Did you know how easy it is to simulate thermal bonding in ANSYS Mechanical? You do not have to use our Element Birth/Death extension or deal with pinball regions. You can just raise the temperature of the body in a Static Structural analysis with a simple Thermal Condition. An example of this is below.
The secret to doing this is the TBND property, good ole real constant #35. If this seems like gibberish to you, this may be a good time to check out the Contact Technology Guide in the Mechanical APDL documentation or to check out the image below:
Your contact in Mechanical already has a real constant that contains things like the normal contact stiffness (#3: FKN) and pinball region (#6: PINB) and all the other extra information that goes into contacts. If we want to add to this for a given contact, we can insert a command object and take advantage of the helpful cid and tid parameters that Mechanical provides. Taking advantage of TBND is as simple as using the appropriate APDL command to set real constant 35 to our critical bonding temperature of 30 (units in whatever you have selected at the time). We have to do this twice just in case the auto-symmetric algorithm switches the target and contact surface on us (make sure to review the Mechanical Nonlinearities Training if you don’t know what this means).
The once the temperature of the contact surface exceeds the TBND temperature, they are bonded forever. If you are feeling frisky, you can substitute an APDL table (or even a UPF) and have the bonded behavior depend on time, temperature, contact pressure or penetration. In this scenario, instead of setting a critical bonding temperature you would return 1 or greater to change to bonded, depending on the quantity that you choose. A nice way to simulate other types of adhesion!
You can download the project shown in the above animation below:
If this was useful to you and you’d like to hear more, subscribe to our newsletter below: