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".

  1. Give example a Title Utility Menu > File > Change Title ...
    /title, Element Death

  2. Open preprocessor menu ANSYS Main Menu > Preprocessor

  3. Create Rectangle Preprocessor > Modeling > Create > Areas > Rectangle > By 2 Corners

    Fill in the window with the following dimensions:
    WP X = 0
    WP Y = 0
    Width = 0.03
    Height = 0.03


  4. Define the Type of Element
  5. Preprocessor > Element Type > Add/Edit/Delete...

    For this example, we will use PLANE55 (Thermal Solid, Quad 4node 55). This element has 4 nodes and a single DOF (temperature) at each node. PLANE55 can only be used for 2 dimensional steady-state or transient thermal analysis.

  6. Define Element Material Properties Preprocessor > Material Props > Material Models > Thermal > Conductivity > Isotropic
    In the window that appears, enter the following properties:
    1. Thermal Conductivity KXX: 1.8

    Preprocessor > Material Props > Material Models > Thermal > Specific Heat
    In the window that appears, enter the following properties:
    1. Specific Heat C: 2040

    Preprocessor > Material Props > Material Models > Thermal > Density
    In the window that appears, enter the following properties:
    1. Density DENS: 920

  7. Define Mesh Size Preprocessor > Meshing > Size Cntrls > ManualSize > Areas > All Areas...

    For this example we will use an element edge length of 0.0005m.

  8. Mesh the frame Preprocessor > Meshing > Mesh > Areas > Free > click 'Pick All'

  1. Define Analysis Type
  2. Solution > Analysis Type > New Analysis > Transient

    The window shown below will pop up. We will use the defaults, so click OK.


  3. 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.

  4. Set Solution Controls
  5. Solution > Analysis Type > Sol'n Controls

    The following window will pop up.

    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.

  6. Apply Initial Conditions
  7. Solution > Define Loads > Apply > Initial Condit'n > Define > Pick All

    Fill in the IC window as follows to set the initial temperature of the material to 268 K:

  8. Apply Boundary Conditions
  9. 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.

    Solution > Define Loads > Apply > Thermal > Convection > On Lines > Pick All

    Fill in the pop-up window as follows, with a film coefficient of 10 and a bulk temperature of 368.

    The model should now look as follows:

  10. Solve the System
  11. Solution > Solve > Current LS

  1. Read Results General Postproc > Read Results > Last Set

  2. Create Element Table

    Element 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.

  3. Select Elements to Kill

    Assume 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 > Entities

    Use 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.

  1. 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.

  2. Kill Elements

    The 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.

  1. Select Live Elements Utility Menu > Select > Entities

    Fill 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.

  2. View Results General Postproc > Plot Results > Contour Plot > Nodal Solu > DOF solution > Temperature TEMP

    The final melted shape should look as follows:

    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.

The above example was solved using a mixture of the Graphical User Interface (or GUI) and the command language interface of ANSYS. This problem has also been solved using the ANSYS command language interface that you may want to browse. Open the .HTML version, copy and paste the code into Notepad or a similar text editor and save it to your computer. Now go to 'File > Read input from...' and select the file. A .PDF version is also available for printing.