

April 27, 2022 at 9:11 amKhanhminhSubscriber
I analyzed corrosion RC beam so I used the element Combin39 to model the bond between concrete and steel.
This element required force and deflection along the length Xaxis (axis of the beam). I transform the bondslip (MPamm) to forcedisplacement (Nmm) to enter a value in real constant.
I validated exactly the loaddeflection of RC beams from the simulation model and experimental program.
Nevertheless, I would like to understand how Ansys transforms forcedeflection input data into a stressstrain for the element to solve the problem. Since FEM generally requires stress and strain. Please explain relates the length of the element or related forcestress. Thank you for considering.

May 4, 2022 at 10:09 pmSheldon ImaokaAnsys Employee
COMBIN39 is just a nodetonode element. Thus, the node is not directly associated with an area or volume  that is why we use force vs. deflection in its definition. It is just basically a spring, like K*x=F, similar to the FE matrix equation we solve [K]{x}={F}.
When you have solid elements, for example, the integration point for the constitutive relationship is associated with a 'volume', so that is why you end up with stress vs. strain definition instead. From the constitutive relationship (stress vs. strain) and element properties, we go to a form of [K]{x}={F}. So your comment is reversed  we do not go from COMBIN39 forcedeflection curve to stress vs. strain but do the opposite; everything is transformed to stiffness [K], deformation {x}, and forces {F} to solve as a matrix equation.
If you have traction vs. separation (bondslip), did you intend to use something like a cohesive zone model? If your reinforcement is modeled as a beam element (single node describing crosssection), then the COMBIN39 is suitable, and you need to estimate the area associated with a node to convert the bondslip relationship to forcedisplacement. If, however, your reinforcement is a solid, then you may want to look at the cohesive zone model instead (see Fracture Analysis Guide, Sections 3.5 and 3.6 on modeling interface delamination). The cohesive zone model is defined as a tractionseparation law (units of stress vs. displacement, such as MPa  mm).

May 5, 2022 at 4:33 amKhanhminhSubscriberThank you so much for your information
Since I used the link 180 and solid65 to model the reinforce and concrete respectively. I didn't consider the traction vs separation. So is there available to model the Combin39 at the coincidence node like in the following picture? (You may see the letter KO at the node)
Here I only consider the corroded tensile bar. The model bondslip model according to fib Model code 2010 Here is bond stress (Mpa) then I convert to force F=3.14*d*L*bond (N)
So the input data in the real constant, I simply use the Force converted and value slip on the graph. Is that any inaccuracy?
Once again very thank you.

May 10, 2022 at 3:16 pmSheldon ImaokaAnsys Employee
By using total area (pi*diameter*length), you're assuming that the bond separates around the entire surface at once. I can't comment whether or not this is a reasonable assumption for your application, but I just wanted to point this out. Of course, if you model the reinforcement as a LINK180 element, you don't have any 'partial' area but need to treat the bond around the circumference since it is just a single node, not an actual surface, so what you did seemed reasonable for the modeling you used, but I just wanted to point out that you're treating the failure to occur around the entire circumference of the reinforcement rather than a smaller area, which may happen in real life.
Regards Sheldon

 You must be logged in to reply to this topic.
Boost Ansys Fluent Simulations with AWS
Computational Fluid Dynamics (CFD) helps engineers design products in which the flow of fluid components is a significant challenge. These different use cases often require large complex models to solve on a traditional workstation. Click here to join this event to learn how to leverage Ansys Fluids on the cloud, thanks to Ansys Gateway powered by AWS.
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.
 Saving & sharing of Working project files in .wbpz format
 Solver Pivot Warning in Beam Element Model
 Understanding Force Convergence Solution Output
 An Unknown error occurred during solution. Check the Solver Output…..
 What is the difference between bonded contact region and fixed joint
 The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
 whether have the difference between using contact and target bodies
 Defining rigid body and contact
 Colors and Mesh Display
 A solver pivot warning or error has been detected

8752

4658

3151

1678

1454
© 2023 Copyright ANSYS, Inc. All rights reserved.