Hi Dennis,
First off, welcome to the Autodesk forums. Second, Simulation Mechanical is a name of a program produced by Autodesk. If your questions are strictly about Fusion 360, then I will move this thread to the Fusion forum. If you are more interested in whether any Autodesk software can handle it, then I will move this thread of appropriate.
There are several aspects to your question, so I am listing them here and answering them at the bottom:
- A flat plate (flat) is heated. Thermal and mechanical loads should be combined.
- Then pressed into a organic shaped mould by a punch (counterpart).
- The punch is removed.
- After the pressing process, the plate that has now been brought into shape is removed.
- Is there a way in Fusion360 to simulate plastic behaviour?
1. If the plate has a uniform temperature, and if the temperature change is insignificant during the punching operation, then thermal loads are not important. The material properties at the operating temperature can be entered; there would be no need to enter temperature-dependent material properties. (I am also ignoring the thermal expansion, which I assume is small compared to the punching operation.)
If the temperature is not uniform but constant throughout the process, this step could be handed by Inventor and Inventor Nastran in a Nonlinear Static analysis. (Inventor Nastran also has nonlinear static and Event Simulation, just like Fusion 360.) Fusion does not have temperature loads in a Nonlinear or Event Simulation analysis.
If there is a significant temperature change in the plate during the operation, then you will need software that can handle the combined heat transfer and nonlinear, large displacement analysis together. Autodesk does not have any software that can handle that.
Last thing about this step. I am not clear if the heating process is part of your analysis (such as how long it takes and what the temperature distribution is), or if you only need to specify that the plate has a temperature of X degrees. Inventor Nastran has steady state and transient heat transfer analysis; Fusion only has steady state heat transfer.
2. You may be able to do this step with Fusion, using either Nonlinear Static (if the duration is long, like 1 second or longer) or Event Simulation (if the duration is short, like 0.001 second or shorter). One issue you did not mention is how thick the plate is. If it is thin, you should not analyze it with Fusion because Fusion only has solid elements, and thin-walled items modeled as solids is not accurate. Instead, Inventor Nastran should be used where the thin-walled items can be modeled using shell elements.
Another potential problem is the amount of strain. Convergence can be a problem at high strain values.
3. This step can be done in Fusion using Event Simulation, so the total duration needs to be short. It can be done in Inventor Nastran using either nonlinear static or Event Simulation.
4. This step can be done in Fusion using Event Simulation, so the duration needs to be short. It can be done in Inventor Nastran using either nonlinear static or Event Simulation.
5. Both Fusion 360 and Inventor Nastran have nonlinear material behavior. They follow von Mises or Tresca yield criterion, Isotropic or Kinematic hardening rules. Note that these material behaviors do not include a strain rate which could be important depending on the cycle time. (Both Fusion and Inventor Nastran have Mohr - Coulomb and Drucker - Prager material behavior, but I think those soils-related properties are not appropriate for your plastic. 😉)
Let us know if you have any other questions.
John Holtz, P.E. Global Product Support
Autodesk, Inc. If not provided already, be sure to indicate the version of Inventor Nastran you are using!"The knowledge you seek is at knowledge.autodesk.com" - Confucius 😉