Design of Automotive Towing DevicesGh.L. Mogan, I.D. Buzdugan β€” Transilvania University of BraΘ™ov
Software guideGuide.8.3

Checking elements 13 and 2 by FEA (ANSYS)

In the steps below, πŸ–± means a left mouse click (πŸ–±πŸ–± a double click) and β†’ leads to the next action. Labels in the screenshots are those of the ANSYS Workbench interface.

1. Analysis model and input data

Analysis model

Analysis model in the XYZ coordinate system of the ATD

Analysis model in the ANSYS coordinate system

Input data (Ex.1.2.2, Ex.7.1, Ex.8.1)

Forces: FX = 1500 N, FY = 300 N, FZ = 700 N.

Geometric parameters: X1 = 80 mm, X2 = 220 mm, X3 = 150 mm, Y1 = 550 mm, Z1 = 180 mm, Z2 = 250 mm; LY = 120 mm; Lc = 70 mm; b2 = 120 mm; b13 = 120 mm; g2 = 10 mm; g13 = 15 mm; h12 = 50 mm; R = 20 mm.

Material: S235, weldable general-purpose steel, for element 13; E335, steel for mechanical construction, for element 2.

Operating constraints: temperature T = (βˆ’30…40) Β°C.

Parameters of the ANSYS model

Forces: Fx = FY/2 = 150 N, Fy = βˆ’FZ/2 = βˆ’350 N, Fz = FX/2 = 750 N.

Geometric parameters: h13 = g13 = 15 mm, h3 = g2 = 10 mm, b13 = b13 = 120 mm, L7 = 190 mm, LY = 120 mm, Ri = R = 20 mm, Re = R + g2 = 30 mm, h12 = h12 = 50 mm; L1 = 35 mm, L2 = 35 mm; FD1 = 120 mm for Element 2 and FD1 = 270 mm for Element 13; coordinates of the force application point: XCoordinate = Y1 + g13 = 565 mm; YCoordinate = Z1 + Lc = 250 mm; ZCoordinate = X1 + X2 + X3 + b2/2 = 510 mm.

Material: for S235 steel, Οƒat = Οƒ02/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, where usually c > 2); for E335 steel, Οƒat = Οƒ02/c = 335/1.3 β‰ˆ 250 MPa; allowable contact stresses: Οƒas = 90 MPa, the allowable steel-on-steel normal crushing stress, and Ο„as = 45 MPa, the allowable steel-on-steel tangential contact stress.

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

2.1 Launching the application

Downloading, saving and opening the application

FEA_13-2 β†’ [unzip FEA 13-2.zip and save it].

Opening the Workbench (ANSYS) environment

πŸ–± β†’ [the window opens].

Opening the project (application)

πŸ–± () β†’ [select the folder FEA 13-2 containing the file (application)], [select the file name πŸ–±]; the window of the previously developed project A opens, 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

πŸ–±πŸ–± β†’ the window opens with the geometric model.

Changing the dimensions

Changing the section dimensions

πŸ–± β†’ πŸ–± β†’ : [change the dimensions b13, h13 (fig. a)].

πŸ–± β†’ πŸ–± β†’ : [change the dimensions L7, b, Re, Ri, h3 (fig. b)].

a   b

Changing the extrusion lengths

πŸ–± β†’ : [change the dimension FD1 for Element 13 (fig. a)].

πŸ–± β†’ : [change the dimension FD1 for Element 2 (fig. b)].

a   b

Changing the dimensions of the support contour

πŸ–± β†’ πŸ–± β†’ : [change the dimensions L1, L2, h12].

Saving the project and returning to the main window

πŸ–± β†’ πŸ–± (the window with project A appears).

2.2.2 Changing the parameters of the FEA model

Loading the Static Structural module

πŸ–±πŸ–± β†’ the window opens with the FEA model:

Updating the geometric model

β†’ πŸ–± (the modified geometric model appears).

Meshing the model

β†’ πŸ–±; the meshed model appears:

Changing the coordinates of the force application point and the force values

πŸ–± β†’

[change the values , , (fig. a, b)];

[change the values , , (fig. a)].


a

b

Saving the model

πŸ–± β†’ πŸ–±

3. Solving and saving the model

β†’ πŸ–±

4. Results and checks

Viewing the loads and reactions

Viewing the applied forces and moments

πŸ–±

πŸ–±

Viewing the forces in the reaction zone

πŸ–±

πŸ–±

Viewing the displacements

πŸ–± β†’ the model appears

Viewing the stresses

Equivalent stresses on the global model

πŸ–± β†’ the model appears

Equivalent stresses on the model of Element 13

πŸ–±

Equivalent stresses on the model of Element 2

πŸ–±

Viewing the pressures and stresses in the contact zones

Pressures on the contact surfaces

πŸ–±

πŸ–±

Friction stresses on the contact surfaces

πŸ–±

Checks

Stiffness (deflection) check

Ξ΄ ≀ Ξ΄a; 6.19 ≀ 10 mm (satisfied).

Note. The allowable deflection is set by the operating conditions.

Check under combined loading

Οƒech_max ≀ Οƒat; 302.65 ≀ 196 MPa (NOT satisfied),

where Οƒech_max is the maximum equivalent stress in the figure above.

If the inequality above is NOT satisfied, one of the following options can be chosen:

a. choose a better material;

b. change the geometry by increasing one or more dimensions;

c. choose another material and change the geometry.

In this application, option b is adopted and the analysis steps are repeated, as detailed below.

Changing the geometric parameters

Activating the DesignModeler module

πŸ–±πŸ–± β†’ the window opens with the geometric model.

Changing the section dimensions

πŸ–± β†’ πŸ–± β†’ : [change the dimension h3].

Saving the model

πŸ–± β†’ πŸ–±.

Updating the geometric model in the FEA model

πŸ–± β†’ β†’ πŸ–±

Solving the modified model

β†’ πŸ–±.

Post-processing the modified model

Equivalent stresses on the global model

πŸ–± β†’ the model appears.

Re-check under combined loading

Οƒech_max ≀ Οƒat; 121.73 ≀ 180 MPa (satisfied), where Οƒech_max is the maximum equivalent stress in the figure above.

Check of the normal contact pressure

pmax ≀ Οƒas; 30.131 ≀ 90 MPa (satisfied),

where pmax is the maximum pressure in the figure above.

Check of the tangential (friction) contact stress

Ο„max ≀ Ο„as; 40.909 ≀ 45 MPa (satisfied),

where Ο„max is the maximum tangential contact stress (frictional stress) in the figure above and Ο„as the allowable tangential contact stress.