Appendix D. Thermal/Structural Preload Example

This appendix contains an example of a combined thermal/structural preload analysis followed by a structural transient. The example demonstrates the implicit-to-explicit procedure discussed in Implicit-to-Explicit Sequential Solution, with emphasis on how to handle temperature loads in this type of sequential solution (see Special Considerations for Thermal Loading).

The input file creates a cantilever beam structure modeled with thermal brick elements. The analysis is performed in four separate phases. In the first phase, a steady-state heat transfer analysis is conducted using ANSYS thermal elements. A thermal gradient is produced in which the left side of the beam is 20 degrees hotter than the right side.

In the second phase, the thermal elements are converted into ANSYS implicit structural elements. Next, the nonuniform temperatures from the end of the heat transfer analysis are read into the structural model with the LDREAD command. A pressure load is also applied to the top of the beam, and one end of the beam is restrained. A static thermal/structural preload analysis is then conducted.

The results of the second phase show that the temperature gradient causes the beam to bend to the side, and the pressure load causes the beam to bend downward. This is the desired preload condition, which should match the results at the beginning of the subsequent transient dynamic analysis.

In the third phase, the implicit elements are converted into explicit elements and a stress initialization to a prescribed geometry is conducted. This pseudo-dynamic relaxation analysis uses the displacements from the drelax file (but not the temperatures) to establish the preload. The temperatures are applied directly as static thermal loads in the Jobname.K file itself. The results of this analysis (at time = 0) match those of the ANSYS implicit analysis very well.

In phase four, a transient dynamic analysis is conducted. The pressure load is ramped up, while the temperature load is held constant. This is because only one type of thermal load is permitted in any given analysis.

The complete input file is shown below.

fini
/clear

/title, ANSYS LS-DYNA Thermal/Structural Preload Example

! units: kilogram, meter, second, newton, pascal, joule, watts

! = = = = = = = = = = = = = = = = = = = = = = = = = = = = = =

/filnam,thermal

/plopts,info,1
/psf,conv,hcoe,1
/view,,1,2,3

/prep7
et,1,SOLID70           ! thermal brick element
r,1                    ! dummy real constant set

! Temperature-independent thermal material properties:

mp,dens,1,8.03e3       ! kg/m^3
mp,kxx,1,16.3          ! W/m-C
mp,c,1,502.0           ! J/kg-C

block,0,1,0,1,0,11
esize,0.25
vmesh,all
cm,nbeam,node
cm,ebeam,elem
fini

/solu
antype,static          ! steady state heat transfer analysis
time,1.0

nsel,s,loc,x,0         ! left side of beam 
esln
bf,all,hgen,3.0e3      ! 3,000 W/m^3 heat generation on left side

esel,all
nsel,s,ext             ! exterior beam nodes 
nsel,r,loc,x,1.0       ! right side of beam 
sf,all,conv,30.0,0.0   ! hf=30.0 W/m^2-C and Tbulk=0 degrees C
nsel,all

/title, ANSYS Heat Transfer Analysis

save
solve   
fini  

/post1  
set,last
plnsol,temp
/wait,3
save
fini

! = = = = = = = = = = = = = = = = = = = = = = = = = = = =

/filnam,static

/psf,pres,norm,2
/dscale,,1.0

/prep7
bfdele,all,all         ! remove thermal body force (heat generation) loads
sfdele,all,all         ! remove thermal surface (convection) loads

!!!etchg,tts              ! convert SOLID70 elements into SOLID185 elements
!!!keyopt,1,2,1           ! similar formulation to default SOLID164 

et,2,SOLID185          ! desired structural brick element
emodif,all,type,2      ! ETCHG,TTS creates SOLID185 elements 
etdele,1               ! remove thermal bricks
numcmp,type            ! compress element type numbers
keyopt,1,2,1           ! uniform reduced integration to match SOLID164

! Temperature-dependent structural properties

mp,dens,1, 8.03e3               ! kg/m^3 (canNOT be temp-dependent)
mptemp, 1, 0.0, 500.0           ! degrees C, two temperatures 
mpdata,  ex,1,1,193.0e9,93.0e9  ! N/m^2 (temperature-dependent)
mpdata,nuxy,1,1,0.29,0.28       ! unitless (temperature-dependent)
mpdata,alpx,1,1,18.0e-6,16.0e-6 ! m/m-C (temperature-dependent)

