Implicit dynamic quasi-static vs. Explicit quasi-static

[j***@gmail.com]

Dear All,

I have some model which didn't converge using standard implicit static analysis: newton-raphson and riks.
My model consists in a 3d frame loaded on top by concentrated forces. The problem involves contact interactions and UEL with stiffness degradation and failure.

I managed to make it run using implicit *Dynamic,application=QUASI-STATIC,initial=NO. However when I compare my results with experimental results I see some differences, namely the numerical model overestimates the maximum load.
I notice that the kinetic energy begins to be very large when failures begin to occur which I think it is OK. ETOTAL = 0 throughout the analysis.

I think that using *DYNAMIC, EXPLICIT and use a large time increment (to approximate a quasi-static analysis) I may see different results than the ones I got using implicit dynamic analysis and maybe closer to the ones I got in my full scale tests because maybe the kinetic effects will be in this case smaller than using implicit. What is your opinion? Many thanks!

Kind regards,

Joao

[Imran Hyder]

Hey,
I'm running quasi-static models in both Standard and Explicit too. I also
have convergence issues with Implicit. However, when the kinetic energy is
too high when using explicit, the generated solution doesn't match
experiments. So you may be able to get a better solution if you make sure
your explicit solution is quasi-static enough.

Good luck!

Post by j***@gmail.com
Dear All,
I have some model which didn't converge using standard implicit static
analysis: newton-raphson and riks.
My model consists in a 3d frame loaded on top by concentrated forces. The
problem involves contact interactions and UEL with stiffness degradation
and failure.
I managed to make it run using implicit
*Dynamic,application=QUASI-STATIC,initial=NO. However when I compare my
results with experimental results I see some differences, namely the
numerical model overestimates the maximum load.
I notice that the kinetic energy begins to be very large when failures
begin to occur which I think it is OK. ETOTAL = 0 throughout the analysis.
I think that using *DYNAMIC, EXPLICIT and use a large time increment (to
approximate a quasi-static analysis) I may see different results than the
ones I got using implicit dynamic analysis and maybe closer to the ones I
got in my full scale tests because maybe the kinetic effects will be in
this case smaller than using implicit. What is your opinion? Many thanks!
Kind regards,
Joao

[w***@gmail.com]

Joao,

In principle, the solution you get in /Standard and /Explicit should be the same (bar practically insignificant numerical differences due to the solution method and finite precision). The higher-than-real load capacity of your structure probably comes from the model itself, either from the element technology, the material/failure model, or both. In general, if your simulation converges in /Standard you should stay with it, /Explicit is a different beast and requires more care when reviewing results (e.g. it doesn't impose equilibrium during solution, so you have to check it yourself). Also, if you set a high increment time in /Explicit you may run into convergence problems, due to the secant method /Explicit uses in the solver.

If I were you I would explore the consequences of "thinning" your element sections by a small percent to model unaccounted damage effects, imperfections, amplification of damage due to dynamic effects etc, rather than changing the solver. This has a clear physical meaning behind it and is thus a valid modeling approach that can be well justified.

Hope this helps,
Fernando






---In ***@yahoogroups.com, <***@...> wrote:

Dear All,

I have some model which didn't converge using standard implicit static analysis: newton-raphson and riks.
My model consists in a 3d frame loaded on top by concentrated forces. The problem involves contact interactions and UEL with stiffness degradation and failure.

I managed to make it run using implicit *Dynamic,application=QUASI-STATIC,initial=NO. However when I compare my results with experimental results I see some differences, namely the numerical model overestimates the maximum load.
I notice that the kinetic energy begins to be very large when failures begin to occur which I think it is OK. ETOTAL = 0 throughout the analysis.

I think that using *DYNAMIC, EXPLICIT and use a large time increment (to approximate a quasi-static analysis) I may see different results than the ones I got using implicit dynamic analysis and maybe closer to the ones I got in my full scale tests because maybe the kinetic effects will be in this case smaller than using implicit. What is your opinion? Many thanks!

