SOLID65 only predicts the initiation of the cracks, not the cohesive behavir in concrete. That is to say, when the cracks initiates, the solid elements loses its resistence. That's why you have convergence problem. Try Contact/Target 173/170 if you know the crack path.

Clearly state your problem, how you have made crack in your model, how the crushing data is given ?

Trough CivilFEM new concrete material is added and Solid65 behavior is activated. The result in ANSYS Material models - concrete is in the attached file.

SOLID65 only predicts the initiation of the cracks, not the cohesive behavir in concrete. That is to say, when the cracks initiates, the solid elements loses its resistence. That's why you have convergence problem. Try Contact/Target 173/170 if you know the crack path.

Better to try with contact elements

Thank you for the advice, but I am not solving fracture mechanics problem, I solve global behavior problem and I need an exact prediction of the deflections of the structure. I am just trying single beams and columns for now. but I want to solve a whole building eventually.

I think I need to adjust some of the nonlinear analysis options. Some suggestions?

Check what constitutive material model you are using? If for example, it is elastic-fully-plastic, then there will be convergence issues. Such issues can be resolved by applying load in small increments. Further, ramp loading will result in easier convergence than suddenly applied Step loads. Also check other nonlinear options and give attention to error /warning messages at the end of solution termination. Also check the boundary conditions of your model.

I´ve sent some files with examples we have processed using element Solid 65. Hope they can be useful.

Thank you, Himayat Ullah and Gabriel Ribeiro, you have been very helpfull! I will check all these and I hope I will get better results.

The material model I use is parabolic, as per Eurocode 2, so I don't think that is the problem. I will try to solve it with more substeps, so the load increment get smaller.

The boundary conditions are ok I think, because I solved my model without cracking and crushing, and there are no problems there.

Hi Tanya, did you have any luck with your convergence issues? I am having similar issues with my models too, but my convergence values are increasing and decreasing with in a substep.

Try using non-zero value for Tensile Crack Factor ( say 0.5) and the crushing stress should be negative in compared to the positive cracking stress). Also, if you want to get the full response, even post-failure, try using Arc-length method, for displacement controlled analysis.

 Hi Tanya! Did you find your model`s problem? I have the same problem with my study of RC beams.

Thanks!

@Tanya , Amanda; let me know specific convergence issues you see and the load level, material model used.   Possibly i can share some experiences, how i worked out on composite steel girder bridges with concrete slab modeled using Solid65.

Thank you,

Fayaz

Hi Fayaz! Well, I used a stress x strain curve for concrete compression (rate independent) and I used the caracteristics of non-metal plasticity of concrete (open shear =0,2; closed shear = 0,8; ft=0,25 kN/cm² and fcu=2,5 kN/cm²).

For the solution controls I used small displacement static, 50 substeps, with the convergence described in terms of displacement with the tolerance of 0,001.

I think the model stops the convergence when the beam has the first crack because the greatest value of tensile shown in the last substep calculated until the non-convergence was the value I put in the material properties (0,25 kN/cm²).

Can you help me?

Regards,

Amanda,

Here are couple of suggestions you may try, i got help from them:

- Shear transfer coefficients: Open crack = 0.3 and closed crack = 1 based on study of Wolanski ,A.J. (2004). " Flexure behaviour of reinforced concrete beams using finite element analysis." Master's thesis, Marquette Univ., Milwaukee.

- Prefer discrete modeling of reinforcement bars using some link elements like  LINK 180 rather than inbuilt smeared model which is poor in convergence. 

- Adjust value of CSTIF factor it helps a lot. Although, i did not see even its higher values affecting results adversely.

- Provide smaller load steps towards non-convergent load levels, and by trial adjust substeps , number of iterations and maximum number of substeps. I found  at ultimate loads near failure, small load steps but larger substeps helps at times. Although this is not always the case. Trick is somhow you have to avoid the load increment that causes non-convergence issues by adjusting time step.

- If possible it is always good to apply displacement based loading than force based. However this may not always be easy case and applicable.

- Concrete Plasticity model: Multi-linear isotropic plasticity model for compression with failure surface controlled by William and Warnke (1974).

Hope this helps

Thanks,

Fayaz

Fayaz,

I too am having convergence issues and even if I increase the load step the solution stops at a particular load step. It shows error as solution not converged at load step 52..please help me with this

hi andre, did u find the solution to your problem,if without cracking and crushing , the model converges, does that mean the model is right and only load steps must be managed?

