!   en vis-à-vis n'ont pas le meme nombre de noeuds.                         !
!    - Nombre de noeuds présent sous le mot clé GROUP_NO_1: 9                !
!    - Nombre de noeuds présent sous le mot clé GROUP_NO_2: 1                !
! Cette erreur est fatale. Le code s'arrete.                                 !
!----------------------------------------------------------------------------!

With LIAISON_SOLIDE I get:

!-------------------------------------------------------!
! <F> <JEVEUX_57>                                       !
!  Longueur du segment de valeurs à allouer invalide 0. !
! Cette erreur est fatale. Le code s'arrete.            !
!-------------------------------------------------------!

I would very much appreciate somebody taking the time to look at the model and the comm file and making corrections.  I have tried to follow some of the advice of these discussions (http://www.code-aster.org/forum2/viewtopic.php?id=12017 & http://www.code-aster.org/forum2/viewto … 40#p14540).  My situation is not as complex and therefore I am finding the examples too complicated for a starting point.  Jacopo has been very helpful with some of my attempts. My knowledge of French is limited and I have tried to read and understand the user manuals. So if someone could give a more step by step advice (comm file would be useful) I think I can solve the problem.

Later I would like to extend this concept to add a spring element with 6DOFs to the opposite face.  This point spring element would similarly be connected to all the nodes of the opposite face of the cube with many rigid bar elements. Then apply a force to the point mass.

______
|      |
Fixed |------o-----| Cube |-----o --> Force
(Kx, Kx, Ky, Rx,Ry, Rz) |______|    (m)

The left "o" represents the spring element with 6 values (3 translation stiffness values Kx, Ky, Kz and 3 rotation stiffness values Rx, Ry, Rz). This point spring element will be fixed at one end.  The other end is connected to several rigid bar elements in parallel (one of which is represented by the "-----").

The right side "o" represents the point mass (m) to which a force is applied.  The point mass is connected to the face of the cube by numerous other rigid bar elements (one of which is represented by dashes).  A force is to be applied to the point mass.   I think I should use K_TR_DN of DISCRET (Discrete element) in AFFE_CHAR_ELEM (pg 37/52 of U4.42.01-I) for the point spring.

Thank you.

Regards,
JMB

Last edited by JMB365 (2008-08-29 18:27:35)

Attachments:

SalomeMeca 2021
Ubuntu 20.04, 22.04

Offline

## #2 2008-08-08 08:17:58

JMB365
Member
Registered: 2008-01-19
Posts: 781

### Re: [RESOLU] 3D model with rigid bar elements and a point mass

Hello,

Bump.  Anybody willing to help please?!

Regards
JMB

SalomeMeca 2021
Ubuntu 20.04, 22.04

Offline

## #3 2008-08-08 09:30:11

Thomas DE SOZA
Guru
From: EDF
Registered: 2007-11-23
Posts: 3,066

### Re: [RESOLU] 3D model with rigid bar elements and a point mass

Hi,

From what I understand, you might get around your problem with a simple function in Code_Aster. It is AFFE_CHAR_MECA/LIAISON_ELEM/OPTION='3D_POUTRE'.

It lets you connect a beam element to a 3D face. This is quite useful when modelling a slender structure which requires 3D refinement only on a small part and where the remaining part can be modelled with a beam element.

In your case it is also useful since you won't need as many rigid bars as there are nodes. All you have to do is create a simple POU_D_E or POU_D_T element lying on an edge then connect it to the 3D face.

Another solution could be to set a LIAISON_SOLIDE on the 3D face (that is make it rigid) and have a DISCRET element with the first end connected (in the mesh) to one point of the face and the other to the point mass.

In every case, it saves the hassle of defining as many bars as there are nodes on the 3D face.

TdS

Offline

## #4 2008-08-08 10:10:34

JMB365
Member
Registered: 2008-01-19
Posts: 781

### Re: [RESOLU] 3D model with rigid bar elements and a point mass

Thomas DE SOZA wrote:

Hi,

From what I understand, you might get around your problem with a simple function in Code_Aster. It is AFFE_CHAR_MECA/LIAISON_ELEM/OPTION='3D_POUTRE'.

It lets you connect a beam element to a 3D face. This is quite useful when modelling a slender structure which requires 3D refinement only on a small part and where the remaining part can be modelled with a beam element.

In your case it is also useful since you won't need as many rigid bars as there are nodes. All you have to do is create a simple POU_D_E or POU_D_T element lying on an edge then connect it to the 3D face.

Another solution could be to set a LIAISON_SOLIDE on the 3D face (that is make it rigid) and have a DISCRET element with the first end connected (in the mesh) to one point of the face and the other to the point mass.

In every case, it saves the hassle of defining as many bars as there are nodes on the 3D face.

TdS

Thank you for your quick reply!  I think I understand your reasoning for using a beam element and connecting it to a single node node on the 3D Block.  The reason I am considering using many bars connecting to many nodes on the volume mesh is because I want to avoid introducing high localized stresses on the 3D block at that one node (connected to the beam element).  Also the real model I am using has numerous tetra10 and Tria6 elements on the face, unlike the simplified diagram I described above.

In the real world all Boundary conditions are distributed over an area.  Correct me if I am approaching this the wrong way.

Regards,
JMB

SalomeMeca 2021
Ubuntu 20.04, 22.04

Offline

## #5 2008-08-08 10:20:06

Thomas DE SOZA
Guru
From: EDF
Registered: 2007-11-23
Posts: 3,066

### Re: [RESOLU] 3D model with rigid bar elements and a point mass

Hi,

The operator AFFE_CHAR_MECA/LIAISON_ELEM/OPTION='3D_POUTRE' will write the necessary linear relations based of the nodes of the 3D face and the beam characteristics. It is not the same as linking directly a beam with a node on the face.

It is widely used in Code_Aster studies. Another example of its use is : if you want to apply a torque load to a 3D structure, you have to use this kind of approach (since 3D elements do not have rotations degrees of freedom).

The only drawback is that it is valid only for small displacements.

TdS

Offline

## #6 2008-08-08 10:27:13

JMB365
Member
Registered: 2008-01-19
Posts: 781

### Re: [RESOLU] 3D model with rigid bar elements and a point mass

Thomas DE SOZA wrote:

Hi,

The operator AFFE_CHAR_MECA/LIAISON_ELEM/OPTION='3D_POUTRE' will write the necessary linear relations based of the nodes of the 3D face and the beam characteristics. It is not the same as linking directly a beam with a node on the face.

It is widely used in Code_Aster studies. Another example of its use is : if you want to apply a torque load to a 3D structure, you have to use this kind of approach (since 3D elements do not have rotations degrees of freedom).

The only drawback is that it is valid only for small displacements.

TdS

Hello,

I very much appreciate your prompt replies!  Thank you for clarifying the use of  the operator AFFE_CHAR_MECA/LIAISON_ELEM/OPTION='3D_POUTRE'.  You have also answered another long standing question I had about trying to apply a torque to a 3D structure.  I will try based on your advice.  Another question: can these beam elements be given a zero mass since I really am trying to simulate a Boundary Condition?   Subsequently I want to run a modal analysis on the model.

Regards,
JMB

Last edited by JMB365 (2008-08-08 10:31:19)

SalomeMeca 2021
Ubuntu 20.04, 22.04

Offline

## #7 2008-08-08 12:06:03

JMB365
Member
Registered: 2008-01-19
Posts: 781

### Re: [RESOLU] 3D model with rigid bar elements and a point mass

Hello,

I tried the AFFE_CHAR_MECA/LIAISON_ELEM/OPTION='3D_POUTRE'  but I am getting an error:

!-----------------------------------------------------------------!
! <F> <MODELISA6_45>                                              !
!                                                                 !
!                                                                 !
!  impossibilite,le noeud poutre  N27  devrait porter le ddl  DX  !
!                                                                 !
!                                                                 !
!                                                                 !
! Cette erreur est fatale. Le code s'arrete.                      !
!-----------------------------------------------------------------!

The node N27 is called "CG" in the attached model and is supposed to be the common node for the bars where the forces in FX, FY & FZ are applied.  Would you kindly take a look at the attached files and tell me where I am doing something wrong.  Thank you.

Regards
JMB

Attachments:

SalomeMeca 2021
Ubuntu 20.04, 22.04

Offline

## #8 2008-08-12 20:08:37

JMB365
Member
Registered: 2008-01-19
Posts: 781

### Re: [RESOLU] 3D model with rigid bar elements and a point mass

Bump!

Help! Anybody...?

Regards,
JMB

SalomeMeca 2021
Ubuntu 20.04, 22.04

Offline

## #9 2008-08-12 21:07:41

AsterO'dactyle
Registered: 2007-11-29
Posts: 413

### Re: [RESOLU] 3D model with rigid bar elements and a point mass

The answer is in the message of AFFE_MODELE:

SUR LES           27 NOEUDS  DU MAILLAGE Mesh_1
ON A DEMANDE L'AFFECTATION DE            1
ON A PU EN AFFECTER                      0

You can't affect the GROUP_NO "CG" with POU_D_T elements (which are only segments SEG2). The only nodes that can be affected by AFFE_MODELE are the discrete ones (with mesh named "POI1").

The node "CG" would be part of SEG2 element for POU_D_T.

