Quantcast

UMAT: How does Abaqus calculate the inelastic strain?

classic Classic list List threaded Threaded
4 messages Options
Reply | Threaded
Open this post in threaded view
|  
Report Content as Inappropriate

UMAT: How does Abaqus calculate the inelastic strain?

jondar.callus
For my work I got from a colleague a UMAT to calculate creep strain. But I have different understanding difficulties, how Abaqus calculates the resulting strain.

The UMAT consist only the elastic, thermal und creep strain. As I understand, you calculate the Jacobian matrix (DDEDDS) and the stress (STRESS) and Abaqus uses the Jacobian matrix and the stress to estimate the strain rate.

My problem is, in the UMAT is the Jacobian matrix equal to the elastic matrix:
http://en.wikipedia.org/wiki/Hooke%27s_law#Isotropic_materials

The creep and thermal strain rates, which get determinate in the UMAT, are only used, to calculate the new stress tensor. But the results of the simulation is a strain, which isn't purely elastic.

How it is possible, that the simulation results in a strain, which isn't purely elastic, even if the Jacobian matrix is only the elastic matrix?
My colleague couldn't answer me this questions. He said, this UMAT needs to be correct, because the UMAT and measured values match.

Reply | Threaded
Open this post in threaded view
|  
Report Content as Inappropriate

Re: UMAT: How does Abaqus calculate the inelastic strain?

george jefferson
the total strain (or increment) always come directly from the solution,
nodal displacements and element shape functions. The decomposition, elastic,
plastic, creep, etc must be separately reported by the umat (Read the manual
re umat arguments).
Note since the decomposition doesn't actually affect the global solution
your umat might not even specify those things.


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

Reply | Threaded
Open this post in threaded view
|  
Report Content as Inappropriate

Re: UMAT: How does Abaqus calculate the inelastic strain?

Dave Lindeman
In reply to this post by jondar.callus
At each time step, ABAQUS solves the system of equations to obtain the
displacements, and from these (and the element shape functions), the
deformation gradient, strains, and strain invariants can be derived.
Strain decomposition occurs with the constitutive calculations.

When a UMAT is used, ABAQUS passes in the deformation gradient and total
strains.  The programmer of the UMAT is responsible for doing the
appropriate strain decomposition, and, if necessary, must store the
strain components as state variables.  Note that the UMAT subroutine
does not allow you to pass back plastic, creep, or other strain values,
so ABAQUS has no idea what's going on within the subroutine (although
you can pass back plastic and creep dissipation energies).  The UMAT
must pass back the stresses (which are used to evaluate equilibrium),
and the Jacobian (which is used to form the tangent stiffness matrix).

In some cases it is possible to use a purely elastic Jacobian, but this
could prevent or slow convergence.  Convergence will still be based on
achieving equilibrium, however, so as long as the correct stresses are
being passed back, the problem should still converge on the same answer
(if or when it converges).

Regards,
Dave

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

On 4/15/2011 4:02 AM, Jondar Callus wrote:

> For my work I got from a colleague a UMAT to calculate creep strain. But
> I have different understanding difficulties, how Abaqus calculates the
> resulting strain.
>
> The UMAT consist only the elastic, thermal und creep strain. As I
> understand, you calculate the Jacobian matrix (DDEDDS) and the stress
> (STRESS) and Abaqus uses the Jacobian matrix and the stress to estimate
> the strain rate.
>
> My problem is, in the UMAT is the Jacobian matrix equal to the elastic
> matrix:
> http://en.wikipedia.org/wiki/Hooke%27s_law#Isotropic_materials
>
> The creep and thermal strain rates, which get determinate in the UMAT,
> are only used, to calculate the new stress tensor. But the results of
> the simulation is a strain, which isn't purely elastic.
>
> How it is possible, that the simulation results in a strain, which isn't
> purely elastic, even if the Jacobian matrix is only the elastic matrix?
> My colleague couldn't answer me this questions. He said, this UMAT needs
> to be correct, because the UMAT and measured values match.
>
>


