김경종
11 KiB
parameter (zero = 0.d0, half = 0.5d0, one = 1.d0, two=2.d0)
c
dimension rhs(nblock,ndofel), amass(nblock,ndofel,ndofel),
* dtimeStable(nblock),
* svars(nblock,nsvars), energy(nblock,nElEnergy),
* props(nprops), jprops(njprops),
* jElem(nblock), time(nTime), l(nFlags),
* coords(nblock,nnode,ncrd), u(nblock,ndofel),
* du(nblock,ndofel), v(nblock,ndofel), a(nblock, ndofel),
* predef(nblock, nnode, npred, nPred), adlmag(nblock),
* dMassScaleFactor(nblock)
c Notes:
c Define only nonzero entries; the arrays to be defined
c have been zeroed out just before this call
if (jtype .eq. 1001 .and.
* lflags(iProcedure).eq.jDynExplicit) then
area0 = props(1)
eMod = props(2)
anu = props(3)
rho = props(4)
eDampTra = zero
amassFact0 = half*area0*rho
if ( lflags(iOpCode).eq.jMassCalc ) then
do kblock = 1, nblock
c use original distance to compute mass
alenX0 = (coords(kblock,2,1) - coords(kblock,1,1))
alenY0 = (coords(kblock,2,2) - coords(kblock,1,2))
alenZ0 = (coords(kblock,2,3) - coords(kblock,1,3))
alen0 = sqrt(alenX0*alenX0 + alenY0*alenY0 +
* alenZ0*alenZ0)
am0 = amassFact0*alen0
amass(kblock,1,1) = am0
amass(kblock,2,2) = am0
amass(kblock,3,3) = am0
amass(kblock,4,4) = am0
amass(kblock,5,5) = am0
amass(kblock,6,6) = am0
end do
else if ( lflags(iOpCode) .eq.
* jIntForceAndDtStable) then
do kblock = 1, nblock
alenX0 = (coords(kblock,2,1) - coords(kblock,1,1))
alenY0 = (coords(kblock,2,2) - coords(kblock,1,2))
alenZ0 = (coords(kblock,2,3) - coords(kblock,1,3))
alen0 = sqrt(alenX0*alenX0 + alenY0*alenY0 +
* alenZ0*alenZ0)
vol0 = area0*alen0
amElem0 = two*amassFact0*alen0
alenX = alenX0
* + (u(kblock,4) - u(kblock,1))
alenY = alenY0
* + (u(kblock,5) - u(kblock,2))
alenZ = alenZ0
* + (u(kblock,6) - u(kblock,3))
alen = sqrt(alenX*alenX + alenY*alenY + alenZ*alenZ)
area = vol0/alen
ak = area*eMod/alen
c stable time increment for translations
dtimeStable(kblock) = factorStable*sqrt(amElem0/ak)
c force = E * logarithmic strain *current area
strainLog = log(alen/alen0)
fElasTra = eMod*strainLog*area
forceTra = fElasTra
c assemble internal load in RHS
rhs(kblock,1) = -forceTra
rhs(kblock,4) = forceTra
c internal energy calculation
alenOld = svars(kblock,1)
fElasTraOld = svars(kblock,2)
energy(kblock, iElIe) = energy(kblock, iElIe) +
* half*(fElasTra+fElasTraOld)*(alen - alenOld)
c update state variables
svars(kblock,1) = alen
svars(kblock,2) = fElasTra
end do
end if
end if
c
return
end
1.2.15 VUEOS: User subroutine to define equation of state material model.
Product: Abaqus/Explicit
References
• “Equation of state,” Section 25.2.1 of the Abaqus Analysis User’s Guide
• *EOS
“Equation of state material,” Section 2.2.20 of the Abaqus Verification Guide
Overview
User subroutine VUEOS:
• can be used to define the hydrodynamic material model in which the material’s volumetric response is determined by the user-defined equation of state;
• will be called for blocks of material calculation points for which the material definition contains a user-defined equation of state;
• can use and update solution-dependent state variables; and
• can use any field variables that are passed in.
User subroutine interface
subroutine vueos (
C Read only (unmodifiable) variables -
1 nblock,
2 jElem, kIntPt, kLayer, kSecPt,
3 steTime, totalTime, dt, cmname,
4 nstatev, nfieldv, nprops,
5 props, tempOld, tempNew, fieldOld, fieldNew,
6 stateOld, charLength, coordMp,
7 densityMean, refDensity, densityNew,
8 dkk, Em,
C Write only (modifiable) variables -
8 press, dPdRho, dPdEm,
9 stateNew )
C
include 'vaba_param.inc'
C
dimension props(nprops),
1 tempOld(nblock),
2 fieldOld(nblock, nfieldv),
3 stateOld(nblock, nstatev),
4 tempNew(nblock),
5 fieldNew(nblock, nfieldv),
6 charLength(nblock), coordMp(nblock, *),
7 densityMean(nblock), refDensity(nblock),
8 densityNew(nblock),
9 dkk(nblock), Em(nblock),
1 press(nblock), dPdRho(nblock), dPdEm(nblock),
2 stateNew(nblock)
C
character*80 cmname
C
do 100 km = 1, nblock
user coding to define/update press, dPdRho, dPdEm
100 continue
return
end
Variables to be defined
press(nblock)
The material point pressure stress, p.
dPdRho(nblock)
The derivative of the pressure with respect to the density, \partial p / \partial \rho . This quantity is needed for the evaluation of the effective moduli of the material, which enters the stable time increment calculation.
dPdEm(nblock)
The derivative of the pressure with respect to the internal energy, \partial p / \partial E _ { m } . This quantity is needed for the iterative Newton loop used outside of the user subroutine to solve for pressure.
