15.2. Thermal Implicit-to-Explicit Solution

The following is a detailed description of how to perform a thermal implicit-to-explicit sequential solution. Since the temperature loads are step-applied at the beginning of the transient, the analysis should be run for a sufficient amount of time to reduce the effects of the thermal shock loading. If only temperature-dependent material behavior is desired without the effects of thermally induced strain, set the coefficient of thermal expansion equal to zero (ALPX = 0) so that the analysis will be stable from the beginning of the transient. This is a convenient way to vary the modulus of elasticity in a model with only one material definition.

  1. Run the implicit thermal analysis using Jobname1. The only element types that can be used for a thermal implicit-to-explicit sequential solution are:

    PLANE55
    SOLID70
    SHELL131

    Keep in mind that you cannot combine 2-D and 3-D elements in the subsequent explicit analysis. Therefore, you should use only 2-D or only 3-D elements in the thermal analysis phase.

  2. You may define any additional nodes and elements that are necessary to complete the explicit solution. These additional nodes and elements may not be part of the thermal analysis, but they can be defined here if desired. These additional nodes must be constrained to a constant temperature (using D,NODE,TEMP,VALUE).

    Command(s): N, E
    GUI: Main Menu> Preprocessor> Modeling> Create> Nodes or Elements
  3. Solve and finish the analysis.

    Command(s): SOLVE, FINISH
    GUI: Main Menu> Solution> Solve
    Main Menu> Finish
  4. Save the thermal analysis database to file Jobname1.DB.

    Command(s): SAVE
    GUI: Utility Menu> File> Save as

    Note:  If you do not save your Jobname1.DB file at this point, then the database for this thermal run will not be saved. Only the database file for the subsequent explicit run will be saved.


  5. Change to Jobname2 to prevent the thermal results files from being overwritten.

    Command(s): /FILNAME,Jobname2
    GUI: Utility Menu> File> Change Jobname
  6. Reenter the preprocessor.

    Command(s): /PREP7
    GUI: Main Menu> Preprocessor
  7. Convert thermal element types to corresponding companion explicit element types. The corresponding companion thermal-explicit element type pairs are:

    Thermal (Implicit) Element TypeExplicit Element Type
    PLANE55 PLANE162
    SHELL131 SHELL163
    SOLID70 SOLID164
    Command(s): ETCHG,TTE
    GUI: Main Menu> Preprocessor> Element Type> Switch Elem Type
  8. Redefine the key options, real constants, and material property values on the explicit elements. The TYPE, REAL, and MAT numbers from the implicit elements are retained, but the actual key option and real constant values are reset to zero or the default settings. Keep in mind that for temperature loading to take effect, you must use the Temperature Dependent Bilinear Isotropic material model in the explicit analysis.

    Command(s): KEYOPT, R, MP, etc.
    GUI: Main Menu> Preprocessor> Element Type> Real Constants> Material Properties
  9. Define additional nodes and elements, if needed. You may have already completed this task in the thermal analysis portion of the sequential solution (see Step 2). However, if desired, you could wait until the explicit analysis to complete this step.

    Command(s): N, E
    GUI: Main Menu> Preprocessor> Modeling> Create> Nodes or Elements
  10. Reenter the solution processor.

    Command(s): /SOLU
    GUI: Main Menu> Solution
  11. Read temperature results from the thermal analysis results file (Jobname1.RTH) and apply them as loads in the explicit analysis. You can only transfer the temperatures from one time point in the thermal analysis; specify this point by inputting the time value or the corresponding load step and substep numbers on the LDREAD command. If you issue LDREAD more than once, the temperature results specified by the last command will be used.

    Command(s): LDREAD,TEMP
    GUI: Main Menu> Solution> Loading Options> Temp From ANSYS

    The temperatures read in are applied as body loads to the nodes in the explicit model. You can use the BFLIST command to list these temperature loads and the BFDELE command to delete them.

    Command(s): BFLIST, BFDELE
    GUI: Main Menu> Solution> Loading Options> List Temps/Delete Temps
  12. Apply a uniform temperature load, if needed. You can use the TUNIF command (or BFUNIF,TEMP) to apply a uniform temperature load to all nodes in the model. The temperatures read in by LDREAD will overwrite the TUNIF temperature for all nodes that were present in the thermal analysis. Therefore, TUNIF would typically be used only when additional nodes and elements have been defined in the explicit portion of the sequential solution.


    Note:  If you used TUNIF (or BFUNIF,TEMP) to define a uniform temperature in the thermal analysis, the same uniform temperature will be applied automatically to any new nodes added in the explicit analysis phase. If you do not want to apply a uniform temperature in the explicit analysis, you should set TUNIF to zero (or to the TREF temperature, if it is nonzero).