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

Community email addresses:
  Post message: [hidden email]
  Subscribe:    [hidden email]
  Unsubscribe:  [hidden email]
  List owner:   [hidden email]

Shortcut URL to this page:
  http://groups.yahoo.com/group/AbaqusYahoo! Groups Links

<*> To visit your group on the web, go to:
    http://groups.yahoo.com/group/Abaqus/

<*> Your email settings:
    Individual Email | Traditional

<*> To change settings online go to:
    http://groups.yahoo.com/group/Abaqus/join
    (Yahoo! ID required)

<*> To change settings via email:
    [hidden email]
    [hidden email]

<*> To unsubscribe from this group, send an email to:
    [hidden email]

<*> Your use of Yahoo! Groups is subject to:
    http://docs.yahoo.com/info/terms/

Reply | Threaded
Open this post in threaded view
|  
Report Content as Inappropriate

Re: UMAT: How does Abaqus calculate the inelastic strain?

jondar.callus


Thank you, for your response.

I try to understand, how the inelastic strains get calculated.

Abaqus solves the equations by a method of approximation. The Jaccobi matrix is the derivate for the newton's method. In the case of the purely elastic Jacobian in my creep calculations, the derivate is an approximations of the correct model with creep. The inelastic strain gets into the equation by the calculation of the stress. If the elastic Jacobian is sufficient, the newton's method can converge and a deformation gradient will be calculated, which contains the elastic and inelastic strain.




--- In [hidden email], Dave Lindeman <ddlindeman@...> wrote:

>
> At each time step, ABAQUS solves the system of equations to obtain the
> displacements, and from these (and the element shape functions), the
> deformation gradient, strains, and strain invariants can be derived.
> Strain decomposition occurs with the constitutive calculations.
>
> When a UMAT is used, ABAQUS passes in the deformation gradient and total
> strains.  The programmer of the UMAT is responsible for doing the
> appropriate strain decomposition, and, if necessary, must store the
> strain components as state variables.  Note that the UMAT subroutine
> does not allow you to pass back plastic, creep, or other strain values,
> so ABAQUS has no idea what's going on within the subroutine (although
> you can pass back plastic and creep dissipation energies).  The UMAT
> must pass back the stresses (which are used to evaluate equilibrium),
> and the Jacobian (which is used to form the tangent stiffness matrix).
>
> In some cases it is possible to use a purely elastic Jacobian, but this
> could prevent or slow convergence.  Convergence will still be based on
> achieving equilibrium, however, so as long as the correct stresses are
> being passed back, the problem should still converge on the same answer
> (if or when it converges).
>
> Regards,
> Dave
>
> Dave Lindeman
> Lead Research Specialist
> 3M Company
> 3M Center 235-3F-08
> St. Paul, MN 55144
> 651-733-6383
>
> On 4/15/2011 4:02 AM, Jondar Callus wrote:
> > For my work I got from a colleague a UMAT to calculate creep strain. But
> > I have different understanding difficulties, how Abaqus calculates the
> > resulting strain.
> >
> > The UMAT consist only the elastic, thermal und creep strain. As I
> > understand, you calculate the Jacobian matrix (DDEDDS) and the stress
> > (STRESS) and Abaqus uses the Jacobian matrix and the stress to estimate
> > the strain rate.
> >
> > My problem is, in the UMAT is the Jacobian matrix equal to the elastic
> > matrix:
> > http://en.wikipedia.org/wiki/Hooke%27s_law#Isotropic_materials
> >
> > The creep and thermal strain rates, which get determinate in the UMAT,
> > are only used, to calculate the new stress tensor. But the results of
> > the simulation is a strain, which isn't purely elastic.
> >
> > How it is possible, that the simulation results in a strain, which isn't
> > purely elastic, even if the Jacobian matrix is only the elastic matrix?
> > My colleague couldn't answer me this questions. He said, this UMAT needs
> > to be correct, because the UMAT and measured values match.
> >
> >
>


Loading...