# Concrete Modeling - Questions

Good morning!

I am working on my master´s final project and I should simulate concrete behaviour with FRP confinement.

I have been reading several papers, web pages, this forum discussions, etc and I have some questions that maybe you can help me to solve them, thanks in adavance.

1) I have seen some simulations in implicit and others in explicit, I have read that if you do not perform the calculation in explicit it does not take into account the damage in a correct way, is it true? For example if I set up a static structural, concrete NL, drucker praguer and softening ... it will not work correctly, won´t it?

If it is true I also understant that the geomechanical options does not work properly in static structural,

2) Some simulations are performed by using solid 65 element for the concrete in this way the cracks and crushing can be shown. But others paper say that solid65 is an heritage element in Ansys library, is there any other option to simulate concrete? is solid65 the best one?

Also I read something about microplanes.

3) I have read a thesis in which they simulated the concrete by using solid65 and two criterions: willam & wamke in tensile and drucker-prager in compression and the results were very good in comparison with the experimental ones.

4) Did anyone perfomn a simple concrete simulation (explicit or implicit) that can be shared? It would be very helpful.

5) Some examples are in newer ansys versions, do you know if there is any way to have two versions in the same computer?

Thank you very much for your time.

Kind regards.

## Comments

Good evening anchel,

1) You can get correct damage effects in implicit models, it takes a little more skill to build up a comprehensive material model. Contrast this with Explicit Dynamics that has "erosion" or element death upon a simple equivalent strain value as the default behavior and you can see why novice users like that.

2) Yes, newer elements like CPT215 can be used with the newer material models such as microplanes to model damage as described in the attached abstract that was from a talk I attended at a conference earlier this month. Solid65 with CONC material has a well known mesh sensitivity that the method described in the paper mitigates.

3) The method in the paper has good agreement with experiment.

4) I have several examples of the old solid65 and CONC material, but I will attempt to put up a simple model that illustrates the method outlined in the attached abstract.

5) Yes, you can have older and newer versions of ANSYS on the same computer, but you must install them in order from oldest to newest. You can't mix Student license and Research license versions of software on the same computer.

Good afternoon Peteroznewman,

Thank you so much for your answers, it has been very clarifying.

1) You mentioned that you have several examples with solid65 and CONC. Are these examples availables in this forum?

2) In relation to the mesh sensitivity of Solid65 with CONC material, could you point me in the right direction and provide me some articles or webpages in which I can find more information about?

3) I had heard of microplanes to model damage but I have never attempted it. As you mentioned, if you can upload an simple model example that illustrates the method of the abstract, it would be extremely helpful.

Thanks for your time and sorry for bothering you once again.

Have a great day.

Hello Anchel,

3) You can find the attached Technology Guide in the ANSYS Help system for Release 19.1

I will look for the other links in a later post.

Regards,

Peter

Hello Anchel,

Just to add to what peter already said. Here are some papers/resources using Solid 65 elements to model concrete:

Numerical Modeling of Reinforced Concrete Beam

Model concrete using finite elements

Model Concrete Reinforcement Using Finite Elements

Analysis of Reinforced Concrete using ANSYS

Hope it helps a little.

Regards,

Sandeep

From our database: We offer this for concrete modeling- TB,CONCR for use with only SOLID65: This is an old concrete model. It is only supported for SOLID65, an 8-node brick element. SOLID65 allows to model brittle behavior of concrete/rock. Basically, when the stress state hits the failure surface, we lose stiffness completely at the integration point. Hence, think of this as a failure/damage model (where damage=100%). This model separates "cracking" and "crushing" behavior - if an integration point 'cracks', it loses stiffness completely in that direction only in tension, but it can 'close' the crack as well. If the integration point undergoes crushing, it loses stiffness completely in all directions.

TB,MPLANE is the microplane model, supported by current-technology planar (plane strain and axisymmetry only) and solid elements. The failure surface for the microplane model is a bit different from the concrete model noted above - it also does not differentiate between 'crushing' and 'cracking'. Instead of instantly losing 100% stiffness, this is a gradual damage model, so it helps with convergence (TB,CONCR can be harder to converge since we lose 100% stiffness when failure surface is reached; with microplane model, the stiffness loss is a bit more gradual). TB,MPLANE can also be used to model rock and concrete (lower tensile stiffness than compressive).

