Learning Forum

[jli562]

Hi,nGood afternoon! I have a question and I really appreciate your help.nI want to simulate a CFRP-reinforced steel plate (a 90mm*500mm steel plate reinforced by 90mm*250mm CFRP sheets both sides), which has a initial small debonding in the middle of the front bonded area. nThere is a fatigue load (vary from 10KN to 100KN in each cycle), the load cycle should be more than 10000. However I don't know how to simulate the 10000-cycles load.nI want to see the debonding condition of the structure when applying this load.nIs it possible to achieve the simulation in Ansys? I know there is a function called cohesive zone material (CZM), which is used to simulate contact debonding condition. Should I use it?.Thanks a lot.nnKind regards,nJingrongn

[Sean Harvey]

Hello Jingrong, nThanks for your patience. So if we were to take out the fatigue aspect, then we could model this using either VCCT (has initial damage) or CZM (no initial damage). Right now the material models we have seem to be limited to static cases. In which case, we can model the delamination growth. So if your loads produce sufficient energy to cause strain energy release through delamination, we can account for that. So, if your loading was high enough that produces damage, or exceed the GiC or GiiC, etc. then growth will occur, but if you fatigue loading is very small and you don't get to any appreciable strain energy to cause damage, we would not see the fatigue growth with the models I have used. I am going to discuss further with colleagues and see if we have any suggestions and get back to you shortly. Thank you.nnRegards,nSeann

[Sean Harvey]

Hi Jingrong, (). I just @ mentioned you above so you would get notification on this update. Thank you.nnRegards,nSeann

[jli562]

Hi Sharvey,nnThanks a lot for your reply.nDo you mean you have a static case model of delamination growth? If yes, can I have a look at it? nI'm really interested because my model failed to generate the debonding even under a static load.nThank you!Kind regards,nJingrongn

[Sean Harvey]

Hello Jingrong nUnfortunately I am unable to share a model. Some tips to try for czm based contact debonding. n1) Make sure the contact is bondedn2)Make sure analysis settings has large deflection in on with sufficient initial, max, min tip steps using auto time stepping onn3) Have a material with a valid czm model such as separation-distance based debondingn4) Make sure the load is sufficient to introduce damagen5)Use a user defined result expression of CONTNMISC70, CONTNMISC71, CONTNMISC72, CONTNMISC73 ( there is one for each node of the contact element) to plot the damage. (0 undamaged, 1 damaged) To get these results you need to go to analysis settings> output controls>Turn on contact miscellaneous This will help you to visualize if damage is occuringn6) Start with simple model and use displacement based loading to avoid convergence issues that will occur when parts separatenSee if these can help and circle back. Thank you.nRegards,nSeann