Checking elements 5, 6 and joint 5-6 (tube-in-tube) by FEA (ANSYS)

In the steps below, 🖱 means a left mouse click (🖱🖱 a double click) and → leads to the next action. Labels in the screenshots are those of the ANSYS Workbench interface.

1. Analysis model and input data

Analysis model

Loading diagram (in the ATD coordinate system)

FEA model in ANSYS

Geometric parameters in ANSYS

Input data (Ex.3.4, Ex.4.1, Ex.4.2, Ex.4.3)

Forces: F_X = 1500 N, F_Y = 300 N, F_Z = 700 N.

Moments: M_X5 = 25500 Nmm, M_Y5 = 183500 Nmm, M_Z5 = 24000 Nmm.

Geometric parameters: Z₁ = 180 mm; h₄ = 15 mm, L₆ = 70 mm, h₅ = 50 mm, t₅ = 5 mm, h₆ = 60 mm, t₆ = 5 mm; h₇ = 50 mm, x = 5 mm.

Material: S235, weldable general-purpose steel.

Operating constraints: temperature T = (−30…40) °C.

Parameters of the ANSYS model

Forces: F_x = F_X = 1500 N, F_y = F_Y = 300 N, F_z = 0 (the force F_Z is transmitted by the pin joint and is therefore not considered).

Moments: M_x = −M_X5 = −25500 Nmm, M_y = M_Y5 = 183500 Nmm; M_z = M_Z5 = 24000 Nmm.

Geometric parameters: H_e = 60 mm, V_e = 60 mm, H = 50 mm, V = 50 mm, H_i = 30 mm, V_i = 30 mm, H₁ = 50 mm, V₁ = 50 mm, L₁ = 3 mm, L₂ = 10 mm; FD1 = 40 mm and FD4 = 165 mm for Body1; FD1 = 35 mm for Body2.

Material: S235, weldable general-purpose steel, with σ_at = σ₀₂/c_a = 235/1.3 = 180 MPa (since the FEA model is more accurate, a lower allowable safety factor c_a = 1.3 was adopted than for the classical, less accurate design models); allowable contact stresses: σ_as = 90 MPa, the allowable steel-on-steel normal crushing stress, and τ_as = 45 MPa, the allowable steel-on-steel tangential contact stress.

2. Entering the data in the ANSYS Workbench environment (Annex.AN.1)

2.1 Launching the project

Downloading, saving and opening the application

FEA_5-6 → [unzip the application FEA 5-6.zip and save it].

Opening the Workbench (ANSYS) environment

🖱 → [the window opens].

Opening the project (application)

🖱 () → [select the folder containing the file (application)], [select the file name 🖱]; the window opens, showing the previously created project schematic A with its component modules:

Note. All modules are up to date ().

2.2 Pre-processing

2.2.1 Changing the geometric parameters

Loading the DesignModeler module

🖱🖱 → the window opens with the geometric model:

Changing the dimensions

Changing the section dimensions

🖱 → 🖱 → : [change the dimensions He, Ve (fig. c)] → (the modified model appears).

🖱 → 🖱 → : [change the dimensions Hi, Vi, H, V (fig. c)] → (the modified model appears).

Changing the dimensions of the support contour

🖱 → 🖱 → : [change the dimensions H1, V1, L1, L2 (fig. c)] → (the modified model appears).

a b c

Changing the extrusion lengths

🖱 → : [change the dimensions FD1, FD4 (fig. a)] → (the modified model appears).

🖱 → : [change the dimension FD1 (fig. b)] → (the modified model appears).

a b

Saving the project and returning to the main window

🖱 → 🖱 (on the taskbar) → (the window with project schematic A appears).

2.2.2 Changing the parameters of the FEA model

Loading the Static Structural module

🖱🖱 → the window opens with the FEA model:

Updating the geometric model

→ 🖱 (the modified geometric model appears).

Meshing the model

Meshing with the default parameters

→ 🖱; the FEA model appears:

Note. This FEA model was generated with the default meshing parameters. These usually produce a large number of nodes and therefore a much longer solving time, especially on computers with limited hardware. To reduce the solving time, the meshing parameters can be changed and the model re-meshed, as in the next step.

Changing the meshing parameters and re-meshing (if needed)

– changing the finite element size for the bodies,

🖱 → 🖱 → : 🖱, [activate the option 🖱🖱 and change the value in the right-hand column, e.g. 5.0 (fig. a)];