Parametric study using python with UMAT

[dubuprince]

 Dear all

 I'm performing an parametric study of my model using python script.

 I used the command >abaqus script=abaqus_parametric user=umat.for

 However, the script does not suuport the 'user' command.

 Is there any other command invoking Fortran user subroutine?

 Thanks in advance

 Sincerely yours,

 Sang Ha

 

[haydar arslan]

Sang,

I think, you don't need to use user command. To
execute, you just need to write : abaqus
script=scriptname.psf

You  should define your main input file name (which
must include your user subroutine definition) in the
script  such as: inputFiles=('your input file')

I did use aStudy.sample command for the parameters
input,

I hope It helps,

Haydar
 
--- dubuprince <dubuprince@...> wrote:

>
>  Dear all
>
>  I'm performing an parametric study of my model
> using python script.
>
>  I used the command >abaqus script=abaqus_parametric
> user=umat.for
>
>  However, the script does not suuport the 'user'
> command.
>
>  Is there any other command invoking Fortran user
> subroutine?
>
>  Thanks in advance
>
>  Sincerely yours,
>
>  Sang Ha
>
>  
>
>

      ____________________________________________________________________________________
Be a better sports nut!  Let your teams follow you
with Yahoo Mobile. Try it now.  http://mobile.yahoo.com/sports;_ylt=At9_qDKvtAbMuh1G1SQtBI7ntAcJ

[dubuprince]

 Thanks, Haydar

 I use the following script based on the ABAQUS/Benchmark problem

 ===
 # create the study
 cohesiveStudy = ParStudy(par=('sigma', 'delta'),
                     directory=ON, verbose=ON)

 # define the parameters
 cohesiveStudy.define(DISCRETE, par='sigma', domain=(1., 10.))
 cohesiveStudy.define(DISCRETE, par='delta', domain=(0.0001, 0.01))
 
 # sample the parameters
 cohesiveStudy.sample(INTERVAL, par=('sigma', 'delta'), interval=1)

 # generate analysis data
 cohesiveStudy.generate(template='cohesive_parametric')

 ===

 The *.msg file shows "ERROR:USER SUBROUTINE UMAT IS MISSING".

 Of course, I defined the user subroutine in my template input file
 'cohesive_parametric.inp' as '*USER MATERIAL, CONSTANTS=22'.

 Sincerely yours,
 Sang Ha



--- In Abaqus@..., haydar arslan <haydarslan@...> wrote:

>
> Sang,
>
> I think, you don't need to use user command. To
> execute, you just need to write : abaqus
> script=scriptname.psf
>
> You  should define your main input file name (which
> must include your user subroutine definition) in the
> script  such as: inputFiles=('your input file')
>
> I did use aStudy.sample command for the parameters
> input,
>
> I hope It helps,
>
> Haydar
>  
> --- dubuprince <dubuprince@...> wrote:
>
> >
> >  Dear all
> >
> >  I'm performing an parametric study of my model
> > using python script.
> >
> >  I used the command >abaqus script=abaqus_parametric
> > user=umat.for
> >
> >  However, the script does not suuport the 'user'
> > command.
> >
> >  Is there any other command invoking Fortran user
> > subroutine?
> >
> >  Thanks in advance
> >
> >  Sincerely yours,
> >
> >  Sang Ha
> >
> >  
> >
> >
>
>
>
>      

_____________________________________________________________________
_______________
> Be a better sports nut!  Let your teams follow you
> with Yahoo Mobile. Try it now.  
http://mobile.yahoo.com/sports;_ylt=At9_qDKvtAbMuh1G1SQtBI7ntAcJ
>

[Fernando-18]

Hi Sang Ha,

>  I'm performing an parametric study of my model using python script.
>
>  I used the command >abaqus script=abaqus_parametric user=umat.for
>
>  However, the script does not suuport the 'user' command.
>
>  Is there any other command invoking Fortran user subroutine?

The "abaqus script" command allows you to run a python script from the
command line in the same way as you would from within CAE, but without
needing to start the whole GUI. This way, you can do batch processing
more efficiently. If you are doing a parametric study, you have two
alternatives:
a) using python and "abaqus script", submit the job from within python
(it is something like job.submit(), check the docs)
b) using the parametric study capabilities of ABAQUS, define your
input file in terms of the model parameters, define a parametric study
file (check the docs), and let ABAQUS do the rest of the job.

Option b) will let you postprocess the whole results from /Viewer in
an easy and integrated way, while with a) you will have to extract
your results from each file individually.

