Changing young's modulus

classic Classic list List threaded Threaded
5 messages Options
Reply | Threaded
Open this post in threaded view
|

Changing young's modulus

abdulazizsalah
After each step, I want to change the young's modulus of a material. I have written a subroutine in fortran to calculate the new elastic modulus for each time step but I am not sure how or which subroutine to use to transfer the new elastic modulus to Abaqus for each time step.
 

Reply | Threaded
Open this post in threaded view
|

Re: Changing young's modulus

shayan_seg
Hi

Usually, subroutines, such as UMAT, have a parameter for the step number like KSTEP. So, for example, if your material properties reduced by an amount after a particular step, you can easily apply this condition using an IF statement along with the KSTEP in the UMAT. In any cases, you can control this directly in the subroutine by an IF condition.

BR
Seyed Shayan Sajjadinia
Reply | Threaded
Open this post in threaded view
|

Re: Changing young's modulus

George Papazafeiropoulos
In reply to this post by abdulazizsalah
Dear Abdulazizsalah13,
 

 Please check the following Abaqus input file for a possible way to do this:
 

 *Heading
*Preprint, echo=NO, model=NO, history=NO, contact=NO
*Part, name=Part-1
*Node
 1, 0, 0, 0
 2, 1, 0, 0
 3, 1, 1, 0
 4, 0, 1, 0
 5, 0, 0, 1
 6, 1, 0, 1
 7, 1, 1, 1
 8, 0, 1, 1
*Element, type=C3D8R
 1, 1, 2, 3, 4, 5, 6, 7, 8
*Nset, nset=Nall, generate
 1, 8, 1
*Elset, elset=Nall
 1
*Solid Section, elset=Nall, material=Material-1
 ,
*End Part
*Assembly, name=Assembly
*Instance, name=Part-1-1, part=Part-1
*End Instance
*Nset, nset=_PickedSet4, internal, instance=Part-1-1, generate
 1, 4, 1
*Elset, elset=__PickedSurf5_S6, internal, instance=Part-1-1
 1
*Surface, type=ELEMENT, name=_PickedSurf5, internal
 __PickedSurf5_S6, S2
*End Assembly
*Material, name=Material-1
*Elastic, dependencies=1
 3e+06, 0.3, , 1.
 300000., 0.3, , 2.
*Boundary
 _PickedSet4, 1, 1
 _PickedSet4, 2, 2
 _PickedSet4, 3, 3
*Amplitude, name=step
 0,1,1,1
*Initial conditions, type=field, variable=1
 Part-1-1.Nall,1
*Step, name=Step-1, nlgeom=YES
*Static
 1., 1., 1e-05, 1.
*Dsload
 _PickedSurf5, P, 1000.
*Restart, write, frequency=0
*Output, field
*Node Output
 CF, RF, U
*Element Output, directions=YES
 FV, LE, MFR, PE, PEEQ, PEMAG, S, SDV, STATUS, STATUSXFEM, UVARM
*Contact Output
 CDISP, CSTRESS
*Output, history, variable=PRESELECT
*End Step
*Step, name=Step-2, nlgeom=YES
*Static
 1., 1., 1e-05, 1.
*Field, variable=1, amplitude=step
 Part-1-1.Nall,2
*Restart, write, frequency=0
*Output, field
*Node Output
 CF, RF, U
*Element Output, directions=YES
 FV, LE, MFR, PE, PEEQ, PEMAG, S, SDV, STATUS, STATUSXFEM, UVARM
*Contact Output
 CDISP, CSTRESS
*Output, history, variable=PRESELECT
*End Step
 

 Best regards,
 ________________________________________________________
George Papazafeiropoulos
Captain, Infrastructure Engineer, Hellenic Ministry of National Defence
Civil Engineer, M.Sc., Ph.D. candidate, NTUA
Email: [hidden email]


Reply | Threaded
Open this post in threaded view
|

Re: Changing young's modulus

Martin Bäker
In reply to this post by abdulazizsalah
Make young's modulus dependent on a field variable and us UFIELD/USDFLD
to set the variable accordingly.

Am 09 Jul 2019 16:35:03 +0000
schrieb "[hidden email] [Abaqus]" <[hidden email]>:

> After each step, I want to change the young's modulus of a material.
> I have written a subroutine in fortran to calculate the new elastic
> modulus for each time step but I am not sure how or which subroutine
> to use to transfer the new elastic modulus to Abaqus for each time
> step.
>



--
                   Priv.-Doz. Dr. Martin Bäker
                   Institut für Werkstoffe
                   Technische Universität Braunschweig
                   Langer Kamp 8
                   38106 Braunschweig
                   Germany
                   Tel.: 00-49-531-391-3065
                   Fax   00-49-531-391-3058
                   e-mail <[hidden email]>
                   http://www.tu-braunschweig.de/ifw/institut/mitarbeiter/baeker
                http://www.scienceblogs.de/hier-wohnen-drachen
                   Twitter: @Drachenblog
Reply | Threaded
Open this post in threaded view
|

RE: Changing young's modulus

David Lindeman
In reply to this post by abdulazizsalah
Either:


  1.  Define the modulus as a tabular function of a field variable, then calculate and define this field variable value within the USDFLD subroutine.
  2.  Use the UMAT subroutine.

Regards,

Dave Lindeman
Staff Scientist
Corporate Research Systems Laboratory
3M Center 235-3G-08
St. Paul, MN 55144
651-733-6383

From: [hidden email] <[hidden email]>
Sent: Tuesday, July 09, 2019 11:35 AM
To: [hidden email]
Subject: [EXTERNAL] [Abaqus] Changing young's modulus



After each step, I want to change the young's modulus of a material. I have written a subroutine in fortran to calculate the new elastic modulus for each time step but I am not sure how or which subroutine to use to transfer the new elastic modulus to Abaqus for each time step.







________________________________



3M Notice: This communication is from an [EXTERNAL] sender.
If this email looks suspicious, do NOT click or open any links or attachments in the email. To report a suspicious email, click on the Report Phish – Phish Alert icon in the Outlook ribbon or forward this email using the report email as spam link in the text below.

Click here<https://spam.mmm.com/pem/pages/digestProcess/digestProcess.jsf?content=aedaaa864ecbae947655cadeb965d94aae02897fd4c883ade0c51035a25996c9c6c4ff5fb22097b592aab29dac82584f30f60c161a797f8d8d8a621478a2f25250f75f3a4b570e12125b08ef0dd8e5d1dbc7a045714a146255659761471276b9c37b570f20a98a734732948327931bff7a1ab1d0bd24436f2c3880cbe962302417d051a1b719785d> to report this email as spam





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