RE: [LS-DYNA2] Difference between shear deformations in experiment and LS-Dyna
l...@schwer.net
There are number of possible problems with this apparently simple model.
My guess is your material properties are likely not a problem as your model attains nearly the correct ultimate load, i.e. yield stress and hardening are correct
1\ I assume you have contact surfaces defined between the three plates and around the bolts and plate holes?
2\ My first modeling change would be to increase the mesh density of the bolts and plate holes. Modeling circular bolts/holes with straight edged elements requires care and a sufficient number of elements.
3\ In comparing experimental and model load-displacement results, it appears there is some slip, i.e. additional displacement, in the experimental results that is not captured in your model. Perhaps introduce a small gap between the bolts and their holes by shrinking the bolt diameter by a few percent?
4\ As an alternative guess to Item 3, assuming there is “some” tension in the bolts, i.e. compression of the plates, I wonder if the initial load-displacement response is due to over coming friction among the plates?
Good luck, --len
From: ls-d...@googlegroups.com <ls-d...@googlegroups.com> On Behalf Of ??????? ???????
Sent: Sunday, November 17, 2024 4:11 AM
To: LS-DYNA2 <ls-d...@googlegroups.com>
Subject: [LS-DYNA2] Difference between shear deformations in experiment and LS-Dyna
Good afternoon! I am modeling and calculating a bolted joint in LS-Dyna. The joint is a shear joint without bolt pretensioning. The joint consists of three plates connected by two bolts. The actual properties of the plates and bolts were determined by tensile tests. The engineering diagrams were converted to true diagrams and put into LS-Dyna. But, a problem arose, when comparing the actual experiment and the model in LS-Dyna, large differences in shear strain are obtained. For modeling of bolts and plates MAT_024 material map was used. Can you tell me who has faced such a problem and how it can be solved?
--
You received this message because you are subscribed to the Google Groups "LS-DYNA2" group.
To unsubscribe from this group and stop receiving emails from it, send an email to ls-dyna2+u...@googlegroups.com.
To view this discussion visit https://groups.google.com/d/msgid/ls-dyna2/9a65bdc2-f756-4862-b03b-11e7a2516d96n%40googlegroups.com.
James Kennedy
Dear Nikoday,
Perhaps of some interest relating to bolt and plate edge contact
-------------------------------------------------------
Contact between Beam and Shell Elements
In general, *CONTACT_AUTOMATIC_SINGLE_SURFACE, *CONTACT_AUTOMATIC_
GENERAL, or *CONTACT_AUTOMATIC_NODES_TO_SURFACE should handle a beam-
to-shell-surface contact situation. All of these contact types take into account thickness offsets.
The first two contact types mentioned above are single surface contacts and so both the shell
and beams parts should be included on the slave side with the master side being null. For an
automatic_nodes_to_surface contact, the beam part (or its nodes) should be slave, the shell part
(or its segments) should be master. For any of the above, a search is made for penetration of beam
nodes (or more precisely, a sphere around each beam node) through shell surfaces.
If the contact situation is beam-to-shell-EDGE, one might have a problem. In that case, one has
to stick with *CONTACT_AUTOMATIC_GENERAL AND add null beams (low density
beams utilizing *MAT_NULL) along (merged to) the outer edges of the shells. The null beam
part should be added to the slave side of the contact.
-------------------------------------------------------
A relatively new contact which has a short discussion presented here (beam to shell
edge contact with null beams/example provided is also discussed):
http://ftp.lstc.com/anonymous/outgoing/jday/faq/contact.beam-to-shell
An example is also provided here:
http://ftp.lstc.com/anonymous/outgoing/jday/beam_thru_hole.k
This small example illustrates the contact in a beam-to-solid-surface application. Unlike
*contact_automatic_nodes_to_surface, it is clearly able to detect contact anywhere along
the beam length.
-------------------------------------------------------
Be advised that *CONTACT_AUTOMATIC_BEAMS_TO_SURFACE_ID is a node
to surface type contact (b5) which means that the beam must be specified as the slave
entry:
-------------------------------------------------------
*CONTACT_AUTOMATIC_BEAMS_TO_SURFACE_ID
$# cid, title
1
$# ssid, msid, sstyp, mstyp, sboxid, mboxid, spr, mpr
$2, 1, 3, 3, 0, 0, 0, 0
1, 2, 3, 3, 0, 0, 0, 0
-------------------------------------------------------
SSTYP - ID type of SSID:
EQ.0: segment set ID for surface-to-surface contact,
EQ.1: shell element set ID for surface-to-surface contact,
EQ.2: part set ID,
EQ.3: part ID,
EQ.4: node set ID for node to surface contact,
EQ.5: include all for single surface definition.
EQ.6: part set ID for exempted parts. All non-exempted parts are included
in the contact.
For *AUTOMATIC_BEAMS_TO_SURFACE contact either a part set ID or a part ID
can be specified.