Kind regards,

Joao

[João André]

Dear Fernando,

Hi! Many thanks for your reply.
I understand your point. The thing is that I get different results when
using static (NR or Riks) and dynamic (quasi-static).
In the pure static analysis when I use Riks I see a load drop (using a load
proportionality factor) after 81 kN to 80 kN and then the analysis aborts
(but earlier than I want...). If I use NR I can only get up to 81 kN.
However, if I use quasi-static I can get to 100 kN using load control. This
could be because I caught a snap-though behaviour in my structure but when
I compare energies and force vs. displacement graphs I see that for the
static analysis I get larger deformation and larger energies for the same
value of load..... so something else than a pure structural instability
phenomenon is going on.
In 6.3.2 of the Abaqus Analysis User's Manual it is said:
"Quasi-static applications are primarily interested in determining a final
static response. These problems typically show monotonic behavior, and
inertia effects are introduced primarily to regularize unstable behavior.
For example, the statically unstable behavior may be due to temporarily
unconstrained rigid body modes or “snap-through” phenomena. Large time
increments are taken when possible to obtain the final solution at minimal
computational cost. Considerable numerical dissipation may be required to
obtain convergence during certain stages of the loading history."

So I guess using the quasi-static implicit analysis abaqus will add some
dissipation in order to stabilize the solution and this makes the system
resistance larger than what it really is.... just my 50 cents. What do you
think? That's why I'm going to see if a pure dynamic analysis I get
different results more close to the pure static ones....
This issue is not documented elsewhere but I think I'm right. Same
inpfile, same everything, only thing changing is the *STATIC (,
RIKS) or *DYNAMIC, application=QUASI-STATIC. Even the parameters (initial
increment, max increment, min increment are the same).

Many thanks,

Joao

Post by w***@gmail.com
Joao,
In principle, the solution you get in /Standard and /Explicit should be
the same (bar practically insignificant numerical differences due to the
solution method and finite precision). The higher-than-real load capacity
of your structure probably comes from the model itself, either from the
element technology, the material/failure model, or both. In general, if
your simulation converges in /Standard you should stay with it, /Explicit
is a different beast and requires more care when reviewing results (e.g. it
doesn't impose equilibrium during solution, so you have to check it
yourself). Also, if you set a high increment time in /Explicit you may run
into convergence problems, due to the secant method /Explicit uses in the
solver.
If I were you I would explore the consequences of "thinning" your element
sections by a small percent to model unaccounted damage effects,
imperfections, amplification of damage due to dynamic effects etc, rather
than changing the solver. This has a clear physical meaning behind it and
is thus a valid modeling approach that can be well justified.
Hope this helps,
Fernando
Dear All,
I have some model which didn't converge using standard implicit static
analysis: newton-raphson and riks.
My model consists in a 3d frame loaded on top by concentrated forces. The
problem involves contact interactions and UEL with stiffness degradation
and failure.
I managed to make it run using implicit
*Dynamic,application=QUASI-STATIC,initial=NO. However when I compare my
results with experimental results I see some differences, namely the
numerical model overestimates the maximum load.
I notice that the kinetic energy begins to be very large when failures
begin to occur which I think it is OK. ETOTAL = 0 throughout the analysis.
I think that using *DYNAMIC, EXPLICIT and use a large time increment (to
approximate a quasi-static analysis) I may see different results than the
ones I got using implicit dynamic analysis and maybe closer to the ones I
got in my full scale tests because maybe the kinetic effects will be in
this case smaller than using implicit. What is your opinion? Many thanks!
Kind regards,
Joao

--
João André
Engenheiro Civil, Mestre / Civil Engineer, M.Sc.
Bolseiro de Doutoramento / PhD Student
Núcleo de Comportamento de Estruturas / Structural Behaviour Division
Departamento de Estruturas / Structures Department
Laboratório Nacional de Engenharia Civil / National Laboratory for Civil
Engineering
LNEC, Av. Brasil 101, 1700-066 Lisboa / Lisbon, Portugal
Web: http://www.lnec.pt/
E-mail: ***@lnec.pt
Telefone / Phone: [phone]
Fax: [phone]

[Mohamed Sayed]

Hello Joao, 

May i ask you question, when you used the Abaqus implicit (Quasi-static solution) what was the time step, is it one ? you know in the static analysis, the time step is 1.0.

I am asking you this question, becasue i want to use quasi-static analysis and i need to know what should be the time step?

