Implicit analysis

[Manuel Umanzor]

Hello group,

I recently started performing some simulations using the implicit solver, and fortunately there is a really good guide on the dyna support website:

Some guidelines for implicit analyses using LS-DYNA — Welcome to the LS-DYNA support site  

After reading the guides and following the examples provided, I was able to set up my own models, however I still have a few doubts, hopefully someone in the group is familiar with these guides. Particularly, the guides have some recommendations as to how to synchronize the simulation time with loading, however, I am not sure how to create the curve should I need to create one from scratch (this curve is used in the *CONTROL_IMPLICIT_AUTO card).

Another issue that I have encountered is a warning message regarding the *DATABASE_BINARY_INTFOR card, when I star the simulation I get the following message:

"*DATABASE_BINARY_INTFOR keyword found but "s=" is not present in command line. Submit job anyway?"

Any advice is always greatly appreciated.

Sincerely,

Manuel Umanzor

[l...@schwer.net]

As for your *DATABASE_BINARY_INTFOR question, from the User Manual Volume I:

 

INTFOR --- Contact interface database. The intfor database does not have a

default filename, so it must either be given a filename using the FILE

option or using "S=" on the execution line. Also see *CONTACT

fields SPR and MPR.

 

                --len

--
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-dyna2/368aaab8-0044-4d26-abc6-69d4499ef2e4n%40googlegroups.com.

[James M. Kennedy]

Dear Manuel,

 

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

 

In the following Examples Manual,

 

Kennedy, J.M., "Introductory Examples Manual for LS-DYNA Users", Livermore Software

Technology Corporation, Livermore, California, June, 2013.

http://ftp.lstc.com/anonymous/outgoing/jday/manuals/Intro_Examples_Manual_DRAFT.pdf

 

please see 6. Straight Cantilever Beam with Axial End Point Load and its Notes (included

here for your convenience):

 

Notes:

 

1. Using the default values, with an initial time step dt0=0.010, the problem stops at the 12th

iteration due to an energy increase. The *CONTROL_IMPLICIT_GENERAL, *CONTROL_

IMPLICIT_SOLUTION, and *CONTROL_IMPLICIT_SOLVER, with no automatic time

stepping (*CONTROL_IMPLICIT_AUTO) are considered to be the default keywords.

 

2. Allowing more iterations (*CONTROL_IMPLICIT_SOLUTION) will not help to solve the

problem.

 

3. To resolve the energy increase and termination stated above, include the automatic time

stepping (*CONTROL_IMPLICIT_AUTO) entry, in particular the specification of dtmax.

The following situations occur when using different values of dtmax:

 

dtmax =blank (10*dt0) or 0.100 (these are actually the same); the current step size will increase

right off, eventually two energy increases will occur, where time steps are then decreased, with

the simulation then continuing until termination is reached. This takes the least iterations with

ASCII result plots somewhat noisy.

 

dtmax =0.010 (the initial time step); solves very nicely with no energy increases, takes about 50

percent more iterations than dtmax=0.100, with smoother ASCII result plots.

 

dtmax =0.001 yielded the same results as dtmax =0.010. dt0 appeared to still be considered in

the time step options.

4. It is also possible to achieve a successful solution specifying an initial time step of dt0=0.001

and a similar value for the maximum allowable time step (dtmax=0.001 in the *CONTROL_

IMPLICIT_AUTO keyword). Using these parameters will increase the number of iterations

significantly.

 

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

 

Another note which may be of interest:

 

https://www.d3view.com/automatic-timestep-control-for-implicit-simulations/

 

Automatic Timestep Control for Implicit Simulations

September 11, 2006 | by Suri Bala

 

LS-DYNA IMPLICIT

 

The known advantage with implicit simulations is that the solution is unconditionally stable

allowing larger values of timestep. In implicit static simulations (IMASS=0 in *CONTROL_

IMPLICIT_DYNAMICS), the simulation time has no real significance but is rather an in-

dication of the applied load magnitude. For example if we have a simulation where a load is

applied linearly such that it reaches 100% of its magnitude at the termination time of 100

seconds and the current simulation time is 20 seconds using an arbitrary timestep of 1 second,

then we can interpret that our load (assuming linear scale) is 20% of its maximum load. In the

case of implicit dynamic simulations (IMASS=1) time takes real meaning and unlike explicit

solution, the timestep is unconditionally stable and thus allows us to choose a large timestep.

 

By default, LS-DYNA uses a constant implicit timestep, specified using DT0 in *CONTROL_

IMPLICIT_GENERAL , for the entire duration of the simulation time. The magnitude of

DT0 is usually choose as a fraction of the total simulation time and is entirely dependent on

the nonlinearity of the problem. Using a constant timestep is very conservative in nature since

irrespective of the number of iterations each timestep was required to converge, the timestep

is unchanged and this may result in large number of expensive iterations. For a problem whose

non-linearity is unknown, this is actually not a bad thing since smaller timesteps pose lesser

nonlinearity issues and may be easier to converge. However, once the user becomes familiar

with a problem, careful usage of automatic implicit timestep control in LS-DYNA is a very

good alternative to reduce the number of iterations thereby reducing the simulation time.

