site map | contact | login | Protection des données personnelles | Powered by FluxBB | réalisation artaban

You are not logged in.

- Topics: Active | Unanswered

Pages: **1**

Good news! I was able to simulate the modal analysis considering the pretension of the bolts and an initial temperature field of the structure.

Following the advice of Ioannis Christovasilis, I assembled both the stiffness matrix and the geometric stiffness matrix into a "total stiffness" matrix. This is performed with the command ASSEMBLAGE The same procedure is described on pages 21-214 of the book written by Jean Pierre Aubry. I'm grateful to both of them.

Subsequently, I performed a STAT_NON_LINE analysis, where both the bolt pretension and the thermal field are considered as an initial state with ETAT_INIT. The next steps consist in creating the result field with CREA_CHAMP, extraction of the geometric stiffness matrix with CALC_MATR_ELEM(OPTION = 'RIGI_GEOM'), and adding the stiffness matrix to the geometric stiffness matrix to obtain a "total stiffness" matrix K_TOTAL with COMB_MATR_ASSE.

Finally, we can simulate the modal analysis with the command CALC_MODES(MATR_RIGI=K_TOTAL). My next step is to find the response of the structure when it is subjected to forces variable in time, considering the pretension and thermal field.

The list of commands in the .comm file is shown below.

Regards,

Alejandro

```
TermT0 = CREA_CHAMP(AFFE=_F(GROUP_MA=('Group',),
GROUP_NO=('BOLTS_1TOP',...),
NOM_CMP=('TEMP', ),
VALE=(50.0, )),
MODELE=modelT,
OPERATION='AFFE',
TYPE_CHAM='NOEU_TEMP_R')
resther = CREA_RESU(reuse=resther,
AFFE=_F(CHAM_GD=TermT0,
INST=(-1.0, ),
MODELE=modelT),
NOM_CHAM='TEMP',
OPERATION='AFFE',
RESULTAT=resther,
TYPE_RESU='EVOL_THER')
fieldM = AFFE_MATERIAU(AFFE_VARC=_F(EVOL=resther,
GROUP_MA=('Group'),
NOM_VARC='TEMP',
VALE_REF=50.0),
MODELE=modelM)
PREBOLT = CREA_CHAMP(AFFE=(_F(GROUP_MA=('BOLTS_1', ),
NOM_CMP=('N', ),
VALE=(Preload, )),
_F(GROUP_MA=('BOLTS_2',),
NOM_CMP=('N', ),
VALE=(Preload, ))),
MODELE=modelM,
OPERATION='AFFE',
PROL_ZERO='OUI',
TYPE_CHAM='ELGA_SIEF_R')
ETATINIT = CREA_RESU(AFFE=_F(CARA_ELEM=elempro0,
CHAM_GD=PREBOLT,
CHAM_MATER=fieldM,
LIST_INST=InstMecT,
MODELE=modelM),
NOM_CHAM='SIEF_ELGA',
OPERATION='AFFE',
TYPE_RESU='EVOL_NOLI')
ASSEMBLAGE(
MODELE = modelM,
CARA_ELEM = elempro0,
CHAM_MATER = fieldM,
CHARGE = (Loads, Supports ),
MATR_ASSE = (
_F(
MATRICE = CO('K_MAT'),
OPTION = 'RIGI_MECA'
),
_F(
MATRICE = CO('M_MAT'),
OPTION = 'MASS_MECA'
),
_F(
MATRICE = CO('A_MAT'),
OPTION = 'AMOR_MECA'
)
),
NUME_DDL = CO('NUM_DDL')
)
resGeom = STAT_NON_LINE(CARA_ELEM=elempro0,
CHAM_MATER=fieldM,
COMPORTEMENT=_F(DEFORMATION='PETIT',
RELATION='ELAS',
TOUT='OUI'),
CONVERGENCE=_F(ITER_GLOB_MAXI=25,
RESI_GLOB_RELA=0.0001),
ETAT_INIT=_F(EVOL_NOLI=ETATINIT,
INST=-1.0),
EXCIT=(_F(CHARGE=Loads),
_F(CHARGE=Supports)),
INCREMENT=_F(LIST_INST=InstMecT),
METHODE='NEWTON',
MODELE=modelM,
NEWTON=_F(REAC_INCR=1,
REAC_ITER=1),
SOLVEUR=_F(MATR_DISTRIBUEE='OUI',
METHODE='MUMPS',
RENUM='AUTO'))
elgaGeom = CREA_CHAMP(
OPERATION = 'EXTR',
TYPE_CHAM = 'ELGA_SIEF_R',
RESULTAT = resGeom,
NOM_CHAM = 'SIEF_ELGA',
INST=0.0
)
matGeom = CALC_MATR_ELEM(
OPTION = 'RIGI_GEOM',
MODELE = modelM,
CARA_ELEM = elempro0,
SIEF_ELGA = elgaGeom
)
Kgeom = ASSE_MATRICE(
MATR_ELEM = matGeom,
NUME_DDL = NUM_DDL
)
Ktotal = COMB_MATR_ASSE(
COMB_R = (
_F(
MATR_ASSE = K_MAT,
COEF_R = 1.0
),
_F(
MATR_ASSE = Kgeom,
COEF_R = 1.0
)
)
)
modes = CALC_MODES(CALC_FREQ=_F(NMAX_FREQ=5),
IMPRESSION=_F(CRIT_EXTR='MASS_EFFE_UN',
CUMUL='OUI'),
MATR_MASS=M_MAT,
MATR_RIGI=Ktotal,
OPTION='PLUS_PETITE')
```