Try
FEMLin=AFFE_MODELE(MAILLAGE=Mesh_1,
INFO=1,
AFFE=(_F(PHENOMENE='MECANIQUE',
TOUT='OUI',
MODELISATION='3D'),
_F(PHENOMENE='MECANIQUE',
GROUP_MA='Force',
MODELISATION='POU_D_E')),
);

With CG is a node belongs to GROUP_MA "FORCE"

Code_Asterの開発者

Offline

## #10 2008-08-13 02:28:03

JMB365
Member
Registered: 2008-01-19
Posts: 781

### Re: [RESOLU] 3D model with rigid bar elements and a point mass

AsterO'dactyle wrote:

The answer is in the message of AFFE_MODELE:

SUR LES           27 NOEUDS  DU MAILLAGE Mesh_1
ON A DEMANDE L'AFFECTATION DE            1
ON A PU EN AFFECTER                      0

You can't affect the GROUP_NO "CG" with POU_D_T elements (which are only segments SEG2). The only nodes that can be affected by AFFE_MODELE are the discrete ones (with mesh named "POI1").

The node "CG" would be part of SEG2 element for POU_D_T.

Try
FEMLin=AFFE_MODELE(MAILLAGE=Mesh_1,
INFO=1,
AFFE=(_F(PHENOMENE='MECANIQUE',
TOUT='OUI',
MODELISATION='3D'),
_F(PHENOMENE='MECANIQUE',
GROUP_MA='Force',
MODELISATION='POU_D_E')),
);

With CG is a node belongs to GROUP_MA "FORCE"

Hello,

In Salome I tried to make N27 be called the group "Force" but I get an error message "There are duplicated group names in mesh Mesh_1.  You can cancel exporting and rename them, otherwise some group names in the resulting MED file will not match ones in the study"  Do you want to continue? Yes / No"

This is because I already have a group of faces called "Force" which consist of the elements to which the beam elements should be connected.  So I said "No".

With the change you suggested Code-Aster posts the error:

!-----------------------------------------------------------------!
! <F> <MODELISA6_45>                                              !
!  impossibilite,le noeud poutre  N27  devrait porter le ddl  DX  !
! Cette erreur est fatale. Le code s'arrete.                      !
!-----------------------------------------------------------------!

What I am not understanding is how to connect the nodes of the group "Force" (consisting of faces) with beam elements to the single node N27 which I happened to name "CG".  Perhaps if you could try running the model I have attached to my previous message with a comm file corrected by you, I would very much appreciate it.  I am trying my best to understand the French documentation but it is hard for a non Francophone...  Thank you in advance for your help.

Regards,
JMB

Attachments:

SalomeMeca 2021
Ubuntu 20.04, 22.04

Offline

## #11 2008-08-19 01:50:14

JMB365
Member
Registered: 2008-01-19
Posts: 781

### Re: [RESOLU] 3D model with rigid bar elements and a point mass

Bump!

Regards,
JMB

SalomeMeca 2021
Ubuntu 20.04, 22.04

Offline

## #12 2008-08-19 08:30:22

Archibald Archambaud
Member
From: Clamart, France
Registered: 2007-12-03
Posts: 322

### Re: [RESOLU] 3D model with rigid bar elements and a point mass

Hi JMB,

Your mesh has a problem ; Aster tells it to you :

!--------------------------------------------------------------------------------!
! <A> <MODELISA4_6>                                                              !
!                                                                                !
!                                                                                !
!   -> Phase de vérification du maillage : présence de noeuds orphelins.         !
!      Les noeuds orphelins sont des noeuds qui n'appartiennent à aucune maille. !
!                                                                                !
!                                                                                !
!                                                                                !
! Ceci est une alarme. Si vous ne comprenez pas le sens de cette                 !
! alarme, vous pouvez obtenir des résultats inattendus !                         !
!--------------------------------------------------------------------------------!

=> You hase orphans nodes.

The node you want to use for your LIAISON_ELEM must be part of the beam. You can also try to use the keyword "NOEUD_2='N27'".

Furthermore, in Salome, 2 groups cannot have the same names ; all you have to do is call this node FOO and everything will be OK!

AA

Offline

## #13 2008-08-19 09:05:35

Thomas DE SOZA
Guru
From: EDF
Registered: 2007-11-23
Posts: 3,066

### Re: [RESOLU] 3D model with rigid bar elements and a point mass

Hi,

I looked at your files in the zip archive. Option '3D_POU' requires one group of faces, in your case it is 'Force' and it is OK. It also requires a group of nodes (which in fact must contain only one node), in your case it is 'CG'.
However this node should be part of an element which was given a model (in Code_Aster terminology, that is AFFE_MODELE....). What you did was to use a POU_D_E model and apply it to your group of nodes 'CG'. It is wrong since models can only be applied on finite element that is an edge, a face or a solid.
Moreover the GROUP_MA 'Force' should be given a "3D" model (using TOUT='OUI' is enough) since it is a 2D element lying on a 3D model (we need a model on these elements in order to calculate integral quantities for the '3D_POU' option). The manual also tell that quadratic elements are better in order to have more precise integration (more gauss points --> more precise).

