Skip to main content

Adhesive CZM ANSYS Parameters

How to Extract CZM Parameters From Test Data?
A few years ago, I was pulled in to do some adhesive modeling. The project leaders later decided against using adhesives but it peaked my interest on how to simulate adhesives using Cohesive Zone Modeling (CZM). Mode I Peel direction failure was a concern and glue manufacturers sometimes lists the peel strength per ASTM D 1876. Unfortunately, from those values alone, it is difficult to determine the needed parameters for use in ANSYS.

1. CAEAI presentation [link] provides good background information
2. PADT The Focus #56 by Rod Scholl [link] explained the parameters clearly
3. Paper by A. Khayer Dastjerdi & E. Tan & F. Barthelat [link] or [link]
4. Ansys Knowledge Resource #2052789 [link] model with bonded contacts

Simulation Model Goal
Unlike ASTM D1876, the paper by Dastjerdi et al [1] provides a clear way of translating load frame test data into parameters used in ANSYS. The flimsy panels used in the ASTM standard are highly non-linear. The critical contribution of the paper is to replace highly deformable test pieces with a rigid body substrate and providing the math in computing the parameters.

Figure 1: Fixtures used in CZM Adhesive Characterization

The second piece of the puzzle is SR #2052789 which provides many tips on the model setup requirements (e.g. Never update contact stiffness, use fracture object etc). Their attached project file was used as a template for this blog post's project.

The paper by Dastjerdi et al [1] shows how one could calculate the normal traction vs separation from their experimental setup. The experimental setup and corresponding test results were also described well enough to be replicated in ANSYS. As both test data and calculated cohesive laws curve are available in the paper, we could extract CZM CBDD parameters then try to replicate the test in ANSYS to see how well the calculated force measures up to test data. This would be done for the Polyurethane adhesive.

Parameter Setup
Figure 7 & 8 from the paper shows the measured force vs opening and normal traction vs separation respectively. In Figure 2 below, the light turquoise line was appended to approximate the ANSYS load path. Orange lines helps determine some amplitudes for this path.

Figure 2: Appended Plots from Paper

The CZM Separation-Distance Debonding parameters approximated from the turquoise line are:
Figure 3: CZM Properties 

A key snippet is needed for the initial gradient which specifies the stiffness of the contact elements:
Figure 4: Stiffness Specification Location

The snippet is:
rmod,cid,3, -0.07428e12 ! FKN = 5.2e6/70e-6
rmod,cid,11,-0.07428e12 ! FKOP = 5.2e6/70e-6

The negative value tells Ansys to interpret the real constants FKN & FKOP as absolute value and not based on the underlying element stiffness/dimensions. Other details can be found in the archived model.

Results & Discussion
Figure 5 has the calculated force peaks at 97.5N at 0.12mm opening.
Figure 5: Calculated Force

It's a bit smaller than the peak ~112N at ~0.14mm shown in the paper but it's not far in the left field. A bit more parameter tweaking should better match the ANSYS results to the test forces.

Note that a shear test (Mode II) is advised to determine the tangential properties which were (wrongly) assumed to be the same in the above example.

Archive File
ANSYS WB v18.2 [Link]

[1] Khayer Dastjerdi, A., Tan, E. & Barthelat, F. Direct Measurement of the Cohesive Law of Adhesives Using a Rigid Double Cantilever Beam Technique. Exp Mech 53, 1763–1772 (2013).


  1. Thank you very very very much, It was the only single explanations of many confusions. Just a small question why two commands FKN and FKOP is needed? And what is 3 & 11? Can you please tell.

    1. Hi Puhan,
      FKN and FKOP is needed as it defines the contact's normal contact stiffness and opening stiffness respectively. Secondly, the real constants of FKN and FKOP corresponds to 3 and 11 respectively. Please see the help of RMODIF and CONTA171 for further details. Good luck!

  2. Your this article is so helpful to me as I try to CZM analysis for DCB and single lap adhesively joints, I appreciate it. However, I have a problem.
    As you can see in his paper below, he obtained result about 9kN when the lap length is 25 mm (reference Fig. 8). On the other hand, my result is approximate 600N. I don't know the causes.
    I refer to araldite 2015 (Table 1) for analysis.
    He used Abaqus, but I use Ansys mechanical for 2D analysis.
    could you give me any advice?
    in the end, can we define trapezoidal shape in Ansys?

    1. It's hard to troubleshoot your problem without having a closer look. Perhaps try recreating Fig 7 in the reference paper. Being mostly in sheer, some rough hand calculation is possible. Hopefully that provides some insight on where to look for the problem.


Post a Comment

Popular posts from this blog

ANSYS User Defined Results

There is an abundant of options in ANSYS classic when one wishes to post process results. ANSYS workbench default pull down menu post processing options are more limited but they can still be accessed via the User Defined Results. One way not commonly used but can come in handy is as follows: Zeroth: Under Analysis Settings, there is "Output Controls" where you can toggle to "Yes" what you would like to save before the solution starts. This is like OUTRES in APDL. Output Controls First: After solving the model, click on Solution in the tree to highlight it. Solution Second: Click on Worksheet in the toolbar. Worksheet Third: In the worksheet, you will see list of results that are saved. Right click on it to create the User Defined Results. Create User Defined Results So here we have it. You could of look up the different expressions in the help document but I find this method of accessing the results convenient.  Example: Aspec

Export Stiffness Matrix from Ansys

It is sometimes useful to extract the mass and stiffness matrix from Ansys.     *SMAT, MatK, D, IMPORT, FULL, file.full, STIFF       *PRINT, matk, matk, txt Exporting mass matrix would be similar:       *SMAT, MatM, D, import, full, file.full, MASS The above script uses APDL Math to get the job done. (Please see previous post for another example). The ordering of the matrix is unfortunately not concurrently exported. To verify the sequencing is as expected, we will work to replicate a truss example in the  Finite Element Trusses course notes by Bob Greenlee. Figure 1: Truss Problem Setup Model Creation Script to create model: /prep7 !! Creates Model to reflect course notes ! Properties et ,1,1  mp , ex, 1, 29.5e6 r , 1, 1 ! Geometry n ,1 $  n ,2, 40 $  n ,3, 40, 30 $  n ,4, 0, 30 e ,1,2 $  e ,2,3 $  e ,1,3 $  e ,3,4 ! Boundary Conditions d ,1,ux,0 $  d ,1,uy,0 d ,2,uy,0 d ,4,ux,0 $  d ,4,uy,0 f ,2,fx,20e3 f ,3,fy,-25e3 ! solves /solu eqslv , sparse

ANSYS APDL Syntax Highlighting editor

Notepad++ with APDL User Defined Language The editor of my choice is Notepad++  with the available User Defined Language Files for APDL . You can install it without administrative privileges via the zip file. The best part of it is, it's FREE! After installing Notepad++, go to "Language>Define Your Language..." then "Import" the XML file downloaded from the above link. Remember to restart Notepad++ so that the language changes will take into effect. Opening up any *.inp or *.ans files should automatically switch highlighting to APDL. I made some minor edits. Here's my XML file: LINK . I also heard Sublime Text and  Ultraedit  has more advance features but they aren't (totally) free.