-------------------------------------------------------
A second example which illustrates null beams and type 26 contact:
http://ftp.lstc.com/anonymous/outgoing/jday/beam-to-hole-edge.k
-------------------------------------------------------
Some short notes of possible interest:
https://ftp.lstc.com/anonymous/outgoing/support/FAQ_docs/contact_shorter.pdf
https://www.dynasupport.com/tutorial/contact-modeling-in-ls-dyna/contact-types
https://www.dynasupport.com/tutorial/ls-dyna-users-guide/contact-modeling-in-ls-dyna
-------------------------------------------------------
Sincerely,
James M. Kennedy
KBS2 Inc.
November 17, 2024
To view this discussion visit https://groups.google.com/d/msgid/ls-dyna2/002801db3915%24b816f3d0%242844db70%24%40schwer.net.
Николай Водяхин
Yes, I noticed that on the experiment diagram there is some possible slippage at the initial moment, I will try to do some more tests and compare the results
Николай Водяхин
James Kennedy
Dear Nikoday,
The goal of this contribution was to review the different modeling techniques for friction grip bolts in view of their respective spatial discretization, their required contact definitions, their re-stressing application and their load carrying behavior. Moreover, typical problems that arise during explicit and implicit time integration were discussed and solutions to these potential problems were provided. While these potential problems are often overseen in explicit, they become very apparent in implicit simulations when the user runs into convergence problems. This may especially be the case during the pre-stressing phase of the bolts or when the friction grip bolt connection start to slip or fail:
Karajan, N., Gromer, A., Borrvall, T., and Pydimarry, K., "Modeling Bolts in LS-DYNA using Explicit and Implicit Time Integration", 15th International LS-DYNA Users Conference, Dearborn, Michigan, June, 2018.
Karajan, N., Gromer, A., Borrvall, T., and Pydimarry, K., "Modeling Bolts in LS-DYNA using Explicit and Implicit Time Integration", 15th International LS-DYNA Users Conference, Dearborn, Michigan, June, 2018.
Sincerely,
James M. Kennedy
KBS2 Inc.
November 18, 2024
To view this discussion visit https://groups.google.com/d/msgid/ls-dyna2/448516f3-3ca3-4fe4-b146-7d5ffd1f5cc2n%40googlegroups.com.
James Kennedy
Николай Водяхин
Based on the proposed modeling options (types a, b, c, d), my option is D, as I did, but I get these differences
Emine Fulya Akbulut
It seems that your 1 mm of gap in solid model causes in stiffness problem. If you get rid of that gap in the model, then you can see the difference in load.
In addition, you can also use beam element which combines outer plates only.
In order to define contact between beam element and the plate in between you should use *CONTACT_AUTOMATIC_BEAMS_TO_SURFACE.
As a material model of beam, you can use *MAT100 which is for spotweld normally. However, please don't forget to assign these properties:
Below, the diameter of bolt was assumed as 10 mm (TS1: 10 , and TS2:10 )
The next step should be to activate *DATABASE_SWFORC under Database ASCII. With this command you can read shear force acting on the bolt easily.
Don't forget to check penetration, before run the simulation.
I hope, you can find this helpful.
Greetings,
Fulya
Emine Fulya Akbulut
As I mentioned before, you should focus on how stiff your model and experiment.
If you don't want any simplification and want to use solid model, then you can define the diameter of bolt and hole from the standards.
If the hole diameter is 17mm, that refers you use M16 bolt, which means that bolt diameter is 14mm.
Good luck,
Fulya
Николай Водяхин
Between the diameter of the bolt and the hole is provided, as well as in the experiment, but that in the model that in the experiment the bolt rests in the edges of the parts immediately from the 1st stage, ie the plates are immediately shifted to half the size of the gap. In the figure below I have marked in red color where the bolt is in contact with the holes, the arrow indicates the direction of the load.
Emine Fulya Akbulut
Since your model has the similar behavior with experiment, it is clear that your material properties were defined properly (yield stress, ultimate stress and hardening) and you use proper mesh size.
I understand that you want to stick to the measurements and dimensions of the experiments, but sometimes very small differences can lead to significant results.
Therefore, I think it might be better to focus on some dimensional alterations.
Primarily, you can focus on minor diameter of bolt instead of major in simulation to consider this as a simplification of the simulation using such a flat surface to achieve a result obtained with bolt threads.
According to the difference, you can decide how you will continue.
Secondly, you should increase clearance in your model to capture similar slip as in the experiment. Even if you eliminated this gap in the experiment, the curve shows that there is still sliding until 0.25mm displacement.
Could this slip be caused by an insufficiently tightened bolt? Just a question. In that case, I think a small gap between the bolt nut and the plate could be tried.
However, the most reliable evaluation can be made when you have more experimental results. Because sometimes simulations can be more accurate than some experiments :)
Good luck,
Fulya
Николай Водяхин
Thanks for the interesting thoughts and comments! I'll try to tinker with this problem some more, and maybe someone will have some other ideas