Thermal Analysis Using MSC.Nastran

Transcription

1 MSC.Software Corporation 815 Colorado Boulevard Los Angeles, California Tel: (323) Fax: (323) United States MSC.Patran Support Tel: Fax: Tokyo, Japan Tel: Fax: Munich, Germany Tel: (+49) Fax: (+49) Thermal Analysis Using MSC.Nastran NAS104 EXERCISE WORKBO MSC.Nastran Version 70.7 MSC.Patran Version 9.0 NA*70.7*Z*Z*Z*SM-NAS104-WBK May 2000

2 PROPRIETARY NOTICE The MSC.Software Corporation reserves the right to make changes in specifications and other information contained in this document without prior notice. Although due care has been taken to present accurate information, THE MSC.SOFTWARE CORPORATION DISCLAIMS ALL WARRANTIES WITH RESPECT TO THE CONTENTS OF THIS DOCUMENT (INCLUDING WITHOUT LIMITATION WARRANTIES OF MERCHANTABILITY AND FITNESS FOR A PARTICULAR PURPOSE) EITHER EXPRESSED OR IMPLIED. THE MSC.SOFTWARE CORPORATION SHALL NOT BE LIABLE FOR DAMAGES RESULTING FROM ANY ERROR CONTAINED HEREIN, INCLUDING, BUT NOT LIMITED TO, FOR ANY SPECIAL, INCIDENTAL OR CONSEQUENTIAL DAMAGES ARISING OUT OF, OR IN CONNECTION WITH, THE USE OF THIS DOCUMENT. MSC.Patran is a registered trademark of The MSC.Software Corporation. MSC and MSC. are registered trademarks and service marks of The MSC.Software Corporation. ABAQUS is a registered trademark of Hibbitt, Karlsson, & Sorensen, Inc. ANSYS is a registered trademark of ANSYS, Inc. CADDS 5 and Computervision are trademarks of Computervision R&D Inc., a subsidiary of Prime Computer, Inc. CATIA is a registered trademark of Dassault Systemes. EUCLID is a registered trademark of Matra Datavision, S.A. IGES is an acronym for the Initial Graphics Exchange Specification, published by the U.S. Department of Commerce, National Institute of Standards and Technology. MARC is a registered trademark of MARC Analysis Research Corporation. Motif is a trademark of the Open Software Foundation, Inc. MSC.Nastran is an enhanced proprietary version developed, maintained, supported and marketed by The MSC.Software Corporation. NASTRAN is a registered trademark of the National Aeronautics and Space Administration. Pro/ENGINEER is a trademark of Parametric Technology Corporation. Unigraphics is a registered trademark of EDS Unigraphics Division. UNIX is a trademark of AT&T Bell Laboratories. X Window System is a trademark of the Massachusetts Institute of Technology. Training Documentation: Copyright 2000 The MSC.Software Corporation. All Rights Reserved. This notice shall be marked on any reproduction of this documentation, in whole or in part. Any reproduction or distribution of this document, in whole or in part, without the prior written consent of The MSC.Software Corporation is prohibited. If you would like to order more copies of this document, please contact MSC.Software Contracts Processing at (800) U.S.A. orders: All orders must be accompanied by a check or purchase order. Your order will be sent prepaid via UPS or fourth class mail and the shipping charges will be added to the invoice. F.O.B. will be the shipping point. Terms are net amount due within 30 days. Outside U.S.A. orders: Please contact your local MSC.Software office for a quotation.

3 DISCLAIMER The concepts, methods, and examples presented in this text are for educational purposes only and are not intended to be exhaustive or to apply to any particular engineering problem or design. The MSC.Software Corporation assumes no liability or responsibility to any person or company for direct or indirect damages resulting from the use of any information contained herein. Printed in U.S.A by MSC.Software Corporation All rights reserved.

4

5 TABLE OF CONTENTS Lesson Title 1. Getting Started 1a. Creating A Model 1b. Transient Thermal Analysis 2. Free Convection on Printed Circuit Board 3. Forced Convection on Printed Circuit Board 4. Thermal Contact Resistance 5. Typical Avionics Flow 6. Radiation Enclosures 7. Axisymmetric Flow in a Pipe 8. Directional Heat Loads 9. Thermal Stress Analysis from Directional Heat Loads 10. Thermal Stress Analysis of a Bi-Metallic Plate Appendix A Title Transient Thermal Analysis of a Cooling Fin B. Analytical Solution for a Simple Radiation to Space Problem C. Printed Circuit Board using 2 1/2 D Paved Meshing Method D. Create Group and List E. Importing IGES File and Auto_Tet Mesh the Model MSC.Nastran 104 Exercise Workbook 0-3

6 0-4 MSC.Nastran 104 Exercise Workbook

7 WORKSHOP 1a Getting Started Creating A Model Objectives: Create a new database defined for MSC.Nastran thermal analysis. Define geometry for a rectangular plate. MSC.Nastran 104 Exercise Workbook 1a-1

8 1a-2 MSC.Nastran 104 Exercise Workbook

9 WORKSHOP 1a Getting Started Creating A Model Model Description: Figure 1a.1 In this exercise you will first create a aluminum plate. Shown below is a drawing of the model you will be building and suggested steps for its construction. 1 m Aluminum Plate K = 204 W/m- o C C p = 896 J/kg- o C ρ = 2707 kg/m 3 h = 10.0 W/m 2 - o C T amb = 20.0 o C 3 m q = W/m 2 Thickness = 0.1 m T = 50 o C MSC.Nastran 104 Exercise Workbook 1a-3

10 1a-4 MSC.Nastran 104 Exercise Workbook

11 WORKSHOP 1a Getting Started Creating A Model Suggested Exercise Steps: Create a new database defined for MSC.NASTRAN thermal analysis. Define geometry for a rectangular plate. Mesh the structure with quadrilateral elements. Modify the mesh. Define the plate s material as aluminum. Specify a thermal conductivity of 204 W/m-oC, specific heat of 896 J/kg-oC, and a density of 2707 kg/m3. Define the plate s thickness to be 0.1 m. Clean up the display. a temperature of 50 oc to the bottom edge of the plate. heat flux of 5000 W/m2 to the right edge of the plate. to the left edge of the surface a convection boundary condition with heat transfer coefficient of 10.0 W/m2-oC and ambient temperature of 20 oc. Perform a steady-state thermal analysis using MSC.NASTRAN within the MSC.PATRAN system. Visualize the temperature distribution as a contour plot. MSC.Nastran 104 Exercise Workbook 1a-5

12 1a-6 MSC.Nastran 104 Exercise Workbook

13 WORKSHOP 1a Getting Started Creating A Model Exercise Procedure: 1. Open a new database. Name it ex1a. File/New... New Database Name: ex1a The viewport (PATRAN s graphics window) will appear along with a New Model Preference form. The New Model Preference sets all the code specific forms and options inside MSC.PATRAN. In the New Model Preference form set the Analysis Code to MSC.Nastran Tolerance: Analysis Code: Approximate Maximum Model Dimension: 10.0 Analysis Type: 2. Create the Model. Geometry Action: Create Object: Surface Method: XYZ Vector Coordinates List: <1 3 0> Origin Coordinates List: [0 0 0] 3. Mesh the surface with elements. Finite Elements Action: Create Object: Mesh Based on Model MSC/NASTRAN Thermal MSC.Nastran 104 Exercise Workbook 1a-7

14 Type: Surface Global Edge Length: 0.1 Mesher: IsoMesh Surface List: Surface 1 At this point, we will invoke MSC.PATRAN s undo feature so that we can make a coarser mesh. The mesh we have just created (300 elements) is excessive for our example. Your model should look like the following figure. Y Z X At this point, we will invoke MSC.PATRAN s undo feature so we can make a coarser mesh. The mesh we have just created (300 elements) is excessive for our example. Click on the Undo icon. Undo Click on the Refresh Graphics icon. Reset Graphics 1a-8 MSC.Nastran 104 Exercise Workbook

