Reinforcement and Prestress Application in APDL Reinforced Concrete Simulation – Operation Process

Before the reinforcement element became available (approximately versions prior to 2020), early concrete simulation mainly adopted the cutting method and the monolithic method. The monolithic method used concrete element 65 for simulation, with cumbersome real constant calculation and specification, and typically had significant errors. The cutting method, i.e., cutting out rebar lines according to the rebar layout during concrete modeling, was generally only applicable to cases with regular and simple rebar arrangements. Once there were many rebars, the cutting method became very cumbersome and could easily lead to excessive fragmentation of the geometry, causing the computer to freeze. Using reinforcement elements in Workbench is relatively simple – you only need to change the element type to reinforcement in the line properties. So how to operate in APDL? This article introduces how to use reinforcement elements to simulate rebar. Reinforcement elements are mainly divided into Reinf263, 264, and 265, where 263 is used for reinforcement of line elements such as beams and bars, 265 is suitable for simulating rebar mesh, and 264 is suitable for simulating single rebar in 3D. Their finite element geometries are shown below:

Reinf263

Reinf265

Reinf264

When using reinforcement elements, note that since reinforcement elements depend on the parent element for existence, the solid elements must be meshed before defining reinforcement elements. In addition, reinforcement elements cannot determine their cross-section through real constant input; similar to beam elements, they can be input through sectype and secdata.

Given a solid beam with a cross-section of 400*800, length of 4000, top reinforcement of 4 bars of 20mm grade III steel, bottom reinforcement of 4 bars of 22mm, bottom reinforcement subjected to prestress of 100MPa, top subjected to 10KN/M load, without considering material nonlinearity, with both ends fixed.

Key operation points:

1. The solid beam is modeled in APDL;

2. The rebar is modeled in CAD and then imported into APDL;

3. The solid element uses Solid185 for simulation, the rebar uses Reinf264 element for simulation, and the prestress is applied using the Inistate command. Note: When generating 264 elements, you must first use the auxiliary element mesh200 to generate the line element model, and then use the Ereinf command to convert it.

Step 1: Define element properties, rebar properties, etc. in APDL, build the solid model, and mesh it as shown below. If the geometric model is very complex, this process can also be modeled and meshed using other third-party software before importing, or even meshed with HyperMesh before importing. The purpose of this step is only to obtain the parent element, regardless of what method you use:

Step 2: In AutoCAD, draw the rebar mesh model according to the actual position of the rebar mesh, and use the Export command to export it as IGES format.

Step 3: Place the exported IGES file in the ANSYS working folder, click ANSYS main menu File-Import-Iges to import the rebar file just created.

After importing, use the Lplot command to draw the wireframe to check the import status and verify the position. If the position is incorrect, redraw it in CAD as shown below:

Step 4: After confirming everything is correct, mesh the reinforcement elements with the following code:

!Top rebar
lsel,s,loc,y,450,800-1
type,2
secnum,2
lesize,all,40
lmesh,all

!Bottom rebar
lsel,s,loc,y,1,450
lsel,u,loc,x,0
lsel,u,loc,x,4000
type,2
secnum,3
lesize,all,40
lmesh,all

!Convert to reinforcement elements
allsel,all
ereinf

Check whether the reinforcement elements are generated. First, adjust the element transparency to 1 as shown below:

Step 5: Apply prestress

Reinforcement elements support the application of prestress. Use the Inistate command with the following code:

!Prestress application
esel,s,ename,,264
esel,r,cent,y,0,450
inistate,set,-2,stre
inistate,define,all,all,,,100
allsel,all
allsel,all

Step 6: Check if prestress is applied

Considering only prestress, without considering self-weight and external loads, check the contours after calculation to verify whether they match the prestress-only condition. For example, in this case, check the displacement contour, which shows an upward displacement trend, consistent with the general trend, indicating that the prestress was applied successfully.

Step 7: Apply normal loads and perform relevant post-processing.

Structural displacement contour

Rebar stress

The command flow and related material files for this article can be downloaded by paying $2 . If the download fails, copy the URL to your browser to open it~

If you find this useful, welcome to repost and share!