Thanks



On Wednesday, December 4, 2013 6:07 PM, João André <***@gmail.com> wrote:

 
Dear Fernando,

Hi! Many thanks for your reply.
I understand your point. The thing is that I get different results when using static (NR or Riks) and dynamic (quasi-static).
In the pure static analysis when I use Riks I see a load drop (using a load proportionality factor) after 81 kN to 80 kN and then the analysis aborts (but earlier than I want...). If I use NR I can only get up to 81 kN. However, if I use quasi-static I can get to 100 kN using load control. This could be because I caught a snap-though behaviour in my structure but when I compare energies and force vs. displacement graphs I see that for the static analysis I get larger deformation and  larger energies for the same value of load..... so something else than a pure structural instability phenomenon is going on.
In 6.3.2 of the Abaqus Analysis User's Manual it is said:
"Quasi-static applications are primarily interested in determining a
final static response. These problems typically show monotonic behavior, and inertia effects are introduced primarily to regularize unstable behavior. For example, the statically unstable behavior may be due to
temporarily unconstrained rigid body modes or “snap-through” phenomena.
Large time increments are taken when possible to obtain the final
solution at minimal computational cost. Considerable numerical
dissipation may be required to obtain convergence during certain stages
of the loading history."

So I guess using the quasi-static implicit analysis abaqus will add some dissipation in order to stabilize the solution and this makes the system resistance larger than what it really is.... just my 50 cents. What do you think? That's why I'm going to see if a pure dynamic analysis I get different results more close to the pure static ones....
This issue is not documented elsewhere but I think I'm right. Same inp file, same everything, only thing changing is the *STATIC (,RIKS) or *DYNAMIC, application=QUASI-STATIC. Even the parameters (initial increment, max increment, min increment are the same).

Many thanks,

Joao

Post by w***@gmail.com
 
Joao,
In principle, the solution you get in /Standard and /Explicit should be

the same (bar practically insignificant numerical differences due to
the solution method and finite precision). The higher-than-real load
capacity of your structure probably comes from the model itself, either
from the element technology, the material/failure model, or both. In general, if your simulation converges in /Standard you should stay with it, /Explicit is a different beast and requires more care when reviewing results (e.g. it doesn't impose equilibrium during solution, so you have to check it yourself). Also, if you set a high increment time in /Explicit you may run into convergence problems, due to the secant method /Explicit uses in the solver.

Post by w***@gmail.com
If I were you I would explore the consequences of "thinning" your element sections by a small percent to model unaccounted damage effects, imperfections, amplification of damage due to dynamic effects etc, rather than changing the solver. This has a clear physical meaning behind it and is thus a valid modeling approach that can be well justified.
Hope this helps,
Fernando
Dear All,
I have some model which didn't converge using standard implicit static analysis: newton-raphson and riks.
My model consists in a 3d frame loaded on top by concentrated forces. The problem involves contact interactions and UEL with stiffness degradation and failure.
I managed to make it run using implicit *Dynamic,application=QUASI-STATIC,initial=NO. However when I compare my results with experimental results I see some differences, namely the numerical model overestimates the maximum load.
I notice that the kinetic energy begins to be very large when failures begin to occur which I think it is OK. ETOTAL = 0 throughout the analysis.
I think that using *DYNAMIC, EXPLICIT and use a large time increment (to approximate a quasi-static analysis) I may see different results than the ones I got using implicit dynamic analysis and maybe closer to the ones I got in my full scale tests because maybe the kinetic effects will be in this case smaller than using implicit. What is your opinion? Many thanks!
Kind regards,
Joao

--
João André
Engenheiro Civil, Mestre / Civil Engineer, M.Sc.
Bolseiro de Doutoramento / PhD Student
Núcleo de Comportamento de Estruturas / Structural Behaviour Division
Departamento de Estruturas / Structures Department
Laboratório Nacional de Engenharia Civil / National Laboratory for Civil Engineering
LNEC, Av. Brasil 101, 1700-066 Lisboa / Lisbon, Portugal
Web: http://www.lnec.pt/
E-mail: ***@lnec.pt
Telefone / Phone: [phone]
Fax: [phone]

[João André]

Hi!

You can use want time target you want. You have to adapt your amplitudes
accordingly.
What I've found was that implicit quasi-static works well when compared
with explicit quasi-static. The runtimes may differ a lot so you need to
test both of them and see what's faster.

