Material Exploding into red bits

I am relatively new to Ansys and created a simple collision between 2 blocks. One was fixed and the other was sent at 20 m/s. The only properties I had entered for the blocks were the Young's modulus, poison's ratio, and the density. Once I ran the simulation the stationary block began to fracture and explode into red bits. Does anyone know if Ansys auto fills with generic fatigue, fracture and failure properties? Or why this would happen when these blocks had properties about that of generic 6061? 

 

 

Comments

  • peteroznewmanpeteroznewman Member
    edited February 4

    In Explicit Dynamics, the default setting causes elements that exceed a strain of 1.5 to be automatically deleted from the mesh, and the mass of the deleted element is retained and represented as the red dots.

    You can change this behavior under the Output Controls under the Analysis Settings. It is the Erosion control.

  • edited September 16

    If you don't want the red dots, you can turn off the retain inertia of eroded under the ANALYSIS SETTING>Erosion Control.

  • mjimji Forum Coordinator

    When you have failure criteria, please note that these are different from erosion criteria. Please remember that erosion removes cells from the calculation, so it's typically not representative of the physical process but, rather, a method we use to prevent the timestep from getting too small.

    The erosion strain has no relationship to a specific material. It is merely a numerical input defining when a Lagrangian element should be removed from the calculation, i.e. when its effective strain reaches the specified erosion strain. If you set it too high, then the simulation time-step may be controlled by a srcewed element and drastically reduce slowing down the simulation and possibly lead to increased energy errors. If you set it too low, then the element may be removed too early when it could still be affecting the results. The default is 1.5.

    If all elements that are connected to a node in the mesh erode, the inertia of the resulting free node can be retained if this option is set to Yes. The mass and momentum of the free node is retained and can be involved in subsequent impact events to transfer momentum in the system.

    If set to No, all free nodes will be automatically removed from the analysis.

    You can turn the visibility of eroded nodes for explicit dynamics analyses on or off, go to Display tab,  the Display group contains the Show drop-down menu, where you can turn the visibility of eroded nodes on or off.

Sign In or Register to comment.