Therefore you have two choices :

1/ Either you make an edge going from the face of the cube to the point 'CG' : this should look like

|
|
|x('CGbis')------x ('CG')
|
|

Note that CGbis is a new point that is not part of the face 'Force'. Then the edge connecting CGbis to CG can be named 'Beam' and be applied a POU_D_E model. AFFE_CARE_ELEM should be used to give the characteristics of the beam (one important thing is that its section is equal to the area of 'Force').

Then in option 3D_POU, GROUP_MA_1 would still be 'Force' and GROUP_NO_2 'CGbis'.

2/ Or (better solution in your case I think) you can create first move your node 'CG' towards the face :

|
|
|x('CG')
|
|

Then you must create a group of elements (GROUP_MA) from your group of nodes 'CG' with the syntax :

``````Mesh_1=LIRE_MAILLAGE(FORMAT='MED',
INFO=2,);

Mesh_2=CREA_MAILLAGE(MAILLAGE=Mesh_1,
CREA_POI1=_F(NOM_GROUP_MA='CG',
GROUP_NO='CG',),
);``````

Mesh_2 will be your new mesh and it will contain a GROUP_MA which is a point which can be applied a discrete element (called a DISCRET in Aster terminology).

``````FEMLin=AFFE_MODELE(MAILLAGE=Mesh_1,
AFFE=(_F(TOUT='OUI',
PHENOMENE='MECANIQUE',
MODELISATION='3D',),
_F(GROUP_MA='CG',
PHENOMENE='MECANIQUE',
MODELISATION='DIS_TR',),
),
);``````

You must input a stiffness matrix for the discrete element since it can't be deduced from the material characteristics and the geometry of the element. Look in the manual for AFFE_CARA_ELEM for more info.
A mass matrix may also be given. I'm not an expert but I think giving it a zero mass can lead to singularity, it can be small though.

You may find similar approach in the test cases SDLV122A and B as well as in SSLX200A (the command files can be found in the "astest" directory of your Code_Aster version, if you happen to use a distribution which did not include them, you can download the latest source package and extract them manually from the Code_Aster archive).

Good luck,

TdS

Last edited by Thomas DE SOZA (2008-08-19 09:07:07)

Offline

## #14 2008-08-19 12:06:45

todd_alan_martin
Member
Registered: 2008-03-06
Posts: 131

### Re: [RESOLU] 3D model with rigid bar elements and a point mass

Hi JMB

This all seems to be getting rather complicated for a simple model.
I had a look at your first mesh and comm files. Please correct me, if I'm wrong. You want a solid block made of tetrahedral elements with an extra node,  called CG, connected via a rigid element to one face.

When Salome meshes a solid, it creates line, surface and volume elements throughout the geometry. I suggest you delete all SEG3 (1D) and TRIA6 (2D) elements in Salome, as you don't need them.
Then you need to create a mass/discrete element called 'CG' on N27 and add N27 to node group 'FORCE'.
Finally change the element group 'FIXED' to a node group, since the 'FIXED' elements have been deleted from the model.

I'm not sure whether code-aster likes you applying MODELISATION='3D' to all elements, so I suggest you create a group representing just the tetrahedral elements called 'BOX'. Then the following should work

FEMLin=AFFE_MODELE(MAILLAGE=Mesh_1,
AFFE=(_F(GROUP_MA='BOX',
PHENOMENE='MECANIQUE',
MODELISATION='3D',),
_F(GROUP_MA='CG',
PHENOMENE='MECANIQUE',
MODELISATION='DIS_TR',),),);

BCnd=AFFE_CHAR_MECA(MODELE=FEMLin,
DDL_IMPO=_F(GROUP_NO='FIXED',
LIAISON='ENCASTRE',),
LIAISON_SOLIDE=_F(GROUP_NO=('FORCE',),),);

I suspect that trying to list multiple node groups in LIAISON_SOLID merely creates multiple rigid bodies, NOT one collective rigid body, but I haven't checked the documentation on this. Now that node group 'FORCE' contains N27, it should work.

Try again and let us know how it goes.
Good luck.
Todd

Offline

## #15 2008-08-20 05:47:20

JMB365
Member
Registered: 2008-01-19
Posts: 781

### Re: [RESOLU] 3D model with rigid bar elements and a point mass

todd_alan_martin wrote:

Hi JMB

This all seems to be getting rather complicated for a simple model.
I had a look at your first mesh and comm files. Please correct me, if I'm wrong. You want a solid block made of tetrahedral elements with an extra node,  called CG, connected via a rigid element to one face.

When Salome meshes a solid, it creates line, surface and volume elements throughout the geometry. I suggest you delete all SEG3 (1D) and TRIA6 (2D) elements in Salome, as you don't need them.
Then you need to create a mass/discrete element called 'CG' on N27 and add N27 to node group 'FORCE'.
Finally change the element group 'FIXED' to a node group, since the 'FIXED' elements have been deleted from the model.

