Replacing 3-point bending test without the supports and loading pin ? Solid and shell

Greetings,

Lately I have been trying to examine the various was I can fully simulate a 3-point bending test with my sandwich plate with using both shell cylinders and solid rods while my main body consists of solid elements (I am planning on making a shell body as well). 

More than one time I have faced issues with the supports and loading pin like experiencing loss of contact or lack of constraints.

1) Solid model with shell cylinders

 

2) Solid body with solid rods

 

Is there a way when working with solid elements for the main component to simulate exactly the same simulation but without the additional geometry of the frictionless supports and the top loading bar ? 

I know in shell I can split the faces, makes lines and just use simply supported and also have a force from the top be applied, but I am only interested in solid elements at this moment.

Please let me know if you have any suggestions.

Kindly,

Michael

 

«1

Comments

  • peteroznewmanpeteroznewman Member
    edited July 25

    1) Convergence will be easier to achieve and the solution will take less time to compute if you use two orthogonal planes at the center and slice the sample body in 4 pieces and only simulate 1/4 of the sample, using two Symmetry Regions on the two cutting planes. Note that if your sandwich has honeycomb shaped cell walls, you must position the center cutting plane at a symmetric part of the cell, like at the middle of a cell.

    2) The rods should all be Rigid bodies which means only the outside surface of the rod will be meshed.  You don't need to apply symmetry to the rod bodies. The Remote Displacement boundary condition on each rigid body will control all 6 DOF.

     

  • MichaelDelleMichaelDelle Member
    edited July 25
    Dear Peter,
    So you suggest instead of just choosing the top face of the rod (that I have made by using face split) to deform in the -Z axis by lets say 10mm to use remote displacement. Should I still though choose the same area of the rods ?
    Thank you
  • peteroznewmanpeteroznewman Member
    edited July 25

    Once the rod is a Rigid body, a mesh is only created on the face used in the contact. You move or hold a rigid body by a Remote Displacement.

  • MichaelDelleMichaelDelle Member
    edited July 25
    Hello Peter,
    To make the rods rigid bodies do I do that in Design modeller similarly to how I add them as frozen ?
  • peteroznewmanpeteroznewman Member
    edited July 26

    You assign that in Mechanical by clicking on the body under the Geometry tree and in the Details window change the behavior from Flexible to Rigid.

  • MichaelDelleMichaelDelle Member
    edited July 26

    Dear Peter, I am attaching some screenshots from the analysis. I did everything you told me but the solver is still struggling and I am not getting a final solution.

    1) These are the constraints I have for the type of contact between the main body and the rigid rods.

    2) This is the setup I have for making the rods rigid bodies

     

     

    3) These are the constraints when I am applying the remote displacement for the top rod. For the other 2 rods I have put everything at 0.

    Since they are all rigid bodies only the face that is touching the main body is meshed, meaning that I cannot have the top face of the rod as my selection for the displacement in the -Z axis. 

    is there anything specific that I need to edit ? I am not able to figure out what I have wrong here.

    Kindly, Michael

     

  • peteroznewmanpeteroznewman Member
    edited July 26

    Don't use Frictionless contact, use Frictional and type in a non-zero coefficient.

    Under Analysis Settings, turn on Auto Time Stepping and set the Initial Substeps to 100.

    Convergence would be much easier if you used 2 planes of symmetry as I suggested before.

     

  • MichaelDelleMichaelDelle Member
    edited July 26

    I got this solution with having the bottom supports as flexible bodies and not rigid bodies

    How should I set up the left and right supports though ? I changed their behaviour to flexible and made the bottom side of the cylinder to be fixed supports alongside the faces while the top side is set up as the frictionless contact with the main body. Should I also add a deformation for all the nodes of my sandwich panel for them to deform only in the Z axis ? 

  • MichaelDelleMichaelDelle Member
    edited July 26

    Hello again Peter,

    So I did everything that you suggested and finally the simulation did present quite acceptable solutions.

    I want to ask though. What are the differences of Equivalent stress (Von-Mises) and Normal Stress ? They have different values for the core that I am mostly interested in since its a solid block but with Orthotropic properties (AL 5056). Also, when I press play those values change.

    Equivalent Stress: 

    Normal Stress: 

    Should I add any other solution specifically for the purposes of looking if the honeycomb works as intended ? I just want to show that this method works and that its not necessary to model an actual 3d solid honeycomb. 

    Thank you for your time.

    Michael

  • peteroznewmanpeteroznewman Member
    edited July 26

    Read a Mechanics of Materials / Solid Mechanics / Strength of Materials textbook for the equation that transforms the 3D state of stress with 6 components (3 normal stresses and three shear stresses) into a single value called von-Mises stress and how that is useful to compare the 3D state of stress in a complicated part with complicated loads with the simple state of stress in simple tensile test coupon in a tensile testing machine that measure tensile yield strength.

  • MichaelDelleMichaelDelle Member
    edited July 26
    Hello Peter,
    Thank you so much for you help. I have one last question regarding modelling.
    Would it be possible to model the exact same Geometry in 2D ?
    I did draw everything in DM but then when I went to Model I got the message: Unable to attach geometry file and no valid bodies were found.
    Does that mean if I choose an analysis to be 2D it only can be with surface bodies? Cause in material selection all 3 directions still exist.
    Please let me know,
    Michael
  • peteroznewmanpeteroznewman Member
    edited July 26

    To create a 2D Plane Strain analysis, start a new Static Structural model (don't reuse the last model).

    Create rectangles and circles in the X-Y plane in DM.

    In Workbench, click on the Geometry cell, and in the Properties for that, set the Analysis Type to 2D.

    Open the Model in Mechanical, it will show 2D and you can select the 2D type and set it to Plane Strain.

     

  • MichaelDelleMichaelDelle Member
    edited July 26
    So should I choose create surfaces from sketches ? Or even choose extrude? Or should I just draw the rectangles and the circles and just leave them like that ?
    Thank you,
    Michael
  • MichaelDelleMichaelDelle Member
    edited July 26
    Would it be possible to just show a very simple example on a 2D Plane strain analysis? Maybe you have an example ready in another discussion?
    Please let me know,
    Michael
  • peteroznewmanpeteroznewman Member
    edited July 26

    Create surface from sketch.

  • MichaelDelleMichaelDelle Member
    edited July 26
    Dear Peter,
    On Mechanical I should specify any thickness?
    As for the boundary conditions would there be any difference to what I did before? Maybe just have split lines in order to ensure contact exists.
    Kindly,
    M
  • MichaelDelleMichaelDelle Member
    edited July 26
    Reading from the first forum post, from what I understand, it will not be possible to simulate a plane strain + thermal loading analysis in 2D since thickness is not specified.
    So I should probably just discard that aspect of modelling since after the static structural I was planning on adding a steady state thermal simulation on the model.
    Thank you again for your help Peter.
    Michael
  • MichaelDelleMichaelDelle Member
    edited July 27
    What would you suggest would be the best option for a stress-thermal analysis?
  • peteroznewmanpeteroznewman Member
    edited July 27

    Michael, you will have to remain in a 3D model for a stress-thermal analysis. Please create a New Discussion for that topic.

    Perhaps you have found an answer to the original question posed in this Discussion. If so, please mark that post with Is Solution which will mark this discussion as Solved.

Sign In or Register to comment.