Learning Forum

[Mirghani]

Hi Ansys Community

Am studying the debonding between concrete and different materials, the two materials are bonded through adhesive. I did the modeling in workbench static structural. I want to verify the experimental test results through FEM. I am struggling with the contact force reaction validation (inserted a force reaction probe). A displacement controlled load is applied as a function of time (max displacement about 0.8 mm). Of course a CZM material is specified in engineering data with mode II parameters derived from experimental strain gauge readings through some equilibrium equations from literature. 

I tried different concrete/micro-plane models CONC/MPLA with SOLID65/CPT215/SOLID185 elements, however the debonding takes place early (at about 0.59 mm displacement) with low contact force reaction.  

* Force obtained from the instron machine (Experimental force F = 20 KN)

* Force from the model without CZM (default contact in ansys (Program Controlled) > F = 17-18 KN) - Close to experimental.

* Force from the model with CZM activated (Pure penalty - Augmented Lagrange)> F= 12 KN max) - Far From Experimental. (How to increase this value from 12 to be near 20 KN from experimental).

I tried the following

* increase the contact stiffness through commands in order to increase the reaction force but convergence issues occurs. 

* Switching between contact algorithms (Pure penalty - Augmented Lagrange)

* Normal stiffness as program controlled, absolute value and a Factor with stiffness update to (each iteration - never).

Thanks in Advance

[Sandeep Medikonda]

Mirghani,

As for generic comments:

• Check out Chapter 5 of the Technology Demonstration Guide. (Not directly helpful but also see chapter 54 on Concrete)


• CZM models are often mesh-dependent. I notice that you have only 1 layer of elements between the 2 contacting bodies, have you consider the effect of mesh?


• For convergence difficulties, try including a small Artificial Damping Coefficient in the Engineering Data.


• Define a separate frictional contact pair in combination with bonded CZM to support post debonding frictional sliding. Since this is Mode-II.


• Note that, you can define a custom contact stiffness using a command snippet (under the Bonded Contact):

rmod,cid,3,-Arg1

Regards,
Sandeep

[Mirghani]

Dear Mr. Sandeep,

Thank you for your reply. 

• I will go through Chapter 5. maybe I can come up with something


• The 2 materials are bonded through a 1 mm adhesive in experimental, however the adhesive is modeled with contact elements as a zero thickness material in ansys. (I tried with 5mm & 3mm element size mesh and I continued with 5mm mesh)


• Already inserted a damping coefficient of 0.1 s value (Some times with 1e-6/1e-8 values) in engineering data


• do you mean to insert the same contact again manually and assign it as frictional with frictional coefficient??


• already inserted the following command line but  how to define the approximate values for normal & tangential stiffness, I know that ansys uses the following equation for pure penalty itrations

• F = K (tangential) *X (Sliding),

Approach 1: I have the debonding force from experimental as 20000 N & sliding through mounted strain gauges on the specimen as 0.16 mm

then  the above  equation yields a  K value of 20000/0.16 = 125000 N/mm (K - Approach 1 in N/mm units)

Approach 2:  I have the bond-Slip curve from experimental strain gauge readings (bilinear) similar to the below chart. I can also calculate the K value as the slope in (N/mm3) based on Un bar and max shear stress (approximatly 50N/mm3 ). (K-Approach 2 in N/mm3 units) 

•  Which approach is correct

• Contact Command ( Do I need to insert the command for all contact & Target bodies or only contact or target body??)

 RMODIF,CID,3,60    !normal stiffness N/mm/mm^2 for contact (Plate-Contact) 

RMODIF,CID,12,60   !shear stiffness N/mm/mm^2 for contact (Plate-Contact) 

RMODIF,TID,3,60      !normal stiffness N/mm/mm^2 for target (Block-Target) 

RMODIF,TID,12,60     !shear stiffness N/mm/mm^2 for target (Block-Target)

 OR

!force/displacement

 

KEYOPT,CID,2,1        !Pure penalty contact stiffness formulation by setting KEYOPT(2)=1

KEYOPT,CID,3,1        !Set units of contact stiffness to be force/displacement N/mm by setting KEYOPT(3)=1

RMODIF,CID,3,-1.3e5    !normal stiffness N/m

RMODIF,CID,12,-1.3e5   !shear stiffness N/m

[sk_cheah]

Mirghani,

Do I need to insert the command for all contact & Target bodies or only contact or target body??)

