Discussion:
UMAT for finite strains
iwtm16
2004-12-08 09:19:48 UTC
Permalink
Greetings,

I want to implement a time-independant material model (elasto-plastic)
for finite strains in ABAQUS standard. I have read that this is
possible in ABAQUS Standard with a corotational frame for stress
integration. The elastic part should be modelled with Hookes law. The
plastic part should be modelled with a modified mises model. In the
ABAQUS manual "writing user subroutines with ABAQUS" the material
models are described both in normal form (time independant) and rate
form (Jaumann rate). Does anyone know which form is the correct form
to implement my model into UMAT? Does Abaqus use the multiplicative
split of the deformation gradient F or the additive decomposition of
deformation rate d for such an implementation. Which strain measure
does Abaqus use for stress integration?

luc








------------------------ Yahoo! Groups Sponsor --------------------~-->
Make a clean sweep of pop-up ads. Yahoo! Companion Toolbar.
Now with Pop-Up Blocker. Get it for free!
http://us.click.yahoo.com/L5YrjA/eSIIAA/yQLSAA/PMYolB/TM
--------------------------------------------------------------------~->
BenZ
2004-12-08 16:16:34 UTC
Permalink
What you call "normal form" and "Jaumann rate" are the same ! The
formulation used is incremental, i.e. it is a rate form. Even
classical plasticity is given as a rate form. So, the correct form is
the incremental one.
About the form of the plastic-elastic decomposition: good question,
but not relevant for a UMAT. In a UMAT, you choose how you decompose
F or D.
About the strain measure, it is of course the Jaumann strain
for /Standard, i.e. D integrated in the rotating frame of Jaumann.
The incremental stress is then the tangent behavior (jacobian matrix)
times the incremental strain of Jaumann.

BenZ.
Post by iwtm16
Greetings,
I want to implement a time-independant material model (elasto-
plastic)
Post by iwtm16
for finite strains in ABAQUS standard. I have read that this is
possible in ABAQUS Standard with a corotational frame for stress
integration. The elastic part should be modelled with Hookes law. The
plastic part should be modelled with a modified mises model. In the
ABAQUS manual "writing user subroutines with ABAQUS" the material
models are described both in normal form (time independant) and rate
form (Jaumann rate). Does anyone know which form is the correct form
to implement my model into UMAT? Does Abaqus use the multiplicative
split of the deformation gradient F or the additive decomposition of
deformation rate d for such an implementation. Which strain measure
does Abaqus use for stress integration?
luc
------------------------ Yahoo! Groups Sponsor --------------------~-->
Make a clean sweep of pop-up ads. Yahoo! Companion Toolbar.
Now with Pop-Up Blocker. Get it for free!
http://us.click.yahoo.com/L5YrjA/eSIIAA/yQLSAA/PMYolB/TM
--------------------------------------------------------------------~->
iwtm16
2004-12-08 18:54:41 UTC
Permalink
Hello,

thank you for the details. One problem: In the theory manual of Abaqus
(case of geometrical nonlinearity) is mentioned that the strain
measure is an approximation to logarithmic strains? Is that correct?
Can you mention me some literture for the integration in rotating
frame (corotational frame)?
Post by BenZ
What you call "normal form" and "Jaumann rate" are the same ! The
formulation used is incremental, i.e. it is a rate form. Even
classical plasticity is given as a rate form. So, the correct form is
the incremental one.
About the form of the plastic-elastic decomposition: good question,
but not relevant for a UMAT. In a UMAT, you choose how you decompose
F or D.
About the strain measure, it is of course the Jaumann strain
for /Standard, i.e. D integrated in the rotating frame of Jaumann.
The incremental stress is then the tangent behavior (jacobian
matrix)
Post by BenZ
times the incremental strain of Jaumann.
BenZ.
Post by iwtm16
Greetings,
I want to implement a time-independant material model (elasto-
plastic)
Post by iwtm16
for finite strains in ABAQUS standard. I have read that this is
possible in ABAQUS Standard with a corotational frame for stress
integration. The elastic part should be modelled with Hookes law.
The
Post by iwtm16
plastic part should be modelled with a modified mises model. In the
ABAQUS manual "writing user subroutines with ABAQUS" the material
models are described both in normal form (time independant) and
rate
Post by iwtm16
form (Jaumann rate). Does anyone know which form is the correct
form
Post by iwtm16
to implement my model into UMAT? Does Abaqus use the
multiplicative
Post by BenZ
Post by iwtm16
split of the deformation gradient F or the additive decomposition
of
Post by iwtm16
deformation rate d for such an implementation. Which strain
measure
Post by BenZ
Post by iwtm16
does Abaqus use for stress integration?
luc
------------------------ Yahoo! Groups Sponsor --------------------~-->
Make a clean sweep of pop-up ads. Yahoo! Companion Toolbar.
Now with Pop-Up Blocker. Get it for free!
http://us.click.yahoo.com/L5YrjA/eSIIAA/yQLSAA/PMYolB/TM
--------------------------------------------------------------------~->
BenZ
2004-12-10 14:38:48 UTC
Permalink
Maybe it is mentionned, but you can believe me, the Jaumann strain
has nothing to do with the log. strains ! Except in the case of a
triaxial loading (F=U=V), i.e. where's there is no average rotation.
About the integration in the corotationnal frame, look at my PhD (in
french) or check out the books of M.A. Crisfield.

