[SOLVED] Bolt pretension lock

JanBlokes · 2021-11-04 15:44:44

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

Last edited by JanBlokes (2021-12-09 16:12:11)

jeanpierreaubry · 2021-11-04 17:09:30

hello

how do you apply the pretension?

jean pierre aubry

mf · 2021-11-05 08:21:45

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)

JanBlokes · 2021-11-05 12:03:12

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

Attachments:
simple_bracket.PNG, Size: 99.4 KiB, Downloads: 242

jeanpierreaubry · 2021-11-08 08:26:46

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

JanBlokes · 2021-11-08 20:37:04

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

JanBlokes · 2021-11-14 20:26:48

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

Attachments:
preten.pdf, Size: 163.19 KiB, Downloads: 259

JanBlokes · 2021-11-14 20:29:31

The .med and .comm file are here.

Attachments:
bracket.tar, Size: 340 KiB, Downloads: 179

Maggoo · 2021-11-15 00:52:12

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

Attachments:
BoltPret.zip, Size: 5.99 KiB, Downloads: 184

Volker · 2021-11-15 12:16:05

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?

jeanpierreaubry · 2021-11-15 14:17:06

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

JanBlokes · 2021-11-25 10:28:08

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

jeanpierreaubry · 2021-11-26 15:24:00

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

JanBlokes · 2021-11-26 22:34:01

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 coefficient
i 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

jeanpierreaubry · 2021-11-27 09:04:00

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

Attachments:
bolt_pretens-temp.zip, Size: 15.82 KiB, Downloads: 240

JanBlokes · 2021-11-28 13:32:05

jeanpierreaubry wrote:

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

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

jeanpierreaubry · 2021-11-30 09:03:28

there are several ways to apply the TEMP load which is a nodal load

on the whole bolt length
only on the center node
on the whole bolt length excluding the two ends connected to the LIAISON_SOLIDE
experiment with that!

forgetting the SANS_GROUP_NO should produce a failure on the very first step of the calculation

finally there is a proverb that says
"alone one goes faster, together one goes farther"
i would add concerning the scientific matter
"alone one usually goes nowhere"!

JanBlokes · 2021-12-09 16:11:28

jeanpierreaubry wrote:

there are several ways to apply the TEMP load which is a nodal load
on the whole bolt length
only on the center node
on the whole bolt length excluding the two ends connected to the LIAISON_SOLIDE
experiment with that!
forgetting the SANS_GROUP_NO should produce a failure on the very first step of the calculation
finally there is a proverb that says
"alone one goes faster, together one goes farther"
i would add concerning the scientific matter
"alone one usually goes nowhere"!

I'm sorry for the late response, probaly cancelled notifications.

Thank you very much for your hints! They are very useful. Regarding the proverb - I fully agree with that

vietazz · 2022-08-10 15:04:14

jeanpierreaubry wrote:

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

Dear Jean Pierre,

Thank you for the valuable files, they're really helped me.
I reproduce your case, it works just fine using DKT.
But when I change it to COQUE_3D. Of course i converted the mesh to quadratic and then QUAD9, also I converted the bolt lines to lineare mesh since POU_D_T works only with SEG2 elements.

You can find the figure of comparaison attached.

Thank you very much,

Regards

Attachments:
figure_comp.png, Size: 371.5 KiB, Downloads: 86

jeanpierreaubry · 2022-08-10 16:22:24

hello vietazz

why do you want to use COQUE_3D?
what is the advantage over DKT?

jean pierre aubry

vietazz · 2022-08-11 14:56:33

Hello Jean Pierre,

Thank you for your quick answer.
I am trying to add bolts to another model that has been built using COQUE_3D.
To my anderstanding, COQUE_3D is adapted to geometries with high curvature.

Best regards,

#1 2021-11-04 15:44:44

[SOLVED] Bolt pretension lock

#2 2021-11-04 17:09:30

Re: [SOLVED] Bolt pretension lock

#3 2021-11-05 08:21:45

Re: [SOLVED] Bolt pretension lock

#4 2021-11-05 12:03:12

Re: [SOLVED] Bolt pretension lock

#5 2021-11-08 08:26:46

Re: [SOLVED] Bolt pretension lock

#6 2021-11-08 20:37:04

Re: [SOLVED] Bolt pretension lock

#7 2021-11-14 20:26:48

Re: [SOLVED] Bolt pretension lock

#8 2021-11-14 20:29:31

Re: [SOLVED] Bolt pretension lock

#9 2021-11-15 00:52:12

Re: [SOLVED] Bolt pretension lock

#10 2021-11-15 12:16:05

Re: [SOLVED] Bolt pretension lock

#11 2021-11-15 14:17:06

Re: [SOLVED] Bolt pretension lock

#12 2021-11-25 10:28:08

Re: [SOLVED] Bolt pretension lock

#13 2021-11-26 15:24:00

Re: [SOLVED] Bolt pretension lock

#14 2021-11-26 22:34:01

Re: [SOLVED] Bolt pretension lock

#15 2021-11-27 09:04:00

Re: [SOLVED] Bolt pretension lock

#16 2021-11-28 13:32:05

Re: [SOLVED] Bolt pretension lock

#17 2021-11-30 09:03:28

Re: [SOLVED] Bolt pretension lock

#18 2021-12-09 16:11:28

Re: [SOLVED] Bolt pretension lock

#19 2022-08-10 15:04:14

Re: [SOLVED] Bolt pretension lock

#20 2022-08-10 16:22:24

Re: [SOLVED] Bolt pretension lock

#21 2022-08-11 14:56:33

Re: [SOLVED] Bolt pretension lock

Board footer