1. Working folder
A) Create a working folder.
B) Place a Patran shortcut in that folder and change the ‘Properties/start in:’ target to that working directory.
C) For convenience, place any geometry files in that folder.
2. Set Preferences/Analysis: MSC Patran Thermal
NOTE: if you are converting a NASTRAN stress model to a thermal model, be sure to:
1) Delete mechanical material properties (Modulus, thermal expansion, etc.)
2) Delete ANY temperature loads, otherwise they will be carried over to the thermal analysis.
3. Decide on units and stick to them throughout the analysis. Pay particular attention to time (hrs, min., secs) and to ft. and inches.
4. Properties and BCs may be applied to geometry or elements, so you can mesh now or mesh later. Applying them to geometry will allow remeshing without having to reassign properties and BCs to elements.
5. Create fields for temperature dependant material properties.
Fields/Create/Material Properties/General
A) Enter field name
B) Input Data/Select Function Term/
Select function method, i.e.: mpid_indx_linr_tabl
Select proper temp units and fill out property vs. temp table.
OK/OK/Apply
6. Create material properties, enter constant values and select field names for those that are temperature dependant
7. Create time dependant nodal temperature and/ or heat flux BCs
A) Loads BCs/Create/Temperature/Nodal/Time Table
8. Solve: Analysis/Analyze/Full Model/Full Run
A) Solution Type/Transient Run
B) Solution Parameters
Select temperature units
Run Control Parameters
Start Time (if not 0)
Stop Time
Select proper S-B Constant for units used.
Select Initial Temperature
OK/OK
C) Output Requests
Select temperature units
Print Interval Controls
Initial Print Interval
Enter unit time label
Fill out Print Interval vs. Solution Time table.
OK
D. Apply — this will start the analysis solution.
8. Reading Results: A Results file will be generated for each time interval and will be placed in a new folder with the analysis job name. It is possible to read in each result manually at Analysis/Read Result/Results Entities. This could be extremely tedious and time consuming, depending on the number of time intervals solved for. If so, use the following utility for reading results:
A) Utilities/Thermal/Thermal Results Reader
Select proper folder (same as job name)
Recommend following directions for incremental file selection
Get Files
Selected Results: Scroll through and verify that all files are listed
Apply
9. Contour plot – Results/Create/Fringe
A) Select Results/Select desired result time point
B) Target Entities/Select nodes on model to plot.
C) Display Attributes/Choose curve fit, axis labels etc.
D) Plot Options/File name to save to.
E) Animation Options as required.
10. XY plot – Results/Create/Graph/YvsX –
A) Select Results/Select all cases to plot.
B) Target Entities/Current Viewport, Free Faces,
C) Display Attributes/Spectrum, Range, Labels etc.
D) Plot Options/File name to save to.
11. Export XY plot data to Excel – XY Plot/Modify/Curve
A) From Existing Curves, select saved curve (graph)
B) Select ‘Data from keyboard’
Select XY pairs
Select ‘Write Data to File’
Apply
File name: name.xyd
OK
12. Create nodal temperature field for structural analysis – Fields/Spatial/FEM
While in Patran Thermal preference:
Select load case (time) of interest and plot it
Create a “field” load with these temperatures
A) Fields/Spatial/FEM
Give it a field name
Continuous
Scalar
Select Groups
Apply
Switch to the NASTRAN structural preference Preference / Analysis
Create a Temperature Boundary condition
Loads/BCs
Create
Temperature / Node
Label the boundary condition
Input Data – Select Spatial Field you created
Application region – Select all nodes – Add – OK
Apply
Export data for Nastran Structural Analysis
B) File/Export
File name: name.out
Format: Neutral
Neutral Options
Select Node Temperatures
Select appropriate groups
Apply
Delete Boundary condition Temperature you just created
Switch preference back to Patran Thermal