I'm not sure whether code-aster likes you applying MODELISATION='3D' to all elements, so I suggest you create a group representing just the tetrahedral elements called 'BOX'. Then the following should work

FEMLin=AFFE_MODELE(MAILLAGE=Mesh_1,
AFFE=(_F(GROUP_MA='BOX',
PHENOMENE='MECANIQUE',
MODELISATION='3D',),
_F(GROUP_MA='CG',
PHENOMENE='MECANIQUE',
MODELISATION='DIS_TR',),),);

BCnd=AFFE_CHAR_MECA(MODELE=FEMLin,
DDL_IMPO=_F(GROUP_NO='FIXED',
LIAISON='ENCASTRE',),
LIAISON_SOLIDE=_F(GROUP_NO=('FORCE',),),);

I suspect that trying to list multiple node groups in LIAISON_SOLID merely creates multiple rigid bodies, NOT one collective rigid body, but I haven't checked the documentation on this. Now that node group 'FORCE' contains N27, it should work.

Try again and let us know how it goes.
Good luck.
Todd

Hello Todd,

Thank you for your detailed explanation.  Let me clarify why I am trying to create multiple rigid bars.  When I apply force(s) to the node called "CG" I want to have the multiple rigid nodes spread the forces and moments to the entire face of the "Box".  Another reason I do not place this node right on the face is, the effect of the moments will be diminished as a result.  Also I want these multiple rigid bars to have no mass themselves since I will be doing a modal analysis subsequently (without the force(s) acting on this "CG" of course).  Thirdly, this node "CG" needs to have a concentrated mass attached to it (or itself be the concentrated mass), again since the modal frequencies are dependent affected) by it being there.

All of this may seem a complicated approach, but I am trying to accomplish what would be an equivalent of doing this in NASTRAN.  There one would use RBE (Rigid Bar Elements with no mass) to connect to all the nodes of one face of the box, while their opposite ends collectively connect to a concentrated mass.

On the opposite face of the box all the nodes are connected by numerous RBEs again a another single point, where a 6DOF spring simulates the stiffness of the "wall" that this box is attached to.  Again the reason for multiple RBEs is to spread the moments and stresses and the RBE's themselves to not affect the modal analysis to be run subsequently.

I used a simple box as a surrogate in this forum for a more complex 3D shape that I am trying to analyze.  I appreciate your suggestions and will try them and keep you informed of the outcome.  If you have any other suggestions, please let me know.  Thank you.

Regards,
JMB

SalomeMeca 2021
Ubuntu 20.04, 22.04

Offline

## #16 2008-08-20 06:02:44

JMB365
Member
Registered: 2008-01-19
Posts: 781

### Re: [RESOLU] 3D model with rigid bar elements and a point mass

Thomas DE SOZA wrote:

Hi,

I looked at your files in the zip archive. Option '3D_POU' requires one group of faces, in your case it is 'Force' and it is OK. It also requires a group of nodes (which in fact must contain only one node), in your case it is 'CG'.
However this node should be part of an element which was given a model (in Code_Aster terminology, that is AFFE_MODELE....). What you did was to use a POU_D_E model and apply it to your group of nodes 'CG'. It is wrong since models can only be applied on finite element that is an edge, a face or a solid.
Moreover the GROUP_MA 'Force' should be given a "3D" model (using TOUT='OUI' is enough) since it is a 2D element lying on a 3D model (we need a model on these elements in order to calculate integral quantities for the '3D_POU' option). The manual also tell that quadratic elements are better in order to have more precise integration (more gauss points --> more precise).

Therefore you have two choices :

1/ Either you make an edge going from the face of the cube to the point 'CG' : this should look like

|
|
|x('CGbis')------x ('CG')
|
|

Note that CGbis is a new point that is not part of the face 'Force'. Then the edge connecting CGbis to CG can be named 'Beam' and be applied a POU_D_E model. AFFE_CARE_ELEM should be used to give the characteristics of the beam (one important thing is that its section is equal to the area of 'Force').

Then in option 3D_POU, GROUP_MA_1 would still be 'Force' and GROUP_NO_2 'CGbis'.

2/ Or (better solution in your case I think) you can create first move your node 'CG' towards the face :

|
|
|x('CG')
|
|

You must input a stiffness matrix for the discrete element since it can't be deduced from the material characteristics and the geometry of the element. Look in the manual for AFFE_CARA_ELEM for more info.
A mass matrix may also be given. I'm not an expert but I think giving it a zero mass can lead to singularity, it can be small though.

You may find similar approach in the test cases SDLV122A and B as well as in SSLX200A (the command files can be found in the "astest" directory of your Code_Aster version, if you happen to use a distribution which did not include them, you can download the latest source package and extract them manually from the Code_Aster archive).

