Cohesive Crack - Tabular definition of Softening

[frabissio]

Modelling a 3-point test of a concrete beam, i used 4-node cohesive elements. I began with a linear and exponential softening functions, and everything was ok. But concrete in tension actually has a bilinear softening, so i tried to use tabular softening definition, by entering the damage function "D". Unfortunately results were very bad. As a test, i introduce a linear softening in tabular form, obtaining anything but the corect results.
Would anybody help me about that problem?

Thanks in advance,

Francisco

 

[abaqusmaster]

please leave your model for more considerations.
Regards,

Mohammad Shahbazi

http://www.OmranAfzar.com

 

[frabissio]

Mohammad,

Thanks for you answer. Find below a simple one-element model with a 3-point "D" function tabular definition. After analysis, P-displacement do not recovery a bilinear response at all, but a couple of parabollas, both centered with each linear branch, looking like integrals of input lines, or something like that.

Thanks,
Francisco

PS: .inp units are [mm] and [kg].


*HEADING
*PREPRINT, PARVALUES=YES, ECHO=YES, MODEL=YES, HISTORY=YES
*NODE
1, 0, 0,
2, 1, 0,
3, 1, 1,
4, 0, 1,
*ELEMENT, TYPE=COH2D4, ELSET=COHESIVOS
1, 2, 3, 4, 1
*NSET, NSET=APOYO
1
4
*NSET, NSET=CARGA
2
3
*COHESIVESECTION, ELSET=COHESIVOS, MATERIAL=COHESIVO, RESPONSE=TRACTION SEPARATION,THICKNESS=SPECIFIED
1.0, 1.0
*MATERIAL, NAME=COHESIVO
*ELASTIC, TYPE=TRACTION
3400.00, 1, 1
*DAMAGE INITIATION, CRITERION=MAXS
0.29, 1, 1
*DAMAGE EVOLUTION, TYPE=DISPLACEMENT, SOFTENING=TABULAR
0., 0.,
0.90, 0.025
1, 0.181,
*STEP, NAME=CARGA, INC=200
*STATIC
1E-03., 1., 1E-03., 1E-02.
*BOUNDARY
APOYO, 1, 1
CARGA, 1, 1, 0.2
*RESTART, WRITE, FREQUENCY=1
*OUTPUT, FIELD, VARIABLE=PRESELECT
*OUTPUT, HISTORY, VARIABLE=PRESELECT
*EL PRINT, FREQ=999999
*NODE PRINT, FREQ=999999
*END STEP

 

[abaqusmaster]

Francisco,
I had a look at to your model, the result was nonlinear so I think you have to change the damage parameters to get the appropriate result.

Mohammad Shahbazi

http://www.omranafzar.com

shahbazi@omranafzar.com
----------------------------------
Please DO NOT respond to me directly but post all responses here in the newsgroup so that all can share the information.

 

[frabissio]

Mohammad,
Of course, Damage function definition was wrong in the previous inp file. I defined D function correctly as D=1-K/Ko, where Ko is the initial stiffness (corresponding to no gamage), and K is the actual stiffness, calculated as K=sigma/w ( sigma and w from the softening curve). It was neccesary to use a lot of points to define "D" in tabular form, but it worked pretty good. There is only a small problem in the vicinity of maximum stress point (where damage start). Find attached the inp file, if it would be interesting for you. The softening law is bilinear, and it was recovered succesfully in the output.

 

[abaqusmaster]

why you don't use ductile damage or something similar?
did you test them?

Regards,

Mohammad Shahbazi

http://www.omranafzar.com

shahbazi@omranafzar.com

 

[frabissio]

I did not test ductile damage because concrete is a cuasi-brittle material. Nevertheless, the problem is basically solved in the way i described in my previous post & the attached file. Thanks for your help!

 

[abaqusmaster]

I know concrete is quasi brittle material, but using ductile damage properties in maximum stress zone and brittle damage properties in other zones may fix the problem. may be ABAQUS does not allow you to use both damage properties in one material, but it is an idea only.
Please let me know about the solution if you fixed the small problem exactly.

Regards,

Mohammad Shahbazi

http://www.omranafzar.com

shahbazi@omranafzar.com

 

[dbajaj]

Dear Francisco and Mohammad,
I am trying to model tooth enamel using a CT specimen. The 3-point material response of enamel is very similar to that of concrete (quasi-brittle). I came across this post and saw a useful input file that Francisco has written. I have no experience writing subroutines in ABAQUS and it's hard for me to understand the program that you wrote.

Francisco, I was wondering if you would be willing to share this model with me. If I have your model it would be easier for me to understand the code. If you want I can send you my ABAQUS model and the damage data that I would like to use a material property.

Thanks,
Devendra