

June 28, 2018 at 3:53 amJoseph LimSubscriber
Dear community,
I was trying to using the finite element method to model the failure behaviour of the structural reinforced concrete beam element. From the literature review, I had found that the reinforced concrete was able to deform plastically and cracks in the direction of x, y, and z, by modelling the solid element with three degrees of freedom in each point. However, I was not able to find the degrees of freedom setting. May I know where can I find the setting (degrees of freedom)?
Thank you in advance.

June 28, 2018 at 4:46 amBhargava SistaAnsys Employee
Lim,
The finite elements are made of the nodes and each node already has the degrees of freedom depending on the type of element. For instance, 3D structural solid elements are made of nodes which have 3 degrees of freedom each (X, Y and Z translations). You need not turn them on using any setting, the solver is already calculating for them. You may want to check the literature to see if they refer to any particular type of elements, then search for them in the help document. You'll find all the relevant details in there.

June 28, 2018 at 8:32 amAshish KhemkaAnsys EmployeeFrom 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 8node 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 currenttechnology 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 DruckerPrager 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.

July 31, 2018 at 8:36 amjackheroSubscriber
How to define the smeared reinforcement in Solid65 in Ansys workbench? I found out from the search that one should define Real Constants for Solid65 in order to define fiber reinforcement in Solid65 using APDL commands.
I could not find any commands for Solid65 smeared reinforcement. If you could mention the commands here it would be of much help.

July 31, 2018 at 12:34 pmJohn DoyleAnsys Employee
SOLID65 element is legacy element technology not under active development. Workbench already uses SOLID18x elements and the latest geomechanics material options for concrete are already exposed in Engineering Data. Could you use this together with discrete or smear reinforcement? Reinforcing sections (SECTYPE,,REINF) define the location and orientation of the reinforcing (SECDATA). The sections are referenced by REINF263, REINF264 and REINF265 elements, or MESH200 elements when used to temporarily define reinforcing locations. See also the EREINF command.

 You must be logged in to reply to this topic.
Simulation World 2022
Check out more than 70 different sessions now available on demand. Get inspired as you hear from visionary companies, leading researchers and educators from around the globe on a variety of topics from lifesaving improvements in healthcare, to bold new realities of space travel. Take a leap of certainty and check out a session today here.
Earth Rescue – An Ansys Online Series
The climate crisis is here. But so is the human ingenuity to fight it. Earth Rescue reveals what visionary companies are doing today to engineer radical new ideas in the fight against climate change. Click here to watch the first episode.
Ansys Blog
Subscribe to the Ansys Blog to get great new content about the power of simulation delivered right to your email on a weekly basis. With content from Ansys experts, partners and customers you will learn about product development advances, thought leadership and trends and tips to better use Ansys tools. Sign up here.
 How to calculate the residual stress on a coating by Vickers indentation?
 An Unknown error occurred during solution. Check the Solver Output…..
 Saving & sharing of Working project files in .wbpz format
 Solver Pivot Warning in Beam Element Model
 Understanding Force Convergence Solution Output
 Colors and Mesh Display
 whether have the difference between using contact and target bodies
 The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
 Massive amount of memory (RAM) required for solve
 What is the difference between bonded contact region and fixed joint

1970

1726

943

708

395
© 2022 Copyright ANSYS, Inc. All rights reserved.