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

You are not logged in.

- Topics: Active | Unanswered

Pages: **1**

**JanBlokes****Member**- From: Ostrava
- Registered: 2018-09-06
- Posts: 26

Hello,

is it possible to lock the pretension of bolt during the static (and dynamic) nonlinear analysis? I have bolts modeled by beam elements.

1. step = assembling with tightening of bolts and frictional contact between two plates

2. step = external loading with signal - I wish to observe the change of pretension during this step

Can anybody confirm that it can be done with ETAT_INIT?

Thank you,

Jan

Offline

**jeanpierreaubry****Guru**- From: nantes (france)
- Registered: 2009-03-12
- Posts: 3,670

hello

how do you apply the pretension?

jean pierre aubry

consider reading my book

freely available here https://framabook.org/beginning-with-code_aster/

Offline

**mf****Member**- Registered: 2019-06-18
- Posts: 270

Hello,

yes, that is possible if you use something like

PRETBOLT = CREA_CHAMP(AFFE=_F(GROUP_MA=('BOLT2_ALL', 'BOLT1_ALL'),

NOM_CMP=('N', ),

VALE=(pretension_M24_8dot8, )),

MODELE=model,

OPERATION='AFFE',

PROL_ZERO='OUI',

TYPE_CHAM='ELGA_SIEF_R')

and a corresponding ETAT_INIT

ETATINIT = CREA_RESU(AFFE=_F(CARA_ELEM=elemprop,

CHAM_GD=PRETBOLT,

CHAM_MATER=fieldmat,

LIST_INST=listr,

MODELE=model),

NOM_CHAM='SIEF_ELGA',

OPERATION='AFFE',

TYPE_RESU='EVOL_NOLI')

I have uploaded an example here ('TEST51....'):

https:__//www.code-aster.org/forum2/viewtopic.php?id=25524 (please remove the __ links are not allowed)

A possible refinement of this model is to use a 3D model of the bolt head, connect the beam to it and use DEFI_CONTACT in the underhead areas. This way you could also 'tune' the friction in the underhead if your model has a lot of lateral displacement (maybe due to changing temperature). Today I would do it this way, not like in the example above, it is worth the additional work.

Mario.

*Last edited by mf (2021-11-05 08:25:05)*

Offline

**JanBlokes****Member**- From: Ostrava
- Registered: 2018-09-06
- Posts: 26

Hello,

thank you for you replies! The picture in attachment shows what I am trying to do. It is a bracket with a mass point attached on the frame which I would like to excite. The frame and bracket are bolted together with 4 beam elements and LIAISON_SOLIDE so far.

To Jean-Pierre:

CREA_CHAMP(AFFE=_F(GROUP_MA=('bolts', ),

NOM_CMP=('N', 'VY', 'VZ', 'MT', 'MFY', 'MFZ'),

VALE=(-50000.0, 0.0, 0.0, 0.0, 0.0, 0.0)),

AFFE_SP=_F(CARA_ELEM=CARELEM),

MODELE=MO,

OPERATION='AFFE',

PROL_ZERO='OUI',

TYPE_CHAM='ELGA_SIEF_R')

The pretension works but I found out the contact between shells does not. I have to study it little bit more.

To Mario:

Great, thank you for the hint! I will investigate your example.

Jan

Offline

**jeanpierreaubry****Guru**- From: nantes (france)
- Registered: 2009-03-12
- Posts: 3,670

hello

to apply pre stress to elements i much prefer to cool them as explained in chapter 10 of my book

the method described here with CREA_CHAMP and CREA_RESU does not seem to be applicable if

the model contains elements with SOUS POINTS i.e. shell elements

or if

the models needs to use DEFORMATION='GROT_GDEP' as is the case with cables

cooling the elements is more versatile and with the ad-hoc ramp on you can apply whatever tension you want at whatever time

of course you need to do a little bit of math before hand to get the proper relation temperature to force