Good luck,

TdS

Hello Thomas DE SOZA,

I appreciate your explanations and reply.  I cannot use alternative 2 and move the node CG to the face, since that will change the moment created by the forces applied to it.  In the simplistic model I had posted, my intent to apply forces in all three directions was not shown.

I will take your advice and look at the examples you have suggested.  I realize that a stiffness matrix will have to specified and it is my intent to do so, I am just struggling to understand how to do so in Code-Aster.  Also my reply to Todd in this topic (thread) will perhaps clarify why I need to use multiple RBEs (Rigid Bar Elements) in the model, unless you are trying to tell me that the results will be the same by using one beam element.  My thinking is (perhaps incorrect) that using one thick beam element that covers the face will falsify the modal analysis, unless I can give it zero density.   Correct me if I am wrong.

Regards,
JMB

SalomeMeca 2021
Ubuntu 20.04, 22.04

Offline

## #17 2008-08-20 10:15:39

todd_alan_martin
Member
Registered: 2008-03-06
Posts: 131

### Re: [RESOLU] 3D model with rigid bar elements and a point mass

Hi JMB

Are you saying you would normally use multiple RBAR elements or a single RBE2? (I have a NE/Nastran solver)

My assumption was that the LIASON_SOLID command replicated an RBE2, without the need to specify an independent node and with all 6 DOFs constrained. In which case, it should connect the CG node to the face just like an RBE2.

I have now looked at the documentation for LIAISON_SOLID and it isn't clear if my assumption is correct. I hope you can provide some feedback after trying it.

Todd.

Offline

## #18 2008-08-20 14:23:34

JMB365
Member
Registered: 2008-01-19
Posts: 781

### Re: [RESOLU] 3D model with rigid bar elements and a point mass

todd_alan_martin wrote:

Hi JMB

Are you saying you would normally use multiple RBAR elements or a single RBE2? (I have a NE/Nastran solver)

My assumption was that the LIASON_SOLID command replicated an RBE2, without the need to specify an independent node and with all 6 DOFs constrained. In which case, it should connect the CG node to the face just like an RBE2.

I have now looked at the documentation for LIAISON_SOLID and it isn't clear if my assumption is correct. I hope you can provide some feedback after trying it.

Todd.

Hello Todd,

Thank you for your email.  I do not have NASTRAN, so I am not exactly sure how it works.  What I know is, that I am supposed to use RBE3/RBE2 for constraining one side of the "Box" but connected to one spring element with 6DOFs or perhaps 6 spring elements each providing 1DOF.  I can compromise by skipping the 3 rotational DOFs.  I can use RBE3 for the stress analysis and RBE2 for the modal analysis.

The other face of the box needs to be connected to a point mass at a certain distance away from the face so that moments generated by the 3D forces acting on the mass are correctly applied upon that face.

From reading the Hypermesh User Manual it states:

"RBE3 Multi-noded element with one dependent node and a variable number of
independent nodes. Each node contains a coefficient (weighting factor) and a
user-defined degrees of freedom (configuration 56)."

So I suppose, I would use RBE3/RBE2 on the spring side as long as I can define the Kx,Ky,Kz and KRx, KRy & KRz (the Linear and Rotational stiffnesses respectively) for that single end.  For the side that has the mass attached, maybe you can advise whether the use of RBE3/RBE2 would be appropriate, since you have NE/Nastran.

Hope I have clarified what I am trying to accomplish.  If not please ask me.  Thank you very much for all the help you are providing.

Regards,
JMB

Edited to include RBE2/RBE3...

Last edited by JMB365 (2008-08-20 14:51:37)

SalomeMeca 2021
Ubuntu 20.04, 22.04

Offline

## #19 2008-08-21 02:53:00

JMB365
Member
Registered: 2008-01-19
Posts: 781

### Re: [RESOLU] 3D model with rigid bar elements and a point mass

JMB365 wrote:

Hello,

In Salome I tried to make N27 be called the group "Force" but I get an error message "There are duplicated group names in mesh Mesh_1.  You can cancel exporting and rename them, otherwise some group names in the resulting MED file will not match ones in the study"  Do you want to continue? Yes / No"

This is because I already have a group of faces called "Force" which consist of the elements to which the beam elements should be connected.  So I said "No".

Regards,
JMB

The inability to create two groups with dissimilar entities (edge and face) or (face and volume) or any combination of two or more of these cannot be processed correctly by Salome329!  I discovered this PAINFULLY by experimenting with the following process:

sslx200a.mail -> [ASTK Translator] -> sslx200a.mail.med -> [Salome329] -> sslx200a.med -> [ASTK Translator] -> sslx200a-1.mail

using the file from /opt/aster/STA9.2/astest/....  When I compare the original sslx200a.mail file to the final sslx200a-1.mail file I can see the major mess-up!

Hope I am wrong and hope this helps somebody else, before they waste a lot of time...