Joao

Post by Mohamed Sayed
Hello Joao,
May i ask you question, when you used the Abaqus implicit (Quasi-static
solution) what was the time step, is it one ? you know in the static
analysis, the time step is 1.0.
I am asking you this question, becasue i want to use quasi-static analysis
and i need to know what should be the time step?
Thanks
Dear Fernando,
Hi! Many thanks for your reply.
I understand your point. The thing is that I get different results when
using static (NR or Riks) and dynamic (quasi-static).
In the pure static analysis when I use Riks I see a load drop (using a
load proportionality factor) after 81 kN to 80 kN and then the analysis
aborts (but earlier than I want...). If I use NR I can only get up to 81
kN. However, if I use quasi-static I can get to 100 kN using load
control. This could be because I caught a snap-though behaviour in my
structure but when I compare energies and force vs. displacement graphs I
see that for the static analysis I get larger deformation and larger
energies for the same value of load..... so something else than a pure
structural instability phenomenon is going on.
"Quasi-static applications are primarily interested in determining a final
static response. These problems typically show monotonic behavior, and
inertia effects are introduced primarily to regularize unstable behavior.
For example, the statically unstable behavior may be due to temporarily
unconstrained rigid body modes or “snap-through” phenomena. Large time
increments are taken when possible to obtain the final solution at minimal
computational cost. Considerable numerical dissipation may be required to
obtain convergence during certain stages of the loading history."
So I guess using the quasi-static implicit analysis abaqus will add some
dissipation in order to stabilize the solution and this makes the system
resistance larger than what it really is.... just my 50 cents. What do you
think? That's why I'm going to see if a pure dynamic analysis I get
different results more close to the pure static ones....
This issue is not documented elsewhere but I think I'm right. Same inpfile, same everything, only thing changing is the *STATIC (,
RIKS) or *DYNAMIC, application=QUASI-STATIC. Even the parameters (initial
increment, max increment, min increment are the same).
Many thanks,
Joao
Joao,
In principle, the solution you get in /Standard and /Explicit should be
the same (bar practically insignificant numerical differences due to the
solution method and finite precision). The higher-than-real load capacity
of your structure probably comes from the model itself, either from the
element technology, the material/failure model, or both. In general, if
your simulation converges in /Standard you should stay with it, /Explicit
is a different beast and requires more care when reviewing results (e.g. it
doesn't impose equilibrium during solution, so you have to check it
yourself). Also, if you set a high increment time in /Explicit you may run
into convergence problems, due to the secant method /Explicit uses in the
solver.
If I were you I would explore the consequences of "thinning" your element
sections by a small percent to model unaccounted damage effects,
imperfections, amplification of damage due to dynamic effects etc, rather
than changing the solver. This has a clear physical meaning behind it and
is thus a valid modeling approach that can be well justified.
Hope this helps,
Fernando
Dear All,
I have some model which didn't converge using standard implicit static
analysis: newton-raphson and riks.
My model consists in a 3d frame loaded on top by concentrated forces. The
problem involves contact interactions and UEL with stiffness degradation
and failure.
I managed to make it run using implicit
*Dynamic,application=QUASI-STATIC,initial=NO. However when I compare my
results with experimental results I see some differences, namely the
numerical model overestimates the maximum load.
I notice that the kinetic energy begins to be very large when failures
begin to occur which I think it is OK. ETOTAL = 0 throughout the analysis.
I think that using *DYNAMIC, EXPLICIT and use a large time increment (to
approximate a quasi-static analysis) I may see different results than the
ones I got using implicit dynamic analysis and maybe closer to the ones I
got in my full scale tests because maybe the kinetic effects will be in
this case smaller than using implicit. What is your opinion? Many thanks!
Kind regards,
Joao
--
João André
Engenheiro Civil, Mestre / Civil Engineer, M.Sc.
Bolseiro de Doutoramento / PhD Student
Núcleo de Comportamento de Estruturas / Structural Behaviour Division
Departamento de Estruturas / Structures Department
Laboratório Nacional de Engenharia Civil / National Laboratory for Civil
Engineering
LNEC, Av. Brasil 101, 1700-066 Lisboa / Lisbon, Portugal
Web: http://www.lnec.pt/
Telefone / Phone: [phone]
Fax: [phone]

[Dave Lindeman]

It depends on what you mean by "quasi-static". If you mean *STATIC,
then the time scale is irrelevant (it just happens to default to 1.0).
If you mean *VISCO (and you have viscoelastic or creep properties
defined), then the time scale becomes meaningful.