Hope this helps,
Fernando

[fehrich ()]

Fernando-18 wrote:

The "abaqus script" command allows you to run a python script from the
command line in the same way as you would from within CAE, but without
needing to start the whole GUI. This way, you can do batch processing
more efficiently. If you are doing a parametric study, you have two
alternatives:
a) using python and "abaqus script", submit the job from within python
(it is something like job.submit(), check the docs)
b) using the parametric study capabilities of ABAQUS, define your
input file in terms of the model parameters, define a parametric study
file (check the docs), and let ABAQUS do the rest of the job.

Option b) will let you postprocess the whole results from /Viewer in
an easy and integrated way, while with a) you will have to extract
your results from each file individually.

Hope this helps,
Fernando

Hi everyone,

I want to perform a parametric study using VUMAT.
However, I don't really know how I can combine the Python script with my fortran material definition.

So far I executed abaqus with the VUMAT in the command window as follows:

abaqus input=input_file_name user=VUMAT_file_name

Can anyone describe how to combine Python script and VUMAT/UMAT in more detail?

Many thanks
Fabian

[Frank Richter-2]

Here is a template for your filename.psf with hexp being varied:

parst = ParStudy(par=('hexp'), name='filename',directory=ON)

parst.define(DISCRETE, par='hexp',domain=(-5,-10,-15))
parst.sample(REFERENCE, par='hexp', reference=1, interval=1, numSymPairs=1)

parst.combine(MESH)

parst.generate(template='filename')

parst.execute(ALL,execOptions='user=filename.for')



Frank



-------- Original-Nachricht --------
> Datum: Wed, 4 Nov 2009 01:07:32 -0800 (PST)
> Von: fehrich <f.ehrich09@...>
> An: ABAQUS@...
> Betreff: Re: [ABAQUS] Parametric study using python with UMAT

>
>
> Fernando-18 wrote:
> >
> >
> > The "abaqus script" command allows you to run a python script from the
> > command line in the same way as you would from within CAE, but without
> > needing to start the whole GUI. This way, you can do batch processing
> > more efficiently. If you are doing a parametric study, you have two
> > alternatives:
> > a) using python and "abaqus script", submit the job from within python
> > (it is something like job.submit(), check the docs)
> > b) using the parametric study capabilities of ABAQUS, define your
> > input file in terms of the model parameters, define a parametric study
> > file (check the docs), and let ABAQUS do the rest of the job.
> >
> > Option b) will let you postprocess the whole results from /Viewer in
> > an easy and integrated way, while with a) you will have to extract
> > your results from each file individually.
> >
> > Hope this helps,
> > Fernando
> >
> >
> >
>
>
> Hi everyone,
>
> I want to perform a parametric study using VUMAT.
> However, I don't really know how I can combine the Python script with my
> fortran material definition.
>
> So far I executed abaqus with the VUMAT in the command window as follows:
>
> abaqus input=input_file_name user=VUMAT_file_name
>
> Can anyone describe how to combine Python script and VUMAT/UMAT in more
> detail?
>
> Many thanks
> Fabian
> --
> View this message in context:
> http://old.nabble.com/Parametric-study-using-python-with-UMAT-tp14127909p26160170.html
> Sent from the Abaqus Users mailing list archive at Nabble.com.
>

--
-----------------------------------------------------------------------
Frank Richter
Institute of Materials Science
Ruhr-Universitaet Bochum
Bochum
Germany



Jetzt kostenlos herunterladen: Internet Explorer 8 und Mozilla Firefox 3.5 -
sicherer, schneller und einfacher! http://portal.gmx.net/de/go/chbrowser

[fehrich ()]

Hi Frank,
Thank you for your answer!

I now defined my script.psf as follows:


# create the parametric study
aStudy=ParStudy (par='load_x', name='job1', directory=ON)

# define the parameter
aStudy.define(DISCRETE, par='load_x', domain=(0.5, 2.))


# sample the parameter
aStudy.sample(NUMBER, par='load_x', number=1)


aStudy.combine(MESH)

# generate analysis data
aStudy.generate(template='job1')

# execute all analysis jobs sequentially
aStudy.execute(ALL,execOptions='user=''vumat_orth.for')

However, if I run it wit the command 'abaqus script=script.psf' there is an ERROR saying that my VUMAT-file can't be found. But it is in the working directory!

Cheers
Fabian

Frank Richter-2 wrote:

Here is a template for your filename.psf with hexp being varied:

parst = ParStudy(par=('hexp'), name='filename',directory=ON)

parst.define(DISCRETE, par='hexp',domain=(-5,-10,-15))
parst.sample(REFERENCE, par='hexp', reference=1, interval=1, numSymPairs=1)

parst.combine(MESH)

parst.generate(template='filename')

parst.execute(ALL,execOptions='user=filename.for')



Frank

[Frank Richter-2]

Hello,

you start your inp-file with

*PARAMETER
hexp = -5

Whenever this value is referred to in the inp-file, you need to put it into parentheses like <hexp>. The psf-file starts a sequence of simulations wherein hexp is replaced with the values given in the list.