Regards,
JMB

SalomeMeca 2021
Ubuntu 20.04, 22.04

Offline

## #20 2008-08-21 04:17:09

todd_alan_martin
Member
Registered: 2008-03-06
Posts: 131

### Re: [RESOLU] 3D model with rigid bar elements and a point mass

Hi JMB

I understand what you're trying to do.
I suggested you "add" N27 to the "force" group, NOT create a second group.
Did you delete the 1D and 2D elements in Salome as I mentioned previously?

Forget about the spring and the mass for the moment. Just fix the back face and create a LIAISON_SOLID for the 'force' group. Apply the load to node CG. Make sure your problem solves.

Todd.

Offline

## #21 2008-08-22 05:11:28

JMB365
Member
Registered: 2008-01-19
Posts: 781

### Re: [RESOLU] 3D model with rigid bar elements and a point mass

todd_alan_martin wrote:

Hi JMB
I understand what you're trying to do.
I suggested you "add" N27 to the "force" group, NOT create a second group.
Did you delete the 1D and 2D elements in Salome as I mentioned previously?
Forget about the spring and the mass for the moment. Just fix the back face and create a LIAISON_SOLID for the 'force' group. Apply the load to node CG. Make sure your problem solves.
Todd.

Hello,

I tried what you suggested (removed the spring, mass, 1D & 2D elements and made N27 part of group "Force") and I used:

BCnd=AFFE_CHAR_MECA(MODELE=Model,
DDL_IMPO=_F(GROUP_NO='Fixed',
DX=0.,
DY=0.,
DZ=0.,),
LIAISON_SOLIDE=_F(GROUP_NO='Force',),);

FORCE_NODALE=_F(GROUP_NO='CG',
FX=10.,
MY=2.,
MZ=3.,),);

and I get:

!-----------------------------------------------------------------------!
! <F> <MODELISA8_30>                                                    !
!                                                                       !
!  Erreur utilisateur:                                                  !
!     On cherche à imposer une condition aux limites sur le ddl DX      !
!     du noeud N27.                                                     !
!     Mais ce noeud ne porte pas ce ddl.                                !
!                                                                       !
!     Conseils :                                                        !
!      - vérifier le modèle et les conditions aux limites :             !
!         - le noeud incriminé fait-il partie du modèle ?               !
!         - le noeud porte-t-il le ddl que l'on cherche à contraindre ? !
!                                                                       !
! Cette erreur est fatale. Le code s'arrete.                            !
!-----------------------------------------------------------------------!

!-----------------------------------------------------------------------!
! <F> <MODELISA8_30>!
! !
! Error user:!
! It seeks to impose a boundary condition on DOF DX!
! node N27. !
! But this node does not DOF. !
! !
! Tips:!
! -- Check the model and boundary conditions:!
! -- The offending node is it part of the model? !
! -- Node DOF we are trying to force the door? !
! !
! This error is fatal. The code stops. !
!-----------------------------------------------------------------------!

If I remove N27 from the "Force" group I get:

!-------------------------------------------------------!
! <F> <DVP_1>                                           !
!                                                       !
!    Erreur de programmation : condition non respectée. !
!                                                       !
! Cette erreur est fatale. Le code s'arrete.            !
! Il y a probablement une erreur dans la programmation. !
! Veuillez contacter votre assistance technique.        !
!-------------------------------------------------------!

!-------------------------------------------------------!
! <F> <DVP_1>!
! !
! Programming error: condition not respected. !
! !
! This error is fatal. The code stops. !
! There is probably an error in programming. !
!-------------------------------------------------------!

Mess file of this (first attempt above with N27 part of "Force") is attached.  Any further ideas?  Thank you.

Regards,
JMB

Attachments:

SalomeMeca 2021
Ubuntu 20.04, 22.04

Offline

## #22 2008-08-22 05:49:52

JMB365
Member
Registered: 2008-01-19
Posts: 781

### Re: [RESOLU] 3D model with rigid bar elements and a point mass

Thomas DE SOZA wrote:

Hi,

You may find similar approach in the test cases SDLV122A and B as well as in SSLX200A
Good luck,

TdS

Thank you for the suggestion.  I used SSLX2000A and was able to solve a model.  My model is:

#                o     (N27: CG)
#                |
#                |Bar
#                |
#             ___*____ (N28: ForcePt)
#            |        |
#            |  Box   |(Edges, Faces, Volumes)
#            |________|
#                *     (N29: FixedPt)
#
#   Z Y
#   |/    Global Axes
#   .--X
#
# The "*" represent multiple beams connecting  every node on the face of Box to nodes N28 or N29.
# The "----" represents a single rectangular X-Section "Bar" between nodes N27 "CG" & N28

(A fixed width font will make viewing easier)

There are two problems with the model, yet.