    Command(s): TUNIF
    GUI: Main Menu> Solution> Loading Options> Uniform Temp
  13. Define a reference temperature. The thermal loading is defined as the difference between the applied temperature and the reference temperature. If the reference temperature is not specifically defined, it defaults to zero.

    Command(s): TREF
    GUI: Main Menu> Solution> Loading Options> Reference Temp
  14. Apply any additional loading needed for the explicit run.

    Command(s): EDVEL, EDLOAD, EDCURVE, etc.
    GUI: Main Menu> Solution> Initial Velocity
    Main Menu> Solution> Loading Options> Specify Loads
    Main Menu> Solution> Loading Options> Curve Options
  15. Solve and finish the explicit dynamic analysis.

The following is a sample input stream for performing a thermal implicit-to-explicit sequential solution.

/clear

/title, Thermal Implicit-to-Explicit Sequential Solution

/view,,1,2,3
/plopts,info,1

/filenam,thermal       ! define unique name for thermal analysis

/prep7
et,1,SOLID70           ! thermal brick element
r,1
mp,kxx,1,16.3          ! thermal conductivity, W/m-C
mp,c,1,502.0           ! specific heat, J/kg-C

block,0,1,0,1,0,11     ! create and mesh model
esize,0.5
vmesh,all
finish

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

nsel,s,loc,z,0
d,all,temp,300.0       ! 300 Celsius constraint at far end of beam

nsel,s,loc,z,11
cm,ntip,node
esln
cm,etip,elem
bf,all,hgen,20.0e3     ! 20,000 W/m^3 heat generation at near end ...

esel,all
nsel,s,ext             ! exterior beam nodes 
sf,all,conv,6.0,0.0    ! hf=6.0 W/m^2-C and Tbulk=0 degrees C
nsel,all

save
solve
fini

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


/filnam,explicit       ! define unique name for explicit analysis

/prep7
bfdele,all,all         ! delete thermal analysis heat generation loads
sfdele,all,all         ! delete thermal analysis convection loads
ddele,all,all          ! delete thermal analysis temp. constraints

etchg,tte              ! convert thermal element types to explicit

mp,dens,1,8030.0       ! kg/m^3 - density cannot be temp. dependent
edmp,hgls,1,5          ! add hourglass control

! Define temperature-dependent BISO model

! Specify material temperatures, degrees Celsius
mptemp,1, 0, 500, 700, 900, 1100, 1200

! Modulus of elasticity, N/m^2 (pascal)
mpdata,ex,1,1, 1.93e11, 1.5e11, 1.0e11, 0.9e11, 0.8e11, 0.7e11

! Poisson's ratio, unitless
mpdata,nuxy,1,1, 0.3, 0.31, 0.32, 0.33, 0.34, 0.35

! Coefficient of thermal expansion, m/m-C 
mpdata,alpx,1,1, 1.78e-5, 2.5e-5, 5e-5, 5.5e-5, 6.0e-5, 6.5e-5

tb,biso,1,6
tbtemp,0
tbdata,1,30000,3e6
tbtemp,500
tbdata,1,20000,2e6
tbtemp,700
tbdata,1,10000,1e6
tbtemp,900
tbdata,1,9000,0.9e6
tbtemp,1100
tbdata,1,8000,0.8e6
tbtemp,1200
tbdata,1,7000,0.7e6

edpart,create
eddamp,all,,0.01
fini

/solu
ldread,temp,last,,,,thermal,rth   ! apply temperature body loads
bflist

nsel,s,loc,z,0
d,all,ux,0.0,,,,uy,uz  ! structural displacement constraints
esel,all
nsel,all

time,0.15              ! use sufficient time (see below)

! Note: Since the temperatures are step-applied at the beginning of 
!       the transient, a thermal shock condition is created.  You 
!       should run the analysis for a sufficient amount of time 
!       before adding any structural loads in order for the structure 
!       to stabilize (i.e., stop vibrating).  Animation plots of both 
!       stress and strain are helpful in verifying this condition.  
!
!       Alternately, if only temperature-dependent material properties 
!       (e.g., modulus of elasticity) are desired, you can avoid the 
!       thermal shock condition by setting the coefficient of thermal 
!       expansion equal to zero (ALPX=0).  Large plastic strains can 
!       develop due to a thermal shock scenario, so care must be 
!       used when running a thermal-to-explicit sequential solution.

edrst,100
edhtime,500
edhist,ntip
edhist,etip
edout,glstat
save
solve
fini

/post1
set,last
/dscale,,10            ! 10 times displacement magnification
plnsol,epto,x,2        ! X and Y strains are the same ...


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