Structural  Analysis  with Pro/Mechanica

 

 

Pro/MECHANICA is part of the Pro/Engineer suite of software tools produced by Parametric Technology Corp. It features three main components:

·            Pro/MECHANICA MOTION — a motion analysis package that provides mechanism modeling and mechanism design optimization capabilities. This product enables you to analyze your mechanism’s motion and forces.

·            Pro/MECHANICA STRUCTURE — a structural analysis package that provides structural modeling and optimization capabilities for both parts and assemblies. This product features static, modal, buckling, contact and vibration analysis. You can also use the product to determine how sensitive your model is to shape and property changes.

·            Pro/MECHANICA THERMAL — a thermal analysis package that features many of the capabilities of Structure along with heat transfer analysis and thermal design optimization.

You can use all three products integrated within Pro/ENGINEER. Structure and Thermal are available in part mode or assembly mode. Motion is available in assembly mode only. We will use only Pro/M Structure and this only in integrated mode.

 

To get from the “real world” physical problem to the approximate FEA solution Pro/M can provide, we must go through a number of simplifying steps. At each step, it is necessary to make decisions about what assumptions or simplifications will be required in order to reach a final workable model. By “workable”, we mean that the FEA model must allow us to compute the results of interest (for example, the maximum stress in the material) with sufficient accuracy and with available time and resources. It is no good building a model that is over-simplified to the point where it cannot produce the results with sufficient accuracy. It is also no good producing a model that is “perfect” but will not yield useful computational results for several weeks! Quite often, the FEA user must compromise between the two extremes - accepting a slightly less accurate answer in a reasonable solution time.

Starting from the simplified geometric model, there are generally several steps to be followed in the analysis. These are:

 

 

A good general rule is:  Make it simple!

 

Eliminate feature lines - radii - chamfers if possible.

                        Analyze only a portion (section along symmetry axes, when loading permits).

                        Do 2D analysis when possible.

                        A general 3D analysis on a complex part requires a lot of work and computer resources.

 

 

The 4-Step Design Analysis Procedure

 

FEM creates a mathematical model of your design so that you can simulate its behavior in its operating environment. The finite element method models your design by discretizing your geometry into individual finite elements that collectively approximate the shape of your model. This process results in a system of equations that, when solved, gives you information about the behavior of your design under the specified environment. You can visualize the results in graphical or tabular formats. The 4-step design analysis procedure is summarized below.

 

Step 1: Create Your Design

Create your design either in Pro/Engineer or Mechanica directly. There are some differences in capabilities and model setup between creating geometry in Mechanica and when transferring it from Pro/Engineer.

A CAD model is not the same as a FEA model!

Features of little or no importance are suppressed in FEA models. Often geometric and loading symmetry can be exploited to model only portions of whole part.

 

Step 2: Model Set Up - Material Selection, Load and B.C. definition and Meshing

Material Assignment

After you create the model’s geometry, you can choose materials and assign them to the whole design or parts of it. Materials will automatically adjust to changes in the geometry

Loads and Boundary Conditions

Loads and boundary conditions define the operating conditions in which your design will function. Like materials, loads and boundary conditions are fully associative to geometry, and automatically adjust to any geometry changes.

 

Meshing

When working in integrated mode meshing is done automatically and hidden by using AutoGEM. This stands for automatic mesh generation. In this case you will not see the generated element mesh at all.

 

Step 3: Perform Analysis

The basic configuration of MECHANICA/Structure gives you analysis capabilities to solve stress, displacement, frequency, and buckling problems. When you model real-life parts accurately, you usually generate a large number of elements and nodes that create a large number of equations that have to be solved simultaneously.

 

 

Step 4: Visualizing the Results

After completing the analysis, MECHANICA/Structure makes results available to you. They can be visualized in a variety of graphical and tabular formats. Moreover, you can perform more than one type of analysis on the same design, and find the results simultaneously.

 

 

 

Plate w. a Hole in Plane Stress

 

Plate

 

Load F = 50,000 N                       Plate thickness = 10 mm

For reasons of symmetry only a quarter of the plate needs to be drawn. In this procedure we will perform the following steps:

·         Create geometry.

·         Mesh the surface with 2D plane stress elements.

·         Define material properties and shell thickness.

·         Specify boundary conditions and load.

·         Create and run static analysis.

·         Visualize the stress results.

 

Create Geometry

 

In Pro/E we will build the model in the FRONT datum plane. We will only make one quarter of the plate.

Create a new part, call it 2d_plate. Delete the default coordinate system. Check for the correct system units mm – N – s. Launch Mechanica/Structure from within Pro/E by:

Applications – Mechanica – Structure – OK

Note a gren WCS is created automatically. Only the front surface of the plate will be used to define our 2D geometry. For a 2D-analysis we need to create a coordinate system as a Simulation feature.

 

Set Up Model

To create the new coordinate system, select:

Use the Coord System icon and select the edge along the global x-axis and the edge along the global y-axis; make sure the orientation of the coordinate system is the same as the WCS. Correct if necessary and then click  Ok.        

 

Setting the model type: 

Edit – Mechanica Model Setup – Advanced and check the Plane Stress (thin Plate) button. Click on Select Geometry and select the front surface of the plate, it will highlight red. Done Sel. Select Select Coordinate System and pick CS0. Click OK.

 

 

As you leave the Model Type window, a warning window will open up to let you know that if the model type is changed (remember the default was a 3D solid), all previously defined FEA modeling entities will be deleted (loads, constraints, materials, and so on). If that happens, you would have to create them again. Click Confirm.  Turn off all the datum axes, planes and so on to remove some of the screen clutter.