Reinforcements - discrete or smeared - can be included with REINF26x elements.

TB,EDP is the Drucker-Prager model that can look at the inelastic behavior of soils or rocks. This is a plasticity model, so it doesn't model cracking/crushing or damage. Instead, it is used to model the inelastic volume change and shearing of soils/rocks. The Cap model is useful since it provides a yield surface for triaxial compression, too.

As you can see, we really have two ways of modeling rock/concrete - if you are looking at the brittle failure, you would look at TB,CONCR or TB,MPLANE. On the other hand, if you wanted to look at the inelastic response prior to brittle failure, you would use TB,EDP.

We also have a porous media model for looking at soil consolidation problems (CPT21x elements), although they currently do not support nonlinear inelastic material models.

Hi everybody,

thank you for your messages, they are explanatory,

Mr. Peter,

Thank you for the attached Technology Guide in the ANSYS Help system for Release 19.1, I do not have the 19.1 version yet, I will have a look soon. Do you know if apart from the attached pdf it is available the wbpz (or wbpj) of the paper example? it would be great since I have found other documents about microplanes but there is not explanation about how to extract, for example: the damage, compression damage and tension damage.

It looks like the model is developed in ANSYS APDL but I assume that the same can be performed in Workbench.

Mr. Smedikon

Thank you so much for your links, I had seen some of the paper before but other are new to me.

Dear Akhemka,

Thanks for you comprehensive response. I am studying concrete confinement by FRP therefore I want to study the strength rise of concrete column up to the failure, therefore with Drucker-Prager failure can be enough however I would like to explore other options and to have a concrete damage plasticity model.

In a paper I read that they reached a good convergence with a model by using Solid65 element, Willam and Wranke model for failure in tension and Drucker Prager for failure in compression. I have not been able to introduce in my simulation the two theories (but I know that it is possible (https://www.sharcnet.ca/Software/Ansys/16.2.3/en-us/help/ans_thry/thy_el65.html)

I read that if you introduce fc = -1, ANSYS does not check the crushing with Willam & Wamke and it uses Drucker Prager, avoiding in this way some problems.

Other options that I am assuming is to use the new Menetrey-Willam failure model that it is available in ANSYS Geomechanics, but I have been unable to find concrete examples with it.

I would appareciate your responses to theses comments / questions.

Kind regards

Anchel,

Attached is a zip file with the files referenced by the Technology Guide I provided the pdf reference in my post above. There is no .wbpz file, there is a .cbd file that can be opened in classic ANSYS.

Regards,

Peter

Hello eveyone,

I want to simulate a 4 point bending test of ultra high performance concrete. To be more specific I want to investigate how the crack propagation is affected by the existence of flaws. For this reason, I chose to insert the command of solid65, to see the crack propagation at failure. However, there is something wrong and "An unknown error occurred during solution. Check the Solver Output on the Solution Information object for possible causes." The Solver output has only warnings like: "Specified degree of freedom constraint UZ at unused node 3786.".

The command I inserted is the following:

ET,MATID,SOLID65

R,MATID,0,0,0,0,0,0

RMORE,0,0,0,0,0

MP,EX,MATID,48000

MP,PRXY,MATID,0.18

MPTEMP,MATID,0

TB,CONCR,MATID,1,9

TBTEMP,22

TBDATA,1,0.2,0.8,15,120

TB,MISO,MATID,1,3,0

TBTEMP,22

TBPT,,0.0015,72

TBPT,,0.0025,108

TBPT,,0.0035,120

Could you please help me?

Thank you in advance.

Zoi

Dear Peter,

Hi, sorry for asking this basic question. I'm currently learning the ANSYS APDL

Is the file that you upload have already contained all of the setting and the result?

Because I want to rerun it again so I could get the similar result with the PDF you attached before

I already open the file, it has similar geometry but it can't seems to run it. Can you help? thank you. Stay Safe

Regards,

Ricky