! Note:  Do not define plasticity in this ANSYS implicit preload 
!        analysis, since implicit-to-explicit sequential solutions 
!        assume linear elastic material properties and small strain.  
!        Plasticity can be added in the subsequent transient run

mplist,all,all
fini

/solu
antype,static          ! thermal strain (preload) structural analysis

time,1.0
nsubst,2,1000,2
outres,all,last

ldread,temp,last,,,,thermal,rth   ! temperature body loads (overwrites TUNIF)

tref,0.0               ! reference temperature for "instantaneous" alpha
bflist,all,temp

nsel,s,loc,y,1
cm,nbeamtop,node
esln
cm,ebeamtop,elem
sf,all,press,1.1e5     ! apply pressure load (N/m^2) to top of beam

nsel,s,loc,z,0
d,all,uz,0.0           ! restrain aft end of beam
nsel,s,loc,z,0
nsel,r,loc,y,0.5
d,all,uy,0
nsel,s,loc,z,0
nsel,r,loc,x,0.5
d,all,ux,0

nsel,all
esel,all

/title, ANSYS Implicit Static Preload Analysis

save
solve
fini

/post1  
set,last
/dscale,,10            ! exaggerate displacement
plnsol,s,eqv,2
/wait,3

! Note:  Make sure that the yield stress is not exceeded, since 
!        the preload needs to have a linear response for the 
!        subsequent dynamic relaxation analysis

save
fini

! = = = = = = = = = = = = = = = = = = = = = = = = = = = = = = = = = 

/filnam,dynamic

/psf,pres,norm,2
/dscale,,1.0

/prep7
sfdele,all,all         ! remove structural surface (pressure) loads

etchg,ite              ! convert SOLID185 elements into SOLID164 elements

! Add plasticity to temperature-dependent properties

tb,biso,1,2            ! temperature-dependent BISO (2 temperatures)
tbtemp,0.0             ! first temperature
tbdata,1,66.7e6        ! N/m^2, yield stress at 0 degrees
tbdata,2,1.93e9        ! N/m^2, tangent modulus at 0 degrees
tbtemp,500.0           ! second temperature
tbdata,1,60.0e6        ! N/m^2, yield stress at 500 degrees
tbdata,2,0.93e9        ! N/m^2, tangent modulus at 500 degrees

! Note:  Be sure to define a temperature range that exceeds the 
!        actual resulting temperatures.  In this particular case, 
!        LS-DYNA will expect all temperatures to be between 0 and 
!        500 degrees C.  This requirement is on the LS-DYNA side.  

edmp,hgls,1,5          ! add hourglass control
edpart,create          ! create part list

eddamp,all,,0.10       ! mass (alpha) damping
eddamp,1,,1.0e-6       ! stiffness (beta) damping

mplist,all,all
tblist,all,all
fini

/solu
time,0.2               ! termination time (seconds)

rexport,dyna,,,,,static,rst   ! create drelax file

! Note:  The temperatures written to the drelax file are NOT used by 
!        LS-DYNA to establish the thermal preload condition.  Instead, 
!        the temperatures written via the *LOAD_THERMAL_CONSTANT_NODE 
!        command are used.  The latter are stored in the ANSYS database 
!        as body force BF loads from the LDREAD command.  These thermal 
!        loads remain active unless deleted (BFDELE,ALL,TEMP).  

bflist,all,temp        ! no need to re-issue LDREAD command

eddrelax,ansys         ! stress initialization to a prescribed geometry

! Increase the pressure load after a bit to introduce plasticity in 
! the beam.  The beam should remain bent in the XZ plane (due to the 
! thermal load) while bending further downward in the YZ plane.  

*dim,etime,,5,1,1
*dim,epress,,5,1,1
etime(1)=0.0,0.025,0.050,0.100,0.201       ! extend curve out 
epress(1)=1.1e5,1.1e5,2.2e5,2.2e5,4.4e5    ! force into plasticity 
edload,add,press,4,ebeamtop,etime,epress   ! pressure (N/m^2) on beam top

dlist,all,all          ! keep beam restraints from previous implicit run

edrst,100
edhtime,200
edhist,nbeamtop
edhist,ebeamtop
edenergy,1,1,1,1
edout,glstat
edopt,add,,both
edwrite,both,,k

nsel,all
esel,all

/title, ANSYS LS-DYNA Dynamic Relaxation and Transient Analyses

save
solve
fini

/post1  
set,first
/dscale,,10            ! exaggerate displacement

/title, ANSYS LS-DYNA Dynamic Relaxation Analysis
plnsol,s,eqv,2
/wait,3

set,last

/title, ANSYS LS-DYNA Transient Dynamic Analysis (Plastic State)
plnsol,s,eqv,2
/wait,3

save
fini
/exit,nosav

Release 18.2 - © ANSYS, Inc. All rights reserved.