15 WORKSHOP 1a Getting Started Creating A Model Note that the Finite Elements form is still visible. Change the Global Edge Length from 0.1 to 0.2. This will create elements of 0.2 units (meters) in length, which will result in a coarser mesh of 75 quadrilateral elements. Finite Elements Global Edge Length: 0.2 Your model should look like the following figure. Y Z X 4. Specify Material Properties. Our material for this exercise will be aluminum. Click on the Materials application. The Material form will appear with certain default options. Materials Action: Create Object: Isotropic Method: Manual Input Material Name: alum MSC.Nastran 104 Exercise Workbook 1a-9

16 Input Properties... Thermal Conductivity: 204 Specific Heat: 896 Density: 2707 Cancel 5. Our next task is to specify a thickness of 0.1 to our aluminum elements. Properties Action: Create Object: 2D Type: Shell Property Set Name: Input Properties... Material Name: From the Element Properties form, click on the Select Members databox. MSC.PATRAN will display two icons to the left of the Element Properties form. The first icon represents surface or face, the second represents 2D element. The two options allow you to apply properties either on the geometric entity (in this case, the surface) or on the finite elements. Click on the Surface or Face icon. plate Thickness: 0.1 Surface or Face m:alum Now click anywhere on the geometric surface. The surface will be highlighted in red. The Select Members databox will now appear as Surface 1. Add 1a-10 MSC.Nastran 104 Exercise Workbook

17 WORKSHOP 1a Getting Started Creating A Model 6. the load and boundary conditions. Load/BCs Action: Create Object: Temp(Thermal) Type: Nodal New Set Name: tempbc Input Data... Boundary Temperature: 50 Select Application Region... Geometry Filter: Geometry Click on the Curve or Edge icon. Curve or Edge With your mouse, position the cursor on the bottom edge of the surface. Click on the edge. You will see Surface 1.4 appear in the Select Geometry Entities databox. This means we have selected Edge number 4 in Surface number 1. Add 7. We will now apply heat flux to the model using the Loads/Boundary Conditions form. Load/BCs Action: Create Object: Applied Heat Type: Element Uniform MSC.Nastran 104 Exercise Workbook 1a-11

18 Option: Normal Fluxes Analysis Type: Thermal New Set Name: flux Target Element Type: 2D Because the problem is a 2D one, we need to toggle that Target Element Type setting to 2D. Even though we are applying heat flux along an edge, which we normally think of as 1D, our finite element problem is 2D; i.e., we are modeling heat conduction in two dimensions. Input Data... Form Type: Basic Surface Option: Edge Edge Heat Flux: 5000 Select Application Region... Geometry Filter: Geometry Click on the Edge icon. Edge Position the cursor over the right edge of the surface and click on this edge with the mouse. MSC.PATRAN will insert Surface 1.3 in the databox under the heading Select Surfaces or Edges. Add A yellow flag will appear on the right edge of your surface indicating that a heat flux of 5000 W/m 2 has been applied along the right edge. 1a-12 MSC.Nastran 104 Exercise Workbook

19 WORKSHOP 1a Getting Started Creating A Model Your model should look like the following figure Y Z X We will now apply a convention boundary condition to the left edge of the plate-- again, using the Loads/BCs form. Load/BCs Action: Create Object: Convention Type: Element Uniform Option: To Ambient Analysis Type: Thermal New Set Name: conv Target Element Type: 2D Input Data... Surface Option: Edge Edge Convection Coef: 10 Ambient Temperature: 20 MSC.Nastran 104 Exercise Workbook 1a-13

20 Select Application Region... Geometry Filter: Geometry Click on the Edge icon. Edge Position the cursor over the left edge of the surface and click on the edge with the mouse. MSC.PATRAN will insert Surface 1.1 in the databox under Select Surfaces or Edges Add A green label will appear confirming that you have applied a convection coefficient of 10.0W/m2-oC at this location of your model. Your model should look like the following figure Y Z X a-14 MSC.Nastran 104 Exercise Workbook

21 WORKSHOP 1a Getting Started Creating A Model 9. We are now ready to submit the model for MSC.NASTRAN steadystate thermal analysis. Click on the Analysis application located on the MSC.PATRAN main form. Analysis Action: Analyze Object: Entire Model Method: Analysis Deck Job Name: ex1a MSC.Nastran 104 Exercise Workbook 1a-15

22 Submitting the Input File for Analysis: 10. Submit the input file to MSC.NASTRAN for analysis. To submit the MSC.PATRAN.bdf file for analysis, find an available UNIX shell window. At the command prompt enter: nastran ex1a.bdf scr=yes. Monitor the run using the UNIX ps command. 11. When the run is completed, edit the ex1a.f06 file and search for the word FATAL. If no matches exist, search for the word WARNING. Determine whether existing WARNING messages indicate modeling errors. 1a-16 MSC.Nastran 104 Exercise Workbook

23 WORKSHOP 1a Getting Started Creating A Model 12. MSC.Nastran Users have finished this exercise. MSC.Patran Users should proceed to the next step. 13. Proceed with the Reverse Translation process, that is, attaching the ex1a.xdb results file into MSC.Patran. To do this, return to the Analysis form and proceed as follows: Analysis Action: Attach XDB Object: Result Entities Method: Local Select Results File... Select Results File 14. Display the Results. ex1a.xdb Results Select Results Cases: Select Fringe Result: Default, PW Linear: 100. % of Load Temperatures A contour plot displaying temperature distributions will appear. MSC.Nastran 104 Exercise Workbook 1a-17

24 Your model should look like the following figure. Select the Save and Close operations from the Fil menu to save your plate.db file. We will perform a transient thermal analysis on this model in the next workshop. 15. Close database and quit MSC.Patran to complete this exercise. File/Quit... 1a-18 MSC.Nastran 104 Exercise Workbook

25 WORKSHOP 1b Transient Thermal Objectives: Open the database created in Workshop 1a. Define time dependent funtions using the Field application. Create a trasient load case. MSC.Nastran 104 Exercise Workbook 1b-1

26 1b-2 MSC.Nastran 104 Exercise Workbook

27 WORKSHOP 1b Transient Thermal Analysis Model Description: Figure 1b.1 This exercise describes transient thermal analysis, it is an extension of the steady state modeling exercise given in Workshop 1a. This workshop contains step-by-step descriptions of the menu picks involved in the modeling process. Shown below is a drawing of the model you will be building and suggested steps for its construction 0.4 m 1 m Aluminum Plate k = 204 W/m- o C C p = 896 J/kg- o C ρ = 2707 kg/m 3 h = 10.0 W/m 2 - o C T amb = 20.0 o C 3 m q = q flux (t) W/m 2 q = q vol (t) W/m 3 Thickness = 0.1 m T 0 = 50 o C T = 50 o C MSC.Nastran 104 Exercise Workbook 1b-3

28 1b-4 MSC.Nastran 104 Exercise Workbook

29 WORKSHOP 1b Transient Thermal Analysis Suggested Exercise Steps: Open the database created in Workshop 1a. Define time dependent functions using the Field application. Create a transient load case. Add two existing load sets (temperature and convection boundary conditions) to this transient load case. time varying heat flux to the right edge of the plate a transient volumetric heat generation inside the shaded area of the plate Select solution type as transient analysis. Specify the default initial temperature. Define time steps. Select a transient load case. Perform a transient thermal analysis using MSC.NASTRAN within the MSC.PATRAN system Postprocess the transient results (Contour and XY plots). MSC.Nastran 104 Exercise Workbook 1b-5