Thank you for your answer Jean Pierre Aubry.

In my current model, I'm using a linear contact model (LIAISON_MAIL with DNOR option) in the surfaces in contact due to the bolts. Nevertheless, you are right, I don't think it is possible to include such pretension in a linear analysis.

I will start by gluing the joints and check the results, perhaps the structure becomes stiffer, resulting in higher eigenvalues.

Then, I will try the DYNA_NON_LINE to see how it goes.

Regards,

Alejandro

**alealbanesi**- Replies: 3

Hi everyone,

I have the model of a 3D structure (hexahedral mesh), which has a series of bolts with pretension (modeled as beams POU_D_E). This model was successfully simulated with the STAT_NON_LINE command, where the pretension of the bolts was defined as a result with the CREA_RESU command, and such result is loaded as an initial state with the ETAT_INIT command inside the STAT_NON_LINE analysis.

Subsequently, I would like to simulate the dynamic/harmonic analysis to find the response of the structure when it is subjected to a set of forces that are variable in time.

As a first step before the dynamic/harmonic analysis, I'm trying to simulate the modal analysis (eigenvalues and eigenvectors under free vibrations) with the CALC_MODES command. This modal analysis seems to be working, however, I cannot include the pretension of the bolts in such analysis. When observing the results, the bolts seem to relax and I think that results may be wrong.

My questions are:

1) Is there a way to include the pretension of bolts when simulating a modal analysis under free vibrations?

2) What type of analysis should I perform to find the response of the structure when it is subjected to forces variable in time, and consider the pretension of the bolts? I did not find a way to pass an initial state to DYNA_VIBRA analysis.

I would appreciate any comments. Thank you in advance,

Alejandro

mf wrote:

The attached example is an example of such a connection, but it's a stupid example because it is a very poorly designed connection (you should never connect 2 bodies like this :-) ). Pay attention to how the bolt relaxes in t=1, so the before applied pretension is lowered by the bodies being pulled together. In this example the pretension drops from 163kN (DIN 8.8 M24 bolt) in t=0 to 127kN in t=1 when they relax.

Mario.

Hi Mario, thank you for your example, it helped me a lot. I got my bolts configured as Euler beams now, and things are working just fine!

Bolts are working ok, the stress level is correct, and I can see the relaxation in the intermediate time-step. Printing the results in a text file is also very useful!

I had some trouble with thermal loads on the beams (this is something that I also found in an older post made by you). With the help of Johannes, I managed to solve that part of the problem.

Thanks for the great help, regards,

Alejandro

Thank you Johannes_ACKVA! Sorry for my late reply, It took me a while to configure all things the right way, but after several tries, it worked just fine! Your right, I'm running a linear thermal analysis, but the mechanical part is non-linear and has several contacts with Coulomb friction and bolts modeled as Euler beams.

Following your advice, I separated 3d from beams using the GROUP_MA command in both thermal and mechanic analysis. In particular, the AFFE_MATERIAU command in the mechanic analysis seemed to be the most critical part due to the AFFE_VARC option, and once this was correctly configured, the test cases started to work.

Also, one should be very careful with the setup of the time-stepping function to account for the pretightening of the bolts, and the projection of the thermal results on the mechanical model.

Thank you again for the great help, regards,

Alejandro

Hi guys,

I see that this post is several months old, but I'm running into the same issues when modeling bolts as Euler beams.

I have a thermomechanical problem that combines 3D and beam elements, and POU_D_E elements cannot be used in a thermal model. My problem consists of 2 stages, thermal and mechanical. In the mechanical problem, I project the thermal solution field. The problem is that I can't project anything in POU_D_E elements since these are not taken into account in the thermal problem.

In the mechanical problem, is there a way to project the thermal field in the rest of the 3D model, and then manually assign temperatures only to the beam elements?

I assume that one can only use a single AFFE-MODELE and AFFE_MATERIAU statements in a problem, right? Any help is greatly appreciated, regards,

Alejandro

Thank you Mario.

I'm about to test all this in my model. I'll let you know what happens.

Regards,

Alejandro

mf wrote:

If you are interested in the stress distribution WITHIN the bolt you should model the bolt (in 2D or 3D) itself, so it will be something similar to the above example

Hi Mario,

I've studying and testing your files, it is very interesting and helped me a lot. One of the key aspects is the correct use of the time-stepping, so that loads and pretensions are correctly assigned to the model.