You should also define an elastoplastic behavior or including the rebars. Otherwise it is very complicated that the model converges. Think that the elements lose all their stiffness when tension cracks appear, it there is not anything else that sustains the strain the model collpases, that is to say, it will not converge. By the way, I would recommend a displacement-controlled simulation.

I have problems too with the convergence. I am modeling a concrete reinforced slab using solid65 and link180.

the slab have only self weigh and 3 colums (one corner is free). Some suggestions?

dear Yolanda,

If the concrete crash is activated within the program, the problems of non-convergence of the nonlinear solution are shown. The concrete, which is directly under the load, begins to crash. The adjacent concrete begins to collapse in the subsequent steps of the load. The local hardness is reduced, large transitions appear and the solution distinguishes.

Therefore, the Disable of the possibility of a concrete crash in the finite elements model,it reduce the problems of non-convergence of the nonlinear solution which is consistent with the recommendations of using Solid 65 in ANSYS>

best regards,

hala

Hello, try this: (undocumented)

keyopt,4,7,2 ! Stress relaxation

My simulation only worked till the peak of the force-displacement curve; after adding the above "keyopt" I'm also able to calculate the softening behaviour post-peak. It took me a long time to solve this problem....

Jürgen Ries , thanks a lot. I am going to try it!!!

Thanks to all,

Please check references below.. hope it will be helpful for you… Regards…

http://www.corcon.com/thesis/Chapter%205.pdf

https://digitalcommons.usu.edu/cgi/viewcontent.cgi?article=1462&context=etd

thank you very much

best regards,

hala

SOLID65 has a well known relation with concrete material in ansys APDL/workbench (through commands). however the convergence issues associated with SOLID65 element and the mesh sensitivity of the CONCRETE/SOLID65 combination was one of the motivations for moving to the Micro-plane model that tracks the softening behavior of the concrete as it fails, without having to track individual cracks. The microplane model with a newer CPT215 element delivered Force - Displacement results that had no significant mesh sensitivity, and agreed very well with the experimental data. A Technology Guide shows how to use the Micro-plane model with the CPT215 element. Find the youtube video link below (in Russian language). They are comparing the results of the old method using SOLID65 with the new micro-plane model with current technology elements.

youtube link: https://www.youtube.com/watch?v=Vb-xVXdY3Go&t=382s

Hi

see below link and help to extend this learning work https://www.researchgate.net/post/Experimental_and_Simulation_Verify_of_Reinforcement_Concrete_Beam_Bending_Crack_with_Ansys_Workbench

Tanya Chardakova Yolanda Gutierrez Diego Hala Tawfek Hasan Ahmed Mirghani

To overcome the non-convergence difficulties with solid65 at cracking, please apply the following professionally,

0- Refine the load increments ... make many load steps and huge member of substeps... refine and refine and again refine and again refine... this is the key... Please understand you are doing failure analysis ... It is the most complicated in structural analysis and needs expert... any veryyyyyyy small load makes big difference after cracks starts..... Again refine and refine...

Apply the load as displacement.. NOT FORCES

1-Please use Keyopt7 stress relaxation=1 to make the element stiffness reduced gradually to help convergence and relax (postpone or avoid) the cracking of adjacent elements... this is similar to Jürgen Ries advice...

2- Use the Real Constant CSTIF and increase its default 1.0E-6 to make the cracked/crushed element has enough insignificant stiffness to overcome the instability, cracking of adjacent elements, and the convergence problem...

3- Check carefully the convergence criteria data ... It is not easy job in Ansys. It depends on many parameters and needs to be set professionally .. You may prescribe tough impossible inputs to achieve... This is very important...

4- Use appropriate mesh and appropriate SOLID65 Concrete Material Data as its mesh sensitive as Ahmed Mirghani told. Make the mesh fine as much as possible... It needs trials... It is not easy task..

Below attached data shows ANSYS help for Keyopt7 & real constant CSTIF "stiffness multiplier"

------------

KEYOPT(7)

Stress relaxation after cracking:

0 -- 

No tensile stress relaxation after cracking

1 -- 

Include tensile stress relaxation after cracking to help convergence

------------------

When the element is cracked or crushed, a small amount of stiffness is added to the element for numerical stability. The stiffness multiplier CSTIF is used across a cracked face or for a crushed element, and defaults to 1.0E-6.

------------------

Best Wishes,

Ahmed