General Mechanical

General Mechanical

VCCT Calculation, Energy release rate mode III

    • Ali_sh
      Subscriber

      Hello,

      I am using ANSYS 2021 R1 to calculate energy release rate for mode III.

      The ANSYS fracture tool distribution of energy release rate is different when I obtain the energy release rate from nodal value directly. They are totally different at one side; moreover, there is a small difference between the values of Fracture tool and my calculation.

      I have attached here both the values and graph.

      Direct VCCT is the result of Fracture tool. In nodal VCCT, I export nodal force and displacement directly and calculate VCCT using the same formula that ANSYS uses.

      ANSYS help for VCCT: https://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v212/en/ans_frac/frac_parmcalctypes.html%23advvcctenrelrate

      Does anyone have any suggestions about the root of this inconsistency and how I can solve it?

      Thank you.

    • David Weed
      Ansys Employee

      For the last calculation, is the reaction force recorded as zero on that node?
    • Ali_sh
      Subscriber
      Hi @davidW Actually no. The value of force and displacement are not zero at that node.
    • David Weed
      Ansys Employee
      Thanks, just curious as to how the value came out to zero at that node. Can you give a bit more detail about the loading and general model setup?
    • Ali_sh
      Subscriber

      Thank you for your answer.
      I modeled DCB under mix mode I & III loading condition. I attached the geometry here.
      Indeed, the problem is not limited to the value of edges merely.
      I have attached here the distribution of mode I and mode III energy release rate. The fracture tool cannot obtain energy release rate at the edges and center of the specimen for both mode I & III when I use a refined mesh. However, the nodal vcct works perfect. (Nodal VCCT: First, extract the nodal force and displacement and calculate the energy release rate myself)
      In my opinion, this is a postprocess error, because I have to arrange(sort) the data to calculate the energy release rate myself.
      I hope you can help me to solve this problem. My colleagues ask me to switch to ABAQUS instead of working with ANSYS to analyze the fracture behavior.

    • David Weed
      Ansys Employee
      thanks for the additional detail. Would it be possible to scale down the model (mesh-wise) and then post your ds.dat code, leaving out extraneous details, as a forum post/comment here (unfortunately, we don't allow users to share actual files as attachments)? If we can get the APDL commands which have produced the model, we can take a closer look.
    • Ali_sh
      Subscriber
      Dear Hi I am really sorry for the late answer.
      I have attached here a simplified model(the .dat file).
      Again, I calculate ERR by formula and plot it against the fracture tool for mode I and mode III.
      Thank you for your time.
    • Ali_sh
      Subscriber

      Another problem that I have with the fracture tool comes from the local coordinate system of the crack tip.
      I explain it here.
      For example, the first picture shows the ERR for mode I and III for the defined coordinate system. However, clearly, this is not correct. (in both images, the right is the mode I, and the left is mode III)
      By rotating the coordinate system, the value becomes acceptable somehow. (the edge and center values are not satisfactory)
      By definition, both of them must work; nevertheless, the fracture tool cannot calculate the ERR in the first case.
      Indeed, the crack-normal and the crack-tangent are well defined by each method.

    • Ali_sh
      Subscriber
      Hello
      It has been some days, and I could not find almost anything in this forum. Can anyone have a discussion on this, please?

      Bests Ali
    • Ali_sh
      Subscriber
      Dear Would you please take a look at the file and help me with the issue that I have?

      Bests Ali Shivaie
    • David Weed
      Ansys Employee
      going to check in with our developers on this and get back soon.
    • David Weed
      Ansys Employee
      the local crack cs appears to be flush with the crack front. Can you move it slightly, so that it is still on the open side of the crack, but not flush with the crack front?
    • Ali_sh
      Subscriber

      I appreciate your help.
      I checked what you mentioned, and it solved the problem.
      I attached the result here.

    • David Weed
      Ansys Employee
      this looks good. This is stated in the help, but it's a bit obscure: https://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v221/en/wb_sim/ds_crack_overview.html
      For thePre-Meshed CrackandArbitrary Crackobjects, the origin of the coordinate system must be located on the open side of the crack.
Viewing 13 reply threads
  • You must be logged in to reply to this topic.