Checking elements 7, 8 and joint 7-8 (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 XYZ coordinate system of the ATD

Analysis model (FEA) in ANSYS

Geometric parameters in ANSYS

Input data (Ex.5.1)

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

Moments: M_X7 = 75000 Nmm, M_Y7 = 452000 Nmm, M_Z7 = 33000 Nmm.

Geometric parameters: L₇ = 115 (105) mm, L₈ = 85 (95) mm; L_7-8 = 60 mm; h₇ = 50 mm, t₇ = 5 mm, h₈ = 60 mm, t₈ = 5 mm.

Material: S235, weldable general-purpose steel.

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

Parameters of the ANSYS model

Forces: F_x = F_Y = 300 N, F_y = −F_Z = −700 N, F_z = F_X = 1500 N.

Moments: M_x = M_Y7 = 452000 Nmm, M_y = M_Z7 = 33000 Nmm; M_z = −M_X7 = −75000 Nmm.

Geometric parameters: H_e = 60 mm, V_e = 60 mm, H = 50 mm, V = 50 mm, H_i = 40 mm, V_i = 40 mm; FD1 = 30 mm and FD4 = 55 mm for Body2; FD1 = 85 mm and FD4 = 30 mm for Body1.

Material: S235, weldable general-purpose steel, with σ_at = σ₀₂/c = 235/1.3 = 180 MPa (since the FEA model is more accurate, a lower safety factor c = 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 ANSYS (Annex.AN.1)

2.1 Launching the project

Downloading, saving and opening the application

FEA_7-8 → [unzip FEA_7-8.zip and save it].

Opening the Workbench (ANSYS) environment

🖱 → [the window opens].

Opening the project (application)

🖱 () → [select the folder FEA 7-8 containing the file (application)], [select the file name 🖱]; the window opens, showing the previously developed project 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. a)].

🖱 → 🖱 → : [change the dimensions Hi, Vi, H, V (fig. b)].

a b

Changing the extrusion lengths

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

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

a b

Saving the project and returning to the main window

🖱 → 🖱 (the window with project 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

→ 🖱; 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)];

– changing the finite element size in the contact zones,

🖱 → 🖱 → : [activate the option 🖱🖱 and change the value in the right-hand column, e.g. 5.0 (fig. b)] (repeat this sequence for the groups , and ).

a b

– re-meshing with the changed parameters,

→ 🖱 (the modified FEA model appears).

Changing the loads

🖱.

Changing the forces

🖱 → : [change the values , , , e.g. 300, −700, 1500 (fig. a)].

Changing the moments

🖱 → : [change the values , , , e.g. 452000, 33000, −75000 (fig. b)].

a b

🖱 → 🖱.

3. Solving and saving the model

→ 🖱.

4. Results and checks

Viewing the loads and reactions

Viewing the support zone and the applied forces and moments

🖱

Viewing the forces in the reaction zone

🖱

Viewing the displacements

🖱 → the model appears.

Viewing the stresses

Equivalent stresses on the global model

🖱 → 🖱 (marks local stress values at points) → [move the cursor and 🖱 click the point on the model where the stress value should be shown]; to delete a local value: 🖱 (Label) → [🖱 select the value, then press the Delete key];