BenZ.
Post by iwtm16
Hello,
thank you for the details. One problem: In the theory manual of Abaqus
(case of geometrical nonlinearity) is mentioned that the strain
measure is an approximation to logarithmic strains? Is that
correct?
Post by iwtm16
Can you mention me some literture for the integration in rotating
frame (corotational frame)?
Post by BenZ
What you call "normal form" and "Jaumann rate" are the same ! The
formulation used is incremental, i.e. it is a rate form. Even
classical plasticity is given as a rate form. So, the correct
form
Post by iwtm16
is
Post by BenZ
the incremental one.
About the form of the plastic-elastic decomposition: good
question,
Post by iwtm16
Post by BenZ
but not relevant for a UMAT. In a UMAT, you choose how you
decompose
Post by iwtm16
Post by BenZ
F or D.
About the strain measure, it is of course the Jaumann strain
for /Standard, i.e. D integrated in the rotating frame of
Jaumann.
Post by iwtm16
Post by BenZ
The incremental stress is then the tangent behavior (jacobian
matrix)
Post by BenZ
times the incremental strain of Jaumann.
BenZ.
Post by iwtm16
Greetings,
I want to implement a time-independant material model (elasto-
plastic)
Post by iwtm16
for finite strains in ABAQUS standard. I have read that this is
possible in ABAQUS Standard with a corotational frame for
stress
Post by iwtm16
Post by BenZ
Post by iwtm16
integration. The elastic part should be modelled with Hookes law.
The
Post by iwtm16
plastic part should be modelled with a modified mises model. In
the
Post by BenZ
Post by iwtm16
ABAQUS manual "writing user subroutines with ABAQUS" the
material
Post by iwtm16
Post by BenZ
Post by iwtm16
models are described both in normal form (time independant) and
rate
Post by iwtm16
form (Jaumann rate). Does anyone know which form is the correct
form
Post by iwtm16
to implement my model into UMAT? Does Abaqus use the
multiplicative
Post by BenZ
Post by iwtm16
split of the deformation gradient F or the additive
decomposition
Post by iwtm16
Post by BenZ
of
Post by iwtm16
deformation rate d for such an implementation. Which strain
measure
Post by BenZ
Post by iwtm16
does Abaqus use for stress integration?
luc
------------------------ Yahoo! Groups Sponsor --------------------~-->
Make a clean sweep of pop-up ads. Yahoo! Companion Toolbar.
Now with Pop-Up Blocker. Get it for free!
http://us.click.yahoo.com/L5YrjA/eSIIAA/yQLSAA/PMYolB/TM
--------------------------------------------------------------------~->
meyh2002
2004-12-31 01:33:00 UTC
Permalink
Happy Holiday, Ben.

"About the form of the plastic-elastic decomposition: good question,
but not relevant for a UMAT. In a UMAT, you choose how you
decompose F or D."

I 'll agree this is an interesting question.But not very clearly
about what you said. Do you mean that UMAT only deal with F or D not
strain/stress ? If that is the case where should we caculate
strain/stress?

Could you give a detailed explaination?
Post by BenZ
What you call "normal form" and "Jaumann rate" are the same ! The
formulation used is incremental, i.e. it is a rate form. Even
classical plasticity is given as a rate form. So, the correct form is
the incremental one.
About the form of the plastic-elastic decomposition: good
question,
Post by BenZ
but not relevant for a UMAT. In a UMAT, you choose how you
decompose
Post by BenZ
F or D.
About the strain measure, it is of course the Jaumann strain
for /Standard, i.e. D integrated in the rotating frame of Jaumann.
The incremental stress is then the tangent behavior (jacobian
matrix)
Post by BenZ
times the incremental strain of Jaumann.
BenZ.
Post by iwtm16
Greetings,
I want to implement a time-independant material model (elasto-
plastic)
Post by iwtm16
for finite strains in ABAQUS standard. I have read that this is
possible in ABAQUS Standard with a corotational frame for stress
integration. The elastic part should be modelled with Hookes
law.
Post by BenZ
The
Post by iwtm16
plastic part should be modelled with a modified mises model. In the
ABAQUS manual "writing user subroutines with ABAQUS" the
material
Post by BenZ
Post by iwtm16
models are described both in normal form (time independant) and
rate
Post by iwtm16
form (Jaumann rate). Does anyone know which form is the correct
form
Post by iwtm16
to implement my model into UMAT? Does Abaqus use the
multiplicative
Post by BenZ
Post by iwtm16
split of the deformation gradient F or the additive
decomposition
Post by BenZ
of
Post by iwtm16
deformation rate d for such an implementation. Which strain
measure
Post by BenZ
Post by iwtm16
does Abaqus use for stress integration?
luc
------------------------ Yahoo! Groups Sponsor --------------------~-->
$4.98 domain names from Yahoo!. Register anything.
http://us.click.yahoo.com/Q7_YsB/neXJAA/yQLSAA/PMYolB/TM
--------------------------------------------------------------------~->
BenZ
2004-12-31 12:19:19 UTC
Permalink
Heyhey, thx !!! Happy new year !!

In the UMAT, you get the strain increment that is, in fact, D times
dt given in the corotationnal basis (Jaumann for /Standard). Let me
point out that D is taken at the midstep, consistently with the
Hughes-Winget integration algorithm.
So you get dEij=Dijdt, but dEij (the strain increment) might not be
the one you want. But you have D, so you can do what you want.
You have to return to Abaqus Sij with the aid of dSij that you have
to compute.
As you see, the real tensorial variable are Fij and Dij, but one that
isn't aware of large deformations would take dEij, compute dSij as
CkldEkl and return Sij=Sij(old)+dSij...

BenZ.
Post by meyh2002
Happy Holiday, Ben.
"About the form of the plastic-elastic decomposition: good
question,
Post by meyh2002
but not relevant for a UMAT. In a UMAT, you choose how you
decompose F or D."
I 'll agree this is an interesting question.But not very clearly
about what you said. Do you mean that UMAT only deal with F or D not
strain/stress ? If that is the case where should we caculate
strain/stress?
Could you give a detailed explaination?
Post by BenZ
What you call "normal form" and "Jaumann rate" are the same ! The
formulation used is incremental, i.e. it is a rate form. Even
classical plasticity is given as a rate form. So, the correct
form
Post by meyh2002
is
Post by BenZ
the incremental one.
About the form of the plastic-elastic decomposition: good
question,
Post by BenZ
but not relevant for a UMAT. In a UMAT, you choose how you
decompose
Post by BenZ
F or D.
About the strain measure, it is of course the Jaumann strain
for /Standard, i.e. D integrated in the rotating frame of
Jaumann.
Post by meyh2002
Post by BenZ
The incremental stress is then the tangent behavior (jacobian
matrix)
Post by BenZ
times the incremental strain of Jaumann.
BenZ.
Post by iwtm16
Greetings,
I want to implement a time-independant material model (elasto-
plastic)
Post by iwtm16
for finite strains in ABAQUS standard. I have read that this is
possible in ABAQUS Standard with a corotational frame for
stress
Post by meyh2002
Post by BenZ
Post by iwtm16
integration. The elastic part should be modelled with Hookes
law.
Post by BenZ
The
Post by iwtm16
plastic part should be modelled with a modified mises model. In
the
Post by BenZ
Post by iwtm16
ABAQUS manual "writing user subroutines with ABAQUS" the
material
Post by BenZ
Post by iwtm16
models are described both in normal form (time independant) and
rate
Post by iwtm16
form (Jaumann rate). Does anyone know which form is the correct
form
Post by iwtm16
to implement my model into UMAT? Does Abaqus use the
multiplicative
Post by BenZ
Post by iwtm16
split of the deformation gradient F or the additive
decomposition
Post by BenZ
of
Post by iwtm16
deformation rate d for such an implementation. Which strain
measure
Post by BenZ
Post by iwtm16
does Abaqus use for stress integration?
luc
------------------------ Yahoo! Groups Sponsor --------------------~-->
Make a clean sweep of pop-up ads. Yahoo! Companion Toolbar.
Now with Pop-Up Blocker. Get it for free!
http://us.click.yahoo.com/L5YrjA/eSIIAA/yQLSAA/PMYolB/TM
--------------------------------------------------------------------~->
nhabe1
2005-01-01 13:42:27 UTC
Permalink
hei, Benz,
Happy new year!