Regards,

Dave Lindeman
Lead Research Specialist
3M Company
3M Center 235-3F-08
St. Paul, MN 55144
651-733-6383

Post by Mohamed Sayed
Hello Joao,
May i ask you question, when you used the Abaqus implicit
(Quasi-static solution) what was the time step, is it one ? you know
in the static analysis, the time step is 1.0.
I am asking you this question, becasue i want to use quasi-static
analysis and i need to know what should be the time step?
Thanks
On Wednesday, December 4, 2013 6:07 PM, João André
Dear Fernando,
Hi! Many thanks for your reply.
I understand your point. The thing is that I get different results
when using static (NR or Riks) and dynamic (quasi-static).
In the pure static analysis when I use Riks I see a load drop (using a
load proportionality factor) after 81 kN to 80 kN and then the
analysis aborts (but earlier than I want...). If I use NR I can only
get up to 81 kN. However, if I use quasi-static I can get to 100 kN
using load control. This could be because I caught a snap-though
behaviour in my structure but when I compare energies and force vs.
displacement graphs I see that for the static analysis I get larger
deformation and larger energies for the same value of load..... so
something else than a pure structural instability phenomenon is going on.
"Quasi-static applications are primarily interested in determining a
final static response. These problems typically show monotonic
behavior, and inertia effects are introduced primarily to regularize
unstable behavior. For example, the statically unstable behavior may
be due to temporarily unconstrained rigid body modes or “snap-through”
phenomena. Large time increments are taken when possible to obtain the
final solution at minimal computational cost. Considerable numerical
dissipation may be required to obtain convergence during certain
stages of the loading history."
So I guess using the quasi-static implicit analysis abaqus will add
some dissipation in order to stabilize the solution and this makes the
system resistance larger than what it really is.... just my 50 cents.
What do you think? That's why I'm going to see if a pure dynamic
analysis I get different results more close to the pure static ones....
This issue is not documented elsewhere but I think I'm right. Same inp
file, same everything, only thing changing is the *STATIC (,RIKS) or
*DYNAMIC, application=QUASI-STATIC. Even the parameters (initial
increment, max increment, min increment are the same).
Many thanks,
Joao
Joao,
In principle, the solution you get in /Standard and /Explicit
should be the same (bar practically insignificant numerical
differences due to the solution method and finite precision). The
higher-than-real load capacity of your structure probably comes
from the model itself, either from the element technology, the
material/failure model, or both. In general, if your simulation
converges in /Standard you should stay with it, /Explicit is a
different beast and requires more care when reviewing results
(e.g. it doesn't impose equilibrium during solution, so you have
to check it yourself). Also, if you set a high increment time in
/Explicit you may run into convergence problems, due to the secant
method /Explicit uses in the solver.
If I were you I would explore the consequences of "thinning" your
element sections by a small percent to model unaccounted damage
effects, imperfections, amplification of damage due to dynamic
effects etc, rather than changing the solver. This has a clear
physical meaning behind it and is thus a valid modeling approach
that can be well justified.
Hope this helps,
Fernando
Dear All,
I have some model which didn't converge using standard implicit
static analysis: newton-raphson and riks.
My model consists in a 3d frame loaded on top by concentrated
forces. The problem involves contact interactions and UEL with
stiffness degradation and failure.
I managed to make it run using implicit
*Dynamic,application=QUASI-STATIC,initial=NO. However when I
compare my results with experimental results I see some
differences, namely the numerical model overestimates the maximum
load.
I notice that the kinetic energy begins to be very large when
failures begin to occur which I think it is OK. ETOTAL = 0
throughout the analysis.
I think that using *DYNAMIC, EXPLICIT and use a large time
increment (to approximate a quasi-static analysis) I may see
different results than the ones I got using implicit dynamic
analysis and maybe closer to the ones I got in my full scale tests
because maybe the kinetic effects will be in this case smaller
than using implicit. What is your opinion? Many thanks!
Kind regards,
Joao
--
João André
Engenheiro Civil, Mestre / Civil Engineer, M.Sc.
Bolseiro de Doutoramento / PhD Student
Núcleo de Comportamento de Estruturas / Structural Behaviour Division
Departamento de Estruturas / Structures Department
Laboratório Nacional de Engenharia Civil / National Laboratory for Civil Engineering
LNEC, Av. Brasil 101, 1700-066 Lisboa / Lisbon, Portugal
Web: http://www.lnec.pt/
Telefone / Phone: [phone]
Fax: [phone]

[Mohamed Sayed]

I squeeze a deformable rock sample between two rigid platens. it is the regular uniaxial compression test. However due to non linearity because of contact and the stiffness degradation of the material, i could use *static approach. I found that abaqus implicit dynamic with quasi-static approach helped me overcome convergence problem. But the question now what should be the time period?

As you mentioned if the procedure is static so the time scale is irrelevant. Does it the same for quasi-static ( abaqus implicit- dynamic)?

Suppose that squeezing that rock samples takes 20 second in reality, and i will use abaqus implicit dynamic, so i should make the time period 20 sec?

Thank you so much.



On Wednesday, December 18, 2013 9:49 AM, Dave Lindeman <***@mmm.com> wrote:

 
It depends on what you mean by "quasi-static".  If you mean *STATIC, then the time scale is irrelevant (it just happens to default to 1.0).  If you mean *VISCO (and you have viscoelastic or creep properties defined), then the time scale becomes meaningful.

Regards,

Dave Lindeman
Lead Research Specialist
3M Company
3M Center 235-3F-08
St. Paul, MN 55144
651-733-6383
On 12/16/2013 7:48 PM, Mohamed Sayed wrote:

 

Post by Mohamed Sayed
Hello Joao, 
May i ask you question, when you used the Abaqus implicit (Quasi-static solution) what was the time step, is it one ? you know in the static analysis, the time step is 1.0.
I am asking you this question, becasue i want to use quasi-static analysis and i need to know what should be the time step?
Thanks
 
Dear Fernando,

Hi! Many thanks for your reply.
I understand your point. The thing is that I get different results when using static (NR or Riks) and dynamic (quasi-static).
In the pure static analysis when I use Riks I see a load drop (using a load proportionality factor) after 81 kN to 80 kN and then the analysis aborts (but earlier than I want...). If I use NR I can only get up to 81 kN. However, if I use quasi-static I can get to 100 kN using load control. This could be because I caught a snap-though behaviour in my structure but when I compare energies and force vs. displacement graphs I see that for the static analysis I get larger deformation and  larger energies for the same value of load..... so something else than a pure structural instability phenomenon is going on.

Post by Mohamed Sayed
"Quasi-static applications are

primarily interested in
determining a final static
response. These problems
typically show monotonic behavior, and inertia effects are introduced primarily to regularize unstable behavior. For example, the statically unstable behavior may be due to temporarily unconstrained rigid body modes or “snap-through” phenomena. Large time increments are taken when possible to obtain the final solution at minimal computational cost. Considerable numerical dissipation may be required to obtain convergence during certain stages of the loading history."
So I guess using the quasi-static implicit analysis abaqus will add some dissipation in order to stabilize the solution and this makes the system resistance larger than what it really is.... just my 50 cents. What do you think? That's why I'm going to see if a pure dynamic analysis I get different results more close to the pure static ones....
This issue is not documented elsewhere but I think I'm right. Same inp file, same everything, only thing changing is the *STATIC (,RIKS) or *DYNAMIC, application=QUASI-STATIC. Even the parameters (initial increment, max increment, min increment are the same).
Many thanks,

Post by Mohamed Sayed
Joao
 

Post by w***@gmail.com
Joao,
In principle, the

solution you get in
/Standard and
/Explicit should be
the same (bar
practically
insignificant
numerical differences
due to the solution
method and finite
precision). The
higher-than-real load
capacity of your
structure probably
comes from the model
itself, either from
the element
technology, the
material/failure
model, or both. In
general, if your
simulation converges
in /Standard you
should stay with it,
/Explicit is a
different beast and
requires more care
when reviewing results
(e.g. it doesn't
impose equilibrium
during solution, so
you have to check it
yourself). Also, if
you set a high
increment time in
/Explicit you may run
into convergence
problems, due to the
secant method
/Explicit uses in the
solver.