 

Automatic timestep control is activated using *CONTROL_IMPLICIT_AUTO by setting

AUTO = 1. The built-in logic in LS-DYNA then takes over to ‘auto-adjust’? the timestep

and the logic is purely based on the number of iterations that was taken at the current timestep.

The parameter ITEOPT (default is 11) allows the user to specify an ‘optimum’? number of

iterations which is to be used to decide where a auto-adjust the current timestep. If the number

of iterations to converge at the current timestep is greater than ITEOPT, LS-DYNA then

reduces the current timestep (using a built in scale-factor) in an attempt to reduce the non-

linearity of the problem. However, if the number of iterations at the current timestep is less

than ITEOPT, LS-DYNA then increases the current timestep (using a built-in scale-factor)

assuming the problem is getting in easier to solve. To allow some tolerance to the value of

ITEOPT, the parameter ITEWIN is a very useful feature which prevents LS-DYNA to hastily

auto-adjust the timestep. When ITEWIN is defined (default is 15) and the number of iter-

ations at the current timestep falls in the rage of ITEOPT +/- ITEWIN, then LS-DYNA by-

passes the auto-adjust of the timestep. This is shown in the following figure.

 

AutoAdjust

 

To provide a minimum allowable timestep size that LS-DYNA can auto-adjust to, the para-

meter DTMIN can be specified. To defined maximum allowable timestep, there are two

possible ways using the parameter DTMAX. When DTMAX is greater than zero, then

LS-DYNA will not auto-adjust such that the timestep is either equal to or below DTMAX.

When DTMAX is less than zero, it then refers to a load curve which can be used to define

a variable maximum allowable timestep. This is illustrated in the following figure.

 

variable implicit dtmax

 

A Few Important Notes on Using Automatic Timestep Control

As mentioned above, the auto timestepping is purely based on the number of iterations that

was taken at the current timestep. It does not understand any issues related to contact-impact

interactions. For cleaner contact interaction, a smaller timestep is preferable which when vio-

lated, results in contact breakdown or instability due to the application of large penalty forces.

To aid better contact treatment while maximizing the advantages of auto-timestepping feature,

the value of DTMAX must be carefully chosen such that large values do not cause contact

difficulties. In the case of contact breakdown, LS-DYNA may still converge and yield a

solution but with interpenetration which should be avoided. Unless a user becomes familiar

with a problem, a constant timestep is a safer method and as the experience with the problem

increases, a good auto time stepping can significantly reduce simulation time while main-

taining the accuracy of the solution.

 

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

 

Three examples using * CONTROL_IMPLICIT_AUTO (plus solutions):

 

https://www.dynaexamples.com/implicit/exercises8_solutions.pdf/

 

https://www.dynaexamples.com/implicit/basic-examples/basics-ii

https://www.dynaexamples.com/implicit/basic-examples/springback-i

https://www.dynaexamples.com/implicit/basic-examples/springback-ii

 

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

 

Sincerely,

James M. Kennedy

KBS2 Inc.

March 2, 2021

 

 

From: ls-d...@googlegroups.com [mailto:ls-d...@googlegroups.com] On Behalf Of Manuel Umanzor
Sent: Monday, March 01, 2021 7:36 PM
To: LS-DYNA2 <ls-d...@googlegroups.com>
Subject: [LS-DYNA2] Implicit analysis

 

Hello group,

--

[Manuel Umanzor]

Hello Dr. Schwer,

Thanks for sharing these notes, I added the missing information to the execution line, and now I see the intfor results as well.

Sincerely,

Manuel

To view this discussion on the web visit https://groups.google.com/d/msgid/ls-dyna2/004101d70f71%24cffa08b0%246fee1a10%24%40schwer.net.

--

Manuel E. Umanzor, MScEng

PhD Candidate, Materials Science and Engineering

Virginia Tech Foundry Institute for Research & Education

[Manuel Umanzor]

Dear Dr. Kennedy,

Thanks for sending this information, these guides are great. By the way, does element failure play a role in convergence as well? In my model, I am trying to use MAT_124 with data from tests performed in cast aluminum, which suffers from low ductility under tension (just over 3% EL). In contrast, the compressive strength test reaches much higher strains before showing signs of fracture. I tried a few scenarios for the failure strain and I noticed that once my simulation is nearly done I get several "negative eigenvalue" warnings and then the simulation ends in an error. If I keep the eps at fracture from the test as the failure criteria in the FE model, the simulation reaches its termination time, hence, I am wondering if I should use MAT_24 with just the compressive strength data.

Thank you,

Manuel

[James M. Kennedy]

Dear Manuel,

 

See if this is of some help:

 

Johansen, T., et al., "Overview, How to Set Up Implicit Analysis and Improve Convergence", 2016 Nordic LS-DYNA Users Forum, Gothenburg, Sweden, October, 2016.

 

https://www.dynamore.se/en/resources/papers/DmN_UsersC_2016/papers/implicit-analyses-in-ls-dyna.-johansen

 

Implicit analyses in LS-DYNA - ResearchGate

 

Sincerely,

James M. Kennedy

KBS2 Inc.

March 3, 2021