See the User's Manual chapter on 'parametric studies'.

Frank


-------- Original-Nachricht --------
> Datum: Thu, 5 Nov 2009 10:37:29 -0800 (PST)
> Von: fehrich <f.ehrich09@...>
> An: ABAQUS@...
> Betreff: Re: [ABAQUS] Parametric study using python with UMAT

>
> Hi Frank,
> Thank you for your answer!
> However, I could not fully follow the procedure...
>
> So I write a filename.psf where I define my parameter (hexp) and how it
> should be varied according to your template.
>
> But how does it relate to my input-file model.inp?
>
> Cheers
> Fabian
>
>
>
> Frank Richter-2 wrote:
> >
> >
> >
> > Here is a template for your filename.psf with hexp being varied:
> >
> > parst = ParStudy(par=('hexp'), name='filename',directory=ON)
> >
> > parst.define(DISCRETE, par='hexp',domain=(-5,-10,-15))
> > parst.sample(REFERENCE, par='hexp', reference=1, interval=1,
> > numSymPairs=1)
> >
> > parst.combine(MESH)
> >
> > parst.generate(template='filename')
> >
> > parst.execute(ALL,execOptions='user=filename.for')
> >
> >
> >
> > Frank
> >
> >
> >
> >
> >
> >
>
> --
> View this message in context:
> http://old.nabble.com/Parametric-study-using-python-with-UMAT-tp14127909p26217369.html
> Sent from the Abaqus Users mailing list archive at Nabble.com.
>

--
-----------------------------------------------------------------------
Frank Richter
Institute of Materials Science
Ruhr-Universitaet Bochum
Bochum
Germany



DSL-Preisknaller: DSL Komplettpakete von GMX schon für
16,99 Euro mtl.!* Hier klicken: http://portal.gmx.net/de/go/dsl02

[fehrich]

Sorry Guys,

as it looks like the name of my VUMAT-file did not go well. Changed the name and now it seems to work.

Thanks you all
Fabian


Hi Frank,
Thank you for your answer!

I now defined my script.psf as follows:


# create the parametric study
aStudy=ParStudy (par='load_x', name='job1', directory=ON)

# define the parameter
aStudy.define(DISCRETE, par='load_x', domain=(0.5, 2.))


# sample the parameter
aStudy.sample(NUMBER, par='load_x', number=1)


aStudy.combine(MESH)

# generate analysis data
aStudy.generate(template='job1')

# execute all analysis jobs sequentially
aStudy.execute(ALL,execOptions='user=''vumat_orth.for')

However, if I run it wit the command 'abaqus script=script.psf' there is an ERROR saying that my VUMAT-file can't be found. But it is in the working directory!

Cheers
Fabian

Frank Richter-2 wrote:

Here is a template for your filename.psf with hexp being varied:

parst = ParStudy(par=('hexp'), name='filename',directory=ON)

parst.define(DISCRETE, par='hexp',domain=(-5,-10,-15))
parst.sample(REFERENCE, par='hexp', reference=1, interval=1, numSymPairs=1)

parst.combine(MESH)

parst.generate(template='filename')

parst.execute(ALL,execOptions='user=filename.for')



Frank

[Frank Richter-2]

Hello group,

we want to understand how ABAQUS computes the bending moment in a beam element.

The theory manual provides an equation following the line
'We now introduce the generalized section forces as defined below:'

This equation depends on f, which is defined as a 'cross-sectional scaling factor'. That definition is provided right at the beginning of the chapter entitled '3.5.2 BEAM ELEMENT FORMULATION'.

From
'the cross-sectional coordinates S_alpha, which are assumed to be distances measured in the original (reference) configuration of the beam'
and requiring consistent units it can be inferred that f is a constant (as the difference in S_beta - S_beta_c must be a factor in order to arrive at Newton*meter for the moment, so this difference is not meant to be a parameter for f).

Can anyone give me a clue how this 'cross-sectional scaling factor' is to be computed in the course of the deformation ?

Thank you for your expertise in advance,

Frank
--
-----------------------------------------------------------------------
Frank Richter
Institute of Materials Science
Ruhr-Universitaet Bochum
Bochum
Germany



DSL-Preisknaller: DSL Komplettpakete von GMX schon für
16,99 Euro mtl.!* Hier klicken: http://portal.gmx.net/de/go/dsl02