Post by Mohamed Sayed

Post by w***@gmail.com
If I were you I would

explore the
consequences of
"thinning" your
element sections by a
small percent to model
unaccounted damage
effects,
imperfections,
amplification of
damage due to dynamic
effects etc, rather
than changing the
solver. This has a
clear physical meaning
behind it and is thus
a valid modeling
approach that can be
well justified.

Post by Mohamed Sayed

Post by w***@gmail.com
Hope this helps,
Fernando
Dear All,
I have some model

which didn't
converge using
standard implicit
static analysis:
newton-raphson and
riks.

Post by Mohamed Sayed

Post by w***@gmail.com
My model consists

in a 3d frame
loaded on top by
concentrated
forces. The
problem involves
contact
interactions and
UEL with stiffness
degradation and
failure.

Post by Mohamed Sayed

Post by w***@gmail.com
I managed to make

it run using
implicit
*Dynamic,application=QUASI-STATIC,initial=NO.
However when I
compare my results
with experimental
results I see some
differences,
namely the
numerical model
overestimates the
maximum load.

Post by Mohamed Sayed

Post by w***@gmail.com
I notice that the

kinetic energy
begins to be very
large when
failures begin to
occur which I
think it is OK.
ETOTAL = 0
throughout the
analysis.

Post by Mohamed Sayed

Post by w***@gmail.com
I think that using

*DYNAMIC, EXPLICIT
and use a large
time increment (to
approximate a
quasi-static
analysis) I may
see different
results than the
ones I got using
implicit dynamic
analysis and maybe
closer to the ones
I got in my full
scale tests
because maybe the
kinetic effects
will be in this
case smaller than
using implicit.
What is your
opinion? Many
thanks!

Post by Mohamed Sayed

Post by w***@gmail.com
Kind regards,
Joao

--
João André
Engenheiro Civil, Mestre / Civil

Engineer, M.Sc.

Post by Mohamed Sayed
Bolseiro de Doutoramento / PhD Student
Núcleo de Comportamento de Estruturas

/ Structural Behaviour Division

Post by Mohamed Sayed
Departamento de Estruturas /

Structures Department

Post by Mohamed Sayed
Laboratório Nacional de Engenharia

Civil / National Laboratory for Civil
Engineering

Post by Mohamed Sayed
LNEC, Av. Brasil 101, 1700-066 Lisboa

/ Lisbon, Portugal

Post by Mohamed Sayed
Web: http://www.lnec.pt/
Telefone / Phone: [phone]
Fax: [phone]

[Dave Lindeman]

Implicit dynamics is NOT a quasi-static procedure. It is a dynamic
procedure (just like explicit dynamics), and so, with respect to
inertial effects, the time scale is relevant and meaningful. You're not
really talking about a quasi-static solution -- you're talking about
running dynamic procedures for a sufficiently long time so that dynamic
effects are damped out, and the solution approaches the steady-state.
In general you want to use the true time scale associated with your
experiment. But, if you want the "static" solution, then you need to
look at the kinetic energy history to see if inertial effects have been
damped out.

Regards,

Dave Lindeman
Lead Research Specialist
3M Company
3M Center 235-3F-08
St. Paul, MN 55144
651-733-6383

Post by Mohamed Sayed
I squeeze a deformable rock sample between two rigid platens. it is
the regular uniaxial compression test. However due to non linearity
because of contact and the stiffness degradation of the material, i
could use *static approach. I found that abaqus implicit dynamic with
quasi-static approach helped me overcome convergence problem. But the
question now what should be the time period?
As you mentioned if the procedure is static so the time scale is
irrelevant. Does it the same for quasi-static ( abaqus implicit- dynamic)?
Suppose that squeezing that rock samples takes 20 second in reality,
and i will use abaqus implicit dynamic, so i should make the time
period 20 sec?
Thank you so much.
On Wednesday, December 18, 2013 9:49 AM, Dave Lindeman
It depends on what you mean by "quasi-static". If you mean *STATIC,
then the time scale is irrelevant (it just happens to default to
1.0). If you mean *VISCO (and you have viscoelastic or creep
properties defined), then the time scale becomes meaningful.
Regards,
Dave Lindeman
Lead Research Specialist
3M Company
3M Center 235-3F-08
St. Paul, MN 55144
651-733-6383

