Introduction
This tutorial was completed using ANSYS 7.0 The purpose of the tutorial is to outline the steps required to use element death to model melting of a material. Element death is the "turning off" of elements according to some desired criterion. The elements are still technically there, they just have zero stiffness and thus have no affect on the model.
This tutorial doesn't take into account heat of fusion or changes in thermal properties over temperature ranges, rather it is concerned with the element death procedure. More accurate models using element death can then be created as required. Element birth is also possible, but will not be discussed here. For further information, see Chapter 10 of the Advanced Guide in the ANSYS help file regarding element birth and death.
The model will be an infinitely long rectangular block of material 3cm X 3cm as shown below. It will be subject to convection heating which will cause the block to "melt".
Preprocessing: Defining the Problem
- Give example a Title
Utility Menu > File > Change Title ...
/title, Element Death - Open preprocessor menu
ANSYS Main Menu > Preprocessor
/PREP7 - Create Rectangle
Preprocessor > Modeling > Create > Areas > Rectangle > By 2 CornersFill in the window with the following dimensions:
WP X = 0
WP Y = 0
Width = 0.03
Height = 0.03
BLC4,0,0,0.03,0.03 - Define the Type of Element
- Define Element Material Properties
Preprocessor > Material Props > Material Models > Thermal > Conductivity > Isotropic
In the window that appears, enter the following properties:- Thermal Conductivity KXX: 1.8
Preprocessor > Material Props > Material Models > Thermal > Specific Heat
In the window that appears, enter the following properties:- Specific Heat C: 2040
Preprocessor > Material Props > Material Models > Thermal > Density
In the window that appears, enter the following properties:- Density DENS: 920
- Define Mesh Size
Preprocessor > Meshing > Size Cntrls > ManualSize > Areas > All Areas...For this example we will use an element edge length of 0.0005m. - Mesh the frame
Preprocessor > Meshing > Mesh > Areas > Free > click 'Pick All'
Solution Phase: Assigning Loads and Solving
- Define Analysis Type
- Turn on Newton-Raphson solver
Due to a glitch in the ANSYS software, there is no apparent way to do this with the graphical user interface. Therefore, you must type NROPT,FULL into the commmand line. This step is necessary as element killing can only be done when the N-R solver has been used. - Set Solution Controls
- Apply Initial Conditions
- Apply Boundary Conditions For thermal problems, constraints can be in the form of Temperature, Heat Flow, Convection, Heat Flux, Heat Generation, or Radiation. In this example, all external surfaces of the material will be subject to convection with a coefficient of 10 W/m^2*K and a surrounding temperature of 368 K.
- Solve the System
ANTYPE,4
A) Set Time at end of loadstep to 60 and Automatic time stepping to OFF.
B) Set Number of substeps to 20.
C) Set the Frequency to Write every substep.
Click on the NonLinear tab at the top and fill it in as shown
D) Set Line search to ON .
E) Set the Maximum number of iterations to 100.
For a complete description of what these options do, refer to the help file. Basically, the time at the end of the load step is how long the transient analysis will run and the number of substeps defines how the load is broken up. By writing the data at every step, you can create animations over time and the other options help the problem converge quickly.
The model should now look as follows:
SOLVE
Postprocessing: Prepare for Element Death
- Read Results
General Postproc > Read Results > Last Set
SET,LAST - Create Element TableElement death can be used in various ways. For instance, the user can manually kill, or turn off, elements to create the desired effect. Here, we will use data from the analysis to kill the necessary elements to model melting. Assume the material melts at 273 K. We must create an element table containing the temperature of all the elements.
- From the General Postprocessor menu select Element Table > Define Table...
- Click on 'Add...'
- Fill the window in as shown below, with a title Melty and select DOF solution > Temperature TEMP and click OK.
We can now select elements from this table in the temperature range we desire.
- Select Elements to KillAssume that the melting temperature is 273 K, thus any element with a temperature of 273 or greater must be killed to simulate melting.
Utility Menu > Select > EntitiesUse the scroll down menus to select Elements > By Results > From Full and click OK.
Ensure the element table Melty is selected and enter a VMIN value of 273 as shown.
Solution Phase: Killing Elements
- Restart the Analysis
Solution > Analysis Type > Restart > OK You will likely have two messages pop up at this point. Click OK to restart the analysis, and close the warning message. The reason for the warning is ANSYS defaults to a multi-frame restart, which this analysis doesn't call for, thus it is just warning the user. - Kill ElementsThe easiest way to do this is to type ekill,all into the command line. Since all elements above melting temperature had been selected, this will kill only those elements.
The other option is to use Solution > Load Step Opts > Other > Birth & Death > Kill Elements and graphically pick all the melted elements. This is much too time consuming in this case.
Postprocessing: Viewing Results
- Select Live Elements
Utility Menu > Select > EntitiesFill in the window as shown with Elements > Live Elem's > Unselect and click Sele All.
With the window still open, select Elements > Live Elem's > From Full and click OK.
This procedure can be programmed in a loop, using command line code, to more accurately model element death over time. Rather than running the analysis for a time of 60 and killing any elements above melting temperature at the end, a check can be done after each substep to see if any elements are above the specified temperature and be killed at that point. That way, the prescribed convection can then act on the elements below those killed, more accurately modelling the heating process.
ANSYS Command Listing
finish
/clear
/title, Convection Example
/prep7 ! Enter the preprocessor
! define geometry
k,1,0,0 ! Define keypoints
k,2,0.03,0
k,3,0.03,0.03
k,4,0,0.03
a,1,2,3,4 ! Connect the keypoints to form area
! mesh 2D areas
ET,1,Plane55 ! Element type
MP,Dens,1,920 ! Define density
mp,c,1,2040 ! Define specific heat
mp,kxx,1,1.8 ! Define heat transfer coefficient
esize,0.0005 ! Mesh size
amesh,all ! Mesh area
finish
/solu ! Enter solution phase
antype,4 ! Transient analysis
time,60 ! Time at end of analysis
nropt,full ! Newton Raphson - full
lumpm,0 ! Lumped mass off
nsubst,20 ! Number of substeps, 20
neqit,100 ! Max no. of iterations
autots,off ! Auto time search off
lnsrch,on ! Line search on
outres,all,all ! Output data for all substeps
kbc,1 ! Load applied in steps, not ramped
IC,all,temp,268 ! Initial conditions, temp = 268
nsel,s,ext ! Node select all exterior nodes
sf,all,conv,10,368 ! Apply a convection BC
nsel,all ! Reselect all nodes
/gst,off ! Turn off graphical convergence monitor
solve
finish
/post1 ! Enter postprocessor
set,last ! Read in last subset of data
etable,melty,temp, ! Create an element table
esel,s,etab,melty,273 ! Select all elements from table above 273
finish
/solu ! Re-enter solution phase
antype,,rest ! Restart analysis
ekill,all ! Kill all selected elements
esel,all ! Re-select all elements
finish
/post1 ! Re-enter postprocessor
set,last ! Read in last subset of data
esel,s,live ! Select all live elements
plnsol,temp ! Plot the temp contour of the live elements
Posts
0 comments:
Post a Comment