Ultimate load capacity of a beam

Chiddy22Chiddy22 Member Posts: 7

Hello all,

I am trying to verify the load carrying capacity of a concrete beam reinforced with only longitudinal reinforcement at the bottom. For the analysis, I used nonlinear concrete (which has Drucker-Prager strength parameters defined) and nonlinear steel (which has bilinear isotropic hardening parameters defined) available in ANSYS library. I have carried out the analysis but the results does not look right. To get the ultimate load-deflection curve, I plotted a curve of the total deformation against the force reaction and I am getting a straight line graph. I am not sure if these are the correct parameters to plot to get the curve. Please I am still learning to use ANSYS software and I would appreciate advice and help on how to solve this problem.



  • peteroznewmanpeteroznewman Member Posts: 11,075


    You should go to DesignModeler and Form New Part with the Solids so you don't need any contacts. Note that you can't include the Beams.

    Then in Mechanical, add two Mesh Sizing controls so you get exactly 56 nodes (55 elements) along the edges of the concrete and the lines of the rebar.

    Add a Node Merge Group so that one set of nodes along the rebar is shared with the concrete and not separate from the concrete, 2x56 = 112.

    Now change the Fixed Support to two separate Remote Displacements, one holding X,Y,Z and rotation about Z at 0 leaving the rest free, and the other holding X,Y and rotation about Z at 0 and leaving the rest free. Change the Force to Remote Displacement in Y only. Ignore the warning about not enough constraints appear to be applied.

    I solved for 1 mm of displacement at the center. This may not be a large enough value to reach the yield strength of the material.

    Please tell me, from the Concrete material model you used, what is the value of stress that is the threshold for yielding in tension and in compression?

    You didn't say what version of ANSYS you are using. I could have used any version. I used ANSYS 2020 R1 to open your model and make those changes. If you have an older version, you will not be able to open this archive.

  • Chiddy22Chiddy22 Member Posts: 7
    edited December 2020

    Hello Peter,

    Thanks for your reply and the corrections you made to the model. I originally used ANSYS 19.2 to create the model but I have access to ANSYS 2020 R2 and I was able to open the archive. I used a nonlinear concrete model with yield stress of 40MPa in compression and 3.5MPa in tension. Please at what value of displacement do you suggest will the material yield?. Also, what do I have to plot to get the load-displacement curve?

    Thanks a lot for your help, I really appreciate it.

  • peteroznewmanpeteroznewman Member Posts: 11,075


    I used a one-element model to examine the behavior of the two materials in your model, attached as an ANSYS 2020 R1 archive below.

    The Structural Steel NL behaves properly.

    The concrete NL has the following stress-strain curve under a tensile load.

    You claim this material model has a 3.5 MPa tensile yield strength, but I don't see that in this plot.

  • Chiddy22Chiddy22 Member Posts: 7

    Hello @peteroznewman ,

    I used a nonlinear concrete material which is available in ANSYS Engineering Data sources. The material has Drucker-Prager strength parameters defined and a maximum tensile pressure of 4MPa. Please how can I modify the tensile strength of the concrete material?.

  • peteroznewmanpeteroznewman Member Posts: 11,075


    Open ANSYS Help, go to Mechanical APDL. In the Tutorials column is the Technology Showcase: Example Problems, open that. Scroll down to Example 49. Load Limit Analysis of Reinforced Concrete Slab. Read this chapter and do the example. Apply the knowledge you gain here to your problem.

  • Chiddy22Chiddy22 Member Posts: 7

    @peteroznewman I will do that straight away. I didn't know ANSYS had example problems.

    Thanks a lot for your advice and help. I really appreciate it!.

Sign In or Register to comment.