jean pierre aubry

consider reading my book

freely available here https://framabook.org/beginning-with-code_aster/

Offline

**JanBlokes****Member**- From: Ostrava
- Registered: 2018-09-06
- Posts: 26

jeanpierreaubry wrote:

hello

to apply pre stress to elements i much prefer to cool them as explained in chapter 10 of my book

the method described here with CREA_CHAMP and CREA_RESU does not seem to be applicable if

the model contains elements with SOUS POINTS i.e. shell elements

or if

the models needs to use DEFORMATION='GROT_GDEP' as is the case with cables

cooling the elements is more versatile and with the ad-hoc ramp on you can apply whatever tension you want at whatever time

of course you need to do a little bit of math before hand to get the proper relation temperature to force

jean pierre aubry

Hello Jean Pierre,

thank you for your hints I appreciate it.

I'll compare the way with applied normal force (which seems it works) and temperature and will share the results here.

Jan

Offline

**JanBlokes****Member**- From: Ostrava
- Registered: 2018-09-06
- Posts: 26

Hello,

I'm trying to solve the bolt pretension and contact but got stuck and don't know what is wrong. I have 3 options of pretension:

1. TEMPERATURE (according J. P. AUBRY book)

2. AFFE_CHAR_MECA

3. CREA_RESU - ETAT_INIT (according Mario tutorial)

These 3 options are investigated without contact and with contact.

Without contact:

1. TEMPERATURE - the normal force does not correspond to the inserted temperature

2. AFFE_CHAR_MECA - the normal force is OK but does not change with external force (but should change)

3. CREA_RESU - ETAT_INIT - the normal force=pretension is OK in the initial time but then is 0.

With contact:

1., 2., 3. - total nonsense - looks like

Does it exist anything like Adjust to touch in Ansys? It means the initial gap is exactly 0 even if the geometry (nodes) is not exact.

Results are in the attachment. The example will be in other post.

If anyone knows what I am doing wrong please let me know.

Thank you,

Jan

Offline

**JanBlokes****Member**- From: Ostrava
- Registered: 2018-09-06
- Posts: 26

The .med and .comm file are here.

Offline

**Maggoo****Member**- From: Rio de Janeiro, Brazil
- Registered: 2011-12-21
- Posts: 45

Dear Blokes and all,

I have been trying something very similar. See the file attached.

The first approach used a material, in the middle element of the bolt, whose E is temperature dependent. This is getting no promising results.

When I use the second approach, leading to 'rnl2' in the file 'Stage_1.comm', the results are pretty good, losing only .25N in 10000N when the pretension is released. The system is put to rely only in the locking effect of using a middle element with a much higher E. I used a much lower one in the pretensioning phase to allow all the necessary displacements to occur. The steps may be summarised in:

1. Apply the pretension forces to the middle nodes of the bolt, with the middle element using a material with a very low stiffness.

2. Increase the stiffness of this middle element.

3. Release the forces applied in 1..

Unhappily I am not being able, so far, to stabilize a problem with two plates attached via LIAISON_SOLIDE to the extremes of the bolt, but if this is not a problem you are facing, maybe the approach presented will be of some use.

The method is inspired in what is shown in the test case sslv130.

Hope this helps.

Best regards.

Helio

---------------------------------------------------

Helio Carlos Bortolon,

Mech Engr, M.Eng. and Maggoo

---------------------------------------------------

Offline

**Volker****Member**- From: Chemnitz
- Registered: 2016-05-23
- Posts: 86

I have doubt that in your model all prestessed regions are able to deform in a realistic way of.

(Compare with theorem of virtual work)

One example: you have a M12 bolt 8.8.

Then the stress cross-section is 84,3 mm^2 (acc. ISO898-1)

In EC3 you will find a pretension force of F p,C = 47200 N.

The normal stress after prestressing is 560 MPa in the stress cross-section, now.

The yield point of the bolt is 640 MPa.

As long as your connected plates are deformationless in the direction of the thickness you will only reach a additional external force of 7000 N till reaching the yield point (in contrary to 47200 N prestress force)...