Only for contacts; Target has no real constants that corresponds to stiffness.

 

Already inserted a damping coefficient of 0.1 s value (Some times with 1e-6/1e-8 values) in engineering data

PADT article suggested much lower damping of 0.0001. The write-up is very good.

  

do you mean to insert the same contact again manually and assign it as frictional with frictional coefficient??

The examples I've seen (e.g. here) have been for bonded contacts, not frictional contacts. 

 

Which approach is correct

I'm not following either Approach 1 or 2 in determining FKN or FKT. As your plot Y axis has units of Pressure and X axis units of displacement, FKN and FKT should have units of (N/mm^2)/mm. For mode 2, the pressure numerator would be shear pressure of 20kN divided by area of adhesive. The denominator would be the travel in your experiment. I'm not sure how the strain gage is used here. Apologies as I am not well versed in this type of testing and could be mistaken. 

On the aside, note that quantities defined in command snippets have to reflect the active unit system. This is worth verifying. 


Good luck,
Jason

[Mirghani]

Dear SK_Cheah

 

Thank you for your reply. 

Only for contacts; Target has no real constants that corresponds to stiffness.

I was confused after looking at this  article (they mention TID), that's why I asked about stiffness.

PADT article suggested much lower damping of 0.0001. The write-up is very good.

Thanks for the article, I came across it before but not in details. However  I already inserted several values for damping as (0.1, 1e-6, 1e-. I will try the mentioned value (0.0001)

The examples I've seen (e.g. here) have been for bonded contacts, not frictional contacts. 

Totally Agree, All the examples and video tutorials are considering bonded contact for CZM. I think Mr. Sandeep is pointing to add another frictional contact manually with frictional coefficient to help with convergence in addition to the existing bonded contact. 

I'm not following either Approach 1 or 2 in determining FKN or FKT. As your plot Y axis has units of Pressure and X axis units of displacement, FKN and FKT should have units of (N/mm^2)/mm. For mode 2, the pressure numerator would be shear pressure of 20kN divided by area of adhesive. The denominator would be the travel in your experiment. I'm not sure how the strain gage is used here. Apologies as I am not well versed in this type of testing and could be mistaken. 

Kindly Find below snaps from This article "How to Extract CZM Parameters From Test Data". The same method is used in PADT Article "page No. 4"

On the aside, note that quantities defined in command snippets have to reflect the active unit system. This is worth verifying. 

Already Checked the unit system of workbench and all commands were inserted accordingly.

[jackhero]

I am also interested in this discussion.

Define a separate frictional contact pair in combination with bonded CZM to support post debonding frictional sliding. Since this is Mode-II.

I thought when we add CZM (Mode II) for bonded contacts, after contact debonding the frictional behavior is also added. But from this suggestion it seems like we should to add frictional behavior separately from CZM. For the present case mentioned here by Mirghani in his post, how to add frictional behavior, as suggested, in Ansys workbench for the contact already having the CZM (Mode II) bonded material.

Any suggested article for calculating the frictional behavior contact parameters either experimentally or numerically by equations.

Thank you

[Mirghani]

Hi Jack

Many articles available online, check this article and this is another. 

[sk_cheah]

Kindly Find below snaps from This article "How to Extract CZM Parameters From Test Data". The same method is used in PADT Article "page No. 4"

I'm glad you agree.


Good luck,
Jason

[jackhero]

Thank you Mirghani for the links to the papers.

Although they have used the Coulomb friction and the RCCM model to carry out the simulation. But I am still not clear how to include the frictional behavior/bond in Ansys workbench which shall be activated or come to work after the debonding (defined by CZM Mode II) between the contact and target elements take place. Under connections, I can either include the bonded or frictional bond between the contact and target elements.

If in a model there have a contact and target pair, in which I have already defined the bonded contact (CZM), how can I also include the frictional behavior at the same time so that after debonding the frictional behavior begins? I request guidance on this problem please.

[YCCY]

Dear Dr. Mirghani,

I am a master student doing FRP-concrete debonding simulation.

I get some difficulties for simulating the debonding model using CZM, which are convergence issues.  Consequently, the debonding process automatically terminated.

If possible, can you please help me out if here or update a demo.

Thank you in advance.

Kind Regards,

YC