Bolted joint comparison to Eurocode

2

Comments

  • peteroznewmanpeteroznewman Member
    edited June 2018

    You did a great job on the mesh so far, I'm sure you can whip the column into shape.

    You also know more about keeping the Shared Topology working now.

  • Fabricio.UrquhartFabricio.Urquhart Rio de JaneiroMember
    edited June 2018
    Thank you Peter!!I I reachef an excelent mesh. Now I am modelling a portic, I am studying how to create join between cross section and solid model.

    Best regards!!
  • Fabricio.UrquhartFabricio.Urquhart Rio de JaneiroMember
    edited June 2018

    Peter, good morning!

    Can you help me, explaning how I use line body orientation?Because element orientation is used to solid or shell bodies. So for line bodies I do not know how I change the orientation. Now I will try to change in the geometry. But is it possible to change in the model?

  • peteroznewmanpeteroznewman Member
    edited June 2018

    I think you have to specify beam section alignment in DesignModeler. You can specify it in Mechanical is it is a geometry operation.

  • Fabricio.UrquhartFabricio.Urquhart Rio de JaneiroMember
    edited June 2018

    Ok. I understood. And the symmetry that I have applied, is it OK for the line bodies?

    Another question, is about the load, I will add a load along the beam, and along the beam modelled by solids. So I have two points:

    1 - The local buckling that will occure in the beam solid, or with the symmetry, the load is applied along the center line?

    2 - Do I have to divide the load for two beacuse the symmetry, yes?

     

    Thank you Peter!!

     

  • peteroznewmanpeteroznewman Member
    edited June 2018

    Loads applied to a model using symmetry must be cut in half if the symmetry plane is cutting the face the load is applied to is cut in half.

    When a beam is perpendicular to a plane of symmetry, that I understand is valid. I am unsure about using a beam that lies in the plane of symmetry. What happens to the cross-sectional area of the beam?  Is it automatically handled or do you have to manually alter the beam cross-section for beams that lie in the plane of symmetry?  I can't say for certain without some research.  You could build a small model to see what happens if you are interested.

    If you are interested in local buckling in an I-beam, don't use beam elements.  Beam elements have a fixed cross-section that cannot have local buckling of one flange in a local area.  If you model an I-beam with shell elements, then the shell elements can buckle out of the plane of the flange.

    Regards,

    Peter

  • Fabricio.UrquhartFabricio.Urquhart Rio de JaneiroMember
    edited June 2018

    I have modeled the cross section with the proprietes of the same solid beam, but the half section, because the symmetry plane, so I think if I apply the load in the half load in the beam, and the same load in the top flange of the solid. It will be Ok. The question was, if the local buckling maybe result different stress results.

    The objective is to analyse the stifness of the bolted connection. But now the problem, I think that is the bolts stress, because when the load starts to be applied, the bolts reach the yield stress.

  • peteroznewmanpeteroznewman Member
    edited June 2018

    LOCALIZED BUCKLING OF I-BEAMS
    You have to decide if you want to include this in the model or not. It requires some serious attention if you do, but I don't think it is central to your study of bolted joint stiffness so I recommend you don't try to include this in your model.

    BEAMS THAT LIE IN THE SYMMETRY PLANE
    You haven't convinced me that you know the correct way to treat these in the model. I want to see three models: (1) a beam without symmetry and a full cross-section, (2) a beam with symmetry with a full cross-section and (3) a beam with symmetry with a half a cross-section. Show me which symmetry model (2) or (3) matches the results of the model without symmetry (1).

    FASTENERS ENTERING PLASTIC DEFORMATION
    This is not a problem when taking a bolted joint past its elastic range. Something has to give and the point of the model is to find out what is going to give first. 

  • Fabricio.UrquhartFabricio.Urquhart Rio de JaneiroMember
    edited June 2018

    Peter, thank you!

    I will not include localized buckling of I-beam.

    I will do those models and find the correct way. After that I show it to you. If I haD difficulty with it, I will ask you.

    Ok, something has to give. But the bolt is given before the load is applied. The bolt gave with the pre-load tension. Did you understand?

     

  • peteroznewmanpeteroznewman Member
    edited June 2018

    Fabricio,

    Some people specify tightening a fastener to its yield point. That is not a problem.

    When you report the beams in the plane of symmetry, a simple model is just a beam in tension.

    Regards,
    Peter

  • Fabricio.UrquhartFabricio.Urquhart Rio de JaneiroMember
    edited June 2018

    Peter, but the fasteners are modeled. I think that you would like to say washers, wouldn't you?

  • peteroznewmanpeteroznewman Member
    edited June 2018

    Fabricio,

    This thing that you modeled with the bolt pretension applied, I call that a fastener, you seem to call it a washer.
    A fastener can have a head on one end and a nut on the other end (or it goes into a threaded hole on the joint).
    A washer is the flat circular piece that goes under the head or the nut to spread the load and reduce the friction.

  • Fabricio.UrquhartFabricio.Urquhart Rio de JaneiroMember
    edited June 2018

    Ok. I understood fastener, in portuguese is "fuste". Peter when I work with simmetry and cross section I have this warning:

    One or more MPC contact regions or remote boundary conditions may have conflicts with other applied boundary conditions or other contact or symmetry regions. This may reduce solution accuracy. Tip: You may graphically display FE Connections from the Solution Information Object for non-cyclic analysis. Refer to Troubleshooting in the Help System for more details.

    I did not understand what you mean when you said: "When you report the beams in the plane of symmetry, a simple model is just a beam in tension"

    How can I use symmetry with beam elements without this warning?I think that is not possible, because the joints.

     

  • peteroznewmanpeteroznewman Member
    edited June 2018

    You can ignore the warning for this demo model. It says "may have conflicts". Symmetry will put constraints on the nodes, then you will add a fixed constraint to one of those nodes and it is warning you about that. But there is no conflict. They each constrain a DOF in the same way, to be zero.

  • Fabricio.UrquhartFabricio.Urquhart Rio de JaneiroMember
    edited June 2018

    If you prefer, we can change this comparation to another topic, involving symmetry with solids and cross section... 

  • peteroznewmanpeteroznewman Member
    edited June 2018

    I did move your posts above to this new topic.

  • Fabricio.UrquhartFabricio.Urquhart Rio de JaneiroMember
    edited June 2018

    Peter, I am studying the problem that is hapenning with de bolts. Do you have any article or post that talk about modelling bolts in Ansys?

    Because I think, that applying pretension and using plasticity it will be ok.

    Thank you!

  • Fabricio.UrquhartFabricio.Urquhart Rio de JaneiroMember
    edited June 2018

    Using boolean in the bolts, this peak of stress disappear. See the picture below:

    Thank you Peter!!

    I am learning a lot with you!!!

     

  • peteroznewmanpeteroznewman Member
    edited June 2018

    The reason is Average Across Bodies is set to No by default.

  • Fabricio.UrquhartFabricio.Urquhart Rio de JaneiroMember
    edited July 2018

    Hello Peter, now the model is OK.

    The difficulty is how to determinate the moment that the solid beam transfer to the solid column, to plot Moment X Rotation. The rotation I take from the directional deformation in the center of the beam and column, dividing for the length.

    But the moment I am trying a way to determinate, do you have any article or reference in Ansys that tell about it?

    Thank you, very much!!

Sign In or Register to comment.