Variable that can be updated
stateNew(nblock,nstatev)
State variables at each material point at the end of the increment. You define the size of this array by allocating space for it (see “User subroutines: overview,” Section 18.1.1 of the Abaqus Analysis User’s Guide, for more information).
Variables passed in for information
nblock
Number of material points to be processed in this call to VUEOS.
jElem(nblock)
Array of element numbers.
kIntPt
Integration point number.
kLayer
Layer number.
kSecPt
Section point number within the current layer.
stepTime
Value of time since the step began.
totalTime
Value of total time. The time at the beginning of the step is given by totalTime - stepTime.
dt
Time increment size.
cmname
User-specified material name, left justified. It is passed in as an uppercase character string. Some internal material models are given names starting with the “ABQ_” character string. To avoid conflict, you should not use “ABQ_” as the leading string for cmname.
nstatev
Number of user-defined state variables that are associated with this material type (you define the number as described in “Allocating space” in “User subroutines: overview,” Section 18.1.1 of the Abaqus Analysis User’s Guide).
nfieldv
Number of user-defined external field variables.
nprops
User-specified number of user-defined material properties.
props(nprops)
User-supplied material properties.
tempOld(nblock)
Temperatures at each material point at the beginning of the increment.
tempNew(nblock)
Temperatures at each material point at the end of the increment.
fieldOld(nblock,nfieldv)
Values of the user-defined field variables at each material point at the beginning of the increment.
fieldNew(nblock,nfieldv)
Values of the user-defined field variables at each material point at the end of the increment.
stateOld(nblock,nstatev)
State variables at each material point at the beginning of the increment.
charLength(nblock)
Characteristic element length, which is either the default value based on the geometric mean or the user-defined characteristic element length defined in user subroutine VUCHARLENGTH. The default value is a typical length of a line across an element for a first-order element; it is half the same typical length for a second-order element. For beams, pipes, and trusses, the default value is a characteristic length along the element axis. For membranes and shells it is a characteristic length in the reference surface. For axisymmetric elements it is a characteristic length in the r–z plane only. For cohesive elements it is equal to the constitutive thickness.
coordMp(nblock,*)
Material point coordinates.
densityMean(nblock)
The mean density.
refDensity(nblock)
The reference density.
densityNew(nblock)
The current density for this increment.
dkk(nblock)
The volumetric strain increment.
Em(nblock)
The element specific internal energy (per unit mass)
Example: User subroutine VUEOS to reproduce results obtained with *EOS, TYPE=USUP
As a simple example of coding of user subroutine VUEOS, consider the following form of the Mie-Grüneisen equation of state with 0.0 and a linear dependency between pressure and internal energy:
p = \rho_ {0} c _ {0} ^ {2} \eta (1 - \frac {\Gamma_ {0} \eta}{2}) + \Gamma_ {0} \rho_ {0} E _ {m},
where \eta = 1 - \rho _ { 0 } / \rho . . Therefore, the results obtained with user subroutine VUEOS should be the same as the results obtained with the linear U _ { s } - U _ { p } type of EOS already available in “Equation of state material,” Section 2.2.20 of the Abaqus Verification Guide.
The code in user subroutine VUEOS must return the pressure, , as in the above equation; the derivative of the pressure with respect to the density, \partial p / \partial \rho ; and the derivative of the pressure with respect to the energy, \partial p / \partial E _ { m } . For the case considered here, these values are
\frac {\partial p}{\partial \rho} = \frac {\rho_ {0} ^ {2} c _ {0} ^ {2}}{\rho^ {2}} (1 - \Gamma_ {0} \eta),
\frac {\partial p}{\partial E _ {m}} = \Gamma_ {0} \rho_ {0}.
$$```fortran
subroutine vueos (
C Read only (unmodifiable) variables -
1 nblock,
2 jElem, kIntPt, kLayer, kSecPt,
3 steTime, totalTime, dt, cmname,
4 nstatev, nfieldv, nprops,
5 props, tempOld, tempNew, fieldOld, fieldNew,
6 stateOld, charLength, coordMp,
7 densityMean, refDensity, densityNew,
8 dkk, Em,
C Write only (modifiable) variables -
8 press, dPdRho, dPdEm,
9 stateNew)
C
include 'vaba_param.inc'
C
dimension props(nprops),
1 tempOld(nblock),
2 fieldOld(nblock,nfieldv),
3 stateOld(nblock,nstatev),
4 tempNew(nblock),
5 fieldNew(nblock,nfieldv),
6 charLength(nblock), coordMp(nblock,*),
7 densityMean(nblock), refDensity(nblock),
8 densityNew(nblock),
9 dkk(nblock), Em(nblock),
1 press(nblock), dPdRho(nblock), dPdEm(nblock),
```
<!-- source-page: 500 -->
```txt
2 stateNew(nblock)
C
character*80 cmname
C
parameter ( zero = 0.d0, one = 1.d0, half = 0.5d0 )
C
c0 = props(1)
gamma0 = props(2)
c02 = c0*c0
C
do k=1, nblock
rho0 = refDensity(k)
eta = one - rho0/densityNew(k)
f1 = rho0*c02*eta*(one-half*gamma0*eta)
f2 = gamma0*rho0
press(k) = f1 + f2*Em(k)
C dP/dEm
dPdEm(k) = f2
C dP/dRho
dPdRho(k) = c02*(rho0/densityNew(k))**2*(one-gamma0*eta)
end do
C
return
end
```