30 1b-6 MSC.Nastran 104 Exercise Workbook

31 WORKSHOP 1b Transient Thermal Analysis Exercise Procedure: 1. Open the database created in workshop 1a. File/Open... Existing Database Name: ex1a 2. Define Time Dependent Functions. Before applying time varying loads and boundary conditions, we need to define time dependent functions using the Field application. In this model, two time fields are defined, one for applied heat flux and one for volumetric heat generation. Fields Action: Create Object: Non Spatial Method: Tabular Input Field Name: Input Data... flux_time Fill in the table with the following values using the RETURN or ENTER key : : : : : Time(t): Value: MSC.Nastran 104 Exercise Workbook 1b-7

32 Similarly, a time dependent function for volumetric heating is defined as follows. Fields Action: Create Object: Non Spatial Method: Tabular Input Field Name: Input Data... qvol_time : : : : : Time(t): Value: 3. Create a transient load case. Load Cases Action: Create Load Case Name: transient Load Case Type: Time Dependent 1b-8 MSC.Nastran 104 Exercise Workbook

33 WORKSHOP 1b Transient Thermal Analysis Since the temperature and convection boundary conditions are not changed from Workshop 1a, we can associate these two load sets with the new load case directly. Assign/Prioritize Loads/BCs Highlight Conve_conv and Temp_tempbc within the Select Individual Loads/BCs Sets listbox. At this point, we will impose a transient flux load on the plate s right edge. The magnitude of this flux load is 5000 W/m2 multiplied by the time dependent function flux_time defined earlier under the Fields application. Click on the Loads/BCs application. Loads/BCs Action: Create Object: Applied Heat Method: Element Uniform Option: Normal Fluxes Analysis Type: Thermal New Set Name: tran_flux Target Element Type: 2D Input Data... Surface Option: Edge Edge Heat Flux: 5000 Time Function: Select Application Region... f:flux_time Select 2D Elements: Surface 1.3 Add MSC.Nastran 104 Exercise Workbook 1b-9

34 4. Transient Volumetric Heat Generation Inside the Plate. The volumetric heating can be applied in a similar way, using the Loads and Boundary Conditions form as follows. Loads/BCs Action: Create Object: Applied Heat Method: Element Uniform Option: Volumetric Generation Analysis Type: Thermal New Set Name: tran_qvol Target Element Type: 2D Input Data... Time Function: Next, click on Select Application Region located on the Loads and Boundary Conditions form. We want to apply an internal heat generation inside a section of the plate from x=0.0 m to x=0.4 m. This application region will be selected by graphical cursor using the FEM geometry filter. Select Application Region... f:qvol_time Geometry Filter: FEM Use the mouse cursor to drag a rectangle covering the elements located between x=0.0 m and x=0.4 m. Release the mouse cursor. The first two columns of the elements will turn red indicating the selection. Also, a list of elements will appear in the Select 2D Elements databox. Add 1b-10 MSC.Nastran 104 Exercise Workbook

35 WORKSHOP 1b Transient Thermal Analysis Note: A square yellow marker will appear on the center of the selected element indicating that a volumetric heating has been applied on this element. 5. Now we are ready to set the analysis controls for transient thermal analysis. Analysis Action: Analyze Object: Entire Model Method: Analysis Deck Job Name: Solution Type... TRANSIENT ANALYSIS Solution Parameters... ex1b For transient thermal analysis, we have to employ a starting temperature from which the solution evolves. If the initial temperature distribution is uniform, a default initial temperature is sufficient to specify the initial state. Otherwise, the Initial Temperature object in Loads and BCs application must be used to define initial nodal temperatures explicitly. Default Init Temperature: 50.0 Subcase Create... Available Subcase: Subcase Parameters... Initial Time Step: 10 Number of Time Steps: 100 Cancel Subcase Select... transient MSC.Nastran 104 Exercise Workbook 1b-11

36 Subcases for Solution Sequence: Subcases Selected: transient Default 1b-12 MSC.Nastran 104 Exercise Workbook

37 WORKSHOP 1b Transient Thermal Analysis Submitting the Input File for Analysis: 6. Submit the input file to MSC.NASTRAN for analysis. 6a. To submit the MSC.PATRAN.bdf file for analysis, find an available UNIX shell window. At the command prompt enter: nastran ex1b.bdf scr=yes. Monitor the run using the UNIX ps command. 7. When the run is completed, edit the ex1a.f06 file and search for the word FATAL. If no matches exist, search for the word WARNING. Determine whether existing WARNING messages indicate modeling errors. MSC.Nastran 104 Exercise Workbook 1b-13

38 8. MSC.Nastran Users have finished this exercise. MSC.Patran Users should proceed to the next step. 9. Proceed with the Reverse Translation process, that is, attaching the ex1b.xdb results file into MSC.Patran. To do this, return to the Analysis form and proceed as follows: Analysis Action: Attach XDB Object: Result Entities Method: Local Select Results File... Select Results File ex1b.xdb Note: The heartbeat will change to the color blue, indicating that reading process is underway. When the heartbeat turns green again, the results are ready for postprocess. 10. We will create a contour plot of temperature distributions at time=700 sec using the Results Display form. Results Action: Create Object: Quick Plot Select Results Cases: Select Fringe Result: Transient, Time=700 Temperatures 1b-14 MSC.Nastran 104 Exercise Workbook

39 WORKSHOP 1b Transient Thermal Analysis Your model should look like the following figure. Now we will apply XY plotting to visualize the temperature-time history of Nodes Results Action: Create Object: Graph Method: Y vs. X In the Select Result Case(s) listbox, click an drag mouse to select the time states from transient, Time=0, to transient, time=1020. Within the Select Y Result listbox, highlight Temperatures. Select Y Result: Temperatures Click on the Target Entities icon. Target Entities Target Entity: Nodes MSC.Nastran 104 Exercise Workbook 1b-15

40 Select Nodes: Node 49:54 At this point, we will modeify the Y scale of the XY plot and display grid lines in the Y directly by clicking on the XY Plot application. XY Plot Action: Modify Object: Axis Select Current XY Window: Results Graph Active Axis: Y Scale... Scale: Assignment Method: Enter Lower and Upper Values: Number of Primary Tick Marks: Cancel Grid Lines... Linear Range Display: Primary 6 1b-16 MSC.Nastran 104 Exercise Workbook

41 WORKSHOP 1b Transient Thermal Analysis Your model should look like the following figure. 11. Close the database and quit MSC.Patran when you have completed this exercise. File/Quit... MSC.Nastran 104 Exercise Workbook 1b-17

42 1b-18 MSC.Nastran 104 Exercise Workbook

43 WORKSHOP 2 Free Convection on Printed Circuit Board Objectives: Create surfaces for PCB and electronic devices. thermal loads and boundary conditions. Perform a steady-state analysis. MSC.Nastran 104 Exercise Workbook 2-1

44 2-2 MSC.Nastran 104 Exercise Workbook

45 WORKSHOP 2 Free Convection on Printed Circuit Board Model Description: Shown below depicts a printed circuit board (PCB assembly which has three significant ship devices mounted on it. Each chip is generating heat at a rate that is consistent with the application of a heat flux of 5.0 W/in2 over each device surface area. Heat is dissipated by thermal conduction within the chips and underlying board. Free convection to the ambient environment provides the ultimate heat take. The ambient temperature for convection is assumed to be 20.0 o C, and a heat transfer coefficient of 0.02 W/in2- oc is used to apply convection to the entire assembly surface. We will analyze the printed circuit board to determine the device temperature so that they can be compared to manufacturer allowables. Shown below is a drawing of the model you will be building and suggested steps for its construction. MSC.Nastran 104 Exercise Workbook 2-3