1. It does not contain the point mass at the N27 node called "CG", which I still have not figured out how to include.
2. I really do not want 3D_POU (3D-Beam) elements at both ends.  Earlier I thought that I did, but I was mistaken.  What I really need to do is use the Nastran equivalent of RBE2/RBE3).  Is it LIAISON_SOLIDE that I should use?

In SSLX2000A.comm group "C" has been defined as discrete node "K_TR_D_N" with zero values for all the Kx, Ky, Kz, KRx, KRy & KRz?  Also group "C" has Dx=Dy=Dz=DRx=DRy=DRz=0.  Why would the 6 stiffness & 6DOFs be set to zero?  I can accept 6DOFs being zero, but to me it seems illogical to set the six stiffness values also as zero.  How does the model even work?  Do you (or anybody) have any clues or explanation?

(K_TR_D_N = Translation and Rotation stiffness matrix "K" using Nodal Diagonal only values)

If you have any suggestions I will be grateful.  Thank you.

Regards,
JMB

SalomeMeca 2021
Ubuntu 20.04, 22.04

Offline

## #23 2008-08-22 11:09:09

todd_alan_martin
Member
Registered: 2008-03-06
Posts: 131

### Re: [RESOLU] 3D model with rigid bar elements and a point mass

Hi

You probably need to assign a DIS_TR modelisation to N27 (node group CG) in AFFE_MODELE
and a DISCRETE element (K_TR_D_N) property to N27 in AFFE_CARA_ELEM with (0.,0.,0.,0.,0.,0.)
Did you do that?

Otherwise, N27 is not part of the mesh.

Offline

## #24 2008-08-22 15:05:43

JMB365
Member
Registered: 2008-01-19
Posts: 781

### Re: [RESOLU] 3D model with rigid bar elements and a point mass

todd_alan_martin wrote:

Hi

You probably need to assign a DIS_TR modelisation to N27 (node group CG) in AFFE_MODELE
and a DISCRETE element (K_TR_D_N) property to N27 in AFFE_CARA_ELEM with (0.,0.,0.,0.,0.,0.)
Did you do that?

Otherwise, N27 is not part of the mesh.

Hello,

Thank you for your remarks.  Now I have done DIS_TR and K_TR_D_N for N27.   I am still encountering errors.  I tried 2 ways, N27 (CG) is part of node group "Force" and also NOT part of "Force".  I get two different error messages as shown below:

------  LISTE DES GROUPES DE NOEUDS       ------
1  Fixed            9         1         2         3         4         9
10        11        12        21
2  CG               1        27
3  Force           10        27         5         6         7         8
13        14        15        16        22

!-------------------------------------------------------!
! <F> <JEVEUX_57>                                       !
!                                                       !
! Longueur du segment de valeurs <E0> allouer invalide 0. !
!                                                       !
! Cette erreur est fatale. Le code s'arrete.            !
!-------------------------------------------------------!

------  LISTE DES GROUPES DE NOEUDS       ------
1  CG               1        27
2  Fixed            9         1         2         3         4         9
10        11        12        21
3  Force            9         5         6         7         8        13
14        15        16        22

!--------------------------------------------!
! <F> <FACTOR_21>                            !
!                                            !
! Matrice non factorisable :                 !
!   pivot vraiment nul <E0> la ligne : 175   !
!   pour le noeud N27 et la composante DX    !
!                                            !
! Cette erreur est fatale. Le code s'arrete. !
!--------------------------------------------!

By the way, I attach the mess file because it shows all the lines of the comm file in the beginning and also info about the mesh, groups, error messages etc.  Hope you will agree, if not please tell me why.

I wonder if we can hear from some developers about this issue, since I have been trying for a long time to solve this problem.  I am beginning to wonder if there is a bug?

Regards,
JMB

Attachments:

SalomeMeca 2021
Ubuntu 20.04, 22.04

Offline

## #25 2008-08-24 06:57:40

todd_alan_martin
Member
Registered: 2008-03-06
Posts: 131

### Re: [RESOLU] 3D model with rigid bar elements and a point mass

Hi JMB

------  LISTE DES GROUPES DE NOEUDS       ------
1  Fixed            9         1         2         3         4         9
10        11        12        21
2  CG               1        27
3  Force           10        27         5         6         7         8
13        14        15        16        22

!-------------------------------------------------------!
! <F> <JEVEUX_57>                                       !
!                                                       !
! Longueur du segment de valeurs <E0> allouer invalide 0. !
!                                                       !
! Cette erreur est fatale. Le code s'arrete.            !
!-------------------------------------------------------!

In AFFE_CARA_ELEM try making DISCRET->VALE (0.,0.,0.) instead of (0.,0.,0.,0.,0.,0.)

>By the way, I attach the mess file because it shows all the lines of the comm file in the beginning and >also info about the mesh, groups, error messages etc.

Good point. I should have looked at it.

Todd.

Offline