Contact between rubber and steel
Grzegorz Pawlik
I have problem with simulation of contact between rubber and steel parts. After some period of time, when rubber is pushed on the steel part, some instabilities in rubber occur and high deformations of elements are visible:
Of course beacuse of that calculations are terminated.
Below you can find some basic information regarding both parts.
RUBBER:
mat: MAT077_H-HYPERELASTIC_RUBBER,
elements: tetra 1st order
ELFORM=13
STEEL PART:
mat: MAT024
elements: tetra 2nd order
ELFORM=16
Contact AUTOMATIC_SURFACE_TO_SURFACE is used to simulate contact between these parts.
I have already checked SOFT=0, SOFT=1 and SOFT=2, but it didn't solve the problem.
Could you give me some advice how to deal with that issue?
Thanks in advance.
Regards,
Greg
punith ml
--
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 on the web visit https://groups.google.com/d/msgid/ls-dyna2/c8e872df-ef11-2d60-f8b1-265286e8f4d7%40gmail.com.
Rajesh Kumar
On 5. Oct 2021, at 03:09, punith ml <punit...@gmail.com> wrote:
To view this discussion on the web visit https://groups.google.com/d/msgid/ls-dyna2/CACEy9fOugccU%2BR5ixR4N%2BFAkwwrMDKFsebu%3DFZR-UNpPzgtsrg%40mail.gmail.com.
James M. Kennedy
Dear Greg,
---------------------------------
Some notes on the two tetrahedron formulations you indicated that you were using.
elform=13 (1 point nodal pressure tetrahedron) has no volumetric locking under plastic flow conditions. This element formulation is automatically assigned when 3D R-adaptivity is invoked for bulk forming/forging simulations.
elform=16 (10-node quadratic tetrahedron) has weight factors of the nodes that are not proportionally correct (not equal). This non-proportional weighting is not taken into account when distributing external forces or contact forces.
With an applied pressure, the external forces are applied equally to each triangular loaded segments. Results can be dependent on whether you use segments with no midside nodes (only corner nodes) or segments (four times as many segments) including all the midside nodes. The net force is the same in either case; however, defining load segments which include midside nodes is generally recommended.
If a part id (PID) is used for defining the contact segment entries when using the *CONTACT_AUTOMATIC_xxxx option, four triangular contact segments are automatically generated for each exterior tetrahedron face. If preferred, contact segment sets of four segments per tetrahedron face can also be created manually. Either approach will deliver a portion of the contact load to the midside nodes. Contact segments which do not include the midside nodes (only corner nodes) is not generally recommended.
4 or 5 point numerical integration is available as described in Zienkiewicz [1977] (Section 8.10 Numerical Integration-Triangular or Tetrahedron Regions).
The displacement field for the 10-node quadratic tetrahedron is quadratic while the strain field is linear (pure bending can be modeled).
---------------------------------
For complex solid structures, tetrahedron elements are generally employed; elform=4, 10, 13, 16, or 17 are the available options (any of these formulations are preferable to using degenerate elform=1 tetrahedrons). elform=16/17 are the most accurate tetrahedrons; however, not arbitrarily suited for large strains (due to limitation on the strain increment). elform=13 needs a finer mesh, yet well suited for large strains (need to check if desired material model is supported).
For metals or plastics, with moderate strains, use elform=4, 13, 16, or 17.
For rubber materials, with incompressible, large strains, use elform=13.
For bulk metal forming problems, use elform=13 with 3D r-adaptivity.
---------------------------------
Sincerely,
James M. Kennedy
KBS2 Inc.
October 5, 2021
To view this discussion on the web visit https://groups.google.com/d/msgid/ls-dyna2/CACEy9fOugccU%2BR5ixR4N%2BFAkwwrMDKFsebu%3DFZR-UNpPzgtsrg%40mail.gmail.com.
Grzegorz Pawlik
Rajesh, Len, Punith, James thank you very much for feedback and advices.
I have already made some investigations. I have checked:
- lower timestep (-1e-7)
- steel parts as mat_rigid with lower stiffness
- BSORT=10
- contact MORTAR
- different settings for parameters: SOFT, SBOPT and DEPTH
- HEXA mesh (reduced and full integration) and CONTROL_HOURGLASS (IHQ=1 QH=0.1)
but there are still the same problems with rubber part.
There is not negative volume error, but:
Now I want to check ELFORM=10 for rubber part, because it looks more stable in submodel.
