This tutorial shows how to perform a linear static analysis using 2D shell elements on a simple overhead crane in Simcenter 3D.
The aim is to introduce the user to important basic concepts and the analysis methodology within Simcenter 3D.
Before starting this tutorial, it is worthwhile reading the Simcenter 3D Basics article that explains the various files types used in Simcenter 3D and broadly outlines the analysis methodology.

This tutorial is divided into 4 parts as follows:
1. Geometry Preparation
2. Mesh
3. Apply Loads and Boundary condition
4. Solve and Postprocess

In this article, we will discuss the 1st part:

1.Geometry Preparation:

Step - 01: Create a Simcenter Part Model

Launch a new session of Simcenter

File > New

In the window that appears, select Model from the list of Templates

Set the Name to Overhead_Crane_Analysis.prt

Choose a suitable directory where the model will be saved.

Click OK

File > Import > Parasolid
In the window that appears, browse to the directory where the tutorial Parasolid (Overhead_Crane.x_t) is stored and select it
Click OK
Press Ctrl + F to fit view

File >  Pre/Post
Click New FEM and Simulation button (typically in the top left corner)
The menu shown to the right should appear
Ensure that the Create Idealized Part checkbox is ticked. This will enable clean-up operation to be performed without changing the geometry that was imported
Click OK

Step - 04 - Set the Solution Parameters for the Analysis


The menu that appears allows various solution parameters to be set. Check that:
Solver is Simcenter Nastran
Analysis Type is Structural
Solution Type is SOL 101 Linear Statics
Click Create Solution
In the next menu that appears the default settings will suffice for this analysis. If necessary it is possible to modify these settings at a later stage in the model setup process
Click OK


Step - 05 - Inspect the simulation Navigator

In the tabs at the top of the model viewing window, select the Overhead_Crane_Analysis_sim1.sim
Expand all items in the Simulation Navigator
Observe the positions of the SIM (.sim), FEM (.fem), Idealized Part (_i.prt) and the Part (.prt) in the Navigator
Expand the Simulation File View at the bottom of the Simulation Navigator. Double clicking on any of the files will navigate to that file. Alternatively you can select the relevant tab above model viewing window
Double click the Overhead_Crane_Analysis_fem1_i part in the Simulation File View pane using the left mouse button. An Idealized Part Warning message should appear
Click OK

Click on the Promote button
Select all 5 bodies in the display port
Click OK

Step - 07 - Remove All Edge Blends from I-Beam


Select the Delete Face   tool in the Synchronous Modeling group of the Home tab tool ribbon
In the Delete Face menu change the Type to Blend
Left click and drag the mouse over the top I-Beam of the overhead crane. 8 Blend faces should be selected
Click Apply
 

Step - 08 - Remove All Edge Blends from the A-Frame Supports


 

Left click and drag the mouse over the right A-Frame of the overhead crane. 66 Blend faces should be selected
Click Apply
Repeat the above procedure for the left A-Frame
Once complete, click Cancel

Step - 09 - Create Midsurfaces for Shell Meshing

Select the Midsurface by Face Pairs      tool in the Geometry Preparation group of the Home tab tool ribbon
Left click and drag the mouse over the bodies of the overhead crane. 5 bodies should be selected
Click on the Automatically Create Face Pairs     button
Ensure that the Hide Solid Body Upon Apply checkbox is checked
Press OK

Step - 10 - Create Planes to Divide Surface for Load Application

In the Geometry Preparation tool group, go to More and select Datum Plane
Set the plane type to At Distance in the drop-down menu
Select the outer surface of one of the A-Frames as shown in the adjacent image
Set the Distance to -1450mm and click Apply
Repeat this process using the other side of the overhead crane to split the bottom flange of the I-Beam

Step - 11 - Divide I-Beam to Create Surface for Load Application

Select the Divide Face      tool in the Geometry Preparation group of the Home tab tool ribbon
Select the I-Beam by dragging over it while holding in the left mouse button. 5 faces should be selected
Click the middle mouse button
In the Dividing Objects section, select the two planes created in the previous step
Click OK

Step - 12 - Extend the Edges at the Top of A-Frames

Select the Extend Sheet     tool in the Geometry Preparation group of the Home tab tool ribbon
Set Limit to Until Selected
Select the 4 edges at the top of one of the A-Frames as depicted
Click the middle mouse button
Select the bottom flange of the I-Beam
Click Apply
Repeat this process for the other A-Frame

Step - 13 - Extend the Edges on the Sides of the Gussets

Select the Extend Sheet     tool in the Geometry Preparation group of the Home tab tool ribbon
Set Limit to Until Selected
Select the edge on the side of one of the gussets highlighted orange in the adjacent image
Click the middle mouse button
Select the surface shown in green in the adjacent image
Click Apply
Repeat this process for the other gusset

Step - 14 - Extend the Edges on the Tops of the Gussets


Select the Extend Sheet     tool in the Geometry Preparation group of the Home tab tool ribbon
Set Limit to Until Selected
Select the edge on the side of one of the gussets highlighted orange in the adjacent image
Click the middle mouse button
Select the surfaces shown in green in the adjacent image
Click Apply
Repeat this process for the other gusset
Click Save

Step - 15 - Hide the Solid Polygon Bodies
Double click the Overhead_Crane_Analysis_fem1 part in the Simulation File View pane using the left mouse button, or select the relevant tab
Expand the Polygon Geometry item in the Simulations Navigator
Right click on Polygon Geometry in the Simulations Navigator and set Sort > Type
Uncheck all Polygon Body items with the grey cube () as an icon. This will hide the solid polygon bodies from the display.
Step - 16 - Stitch Midsurface Edges 
Select the Stitch Edge  tool in the Polygon Geometry group of the Home tab tool ribbon
Ensure that Method is set to Automatic
Set Geometry to Stitch to Both
Set the Search Distance and Snap Ends Tolerances to 0.001m
Select all bodies in the display
Click OK

Your geometry is now ready to mesh!
Please follow Overhead Crane Analysis - Part 2 - Mesh to mesh and apply material properties.