46 2-4 MSC.Nastran 104 Exercise Workbook

47 WORKSHOP 2 Free Convection on Printed Circuit Board Suggested Exercise Steps: Create the Surfaces of Printed Circuit Board and Electric Components. Extrude the Surfaces to Create Solids. Mesh the Solids. Specify Materials. Define Element Properties. Merge the Common Nodes. Verify the Free Edges. a heat load on each device. a convection boundary condition on the PCB. Perform the Analysis. Read the analysis results. Display the results. MSC.Nastran 104 Exercise Workbook 2-5

48 2-6 MSC.Nastran 104 Exercise Workbook

49 WORKSHOP 2 Free Convection on Printed Circuit Board Exercise Procedure: 1. Create a New Database and name it free_conv_pcb.db. File/New... New Database Name free_conv_pcb.db 2. Change the Tolerance to Default and the Analysis Code to MSC.Nastran in the New Model Preferences form. Verify that the Analysis Type is Structural. New Model Preference Tolerance Analysis Code: Analysis Type Default MSC/NASTRAN Thermal 3. Create the surfaces of printed circuit board and electronic components.. Action: Object: Method: For Chip 1 Geometry Surface ID List: 1 Create Surface XYZ Vector Coordinates List: <9 6 0 > Origin Coordinates List: [0 0 0] Surface ID List: 2 Vector Coordinates List: < > Origin Coordinates List: [1 1 0] MSC.Nastran 104 Exercise Workbook 2-7

50 .For Chip 2 Surface ID List: 3 Vector Coordinates List: <1 1 0> Origin Coordinates List: [4 4 0] For Chip 3 Surface ID List: 4 Vector Coordinates List: <1 1 0> Origin Coordinates List: [ ] 4. Create the PCB solid by extruding surfaces 1 by -0.1 inch in the Z direction. Extrude surfaces.2,3 and 4 in the Z direction by 0.25 inches. Action: Object: Method: Geometry Solid ID List: 1 If the Auto Execute is ON, you do not need to click on. For Chips 1, 2, 3: Create Solid Extrude Translation Vector: < > Surface List: Surface 1 Solid ID List: 2 Translation Vector: < > 2-8 MSC.Nastran 104 Exercise Workbook

51 WORKSHOP 2 Free Convection on Printed Circuit Board Surface List: Surface 2:4 5. You will now create the model s finite elements. Action: Object: Type: Finite Elements Create Mesh Solid Global Edge Length: 0.25 Element Topology: Hex8 Solid List: Solid 1:4 To obtain a clearer view, select the isometric view by clicking on the Iso View icon. The mesh should look like this. MSC.Nastran 104 Exercise Workbook 2-9

52 6. For this model we will assume that the PCB and chips are manufactured from the isotropic materials having constant conductivities. Kpcb = W/in-oCKchip = 2.24 W/in-oC Action: Object: Method: Materials Material Name: Input Properties... For chips 1, 2, 3: Create Isotropic Manual Input pcb Thermal Conductivitiy Action: Object: Method: Materials Material Name: Create Isotropic Manual Input chip Thermal Conductivity: For a solid model element properties are used to assign the materials to the various parts of the model.. Properties Action: Dimension: Type: Property Set Name: Input Properties... Create 3D Solid pcb 2-10 MSC.Nastran 104 Exercise Workbook

53 WORKSHOP 2 Free Convection on Printed Circuit Board Material Name: m:pcb Select Members: Solid 1 ADD Chips 1, 2, 3 Input Properties... Material Name: m:chip Select Members: Solid 2:4 ADD 8. To verify that the correct material properties have been defined and assigned to the correct model locations, change the Action option to Show and create a scalar plot of the model s materials. Properties Action: Select Property: Display Method Select Groups: Show Material Name Scalar Plot Current Viewport Default Group MSC.Nastran 104 Exercise Workbook 2-11

54 The scalar plot resembles the following. 9. The duplicate nodes located at the PCB and chip interfaces must be merges. Action: Object: Method: Finite Elements Equivalence 10. To check the equivalence process you should verify the element boundaries. If the model has been equivalenced properly you should see a wireframe rendering of your model where only the free edges are components of the wireframe image. Display the view to ensure that the model has no cracks between elements. All Equivalence Tolerance: Finite Elements Tolerance Cube Action: Object: Test: Verify Element Boundaries 2-12 MSC.Nastran 104 Exercise Workbook

55 WORKSHOP 2 Free Convection on Printed Circuit Board Display Type: Free Edges 11. A heat flux will now be applied to the exposed plan from face of the chips. Action: Object: Type: Option: Load/BCs New Set Name: Target Element Type: Input Data... Heat Flux: 5 Select Application Region... Geometry Filter: Create Applied Heat Element Uniform Normal Fluxes flux Use the Free Face Select icon to help you pick the exposed chip faces. 3D Geometry Select Solid Faces: Solid Add 12. The convection boundary condition will now be applied to the back side of the PCB (side opposite the chips).. Load/BCs MSC.Nastran 104 Exercise Workbook 2-13

56 Action: Object: Type: Option: New Set Name: Target Element Type: Input Data... Convection Coefficient: Ambient Temperature: Select Application Region Geometry Filter: Select Solid Faces: Create Convection Element Uniform To Ambient conv 3D Geometry Solid 1.6 Use the Free Face Select icon to help you pick the back face of the PCB. Add 13. Perform the Analysis. Analysis Action: Object: Method: Job Name: Solution Type... Solution Type: Analyze Entire Model Full Run ex2 STEADY STATE ANALYSIS 2-14 MSC.Nastran 104 Exercise Workbook

57 WORKSHOP 2 Free Convection on Printed Circuit Board An MSC.Nastran input file called ex2.bdf will be generated. This process of translating your model into an input file is called the Forward Translation. The Forward Translation is complete when the Heartbeat turns green. MSC.Nastran 104 Exercise Workbook 2-15

58 Submitting the Input File for Analysis: 14. Submit the input file to MSC.Nastran for analysis. 14a. To submit the MSC.Patran.bdf file, find an available UNIX shell window. At the command prompt enter nastran ex2.bdf scr=yes. Monitor the run using the UNIX ps command. 14b. To submit the MSC.Nastran.dat file, find an available UNIX shell window and at the command prompt enter nastran ex2 scr=yes. Monitor the run using the UNIX ps command. 15. When the run is completed, edit the ex2.f06 file and search for the word FATAL. If no matches exist, search for the word WARNING. Determine whether existing WARNING messages indicate modeling errors MSC.Nastran 104 Exercise Workbook

59 WORKSHOP 2 Free Convection on Printed Circuit Board 16. MSC.Nastran Users have finished this exercise. MSC.Patran Users should proceed to the next step. 17. Proceed with the Reverse Translation process, that is, attaching the fin.xdb results file into MSC.Patran. To do this, return to the Analysis form and proceed as follows:. Analysis Action: Object: Method: Select Result Files... Select Results File Attach XDB Result Entities Local ex2.xdb 18. Display the results. Results Object: Select Results Cases: Select Fringe Result: Quick Plot Default, PW Linear: 100%.. Temperature MSC.Nastran 104 Exercise Workbook 2-17

60 The result should resemble the following. The heat generated by the electronic devices is conducted to the printed circuit board, and then spread on the epoxy glass PCB. The cooling mechanism is provided by a free convection heat exchange between the backside of the PCB and the ambient fluid that is maintained at 20 oc. As a result, the largest electronic device has the highest temperature. Because of their indentical size, the other two electronic chips possess nearly the same temperature distribution MSC.Nastran 104 Exercise Workbook

61 WORKSHOP 3 Forced Air Convection on Printed Circuit Board Objective: Create Geometry from MSC.Patran MSC.Nastran 104 Exercise Workbook 3-1

62 3-2 MSC.Nastran 104 Exercise Workbook

63 WORKSHOP 3 Forced Air Convection on Printed Circuit Board Model Description: We will model the previous PCB thermal analysis with forced air convection over the flat plate, using the Coupled Advection feature. The air temperature rises in the X direction as the fluid stream traverses the circuit board. The temperature dependency of the convection coefficient will be defined using a temperature dependent field Z q = 20.0 W/in2. m = 8.33E-3 lbm/sec h = h(t) W/in2-oC X Tin = 20.0 oc 9.0 in X Air K = 6.66E-4 W/in-oC Cp = J/lbm-oC ρ = 5.01E-5 lbm/in3 µ = 1.03E-6 lbm/in-sec MSC.Nastran 104 Exercise Workbook 3-3

64 3-4 MSC.Nastran 104 Exercise Workbook

65 WORKSHOP 3 Forced Air Convection on Printed Circuit Board Suggested Exercise Steps: Create a new database called forced_conv_pcb.db Create a solid that represents the electronic component and the printed circuit board. Mesh surfaces and curves with global edge length of 0.25 using Hex8 as element topology Merge nodes by using Equivalence method under Finite Elements. Use Free Edges to verify the Element Boundaries Input specify Material Properties for the chip, pcb, air, and flow tube. Define the solids properties using pcb and chip for their property names. loads and boundary conditions to the model using Coupled Advection Feature to simulate the forced air convection on the back surface of PCB. heat flux on each device using Element uniform and define the inlet Temperature of the fluid. Perform, read, and display the results MSC.Nastran 104 Exercise Workbook 3-5

66 3-6 MSC.Nastran 104 Exercise Workbook

67 WORKSHOP 3 Forced Air Convection on Printed Circuit Board Exercise Procedure: 1. Create a New Database and name it forced_conv_pcb.db. File/New... New Database Name forced_conv_pcb 2. Change the Tolerance to Default and the Analysis Code to MSC.Nastran in the New Model Preferences form. Verify that the Analysis Type is Thermal. New Model Preference Tolerance Analysis Code: Analysis Type Default MSC/NASTRAN thermal 3. Create the surfaces representing the printed circucit board. Geometry Action: Create Object: Surface Method: XYZ Vector Coordinates List: <9 6 0> Origin Coordinates List: [ ] Vector Coordinates List: < > Origin Coordinates List: [1 1 0] Vector Coordinates List: <1 1 0> Origin Coordinates List: [4 4 0] MSC.Nastran 104 Exercise Workbook 3-7

68 Vector Coordinates List: <1 1 0> Origin Coordinates List: < > When you are finished your model should look like the one shown in the figure below. 4. Extrude the solid Geometry Action: Create Object: Solid Method: Extrude Translation Vector: < > Surface List: Surface MSC.Nastran 104 Exercise Workbook

69 WORKSHOP 3 Forced Air Convection on Printed Circuit Board Translation Vector: < > Surface List: Surface 2:4 5. Mesh the solids to create Hex8 element with global edge length Finite Elements Action: Create Object: Mesh Type: Solid Global Edge Length 0.25 Element Topology Hex8 Solid List Solid 1:4 MSC.Nastran 104 Exercise Workbook 3-9

70 Your model should appear like the one shown below. 6. Equivalence the Finite Elements to reduce the number of elements by eliminating duplicate nodes. Action: Object: Type: Finite Elements 7. Verify the Element Boundaries. Equivalence All Equivalence Tolerance: Finite Elements Tolerance Cube 3-10 MSC.Nastran 104 Exercise Workbook

71 WORKSHOP 3 Forced Air Convection on Printed Circuit Board Action: Object: Test: Display Type: Verify Element Boundaries Free Edges 8. Create the isotropic material properties. Materials Action: Create Object: Isotropic Method: Manual Input Material Name: chip Input Properties... Constitutive Model: Solid properties Thermal Conductivity: 2.24 Material Name: Constitutive Model: pcb Thermal Conductivity: Solid properties 9. Create the model s element properties assigning the material type to the correct region of the model. Properties Action: Dimension: Type: Property Set Name: Create 3D Solid chip MSC.Nastran 104 Exercise Workbook 3-11

72 Input Properties... Material Name: m:chip Select Members: Solid 2:4 Add Property Set Name: pcb Input Properties... Material Names: m:pcb Select Members: Solid 1 Add 10. Define Temperature Dependent Field. Fields Action: Object: Method: Field Name: Active Independent Variables: Create Material Property Tabular Input conv_temp Temperature (T) Input Data... Input Scalar Data: Add Hit Enter Key T.Value MSC.Nastran 104 Exercise Workbook

73 WORKSHOP 3 Forced Air Convection on Printed Circuit Board 11. Select two nodes to create a curve. Geometry Action: Object: Method: Create Curve Point select the Node Icon Starting Point List: Node 938 Ending Point List: Node Define the location of the Air Stream. Action: Object: Method: Geometry Transform Curve Translate Translation Vector: < > Curve List: Curve Mesh the Airstream. preferably, the mesh size should be the same on the air stream as on the PCB. Finite Element Action: Object: Type: Create Mesh Curve MSC.Nastran 104 Exercise Workbook 3-13

74 Global Edge Length: 0.25 Ending Point List: Note: The identical mesh size is not required, but may provide the most accurate model. The Closest Approach method will select the nearest neighboring structure and fluid nodes. 14. Specify the material properties of air. 15. Define flow tube properties. Bar2 Curve List: Curve 2 Action: Object: Method: Materials Material Name: Input Properties... Constitutive Model: Thermal Conductivity: air Create Isotropic Manual Input Fluid properties 6.66e-4 Specific Heat: Density: Dynamic Viscosity: Properties 5.01e e-3 Action: Dimension: Type: Property Set Name: Input Properties... Material Name: Create 1D Flow Tube flow_tube m:air 3-14 MSC.Nastran 104 Exercise Workbook

75 WORKSHOP 3 Forced Air Convection on Printed Circuit Board Diameter at Node 1: 1.0 Select Members Curve 2 Add 16. We will use the Coupled Advection Feature to simulate the forced air convection on the back surface of PCB. Load/BCs Action: Object: Type: Options: Create Convection Element Uniform Coupled Advection There are two application regions: The Structure Region (Application Region 1) can be 1D, 2D, or 3D. In this case we have a 3D structure, and the appropriate Target Element Type is 3D. The Second Application Region must be 1D, which represents the airflow over the flat plate. In this case, select the curve along the X direction. MSC.PATRAN will then couple the fluid to the structure locally by the Closest Approach method. New Set Name: Target Element Type: Region 2: Input Data... Temperature Function Mass Flow Rate: Select Application Region flow_by_plate 3D 1D f:conv_temp 8.33e-3 MSC.Nastran 104 Exercise Workbook 3-15

76 Geometry Filter: Geometry Select Solid Surfaces: Solid 1.6 Active List for companion region Add Select Curves: Curve 2 Add 17. a Heat Flux on Each Device. Load/BCs Action: Create Object: Applied Heat Type: Element Uniform Options: Normal Flux New Set Name: heat_flux Target Element Type: 3D Input Data... Heat Flux: 20 Select Application Region Geometry Filter: Geometry Select Solid Surfaces Solid Add 3-16 MSC.Nastran 104 Exercise Workbook

77 WORKSHOP 3 Forced Air Convection on Printed Circuit Board 18. Define the inlet Temperature of the fluid. Load/BCs Action: Create Object: Temp (Thermal) Type: Nodal New Set Name: inlet_temp Input Data... Boundary Temperature: 20 Select Application Region Geometry Filter: Geometry Select Geometry Entities: Point 35 Add 19. Define the Default Initital Temperature and Perform the analysis. Analysis Action: Analyze Object: Entire Model Method: Full Run Job Name: ex3 Solution Type... Solution Parameters... Data Deck Echo: Sorted Default Init Temperature 100 MSC.Nastran 104 Exercise Workbook 3-17

78 An MSC.Nastran input file called fin.bdf will be generated. This process of translating your model into an input file is called the Forward Translation. The Forward Translation is complete when the Heartbeat turns green MSC.Nastran 104 Exercise Workbook

79 WORKSHOP 3 Forced Air Convection on Printed Circuit Board Submitting the Input File for Analysis: 20. Submit the input file to MSC.Nastran for analysis. 20a. To submit the MSC.Patran.bdf file, find an available UNIX shell window. At the command prompt enter nastran ex3.bdf scr=yes. Monitor the run using the UNIX ps command. 20b. To submit the MSC.Nastran.dat file, find an available UNIX shell window and at the command prompt enter nastran ex3 scr=yes. Monitor the run using the UNIX ps command. 21. When the run is completed, edit the ex3.f06 file and search for the word FATAL. If no matches exist, search for the word WARNING. Determine whether existing WARNING messages indicate modeling errors. MSC.Nastran 104 Exercise Workbook 3-19

80 22. MSC.Nastran Users have finished this exercise. MSC.Patran Users should proceed to the next step. 23. Proceed with the Reverse Translation process, that is, attaching the ex3.xdb results file into MSC.Patran. To do this, return to the Analysis form and proceed as follows: Analysis Action: Object: Method: Select Results File... Select Results File Attach XDB Result Entities Local ex3.xdb 24. Display the Results. Object: Results Select Results Cases: Quick Plot Default, PW Linear: 100. % of Load Select Fringe Result: Temperatures 3-20 MSC.Nastran 104 Exercise Workbook

81 WORKSHOP 3 Forced Air Convection on Printed Circuit Board Your Viewport will appear as follows. The viewport may now be reset by clicking on the broom icon in the main window. File/Quit... MSC.Nastran 104 Exercise Workbook 3-21

82 3-22 MSC.Nastran 104 Exercise Workbook

83 WORKSHOP 4 Thermal Contact Resistance Objective: Create Geometry from MSC.Patran Determine the maximum and minimum temperature on different sides of the circuit board. MSC.Nastran 104 Exercise Workbook 4-1

84 4-2 MSC.Nastran 104 Exercise Workbook

85 WORKSHOP 4 Thermal Contact Resistance Model Description: In this example we will model the contact resistance between two solids. In this case, the contact between an electronic component and a printed wiring board (PWB)--to determine the maximum temperature at the top of the chip and the temperature drop to the bottom of the wiring board. Y 5.0 in 2.0 in 5.0 in 2.0 in 2.0 in Kpwb = 0.6 W/in-oC Kchip = 1.34 W/in-oC 2.0 in X Z q = 10.0 W/in in Contact Coefficient = 1.2 W/in2-oC 0.5 in X T = 20.0 oc MSC.Nastran 104 Exercise Workbook 4-3

86 4-4 MSC.Nastran 104 Exercise Workbook

87 WORKSHOP 4 Thermal Contact Resistance Suggested Exercise Steps: Create a new database called thermal_contact_resistance.db Create a solid that represents the electronic component and the printed wiring board. Mesh surfaces and curves with global edge length of 0.25 using Hex8 as element topology Merge nodes by using Equivalence method under Finite Elements. Input specify Material Properties for both solids. Define the solids properties using pwb and chip for their property names. loads and boundary conditions to the model.contact resistance is modeled in MSC.Patran using the Convection-Coupled menu operation (select the bottom of the chip surface and the top of the printed wiring board to specify the thermal conductance between the two surfaces). heat flux on the top Surface of the chip with Element Uniform Type. Using thermal temperature, the boundary condition is applied to the backside of the PWB. Perform, read, and display the results. MSC.Nastran 104 Exercise Workbook 4-5

88 4-6 MSC.Nastran 104 Exercise Workbook

89 WORKSHOP 4 Thermal Contact Resistance Exercise Procedure: 1. Create a New Database called thermal_contact_resistance.db. File/New... New Database Name thermal_contact_resistance 2. Change the Tolerance to Default and the Analysis Code to MSC.Nastran in the New Model Preferences form. Verify that the Analysis Type is Thermal.. New Model Preference Tolerance Analysis Code: Analysis Type Default MSC/NASTRAN Thermal 3. Create the solid representing the wiring board and eletronic elements. Geometry Action: Create Object: Solid Method: XYZ Solid ID List: 1 Vector Coordinates List: < > Origin Coordinates List: [ ] Solid ID List: 2 Vector Coordinates List: <2 2.25> Origin Coordinates List: [2 2 1] MSC.Nastran 104 Exercise Workbook 4-7

90 4. Mesh the solids to create Hex8 element with global edge length Finite Elements Action: Create Object: Mesh Type: Solid Global Edge Length 0.25 Element Topology Hex8 Solid List Solid 1:2 To obtain a clearer view, select Iso 1 View Your model should appear like the one shown below. 4-8 MSC.Nastran 104 Exercise Workbook

91 WORKSHOP 4 Thermal Contact Resistance 5. Equivalence the Finite Elements to reduce the number of elements by eliminating duplicate nodes. Action: Object: Type: Finite Elements Equivalence 6. Create the isotropic material properties using the material constants specify in figure. All Equivalence Tolerance: Action: Object: Method: Materials Material Name: Input Properties... Constitutive Model: Tolerance Cube Create Isotropic Manual Input pwb Thermal Conductivity: 0.6 Solid properties Material Name: chip Constitutive Model: Solid properties Thermal Conductivity: 1.34 MSC.Nastran 104 Exercise Workbook 4-9

92 7. Create the model s element properties assigning the material type to the correct region of the model. Action: Properties Dimension: Type: Property Set Name: Input Properties... Material Name: Create 8. Contact resistance is modeled in MSC.Patran using the Convection Coupled. This technique enables you to apply a connection through convection between two solid geometric faces without connecting the structures with finite elements. One advantage of this method is that mesh sizes between the two regions need not be congruent. MSC.Patran will automatically find the ambient points closest to the thermal contact area. 3D Solid pwb m:pwb Select Members: Solid 1 Add Property Set Name: Input Properties Material Names: Chip m:chip Select Members: Solid 2 Add Load/BCs Action: Object: Type: Create Convection Element Uniform 4-10 MSC.Nastran 104 Exercise Workbook

93 WORKSHOP 4 Thermal Contact Resistance Options: New Set Name: Target Element Type: Region 2: Input Data... Coupled coup_conv Note: Arrows should be pointing downward into the printed wiring board. 3D 3D Convection Coefficient: 1.2 Select Application Region Geometry Filter: Select Solid Faces: Solid 2.5 Add Active List Select Solid Faces: Solid 1.6 Add Geometry 9. a Heat Flux on the Top Surfaces of the chip. Load/BCs Action: Object: Type: Options: New Set Name: Target Element Type: Input Data... Create Applied Heat Element Uniform Normal Fluxes heat_flux 3D MSC.Nastran 104 Exercise Workbook 4-11

94 Heat Flux: 10 Select Application Region Geometry Filter: Geometry Select Solid Surfaces Solid 2.6 Select the Free Face Solid icon Add 4-12 MSC.Nastran 104 Exercise Workbook

95 WORKSHOP 4 Thermal Contact Resistance 10. a temperature Boundary Condition on the backside of the Load/BCs Action: Create Object: Temp (Thermal) Type: Nodal New Set Name: tempbc Input Data... Boundary Temperature: 20 Select Application Region Geometry Filter: Geometry Select Geometry Entities: Solid 1.5 Select the Surface or Face icon Add PWB. 11. Perform the analysis. Analysis Action: Object: Method: Job Name: Analyze Entire Model Full Run ex4 MSC.Nastran 104 Exercise Workbook 4-13

96 An MSC.Nastran input file called ex4.bdf will be generated. This process of translating your model into an input file is called the Forward Translation. The Forward Translation is complete when the Heartbeat turns green MSC.Nastran 104 Exercise Workbook

97 WORKSHOP 4 Thermal Contact Resistance Submitting the Input File for Analysis: 12. Submit the input file to MSC.Nastran for analysis. 12a. To submit the MSC.Patran.bdf file, find an available UNIX shell window. At the command prompt enter nastran ex4.bdf scr=yes. Monitor the run using the UNIX ps command. 12b. To submit the MSC.Nastran.dat file, find an available UNIX shell window and at the command prompt enter nastran ex4 scr=yes. Monitor the run using the UNIX ps command. 13. When the run is completed, edit the ex4.f06 file and search for the word FATAL. If no matches exist, search for the word WARNING. Determine whether existing WARNING messages indicate modeling errors. MSC.Nastran 104 Exercise Workbook 4-15

98 14. MSC.Nastran Users have finished this exercise. MSC.Patran Users should proceed to the next step. 15. Proceed with the Reverse Translation process, that is, attaching the ex4.xdb results file into MSC.Patran. To do this, return to the Analysis form and proceed as follows:. Analysis Action: Object: Method: Select Results File... Select Results File Attach XDB Result Entities Local ex4.xdb 16. Display the Results. Object: Results Select Results Cases: Your Viewport will appear as follows. Quick Plot Default, PW Linear: 100. % of Load Select Fringe Result: Temperature 4-16 MSC.Nastran 104 Exercise Workbook

99 WORKSHOP 4 Thermal Contact Resistance The viewport may now be reset by clicking on the broom icon in the main window. File/Quit... MSC.Nastran 104 Exercise Workbook 4-17

100 4-18 MSC.Nastran 104 Exercise Workbook

101 WORKSHOP 5 Typical Avionics Flow Objective: Modeling this problem within the MSC.Patran and MSC.Nastran. This method allows the analyst an option to specify non-coincident mesh sizes on the structure and the fluid nodes. MSC.Nastran 104 Exercise Workbook 5-1

102 5-2 MSC.Nastran 104 Exercise Workbook

103 WORKSHOP 5 Typical Avionics Flow Model Description: In this exercise, the compact heat exchanger is being modeled using MSC.Patran. MSC.Patran can associate the structure nodes with the fluid nodes using a technique called the Closet Approach method. This method allows the analyst an option to specity non-coincident mesh sizes on the structure and the fluid nodes. However, it is recommended that you use an identical mesh size for a regular isoparametric rectangular mesh. MSC.Nastran 104 Exercise Workbook 5-3

104 5-4 MSC.Nastran 104 Exercise Workbook

105 WORKSHOP 5 Typical Avionics Flow Suggested Exercise Steps: Create a new database called avionics_flow.db. Create a new surface that has a total of five rectangular ducts. Mesh surfaces and curves with global edge length of 0.25 Merge nodes by using Equivalence method under Finite Elements. Input specify Material Properties Define the thickness of four side walls that separte fluid channels. loads and boundary conditions to the model. Perform analysis and read the analysis results. MSC.Nastran 104 Exercise Workbook 5-5

106 5-6 MSC.Nastran 104 Exercise Workbook

107 WORKSHOP 5 Typical Avionics Flow Exercise Procedure: 1. Create a New Database and name it avionics_flow.db. File/New... New Database Name avionics_flow 2. Change the Tolerance to Default and the Analysis Code to MSC.Nastran in the New Model Preferences form. Verify that the Analysis Type is Thermal. New Model Preference Tolerance Analysis Code: Analysis Type Default MSC/NASTRAN Thermal Whenever possible click Auto Execute (turn off). 3. Create the geometry that represents the the compact heat exchanger with five rectangular ducts. Geometry Action: Create Object: Curve Method: XYZ Vector Coordinates List: <1 0 0> Origin Coordinates List: [ ] MSC.Nastran 104 Exercise Workbook 5-7

108 You will now use Transformation to create the upper part of the rectangular duct. Geometry Action: Transform Object: Finish the rectangular surface by creating verticals lines connecting the two previous horizontal lines. Extrude the surface. Curve Method: Translate Translation Vector: < > Curve List: Curve 1 Geometry Action: Create Object: Curve Method: Point Starting Point: Point 1 Ending Point: Point 3 Starting Point: Point 2 Ending Point: Point 4 Geometry Action: Create Object: Surface Method: Extrude Translation Vector <0 0-10> Curve list Curve 1:4 5-8 MSC.Nastran 104 Exercise Workbook

109 WORKSHOP 5 Typical Avionics Flow Use Iso 1 View Icon to obtain 3D view Create another surface and translate it to another surface Geometry Action: Create Object: Curve Method: XYZ Vector Coordinates List: <0 0-10> Origin Coordinates List: [ ] Geometry Action: Transform Object: Surface Method: Translate Translation Vector: <1 0 0> Repeat Count: 4 Select the Surface Icon Surface List: Surface MSC.Nastran 104 Exercise Workbook 5-9

110 Translate the final curve to complete the rectangular duct Geometry Action: Transform Object: Curve Method: Translate Translation Vector: <1 0 0> Repeat Count: 4 Select the Curve Icon Curve List: Curve 5 When you are finished your model should look like the one shown in the figure below. 4. Mesh Surfaces 1 to 16 to create QUAD4 elements with global edge length Finite Elements Action: Create 5-10 MSC.Nastran 104 Exercise Workbook

111 WORKSHOP 5 Typical Avionics Flow Object: Type: Global Edge Length 0.25 Mesh Surface Element Topology Quad 4 Surface List Surface 1:16 5. Similiarly, mesh Curves 5 to 9 with Bar2 element using a Global Edge Length of Action: Object: Type: Finite Elements Global Edge Length: 0.25 Element Topology: Bar2 Create Mesh Curve Curve List: Curve 5:9 Your model should appear like the one shown below. MSC.Nastran 104 Exercise Workbook 5-11

112 6. Equivalence the Finite Elements to reduce the number of elements by eliminating duplicate nodes. Action: Object: Type: Finite Elements Equivalence 7. Create the isotropic aluminum material properties using the material constants. All Equivalence Tolerance: Action: Object: Method: Materials Material Name: Input Properties... Constitutive Model: Tolerance Cube Create Isotropic Manual Input alum Thermal Conductivity: 4.0 Material Name: Input Properties... Constitutive Model: Thermal Conductivity: Solid properties air Fluid properties 6.66e-4 Specific Heat: Density: Dynamic Viscosity-: 5.01e e MSC.Nastran 104 Exercise Workbook

113 WORKSHOP 5 Typical Avionics Flow 8. Create the model s element properties assigning the material type and element thickness to the correct region of the model. Use the names of inner_wall, and outside_wall for the property names. The Thickness of the four side walls that separte fluid channels is 0.1 inch. The other walls have a thikckness of 0.05 inch. Action: Properties Dimension: Type: Property Set Name: Input Properties... Material Name: Select Front View Icon to choose walls Create 2D Shell outside_wall m:alum Thickness: 0.05 Select Members: Surface 1: :16 Add Property Set Name: Input Properties Material Name: Thickness: 0.1 inner_walls m:alum Select Members Surface 4:13:3 MSC.Nastran 104 Exercise Workbook 5-13