In Abaqus document, there is
"In finite-strain problems the stress tensor has already been
rotated to account for rigid body motion in the increment before
UMAT is called, so that only the corotational part of the stress
integration should be done in UMAT. The measure of stress used is
¡°true¡± (Cauchy) stress."

According this,
---------Is it right that the "STRESS(NTENS)" is cauchy stress
increment in UMAT even when the contitutive is rate form. I think
the "Jaumann rate" is not involved in UMAT, right?

--------the "STRAN(NTENS)" which is passed to UMAT is logarithmic
strain (Hencky strain), right?

I am a novice for UMAT, I am not sure for the above. Could you
give me answer?

Renxc
Post by BenZ
Heyhey, thx !!! Happy new year !!
In the UMAT, you get the strain increment that is, in fact, D
times
Post by BenZ
dt given in the corotationnal basis (Jaumann for /Standard). Let me
point out that D is taken at the midstep, consistently with the
Hughes-Winget integration algorithm.
So you get dEij=Dijdt, but dEij (the strain increment) might not be
the one you want. But you have D, so you can do what you want.
You have to return to Abaqus Sij with the aid of dSij that you
have
Post by BenZ
to compute.
As you see, the real tensorial variable are Fij and Dij, but one that
isn't aware of large deformations would take dEij, compute dSij as
CkldEkl and return Sij=Sij(old)+dSij...
BenZ.
Post by meyh2002
Happy Holiday, Ben.
"About the form of the plastic-elastic decomposition: good
question,
Post by meyh2002
but not relevant for a UMAT. In a UMAT, you choose how you
decompose F or D."
I 'll agree this is an interesting question.But not very
clearly
Post by BenZ
Post by meyh2002
about what you said. Do you mean that UMAT only deal with F or D
not
Post by meyh2002
strain/stress ? If that is the case where should we caculate
strain/stress?
Could you give a detailed explaination?
What you call "normal form" and "" are the same ! The
formulation used is incremental, i.e. it is a rate form. Even
classical plasticity is given as a rate form. So, the correct
form
Post by meyh2002
is
the incremental one.
About the form of the plastic-elastic decomposition: good
question,
but not relevant for a UMAT. In a UMAT, you choose how you
decompose
F or D.
About the strain measure, it is of course the Jaumann strain
for /Standard, i.e. D integrated in the rotating frame of
Jaumann.
Post by meyh2002
The incremental stress is then the tangent behavior (jacobian
matrix)
times the incremental strain of Jaumann.
BenZ.
Post by iwtm16
Greetings,
I want to implement a time-independant material model
(elasto-
Post by BenZ
Post by meyh2002
plastic)
Post by iwtm16
for finite strains in ABAQUS standard. I have read that this is
possible in ABAQUS Standard with a corotational frame for
stress
Post by meyh2002
Post by iwtm16
integration. The elastic part should be modelled with
Hookes
Post by BenZ
Post by meyh2002
law.
The
Post by iwtm16
plastic part should be modelled with a modified mises model. In
the
Post by iwtm16
ABAQUS manual "writing user subroutines with ABAQUS" the
material
Post by iwtm16
models are described both in normal form (time independant) and
rate
Post by iwtm16
form (Jaumann rate). Does anyone know which form is the
correct
Post by BenZ
Post by meyh2002
form
Post by iwtm16
to implement my model into UMAT? Does Abaqus use the
multiplicative
Post by iwtm16
split of the deformation gradient F or the additive
decomposition
of
Post by iwtm16
deformation rate d for such an implementation. Which strain
measure
Post by iwtm16
does Abaqus use for stress integration?
luc
BenZ
2005-01-03 10:43:18 UTC
Permalink
Yo ! You ask for the real interesting issues ! Good start for 2005
heyhey :) !

Lemme answer you :

1/STRESS is the Cauchy stresses given IN the Jaumann's basis. If you
are used to 'unrotated' objective tensors, STRESS has the same
components in the Jaumann's rotated basis as the unrotated STRESS in
the initial orientation (if you use *ORIENTATION) or global basis. So
in fact, the Jaumann's rate IS involved in the UMAT, but the bases
used ensure that the Hughes-Winget formula has the form :
Sijnew=Sijold+dSij.
2/The STRAN tensor is NOT the Hencky's strain measure. It is the
JAUMANN's strain measure, i.e. the integral of D in the rotating
frame. Like STRESS, tt is also given in the rotated basis.