3D Solid model?

Offline

**jeanpierreaubry****Guru**- From: nantes (france)
- Registered: 2009-03-12
- Posts: 3,670

hello jan blokes

MAT = DEFI_MATERIAU(ELAS=_F(E=2000000.0,

RHO=7.85e-09,

every engineer is dreaming of such a material

apart that i do not understand yet the 3 chained STAT_NON_LINE

and i have never made a contact between DKT element

jean pierre aubry

consider reading my book

freely available here https://framabook.org/beginning-with-code_aster/

Offline

**JanBlokes****Member**- From: Ostrava
- Registered: 2018-09-06
- Posts: 26

Hello gentlemen,

thank you for all suggestions.

Finally I got the results what I expected but only for flanges with 3D elements. The bolts can be modeled by either beams or 3D elements. For bolt pretension I used approach from Mario with ETAT_INIT. The way with temperature doesn't work so far.

Answers to your posts:

Maggoo: Please see the post from Mario (mf) below and investigate his approach. It works for beam and LIAISON_SOLID way.

Volker: Well, the material is linear and it should behave according this assumption (the only nonlinearity is contact so far). This case is only to find way of modeling in CA and I don't evaluate the bolts according EC standards.

Jean Pierre: 3 chained STAT_NON_LINE for 3 types of bolt pretension. The higher Young's modulus should be affected only value with temperature way. I corrected it but without any change. There is some mistake in my code.

I'm still trying the way with flanges modeled by shell elements. I will report all results after.

Jan

Offline

**jeanpierreaubry****Guru**- From: nantes (france)
- Registered: 2009-03-12
- Posts: 3,670

hello JanBlokes

your troubles are really puzzling me

i have build a smaller, more basic model

and i get the exactly very same results with temperature or pretension

on beams attached to the plates with LIAISON_SOLID

once the same tension is applied i.e. the right temperature on a material with the right modulus and right thermal expansion coefficient

i one wants i can post the problem here

jean pierre aubry

consider reading my book

freely available here https://framabook.org/beginning-with-code_aster/

Offline

**JanBlokes****Member**- From: Ostrava
- Registered: 2018-09-06
- Posts: 26

jeanpierreaubry wrote:

hello JanBlokes

your troubles are really puzzling me

i have build a smaller, more basic model

and i get the exactly very same results with temperature or pretension

on beams attached to the plates with LIAISON_SOLID

once the same tension is applied i.e. the right temperature on a material with the right modulus and right thermal expansion coefficienti one wants i can post the problem here

jean pierre aubry

Dear Jean Pierre Aubry,

well, I have definitely something wrong in model. I know that the way with temperature is used very often in CA. I would appreciate if you post your comparison here

Thank you,

Jan

Offline

**jeanpierreaubry****Guru**- From: nantes (france)
- Registered: 2009-03-12
- Posts: 3,670

hello

here are

the gmsh script to build the geometry

the .med filefrom it

the .comm file

note

2 differents ways of handling the bolt to plate joint

some lines have to be commented or uncommented according to the calculation type

if anything looks stange ask

jean pierre aubry

consider reading my book

freely available here https://framabook.org/beginning-with-code_aster/

Offline

**JanBlokes****Member**- From: Ostrava
- Registered: 2018-09-06
- Posts: 26

jeanpierreaubry wrote:

hello

here are

the gmsh script to build the geometry

the .med filefrom it

the .comm filenote

2 differents ways of handling the bolt to plate joint

some lines have to be commented or uncommented according to the calculation typeif anything looks stange ask

jean pierre aubry

Dear Jean Pierre Aubry,

thank you very much for the perfect example. It is clear now

Mistakes in my example:

1) Regarding temperature pretension - I didn't use the proper groups in CREA_CHAMP and CREA_RESU

2) Contact results - I didn't use SANS_GROUP_NO and that is why the results were so much affected

Have a nice rest of the weekend,

Jan

Offline

Pages: **1**