I want to simulate placing an object, for simplicity sake a cube, with an elevated temperature on a plate which starts at room temperature. The cube would transfer heat to the plate and after a time would be removed. At this point I want to reset cube’s temperature to simulate a different object under the same initial conditions as the first being placed on the plate, but the plate inherits the end conditions of the last step. I want to determine the resultant max temperature of the plate after n number of cycles as well as the temperature of the cube after cooling on the plate.
Setting the initial conditions and appropriate surface constraints works for the first step, but I have not yet figured out how to reset the temperature of the cube for subsequent steps. Is this possible or is there another way of going about this? Thanks.
You can use amplitudes to control the time variation of boundary conditions (including prescribed temperature) and loads (including prescribed heat flux and body heat source). So you can increase it, then decrease it, let it cool down and increase again and so on. Another way would be to use a thermomechanical analysis where the hot cubes would be physically moved and removed from the plate, using thermal contact between them and the plate but that would be more computationally expensive.
I’ve tried using amplitudes but the problem with this approach is the temperature curve of the cube changes as the plate heats. It’s one of the variables I want to solve for, so I can’t define it as an input.
It doesn’t have to be a temperature boundary condition for the whole cube, maybe just on one of its faces or heat flux load instead. Then the temperature of the cube will be allowed to change.
But the second approach mentioned above can make more sense in such a case. Instead of moving the objects, you could also try activating and deactivating contact between them and the plate via *MODEL CHANGE, TYPE=CONTACT PAIR (added using Keyword Editor). There would be no contact between the hot objects themselves so they wouldn’t “see” each other. Something similar is sometimes done for repeated impact simulations.
I did a very similar simulation some time ago for a project. The goal was to simulate the increase in temperature of a tooling, loaded with hot discs (400°C) for 1 hour with a frequency of 1,5 parts per minute (40s cycle time). The practical test showed good agreement for the three measurment points and almost reached steady state:
It’s an uncoupled thermo-mechanical simulation:
In Step-1 i used a heatflux which heats up the disc from top and bottom side in 2 seconds to 400°C:
Flux= PW/A > PW= mc(Tf-Tin)/t
PW= heating power
A= flux acting area
m= mass
c= specific heat capacity
Tf/Tin = final/initial temperature
t= 2s
Step-2 (2 seconds waiting) is used to reach a balanced, constand temperature over the whole disc thickness.
In Step-3 the tooling gets into contact for 6 seconds.
In Step-5, i reseted the disc temperature to it’s initial 22°C by increasing the film amplitude for one second, which needs to be done by Keyword editing in prepomax:
