Hi,
In an ABAQUS 2D-planar model, is it possible to vary the material properties spatially, say defining modulus (E) as a function of coordinates, E = f(x,y)? One way is to use *DISTRIBUTION feature, but that allows variation based on element-sets and does not allow varying the material properties as function of coordinates. If anyone has solved this or similar problem kindly suggest.
Thank you
Vaibhav
UMAT
I think you can easily realize this by using UMAT in ABAQUS.
In reply to UMAT by Lihua Jin
Hi Lihua, Nice to meet
Hi Lihua,
Nice to meet you here. I believe we’ve
ever studied together in a summer school on multi-filed couplings organized by Xiangtan University.
How are you getting along with your studying life at Harvard?
Best wishes,
Lianhua
In reply to Hi Lihua, Nice to meet by Lianhua Ma
Hi Lianhua, Yes, we
Hi Lianhua,
Yes, we have met in Xiangtan two years ago. I am pretty good at Harvard. How is everything going for you?
Lihua
In reply to Hi Lianhua, Yes, we by Lihua Jin
Everything goeswell, thank
Everything goes well, thank you.
Let's keep in touch by iMechanica.:)
Lianhua
If the material
If the material parameters are assigned as a function of spatial coordinates,
you can define a field variable in terms of coordinates by the subroutine USDFLD,
and further have the material properties dependent on the defined field
variable in .inp.
The below example of USDFLD code is for your reference only.
USDFLD:
SUBROUTINE USDFLD(FIELD,STATEV,PNEWDT,DIRECT,T,CELENT,
1 TIME,DTIME,CMNAME,ORNAME,NFIELD,NSTATV,NOEL,NPT,LAYER,
2 KSPT,KSTEP,KINC,NDI,NSHR,COORD,JMAC,JMATYP,MATLAYO,
3 LACCFLA)
C
INCLUDE 'ABA_PARAM.INC'
C
CHARACTER*80 CMNAME,ORNAME
CHARACTER*3 FLGRAY(15)
DIMENSION FIELD(NFIELD),STATEV(NSTATV),DIRECT(3,3),
1 T(3,3),TIME(2)
DIMENSION ARRAY(15),JARRAY(15),JMAC(*),JMATYP(*),
1 COORD(*)
x=coord(1)
y=coord(2)
CX=SQRT(x**2+y**2)
FIELD(1)=CX
RETURN
END
inp:
......
......
*Elastic, dependencies=1
5.83333E+11,0.3,,0.6
5.46306E+11,0.3,,0.62
5.12695E+11,0.3,,0.64
4.82094E+11,0.3,,0.66
4.54152E+11,0.3,,0.68
4.28571E+11,0.3,,0.7
4.05093E+11,0.3,,0.72
3.83492E+11,0.3,,0.74
3.63573E+11,0.3,,0.76
3.45168E+11,0.3,,0.78
3.28125E+11,0.3,,0.8
3.12314E+11,0.3,,0.82
2.97619E+11,0.3,,0.84
2.83937E+11,0.3,,0.86
2.71178E+11,0.3,,0.88
2.59259E+11,0.3,,0.9
2.4811E+11,0.3,,0.92
2.37664E+11,0.3,,0.94
2.27865E+11,0.3,,0.96
2.18659E+11,0.3,,0.98
2.1E+11,0.3,,1.
*DEPVAR
1,
*USER DEFINED FIELD
..........
.........
In reply to If the material by Lianhua Ma
hi i m new user of abaqus .. can neone tell me how to vary frict
hi sir , can you please tell me if its possible to vary friction angle in mohr coulomb material parameterwith increse or decrese in plastic strain with usdfld... please suggest other some solution. thanks in advance
About UMAT subroutine
Dear all,
I would like to ask you about prof. Huang's UMAT subroutine. I don't know if anyone have used it. But I have the following questions. The subroutine calculates shear strains and stresses along slip planes. How is it possible to obtain the total stress field? Also the normal stresse?
I could use the field output request simply on the odb of abaqus, but I think the results would not be correct on the basis that you loose the ability to calculate the values along the slip planes. The field output I think is more macroscopic.
Regards,
Panos
thanx and i have also two
thanx and i have also two question
1_is it possible that to have the USDFLD to describe the change of E module as a function of a real time just as in creep with out happing an equation for the function just values for both parameters E and T
2_does anybody know how to simulate a change in the density according to the steps, that for every single step the soil has a density , and this density is going to change in other step ofcourse i need this with out using the order MODEL CHANGE becuse i do not want to get intial stresses are equal to zero
thx for any help
sam