 

Applying Loads and Constraints

We will fix the left edge of the geometry and apply a uniformly distributed total load of 25,000 N (half of the total) in the X direction at the right edge. Apply the constraints using

New Displacement Constraints i_button_surf_constrnt

Call the constraint [fixed_edge]. It will be a member of ConstraintSet1. Set References to Edge/Curve. Pick the left vertical edge of the model surface. The available constraints at the bottom of the window are translation in X and Y only for plane stress problems. Leave X FIXED and Y FREE for this edge. Click OK. Now again select

New Displacement Constraints i_button_surf_constrnt

Name this constraint [sym_edge]. It is also a member of ConstraintSet1. Set References to Edge/Curve. Pick the edge along the bottom of the model. This is the symmetry edge. The constraints to be applied here are FREE in the X direction and FIXED in the Y direction. The model must be allowed to stretch out along X, but we cannot allow a Y deflection since this would imply opening a split or crack along the symmetry plane. The constraints along symmetry edges (or planes in a solid model) must be consistent with the behavior of the “missing” part of the model. When you select OK the constraint icons will appear along the edge.

Apply the horizontal load using

New Force/Moment Loads i_button_surf_load

Call the load [endload] (member of LoadSet1). Set References to Edge/Curve and pick the right vertical edge.  Enter an X component of 25,000. Click OK. To have the load arrows going outward from the model, select

View - Simulation Display - Settings

and select Arrow Tails Touching – Ok.

 

Defining Model Properties

So far we have not specified either the plate material, or its thickness (remember the Pro/M model is only 2D geometry up to here!). For 2D plane stress models, we do this using the New Shells new shell icon. This brings up the Shell Definition window. Enter a shell definition name [shell1]. Select the button under Surfaces, pick on the plate front surface and middle click. Enter a thickness value of  10.

Next set the Material, click on the More button, and select AL2014 from the list and move it over to the right box with the right arrow button. Click OK twice. The model is now complete.

 

Setting up and Running the Analysis

We will use initially the AutoGEM defaults for the mesh. Click on the Run a Design Study i_button_run_dialog icon and select File – New Static… set up a QuickCheck analysis called [plate1]. The constraint and load sets should be already selected. Select the ‘Configure run settings’ - icon to set the location for the

 

run files, and then click Start run icon when you are ready. Open the Run Status… window by clicking the Display study status icon.

 

The run will not take very long. AutoGEM creates 2 elements (note that they are listed as 2D Plates). Make a note of the max_disp_mag and max_stress_vm. Assuming no errors were reported with the QuickCheck, go back to the Analyses menu, and Edit the analysis plate1. Change it to a Multipass Adaptive analysis with 5% convergence on Local Displacement, Local Strain Energy and Global RMS Stress, maximum edge order 9 (although we hope we don’t need that many). Run this analysis. The run should converge on pass 8. The final results should be: maximum displacement magnitude 0.06295 mm, maximum Von Mises stress 65.77 MPa.

 

 

Viewing the Results

We want to the usual result windows for design study plate1. We are interested in the Von Mises stress fringe plot, animated deformation, and the convergence behavior of the Von Mises stress and the strain energy. Select Results i_button_results and new window pops up in which the results will be shown.

 

To produce a display of the Stress Contours click on the Insert a new definition icon:

A small window popping up defines the window name for the Result window. As window name enter vm. Now we must tell Pro/M the location of the data for the analysis, click on the ‘Folder’-icon. All info for our run was placed in a subfolder called plate1. Select it with a single click and click Open. Enter following data:

            Title                 Von Mises Stress

            Display Type               Fringe

            Quantity          Stress            Component     Von Mises

Under Display Options tab

Level               9                      Continuous Tone

Next click        OK and Show

 

Displaying Animated Deformation:

To create a new result window it is easiest to copy an existing one. Make sure vm is displayed and click the Copy the selected definition icon, enter as name deform. Change the following definitions:

            Title                 Deformed Shape

            Display Type               Fringe

            Quantity          Displacement    Component           Magnitude

Under Display Options tab

                        Animate

            Frames             24                                Loop

Next click        OK and Show

 

Both results will be displayed. You can control the selections to display with the two icons, ‘Hide definition(s) from selection’ and ‘Display definition(s) from selection’. Display only the deformed results and click Start to animate it. The wire-frame will animate to show you an exaggerated view of the deformation. This is a useful way to see whether the boundary constraints have been set properly. To stop the animation click Stop and File – Exit Results to exit the results display.

 

 

Examining Convergence:

Following the same procedure as before, make two more result window copies and modify the contents to define the following result windows. When editing make sure the proper name is highlighted in the edit column.

            Name               convm

            Title                 Von Mises Convergence

            Display type    Graph

            Quantity          Measure        Select: Max_stress_vm       - OK

Next click        OK and Show

            Name               constr

            Title                 Strain Energy Convergence

            Display type    Graph

            Quantity          Measure        Select: Strain_energy          - OK

Next click        OK and Show

Show only the titles convm and constr highlighted in the Display Result window. Both windows will appear on the screen showing graphs of both quantities as a function of loop pass. Notice the strain energy steadily approaches a limiting value with each pass, while the Von Mises stress behaves a bit erratically.

 

 

Refining the Mesh

We can do a refined mesh and compare the results.

To change the mesh settings, we need to bring up the AGEM Settings window, select:

AutoGEM – Settings… and select the Limits  tab

Change parameters as follows:

     min edge angle to 30

     max edge angle to 155

           max aspect ratio to 2           OK

 

You can view your mesh with:           AutoGEM – Create…

            And next clicking                   Create and Close

 

Then rerun your analysis.

 

Are the results significantly different?

Has the number of convergence loops changed?

Has the CPU time changed?

 

 

 

 

 

 

 

TOP                 RETURN