While doing a snapfit analysis in optistruct, I have given an enforced displacement to one component. While running it in simulation, both the components starts moving simultaneously

Anuj Nandal_21754
Anuj Nandal_21754 Altair Community Member
edited March 2022 in Community Q&A

Please refer to the file attached for reference. As it can be seen that the horizontal beam starts moving before coming in contact. Can someone please help regarding this.image

Tagged:

Answers

  • PaulAltair
    PaulAltair
    Altair Employee
    edited March 2022

    You are displaying the results in linear animation mode (so what you are seeing is a linear interpolation of the final state, not each state in 'time') you need to view in 'transient' mode to view the increments

    image

    When you view it that way, I don't get that with the model you attached. I get the opposite problem (yours on left below) it passes through visually, as you have set a clearance of 5.8mm on the contact, if I reset clearance to blank it looks better (mine on right), my fem and h3d attached

    image

  • Anuj Nandal_21754
    Anuj Nandal_21754 Altair Community Member
    edited March 2022
    Paul Sharp_21301 said:

    You are displaying the results in linear animation mode (so what you are seeing is a linear interpolation of the final state, not each state in 'time') you need to view in 'transient' mode to view the increments

    image

    When you view it that way, I don't get that with the model you attached. I get the opposite problem (yours on left below) it passes through visually, as you have set a clearance of 5.8mm on the contact, if I reset clearance to blank it looks better (mine on right), my fem and h3d attached

    image

    Hey Paul, thanks for being quick with the response, really appreciate this. I just wanted to know if there was any way by which I could show a snap fit simulation through this. Because as of now even with your file, seems like the 2 component stick together, I wanted the horizontal beam to slide back to original position (like a snap fit). I did try increasing the enforced displacement, seems like it is diverging.

  • PaulAltair
    PaulAltair
    Altair Employee
    edited March 2022
    Anuj Nandal_21754 said:

    Hey Paul, thanks for being quick with the response, really appreciate this. I just wanted to know if there was any way by which I could show a snap fit simulation through this. Because as of now even with your file, seems like the 2 component stick together, I wanted the horizontal beam to slide back to original position (like a snap fit). I did try increasing the enforced displacement, seems like it is diverging.

    In the attached, run4 I switched contact to n2s and Consli, with a PCONT with small friction values and STEXP set (to better account for different stiffnesses during iterations) and increased the displacement to 28mm, that seems to work ok

    I tried adding in your plastic mat props (run5) and then it still gets stuck at the end, but I think that might just be down to coarseness of the mesh and the cantilever is plasticly deformed

Categories