Learning Forum

[cagdasakalin]

Dear all,

I would appreciate it if you see why I have yellow colour in the details of "Contact Debonding" and tell me what the correct setup is for that? Please see the picture attached below.

[peteroznewman]

nWhat material properties did you assign to the Resin Epoxy? Please show the details in the Engineering Data tab.nHere are some other discussions on this topic:n/forum/discussion/15589/structural-analysis-cohesive-zonen/forum/discussion/2760/unable-to-define-czm-bilinear-or-exponentialn/forum/discussion/11206/czm-modeln

[cagdasakalin]

@peteroznewman nnThank you for the related discussions through the links you shared .nHere is the screenshot of the page you are asking for.nnnPlease let me know if you need to know more about other details.n

[cagdasakalin]

n

[cagdasakalin]

ArrayUpon your message, I created a new material in the engineering data including the properties related with fracture and debonding. After updating the model, I checked the same details window for Contact Debonding. I realized that the yellow warning related with the material line is resolved, however, Contact Region parameter is still highlighted with yellow colour for some reason. Please see the related screenshots below.nn(1)nn(2)nn(3)nn(4)nnnI am not sure if this warning(yellow colour on the Scope part in the Details of Contact Debonding) is related with the physical gab in the contact region that I tried to demonstrate in the figure below.nn(5)nnYou can also see details assigned for all contacts below.nn(6)nnCan you please share your suggestion to get rid of from this yellow colour?.Thanks in advance.nn

[peteroznewman]

nThe Gap may be the problem. Try changing the Shell Thickness Effect to Yes in the Contact definition.nInsert a Contact Tool under the Connections folder and Evaluate Initial Contact Status. What is the Gap shown by the tool?n

[cagdasakalin]

ArrayAs you suggested, I tried switching Shell Thickness Effect to Yes and I got another yellow as below.nn(1)nnI have the following pages for Initial Contact Status.nn(2)nn(3)nn

[peteroznewman]

nLook at the ANSYS Help documentation and read Chapter 13. It says the Formulation of the Bonded Contact must be set to augmented Lagrangian or pure penalty method. Try setting the formulation to one of those instead of Program Controlled.nAll the examples of Debonding using CZM material definition has bonded contact where the two surfaces had no gap. I don't know if the gap is a problem or not.nI suggest you make some very simple models of a flat lap joint of two sheet bodies. Get that working first. n

[cagdasakalin]

nThank you for your time and suggestions.n

[cagdasakalin]

ArrayAssigning contact formulation either as augmented Lagrangian or Pure Penalty resolves the issue with Contact Debonding definition.But, at this time, it does not converge at all.nBy the way I could not find the Chapter 13 in the Help, can I ask a favor from you to share the link for this help page?.(1)nn(2)nn

[peteroznewman]

Here is the help link.nChapter 13: Debonding (ansys.com)nConvergence is a separate issue that will generally need a lot more substeps and potentially smaller elements.n

[cagdasakalin]

nArrayFirst of all, I looked at the Chapter 13 in the ANSYS Help documentation.nnThe notes I followed for the debonding setup from the documentation areIncluding CONTA172nHowever, there is no difference in terms of results if I compare them when I include CONTA172 and do not include it.nnAugmented Lagrangian method or pure penalty method (KEYOPT(2) = 0 or 1)nPure Penalty has been already chosen for formulation criteria.nnBonded contact (KEYOPT(12) = 2, 3, 4, 5, or 6)nHere is the cotact option as Bonded.nnBilinear material model to be includednCan you please tell me how I can include the bilinear models in the mechanical?.nBased on your suggestion, I configred a quite simple models where I used a pair of sheets. I investigated three different cases for which you can see the bondary conditions below.nSheets with physical gaps or without gap showed no difference in terms of results. In addition to that, I am also suspisious about the results when I see the animation for case I) where I applied 0.015mm displacement. You will see that he upper sheet is being buckled in a strange way; it bends upwards along the mid-section.nncase I)nnstrange buckling behaviour)nnanimation for case I)nArraycase II)nnanimation for caseII)nArraycase III)nnanimation for case III)nArraynPlease note that, for all, displayed results are animated in scale 16.nnI also conducted a convergence study on this simple model to figure out the optimum mesh size. In this convergence study, I used more than 150 design points ranging from 5mm to 0.0625mm. Below you will see the graphs for convergence analysis. I was expecting the curves to reach a plateu at a specific mesh size, see Figure 1). However, what I see is that the curves are continuously climbing as shown below in Figure 1) and in Figure 2).nnnFigure 2)nnnFigure 1)nnI would apprecite it if you share your ideas.n

[peteroznewman]

nYou don't need to add an APDL command object in Mechanical to call out CONTA172. That is automatically used when you define bonded contact.nIt looks like you have setup the other details under contact in order to do debonding.nThe mesh you are using is way too coarse. All the examples I have seen have a much finer mesh.nIn all the examples I have seen of debonding, the two materials are touching and do not have a gap like you show. I don't know if a gap will work.nAll the examples I have seen include an initial crack in the model. In other words, if the two plates are 10 mm long, there could be a 1 mm unbonded length and the bond between the plates is only 9 mm long. That means you have to split the face on each plate to create two faces. There may be 100 elements along the plate. If you pull up on the edge of the plate, there are 10 elements being flexed before the first contact bond.nTo make a bilinear material, use Workbench, double click on the Engineering Data cell to open that tab. In the Toolbox, expand the Plasticity category. Drag the Bilinear Isotropic Hardening model onto your material and fill out the Yield Strength and Tangent Modulus. If you don't know the Tangent Modulus, use 0.n

[peteroznewman]

nCORRECTION: The last paragraph is pointing to the wrong bilinear material model, sorry.nIn the Toolbox, expand the Cohesive Zone category. Drag the Bilinear for Interface Delamination out onto the cohesive zone material. Fill out the yellow fields.n

[cagdasakalin]

nFirst of all, thank you for your comments.nIn addition to your ideas with each paragrapgh, would you say something about the convrgence issue? In the convergence study, the associated values such as stress and strain are monotonically increasing as the mesh size is decreasing. Would not these values be expected to reach a platue or to converge a value as mesh size get decreased? Can you say what the reason is for this behaviour?.

[peteroznewman]

ArraynYou should do a Mesh Convergence Study, changing the element size by a constant factor, such as 1.5 so do a series of element sizes such as: 0.4, 0.26, 0.18, 0.12, 0.08, 0.05 mmnResult quantities don't always change monotonically when the element sizes are much too large, but they should once they get smaller. Different results might converge from above or below the zero element size asymptote. nThe reason results converge as the element size is reduced is because the underlying physics is continuous, but finite elements is digitizing that continuum and introduces an approximation.nSome geometry, such as a sharp interior corner, or other boundary conditions such as Fixed Support, can have a Stress Singularity. The true solution at that point is infinite stress, so as the elements get smaller at that point, the stress continues to increase without limit. A crack tip is an example of a stress singularity. While the stress will not converge at a crack tip, other quantities will converge such as the J-integral, a quantity computed on a contour that encircles the crack tip.n

[peteroznewman]

On further reflection, you can do CZM without requiring an initial crack in the model.nAnother method seems to require an initial crack and can predict crack propagation through a model. That is called VCCT and it also used Bonded Contact.n