Post by Mohamed Sayed
Hello Joao,
May i ask you question, when you used the Abaqus implicit
(Quasi-static solution) what was the time step, is it one ? you know
in the static analysis, the time step is 1.0.
I am asking you this question, becasue i want to use quasi-static
analysis and i need to know what should be the time step?
Thanks
On Wednesday, December 4, 2013 6:07 PM, João André
Dear Fernando,
Hi! Many thanks for your reply.
I understand your point. The thing is that I get different results
when using static (NR or Riks) and dynamic (quasi-static).
In the pure static analysis when I use Riks I see a load drop (using
a load proportionality factor) after 81 kN to 80 kN and then the
analysis aborts (but earlier than I want...). If I use NR I can only
get up to 81 kN. However, if I use quasi-static I can get to 100 kN
using load control. This could be because I caught a snap-though
behaviour in my structure but when I compare energies and force vs.
displacement graphs I see that for the static analysis I get larger
deformation and larger energies for the same value of load..... so
something else than a pure structural instability phenomenon is going on.
"Quasi-static applications are primarily interested in determining a
final static response. These problems typically show monotonic
behavior, and inertia effects are introduced primarily to regularize
unstable behavior. For example, the statically unstable behavior may
be due to temporarily unconstrained rigid body modes or
“snap-through” phenomena. Large time increments are taken when
possible to obtain the final solution at minimal computational cost.
Considerable numerical dissipation may be required to obtain
convergence during certain stages of the loading history."
So I guess using the quasi-static implicit analysis abaqus will add
some dissipation in order to stabilize the solution and this makes
the system resistance larger than what it really is.... just my 50
cents. What do you think? That's why I'm going to see if a pure
dynamic analysis I get different results more close to the pure
static ones....
This issue is not documented elsewhere but I think I'm right. Same
inp file, same everything, only thing changing is the *STATIC (,RIKS)
or *DYNAMIC, application=QUASI-STATIC. Even the parameters (initial
increment, max increment, min increment are the same).
Many thanks,
Joao
Joao,
In principle, the solution you get in /Standard and /Explicit
should be the same (bar practically insignificant numerical
differences due to the solution method and finite precision). The
higher-than-real load capacity of your structure probably comes
from the model itself, either from the element technology, the
material/failure model, or both. In general, if your simulation
converges in /Standard you should stay with it, /Explicit is a
different beast and requires more care when reviewing results
(e.g. it doesn't impose equilibrium during solution, so you have
to check it yourself). Also, if you set a high increment time in
/Explicit you may run into convergence problems, due to the
secant method /Explicit uses in the solver.
If I were you I would explore the consequences of "thinning" your
element sections by a small percent to model unaccounted damage
effects, imperfections, amplification of damage due to dynamic
effects etc, rather than changing the solver. This has a clear
physical meaning behind it and is thus a valid modeling approach
that can be well justified.
Hope this helps,
Fernando
Dear All,
I have some model which didn't converge using standard implicit
static analysis: newton-raphson and riks.
My model consists in a 3d frame loaded on top by concentrated
forces. The problem involves contact interactions and UEL with
stiffness degradation and failure.
I managed to make it run using implicit
*Dynamic,application=QUASI-STATIC,initial=NO. However when I
compare my results with experimental results I see some
differences, namely the numerical model overestimates the maximum
load.
I notice that the kinetic energy begins to be very large when
failures begin to occur which I think it is OK. ETOTAL = 0
throughout the analysis.
I think that using *DYNAMIC, EXPLICIT and use a large time
increment (to approximate a quasi-static analysis) I may see
different results than the ones I got using implicit dynamic
analysis and maybe closer to the ones I got in my full scale
tests because maybe the kinetic effects will be in this case
smaller than using implicit. What is your opinion? Many thanks!
Kind regards,
Joao
--
João André
Engenheiro Civil, Mestre / Civil Engineer, M.Sc.
Bolseiro de Doutoramento / PhD Student
Núcleo de Comportamento de Estruturas / Structural Behaviour Division
Departamento de Estruturas / Structures Department
Laboratório Nacional de Engenharia Civil / National Laboratory for Civil Engineering
LNEC, Av. Brasil 101, 1700-066 Lisboa / Lisbon, Portugal
Web: http://www.lnec.pt/
Telefone / Phone: [phone]
Fax: [phone]