General Mechanical

General Mechanical

Topics relate to Mechanical Enterprise, Motion, Additive Print and more

Divergence due to Highly distorted element with Cohesive zone model crack

    • cheng089413


      I am modeling the crack of ANISO material near the bolt hole based on cohesize zone model, so a bonded contact was created along the predefined crack line and assigned the energy based cohesive zone material. Now the model diverged at a load step.

      Since this bonded contact is intended to open based on CZM criterion, i can see the high Newton raphson residual force on the exposed contact surface inside one element. Also the elements were highly distorted at the last load step. The substeps were already 50 to apply a 2.5mm displacement and still diverged.

      Can anyone give an idea on how to resolve this issue? I am not sure how to change the settings of the bonded cantact defined as CZM given it is supposed to open up.

      Appreciate any discussions or help!



    • cheng089413

      Can anyone give any advice on this? 

      Thank you!

    • David Weed
      Ansys Employee

      Hi, can you show a screen capture of the following:

      1) debonding parameters in Engineering data

      2) CZM contact settings in Mechanical

      3) Analysis settings substep information

      Also, use the contact tool to see what the contact pressure and gap look like at the CZM interface. If it is recording anything, please show a screen capture of that as well.

      • cheng089413

        Hello David,

        Thank you so much for your reply.

        I refined the mesh again and the model output new results and new problems as well. 

        This is a little descriptions about the model. I tried to model a wooden beam (placed vertically in the figure) connected to a column (horizontal one) by steel bolts. At the back shows the steel plate with bolt holes as well to connect the beam and column together. A symmetry plane was created to cut the model into to halves to reduce the work. A displacement loading was applied onto the top of the beam and was divided into 15 load steps with 2.5 mm of increment each. The beam is expected to show brittle failure due to cracks on wood. So I broke down the beam into three multi-body parts (①②③in Fig.1 and created bonded contacts (red lines) with Cohesive zone model between them to simulate the cracks.

        Fig.1 overview of the model

        Fig.2 Back of the model with symmetry plane

        The original post was a model that diverged and now this new model came up with convergent solution. However the crack pattern was not as expected. I expected the cracks to occurred along the red lines in Fig.1 where the CZM interface were created. Usually the cracks started from the bolt holes where the stresses level are high and developed vertically. Now the cracks started at a distance from the bolt holes (Fig.3). and in Fig.4 the local crack did not completely open the full interface which I don’t get why. I expect the crack can be developed along the two vertical lines eventually and lead to the significant drop in the reaction force on the displacement boundary condition. Now the reaction force kept going up and the whole structure did not fail.

        Fig 3 Crack pattern results

        Fig.4 local crack not fully debonded

        As requested the CZM contact settings, analysis settings and CZM material parameters are shown in the last few figures. Also the wood around the bolt holes was modeled as ANISO material by APDL command, for which I also attached a figure. It looks like from the contact tools the other CZM contacts were quite sticky even at the last few substeps. There was no crack at all along the left vertical line. Maybe the settings of the contact or the CZM parameters made so?




      • cheng089413

        Hello David,

        Just a follow up by reviewing the help document of ANSYS about CZM.

        It is said the Pinball radius has to be greater than the maximum separation distance (which is calculated as 0.178mm in my case). It looks like all the PINB of the czm contact satisfy this requirement.

        Also by removing the steel plate in the back i found out there was a through crack there in one of the predefined crack line (Fig.2). Still no idea why the crack cannot be triggered at the other predefined crack line.

        Thank you in advance for your help!

    • cheng089413

      Hi, can anyone give some advice on this model?😉

    • John Doyle
      Ansys Employee

      It is not clear to me from your description, and the pictures, if the convergence failure is indicative of a numerical instability or a physical instability.

      What is your expectation for this application?

      Sometimes it is helpful to post process reaction force vs displacement to ascertain the state of structural stiffness at the point of non-convergence.

      If the structure is going completely plastic thru an entire cross section and CZM is beginning, perhaps the structure lacks sufficient stiffness to resist further loading and the non-convergence is indicative of a physical failure.

      If there is plenty of stiffness in the structure and the convergence failure is exclusively a numerical instability, you could try a number of different things in addition to what you already mentioned about contact stiffness factor:

      • Use many more substeps
      • Add stabilization damping
      • Try dropping midside nodes (in the first pictures you shared, there appeared to be some local hour glassing in a few of the elements at the corner)
      • Sometimes, it helps to add a frictional contact pair on top of the bonded pair to help stabilize the elements at the CZM surface after debonding begins.
      • Force Full Unsymmetric solver (for enhanced solver robustness after debonding)
      • Consider adding local damping to the CZM material model (refer to Section 4.20.5 on ‘Viscous Regulation’ of CZM in the Material Reference Guide.
    • cheng089413

      Hello John, thank you for your professional advice.

      I wanted the czm bonding contacts to debond at the two predefined interfaces. However the debonding only occurred in one of them. 

      1. May I ask how i can visualize or output in WB the energy release rates for modes I and II since the CZM is using the energy related criterion in my model? I wanna check whether the mixed mode criterion was met or not.
      2. The czm region is with high stress levels since it is a bolt hole which is hidden for checking the high newton raphson residuals. Will dropping the midside nodes affect the calculation accuracy per your understanding?
      3. Yes the solution was already set as unsymmetric solver;
      4. Can you elaborate a little bit on how to add a fritional contact pair on top of the bonded pair? I don't know i could add two types of contacts on the same interface.
      5. I read the viscous regulation section and can you give me some idea what value i should set it as the first try?

      Thank  you so much for your time!

      Best regards.

    • cheng089413

      Can any experts share some ideas about this issue? Thank you~😀

    • John Doyle
      Ansys Employee

      You can post process CZM debonding parameters (DPARAM, DENERI and DENERII) using the ETABLE command in a command object in WB-Mechanical.

      Please refer to the MAPDL Commands Manual for the ETABLE command syntax.  Refer also to Table 174.2 of the elements reference manual for the correct NMISC values to use.

      Below is a sample of what your command object might look like in Mechanical for post processing CONTA174 element CZM results via a command object. 

      I really cannot comment any further without seeing and studying your model in detail, which is beyond the scope of this forum.



      esel,s,type,,cid1                                !select contact element type ‘cid1’

      etab,dtstart,nmisc,66                     !load step time during debonding

      etab,dparam,nmisc,70                   !debonding parameter

      etab,deneri,nmisc,140                   !debonding parameter

      pretab,dtstart,dparam,deneri     !print results to solver output



      pletab,deneri                                     !plot critical fracture energy



Viewing 7 reply threads
  • You must be logged in to reply to this topic.