Regards,
Greg
James M. Kennedy
Dear Greg,
-------------------------------
Some comments regarding your error message:
*** termination due to out-of-range forces
number of nodes having out-of-range forces
-------------------------------
A note taken from the LS-DYNA support site:
http://www.dynasupport.com/faq/general/have-you-any-tips-on-how-to-to-combat-instability
“First and foremost, use the latest version/revision of LS-DYNA available.”
-------------------------------
Please see if the following “general” suggestions helps:
1. Velocities reported as NaN (Not a Number) indicate that the analysis has gone
unstable for any number of reasons. Tracking the root cause of NaNs reported late
in the calculation can be difficult. Nevertheless, by activating ISNAN (*CONTROL_
SOLUTION), nodes with force or moment arrays are reported (out-of-range ...) in
the message files.
*CONTROL_SOLUTION
$# soln nlq isnan lcint lcacc ncdcf
$ 0 0 0 100 0 1
0 0 1 100 0 1
*** termination due to out-of-range forces
number of nodes having out-of-range forces 8056
-------------------------------
It would appear that you have a numerical instability.
http://ftp.lstc.com/anonymous/outgoing/support/FAQ/instability.tips
https://www.dynasupport.com/howtos/material/negative-volume-in-soft-materials
-------------------------------
Some possibilities for the instability:
http://www.dynasupport.com/tutorial/contact-modeling-in-ls-dyna/how-contact-works/
Though sometimes it is convenient and effective to define a single contact that will handle any potential contact situation in a model, it is permissible to define any number of contacts in a single model. It is generally recommended that redundant contact, i.e., two or more contacts producing forces due to the same penetration, be avoided by the user as this can lead to numerical instabilities.
To enable flexibility for the user in modeling contact, LS-DYNA presents a number of contact types and a number of parameters that control various aspects of the contact treatment. In the following sections, contact types are first discussed with recommendations regarding their application. A description of the contact parameters then presented.
http://www.dynasupport.com/faq/contact/have-you-any-tips-on-how-to-to-combat-instability/
Contact. Set number of cycles between bucket sorts to zero so that the default sort interval will be used. If the relative velocity between two parts in contact is exceptionally high, it may be necessary to reduce the bucket sort interval (for instance to 5, 2, or even 1). If visible contact penetrations develop during the simulation, switch to *contact_automatic_ surface_to_surface or *contact_automatic_single_surface with SOFT set to 1. Make sure geometry takes into account thickness of shells. If shells are VERY thin, e.g., less than 1 mm, scale up or set the contact thickness to a more reasonable value.
http://www.dynasupport.com/howtos/general/not-a-number-nan-1/
Velocities reported as NaN (Not a Number) indicate that the analysis has gone unstable for any number of reasons. Tracking the root cause of NaNs reported late in the calculation can be difficult.
Nevertheless, by activating ISNAN (*CONTROL_SOLUTION), nodes with force or moment arrays are reported (out-of-range ...) in the message files.
It is always recommended that state data be dumped to the d3plot database more frequently leading up to the instability. This can be done by way of restarting from a D3DUMP or RUNRSF file and changing the output interval in a small restart deck via *CONTROL_BINARY_D3PLOT, or by specifying the output interval via a curve. Having frequent plot states allows the user to see the evolution of the model instability thus narrowing down its origin.
Examples of root causes are a breakdown of contact, or severely distorting elements arising from nonphysical loads, badly conceived material input, or severe hourglassing. Nonphysical damping parameters can also cause an instability to develop as can a timestep that too large. For parts where large physical deformations are expected, it's best to stick with the default element formulations as those tend to be the most robust.
http://www.dynasupport.com/howtos/contact/shooting-node?
"Shooting node logic" can be beneficial in the case where a slave node suddenly finds itself well behind it's master segment (whereas there was no penetration in the preceding cycle). In such a case, the logic prevents a huge contact force that might otherwise cause an instability. The penetrating node is simply placed back on the master surface.
-------------------------------
Sincerely,
James M. Kennedy
KBS2 Inc.
October 8, 2021
p.s.
2. It is always recommended that state data be dumped to the d3plot database more frequently leading up to the instability. This can be done by way of restarting from a D3DUMP or RUNRSF file and changing the output interval in a small restart deck via *CONTROL_BINARY_D3PLOT, or by specifying the output interval via a curve. Having frequent plot states allows the user to see the evolution of the model instability, thus narrowing down its origin.
To view this discussion on the web visit https://groups.google.com/d/msgid/ls-dyna2/b7a46722-9f1f-7774-f518-238f288a9339%40gmail.com.
