XXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXX''"> A Case Study of a Coffee Cup
In addition to creating a new geometry model or importing a CAD model, you can also use Patran to reconstruct an analysis model. To reconstruct a model, you import an existing FEM model from a valid source, such as a Patran database or a MSC Nastran input file.
Reconstructing an analysis model can substantially enhance the your ability to visualize the text input file, and to validate the accuracy and adequacy of the mathematical model. If necessary, you can easily modify essential model definitions, such as material specifications, element properties, or load and boundary conditions. All of these changes can be made through the Patran graphical user interface without intimate knowledge of the analysis solvers.
Problem Description
In this example we will attempt to re-analyze a coffee cup by assuming that the cup is now filled with mercury rather than coffee. We will adjust the load scale factor to 13.51 to account for the difference in density. Since gravity and cup dimensions do not change, the quickest method to update the pressure load is to increase the scale factor of the pressure acting on the cup.
Analysis Procedure
Setup the Analysis Project
Creating a New Database
• On the Patran Main Menu, select File >> New. The New Database form appears.
• Enter the name cup in the Filename textbox.
• Click OK. The New Model Preference form appears next. This form allows you to specify the generic analysis parameters for the model.
Selecting Analysis Parameters
• Set the Tolerance to Default.
• Choose MSC Nastran from the Analysis Code pull-down menu.
• Choose Structural from the Analysis Type pull-down menu and click OK.
Import the Geometry
Importing the Analysis Model
• On the Patran Main Menu, select File >> Import.
• The Import form appears.
• On the Import form, select Source >> MSC Nastran Input.
• Type the name cup in the filename textbox and click Apply.
• Use Fit view and change to Iso3 View.
Plot the Loads and Boundary Conditions (LBC)
Plot the Boundary Conditions Applied to the Cup
• On the Patran Main Menu, click on the Loads/BCs Application button.
• On the top of the Loads/BCs form, select Action >> Plot Marker.
• Under Current Load Case, click on Default, and set the existing load cases from Default to Untitled.SC1.
• In the Assigned Load/BC Sets listbox, select every load/bc set that has Displ in front of its name, and highlight default_group from the Select Groups listbox.
• This selects all the displacements applied to the model.
• Click Apply.
• This plots the selected Load/BC sets.
• Plot the Existing Pressure Applied to the Cup
• On the top of the Loads/BCs form, select Action >> Plot Contour, and Object >> Pressure.
• Under Current Load Case, make sure the existing load cases is Untitled.SC1.
• Select pload4.1.2D in the Existing Sets listbox and Top Surf Pressure in the Select Data Variable listbox.
• Select default_group in the Select Groups listbox and click Apply.
• This plots the pressure load.
Assign a New Pressure Load to the Model
Increase the Pressure Applied to the Cup
• On the Patran Main Menu, click on the Loads/BCs Application button.
• On the top of the Loads/BCs form, select Action >> Modify, Object >> Pressure, Type >> Element Variable.
• In the Select Sets to Modify listbox, select the load/bc set that is called pload4.1.2D, and click on Modify Data button.
• On the top of the Modify Data form, change the Load/BC Set Scale Factor to 13.51. Click OK and then click Apply on the Loads/BCs form.
• The scale factor is due to the difference in density of mercury and coffee. The PCL function that was used to assign the pressure is based on the equation “ρgh”, and since gravity and height do not change in this case, the quickest method to update the pressure load is to increase the scale factor of the pressure acting on the cup.
Create MSC Nastran Input File
Create the MSC Nastran Input (Bulk Data) File
• On the Patran Main Menu, click on the Analysis Application button.
• On the top of the Analysis form, select Action >> Analyze, Object >> Entire Model, Method >> Full Run.
• Click on the Solution Type button.
• On the Solution Type form, select Linear Static. Click OK.
• On the Subcase form, select Untitled.SC1 from the Subcase For Solution Sequence listbox. Click on the Default in the Subcase Selected listbox to delete the default load case. Click OK.
• Click Apply on the Analysis form.
• The analysis will take a few seconds before finishing. A file by the name cup.bdf is created and submitted to MSC Nastran. This assumes proper configuration of the P3_TRANS.INI file (Windows) or the site_setup file (Unix), which point Patran to the proper location of the MSC Nastran executable.
Retrieve the Analysis Results
Translate the Results into Patran for Results Postprocessing
• On the Patran Main Menu, click on the Analysis Application button.
• On the top of the Analysis form, select Action >> Attach XDB, Object >> Result Entities, Method >> Local.
• Click on the Select Results File button.
• On the Select File form, select cup.xdb. Click OK.
• Click Apply on the Analysis form.
Results Postprocessing
Create Fringe and Deformation Plot
• On the Patran Main Menu, click on the Results Application button.
• On the top of the Result form, select Action >> Create, Object >> Quick Plot.
• Click the Select Results icon near the top of the form.
• In the Select Result Cases listbox, select SC1:Untitled.SC1, A1 Static Subcase.
• In the Select Fringe Result listbox, select Stress Tensor.
• In the Select Deformation Result listbox, select Displacement, Translational.
• Click Apply
