Is it possible to get reinforced concrete in Ansys 2020 without needing any apdl code for concrete? Could we see crack in concrete ?
Yes it is possible. If you can look in the Ansys Help - Technology Guide - CHAPTER 49: LOAD LIMIT ANALYSIS OF A REINFORCED CONCRETE SLAB it details the capability. While that example is APDL based, the material models in that example are available in Workbench engineering data for use in Mechanical.
In addition, for the reinforcement 2020 supports surfaces and line bodies to be used as reinforcements of the concrete. You just need to set the model type to reinforcement.
Regarding seeing the actual cracks, you will not, but the effect of the softening can be understood by development of the plastic strains and this too is discussed in that example.
Models with reinforcement capabilities are available within Workbench's Engineering Data module. See the help here:
Both are able to be combined with Hardening, Softening, Dilation (HSD) features. See HSD4 for reinforcement: https://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v202/en/ans_mat/mat_geomechanics.html
18.104.22.168.1.2. Steel Reinforcement HSD Model (TB,CONCR,,,,HSD4)
It may also be instructive to see this tech demo guide (which is in APDL but gives you an idea of the capabilities of the MW and DP models): https://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v202/en/ans_tec/tecdynardo.html
Lastly, for crack visualization, we cannot currently do so in Mechanical. But using the SOLID65 element, which is a legacy element, you can use the PLCRACK command to see which elements are cracked. But note that SOLID65 being a legacy element, this may not be compatible with current technology models.
Thank you @sharvey and @DavidW , I understand this section for reinforced. concrete . But I need to make CFRP concrete like tihs photo.
I didn't use APDL up to present. I started a discussion for this topic. Mr.Wenlog said I need to use apdl. I wonder your thoughts on this subject. I have a curtain wall with concrete like the photo above. How do you model ? (you have a fiber volume for 1 m^3 concrete)
To make it look that photo, you can still use the beam reinforcement. APDL is not necessary as Mr. Wenlong and I chatted since reinforcement is newly exposed in Mechanical some are not yet aware of it's presence. You won't be able to see the break/crack, unless you use solid65 legacy element as David pointed out, but that you will need to use MAPDL and not Mechanical. That solid65 does support reinforcements too. But you can still capture the softened response with the material models David pointed out.
Let us know if that helps
Thank you @sharvey , I will try both of them. But my model has thousands of fibers. It is unreasonable to think about drawing these one by one. This is a great convenience in rebar drawings for columns and beams , but I think it should be a different solution for small sized elements with random orientations.
As a result, these elements are mixed with the concrete mortar. Do you have an idea?
With regards to modeling SFRC, i have attempted that in an ongoing research work. To model the fibers, you can just create a single line body to the specification of your fibre and pattern it to the numbers required in the concrete.
NB: The random orientation is not available for use. but still consider placing your SF on different orientations before patterning that will still produce a random orientation.
i hope it serves.
Thanks for your valuable comment @O_Maxwell . But can you explain the subject in a little more detail? I do not fully understand. This is not like a rebar, we are talking about thousands of very small parts.
Fiber sizes 5 cm and 1 mm in diameter, I still haven't obtained a fiber-powered model on a large scale. I'd appreciate it if you'd help me.
Ansys customers with active commercial software licenses can access the
customer portal and submit support questions. You will need your active account number to register.