BenZ.
Post by nhabe1
hei, Benz,
Happy new year!
In Abaqus document, there is
"In finite-strain problems the stress tensor has already been
rotated to account for rigid body motion in the increment before
UMAT is called, so that only the corotational part of the stress
integration should be done in UMAT. The measure of stress used is
¡°true¡± (Cauchy) stress."
According this,
---------Is it right that the "STRESS(NTENS)" is cauchy stress
increment in UMAT even when the contitutive is rate form. I think
the "Jaumann rate" is not involved in UMAT, right?
--------the "STRAN(NTENS)" which is passed to UMAT is
logarithmic
Post by nhabe1
strain (Hencky strain), right?
I am a novice for UMAT, I am not sure for the above. Could you
give me answer?
Renxc
Post by BenZ
Heyhey, thx !!! Happy new year !!
In the UMAT, you get the strain increment that is, in fact, D
times
Post by BenZ
dt given in the corotationnal basis (Jaumann for /Standard). Let
me
Post by BenZ
point out that D is taken at the midstep, consistently with the
Hughes-Winget integration algorithm.
So you get dEij=Dijdt, but dEij (the strain increment) might not
be
Post by BenZ
the one you want. But you have D, so you can do what you want.
You have to return to Abaqus Sij with the aid of dSij that you
have
Post by BenZ
to compute.
As you see, the real tensorial variable are Fij and Dij, but one
that
Post by BenZ
isn't aware of large deformations would take dEij, compute dSij as
CkldEkl and return Sij=Sij(old)+dSij...
BenZ.
Post by meyh2002
Happy Holiday, Ben.
"About the form of the plastic-elastic decomposition: good
question,
Post by meyh2002
but not relevant for a UMAT. In a UMAT, you choose how you
decompose F or D."
I 'll agree this is an interesting question.But not very
clearly
Post by BenZ
Post by meyh2002
about what you said. Do you mean that UMAT only deal with F or D
not
Post by meyh2002
strain/stress ? If that is the case where should we caculate
strain/stress?
Could you give a detailed explaination?
What you call "normal form" and "" are the same ! The
formulation used is incremental, i.e. it is a rate form. Even
classical plasticity is given as a rate form. So, the correct
form
Post by meyh2002
is
the incremental one.
About the form of the plastic-elastic decomposition: good
question,
but not relevant for a UMAT. In a UMAT, you choose how you
decompose
F or D.
About the strain measure, it is of course the Jaumann strain
for /Standard, i.e. D integrated in the rotating frame of
Jaumann.
Post by meyh2002
The incremental stress is then the tangent behavior (jacobian
matrix)
times the incremental strain of Jaumann.
BenZ.
Post by iwtm16
Greetings,
I want to implement a time-independant material model
(elasto-
Post by BenZ
Post by meyh2002
plastic)
Post by iwtm16
for finite strains in ABAQUS standard. I have read that
this
Post by nhabe1
is
Post by BenZ
Post by meyh2002
Post by iwtm16
possible in ABAQUS Standard with a corotational frame for
stress
Post by meyh2002
Post by iwtm16
integration. The elastic part should be modelled with
Hookes
Post by BenZ
Post by meyh2002
law.
The
Post by iwtm16
plastic part should be modelled with a modified mises
model.
Post by nhabe1
In
Post by BenZ
Post by meyh2002
the
Post by iwtm16
ABAQUS manual "writing user subroutines with ABAQUS" the
material
Post by iwtm16
models are described both in normal form (time independant)
and
Post by BenZ
Post by meyh2002
rate
Post by iwtm16
form (Jaumann rate). Does anyone know which form is the
correct
Post by BenZ
Post by meyh2002
form
Post by iwtm16
to implement my model into UMAT? Does Abaqus use the
multiplicative
Post by iwtm16
split of the deformation gradient F or the additive
decomposition
of
Post by iwtm16
deformation rate d for such an implementation. Which strain
measure
Post by iwtm16
does Abaqus use for stress integration?
luc
madhava prasad tunuguntla
2005-01-03 10:55:18 UTC
Permalink
Hello all,
I want to know the general criteria for selecting elements i.e, How to decide wether we have to use Tetrahedral or hexahedral elements? And how to decide up on wether we have to take linear or qudratic elements?
And suppose if geometry is not allowing for hexahedral mesh then how to mesh? How to decide up on edge length? Warpage? etc

I will be happy even if you give me some references or websites for the above questions.

Thanks in advance,
T M Prasad



Yahoo! India Matrimony: Find your life partneronline.

[Non-text portions of this message have been removed]

Loading...