Bending moment a long a beam

ChomanSalihChomanSalih Australia Member Posts: 2
edited November 2020 in Structures

Hi, I am new to Ansys and I have a simple question (I believe). I want to model a beam resting an elastic foundation. I mean insert elastic support>selct bottom face>unput foundation stiffness.

I have modeled and validated this with given analytical equations on Strand 7 with line body. However, I want to model it as a 3d object and when I model the beam as a 3d object in Ansys, I cannot insert the beam results tool in the solution part (the option is not there anymore). I modeled the beam as rexctangular cross section then extrude to the desired length.

There are many videos on Youtube about shear and bending moment diagrams, but they are all for line bodies with defined cross section. I can do that too but the issue that I have is I cannot insert elastic support for the line body. It just doesnt recognise the 3d beam for the elastic support when modeled as a line.

Can anyone suggest how to model a 3d beam with elastic support with the ability of drawing the bending moment diagram along the beam (along x, around z axis)?

I am using Ansys Workbench 2020 R1

thank you

Answers

  • KaiKai Posts: 113Forum Coordinator

    Hi @ChomanSalih , when you model the beam like geometry with beam 188 element (1D beam), Ansys will be using Timoshenko beam theory to do FEA and provides some easy tools for users to extract beam related results under beam tool. When you model the beam like geometry with solid elements such as solid186, Ansys doesn't know the geometry is a beam. Instead, it will treat it as a regular 3D geometry. For this reason, we don't have any beam tools for 3D geometry. What you may do is to extract force reaction and moment reaction under "probe" along different "surface" (construction geometry). This may give you bending moment diagram.

  • pdvelanipdvelani Posts: 7Member

    Hello, @Kai and @ChomanSalih : I am facing the same challange. Also, I could not implement the solution suggested by @Kai. Can anyone of you please elaborate the solution or guide me to some resource please?

  • pdvelanipdvelani Posts: 7Member
    edited July 5

    @Kai : I could generate the "surface" but could not produce a "moment reaction" using "probe". Please find the below screenshot. I want to generate Bending Moment Diagram along the beam.



    My attempt look like this


    While solving it software throws below error


  • ekostsonekostson Posts: 788Ansys Employee
    edited July 5

    Hi


    First use a surface that is along the zy plane (we need the x nodal forces that cause the moment about global z) - finally under analysis settings, and output controls, set all to yes (so nodal forces, etc).


    Finally to generate the internal moments along that part, we would need to have several surfaces and then several moment reaction results (scoped to these different surfaces) in order to get the moment reaction along different locations along the beam.


    All the best


    Erik

  • pdvelanipdvelani Posts: 7Member

    @ekostson

    Hello,

    Thank you for your reply. I have followed the suggested steps but could not get results.


  • ekostsonekostson Posts: 788Ansys Employee
    edited July 5

    Not sure - try it on one single beam/3Dpart so simplest of models (see below).


    Settings:


    That should work

  • pdvelanipdvelani Posts: 7Member
  • peteroznewmanpeteroznewman Posts: 12,548Member

    @pdvelani

    You changed the Options for Mechanical to use in a new project.

    To change the settings for the current project, you have to be in Mechanical and click on the Analysis Settings as Erik highlighted in his images.

  • ekostsonekostson Posts: 788Ansys Employee

    @peteroznewman , many thanks for that.


    please as shown previously change the settings as shown below:


  • pdvelanipdvelani Posts: 7Member

    @peteroznewman @ekostson

    Thank you for your response. I could generate the Bending Moment values.

    However, I need small clarification/insight regarding the results. I am creating different "origins" at the start, at quarter length, at the midpoint, and at end of a beam as shown below.


    The surfaces are created at respective origins and bending moment values are generated. To my surprise except at the midpoint rest 3 locations the answers are not satisfactory. The values at start and end origins are not matching with the moment generated for the "Boundary condition".

    Correct values based on boundary condition --> -8.79 kN.m


    Inoorrect values based on surface--> - 3.686 kN.m


    Can you guide me in fixing the possible error in modelling?


    Further, Do I have to construct a number of origins and surfaces at all desire locations where I need Bending Moments? Is there any better way to construct Bending moments at many locations other than what we are discussing now?

  • ekostsonekostson Posts: 788Ansys Employee

    That is good.

    Further, Do I have to construct a number of origins and surfaces at all desire locations where I need Bending Moments? Is there any better way to construct Bending moments at many locations other than what we are discussing now?

    Yes


    You should have a coordinate system for each surface and each location where we want the moment in/about.

  • pdvelanipdvelani Posts: 7Member

    @ekostson : Thank you. Any feedback on 1st question? Why there is a difference in values from "surface" and "Boundary condition" "moment reactions"?

  • ekostsonekostson Posts: 788Ansys Employee

    One is the moment reaction on a boundary condition, and the one oe is the moment reaction taken where the surface is defined - so one would not use surface to get the moment at a boundary condition say fixed, we would use the boundary condition option, and ofcourse we need to use the surface option to get the reaction in the mesh and away from the boundary condition, say midway along the length of the beam.


    All the best


    Erik

  • pdvelanipdvelani Posts: 7Member
    edited July 6

    @ekostson : Yes, I completely agree with your explanation.

    To verify the bending moment I am generating a surface at 20 mm before the boundary condition (near the right end of beam). The bending moment at this point is 17.23 kN.m which should be less than - 8.79 kN.m (moment obtained at boundary condition). Hence, I am not yet confident about the result and suspect shortcomings in my modelling.

Sign In or Register to comment.