I never used DEFI_CONTACT as in your file, I will give it a try. I assume that the COEF_PENA_CONT is imposed so that the bodies do not penetrate one on the other. I've read in the forum that the value of this coefficient is some orders of magnitude higher than the Young modulus, which is the case in your example.

Since your bolts are Euler beams, and the ends are glued to the 3D bodies, there is no need to model contact between the shank of the bolt and the hole, right? In the case of 3D bolts, this contact should be considered or at least replaced with LiASION_MAIL and 'DNOR' option.

I assume that as your modeling the bolts as Euler beams, the pretension is a CREA_CHAMP with TYPE_CHAM='ELGA_SIEF_R' and NOM_CMP=('N', ) (N if for normal I think). In case that the bolts are modeled like 3D solids, which CREA_CHAMP will be the equivalent to your example?

This pretension is then used to create an initial state ETATINIT, that is applied in INST=0.0 of resnon1.

In resnon2, the load CHARGE=glueBOLT is of the type TYPE_CHARGE='DIDI', I've read above that this is to consider the stressed state of the material.

Is this analysis correct? Thank you for your help,

Alejandro

Thank you Mario for your reply and example. I will look into it now.

I'm modeling the bolts as 3D solids because I'm interested in stress distribution. The preload stress is a 75% fraction of the material yield stress. Your right, it is time-consuming not only the geometrical setup (dividing geometry and mesh) but also the nonlinear solver execution. The PRE_EPSI option required dividing the volume mesh of the shank part of the bolt to assign the negative pre-deformation.

I will try your example, and see the effect on the steel plates. Perhaps I am not being careful with the time-steps.

Kind regards,

Alejandro

Hi, I have some questions on using bolts with a preload in Code_Aster. I have been reading many posts in the forum and testing some examples. Apparently, there are many ways to simulate a preload or tightening in a bolt.

I have two steel plates that are connected one on top of the other by 4 bolts. The bolts don't have nuts, the threads are glued with LIAISON_MAIL on the lower plate. I am using contacts with a Coulomb coefficient.

* One option is with AFFE_CHAR_MECA - PRE_EPSI. For what I've read, this is a pre-deformation. However, I don't see that the steel plates are pushed or pressed together as expected on a preload.

* Another option I found is using CREA_CHAMP - TYPE_CHAM='ELNO_SIEF_R'. However, I suspect that this creates a stress field compatible with the preload, but it is not a preload. Again, I don't see that the steel plates are pushed against each other.

* Another is with AFFE_CHAR_MEC_F, and LIAISON_GROUP. I have not tested this option but is in one of the tests on the Code_ASter web page.

Can anyone tell me if one of these options will create pressure between the plates? Which could better suit my need?

Thank you in advance,

Alejandro

Thanks for the help Mario. Things are working ok now. I had a mechanical problem that needed 3 hours and 8 minutes for the solution when running on a single core of my CPU.

In parallel, things are much better:

* When using docker, and configuring (mpi_nbcpu=3/ ncpus=2), 57 minutes are needed for the solution.

* When using docker, configuring (mpi_nbcpu=3/ ncpus=2), and following your advice on (MATR_DISTRIBUEE='OUI' in STAT_NON_LINE) and (PARTITIONNEUR='METIS' in AFFE_MODELE.), 47 minutes are needed for the solution.

In my opinion, the scalability level in this parallel problem is great. Of course, the "mpi_nbcpu" and "ncpus" parameters depend on the CPU type. Cheers,

Alejandro

Great Mario, thank you for your reply.

I will try those options in AFFE_MODELE, and see what happens.

Kind regards,

Alejandro

Hi,

I'm trying to run cases in parallel, and I would like to ask for the correct configuration of "mpi_nbcpu" and "ncpus" variables for a multi-core CPU with one socket. I have an CPU with the I7-8700K, it has 6 cores with 2 threads per core (12 threads total) on one socket

I've successfully installed docker following tianyikillua instructions in GitHUB, all tests run Ok in parallel or sequential mode.

I've been doing some tests with some cases that need approximately 8 hours to compute on a single core using MUMPS. So far, the best configuration tested has "mpi_nbcpu = 3" and "ncpus = 2", and total computational time is 6 hours approximately with MUMPS.

Does anyone have other thoughts about this? Perhaps the limit is the single socket?

Thank you in advance,

Alejandro

**alealbanesi**- Replies: 0

Hello everyone,

I'm a researcher from Argentina. I'm a mechanical engineer, and I have a PhD in Computacional Mechanics.

I've been using Salome_Meca for a few months. In my opinion, it is great software.

In the near future, I would like to create my own user routines and Umats. I'm currently trying to run cases in paralell.

Best regards,

Alejandro

Pages: **1**