114 Add For the flow tube elements, the equivalent hydraulic diameter is D h = ( ) ( 2.4) = in \ Properties Action: Create Dimension: 1D Type: Flow Tube Property Set Name: air_flow Input Properties... Material Name: m:air Diameter at Node 1: Select Members: Curve 5:9 Add 9. a heat load on the top surface. Load/BCs Action: Create Object: Applied Heat Type: Element Uniform Options: Normal Flux New Set Name: flux Target Element Type: 2D Input Data... Surface Option: Top Top Surf Heat Flux: MSC.Nastran 104 Exercise Workbook

115 WORKSHOP 5 Typical Avionics Flow Select Application Region Geometry Filter: 10. Define the Inlet Temperature of the Fluid. Geometry Select Surfaces or Edges: Surface 2 6:15:3 Add Action: Object: Type: Load/BCs New Set Name: Input Data... Boundary Temperature: 20 Select Application Region Geometry Filter: Create Temp (Thermal) Nodal inlet_temp Geometry Select Geometry Entities Point 9 27:33:2 Add 11. Coupled Advection. Five load sets, one for each channel, are defined for the fluid-structure coupling. Load/BCs Action: Create MSC.Nastran 104 Exercise Workbook 5-15

116 Object: Type: Option: New Set Name: Target Element Type: Region 2: Input Data... Surface Option: Top Surf Heat Convection Coef: Mass Flow Rate: Select Application Region Geometry Filter: Convection Element Uniform Coupled Advection conv1 2D 1D Top e-3 Geometry Change the view to Front View Select Surfaces or Edges: Surface 1:4 Add Active list For the Companion Region Select Curves: Curve 5 Add 5-16 MSC.Nastran 104 Exercise Workbook

117 WORKSHOP 5 Typical Avionics Flow Do the same for the remaining four(4) channels. New Set Name: Select Application Region Geometry Filter: Active list conv2 Geometry Select Surfaces or edges: Surface 4:7 Add Active list For the Companion Region Select Curves: Curve 6 Add New Set Name Select Application Region Geometry Filter: Active list conv3 Geometry For the Companion Region Select Surfaces or edges: Surface 7:10 Add Active list For the Companion Region Select Curves: Curve 7 Add MSC.Nastran 104 Exercise Workbook 5-17

118 New Set Name Select Application Region Geometry Filter: Active list conv4 Geometry For the Companion Region Select Surfaces or edges: Surface 10:13 Add Active list For the Companion Region Select Curves: Curve 8 Add New Set Name Select Application Region Geometry Filter: Active list conv5 Geometry For the Companion Region Select Surfaces or edges: Surface 13:16 Add Active list For the Companion Region Select Curves: Curve 9 Add 5-18 MSC.Nastran 104 Exercise Workbook

119 WORKSHOP 5 Typical Avionics Flow 12. Analyze the model. Analysis Action: Object: Method: Job Name: Analyze Entire Model Analysis Deck ex5 An MSC.Nastran input file called ex5.bdf will be generated. This process of translating your model into an input file is called the Forward Translation. The Forward Translation is complete when the Heartbeat turns green. MSC.Nastran 104 Exercise Workbook 5-19

120 Submitting the Input File for Analysis: 13. Submit the input file to MSC.Nastran for analysis. 13a. To submit the MSC.Patran.bdf file, find an available UNIX shell window. At the command prompt enter nastran ex5.bdf scr=yes. Monitor the run using the UNIX ps command. 13b. To submit the MSC.Nastran.dat file, find an available UNIX shell window and at the command prompt enter nastran ex5 scr=yes. Monitor the run using the UNIX ps command. 14. When the run is completed, edit the ex5.f06 file and search for the word FATAL. If no matches exist, search for the word WARNING. Determine whether existing WARNING messages indicate modeling errors MSC.Nastran 104 Exercise Workbook

121 WORKSHOP 5 Typical Avionics Flow 15. MSC.Nastran Users have finished this exercise. MSC.Patran Users should proceed to the next step. 16. Proceed with the Reverse Translation process, that is, attaching the ex5.xdb results file into MSC.Patran. To do this, return to the Analysis form and proceed as follows: Analysis Action: Object: Method: Select Results File... Select Results File Attach XDB Result Entities Local ex5.xdb 17. Display the Results. Results Form Type: Select Results Cases Select Fringe Result Basic 1.1 Default, PW Linear: 100. % of Load 1.1 Temperatures Change to Iso 1 View MSC.Nastran 104 Exercise Workbook 5-21

122 The viewport may now be reset by clicking on the broom icon in the main window. File/Quit MSC.Nastran 104 Exercise Workbook

123 WORKSHOP 6 Radiation Enclosures Objective: Create Geometry from MSC.Patran Attain a temperature solution withing MSC.Nastran MSC.Nastran 104 Exercise Workbook 6-1

124 6-2 MSC.Nastran 104 Exercise Workbook

125 WORKSHOP 6 Radiation Enclosures Model Description: In this example we will model three plates that are in radiative equilibrium with a zero-degree ambient environment. Each plate measures 2 m by 3 m, and are arranged as shown in the figure below. The center plate (II) has a heat flux applied to it with a magnitude of 2000 W/m2 in the central region, as illustrated. The emissivity of all surfaces is chosen as 1.0, representing perfect blackbodies. The plate thicknesses are all m, and the material is aluminum. Temperature distribution for each plate will be determined. Aluminum Plate k = 204 W/m-oK ε = 1.0 I II III Cavity 1 Cavity 2 1 1/2 m 3 m Thickness = m Y X 1 m q=2000 W/m2 2 m Z 2 m 3 m MSC.Nastran 104 Exercise Workbook 6-3

126 6-4 MSC.Nastran 104 Exercise Workbook

127 WORKSHOP 6 Radiation Enclosures Suggested Exercise Steps: Create a new database called radiation_enclosures.db Create surfaces that represents three plates. Each plate is meshed with sixteen QUAD8 elements Input specify Material Properties for the plates. Define the element properties using alum as the property name. loads and boundary conditions to the model. Two radiation cavities are defined. Cavity 1 includes all the elements on Plates I and II that view each other. These elements also communicate with zero-degree space. The second cavity is comprised of the elements on Plates II and III, which see each other, and they also communicate with zero-degree space. The non-cavity sides of Plates I and III are treated as adiabatic surfaces (i.e., perfectly insulated The normal heat flux is applied to one side of the centermost four elements of Plate II, for a total heat load of 3000 W. Perform, read, and display the results. MSC.Nastran 104 Exercise Workbook 6-5

128 6-6 MSC.Nastran 104 Exercise Workbook

129 WORKSHOP 6 Radiation Enclosures Exercise Procedure: 1. Create a New Database called it radiation_enclosures.db File/New... New Database Name radiation_enclosures 2. Change the Tolerance to Default and the Analysis Code to MSC.Nastran in the New Model Preferences form. Verify that the Analysis Type is Thermal. New Model Preference Tolerance Analysis Code: Analysis Type Default MSC/NASTRAN Thermal 3. Create the surface representing a plate. Geometry Action: Create Object: Surface Method: XYZ Vector Coordinates List: <2 3 0> Origin Coordinates List: [ ] You will now use Transformation to create the other 2 surfaces parallel with the previous one. Geometry Action: Transform Object: Surface Method: Translate MSC.Nastran 104 Exercise Workbook 6-7

130 Translation Vector: <0 0 2> Surface List: Surface 1 Change the view to Iso 2 View Translation Vector: <0 0 3> Surface List: Surface 2 When you are finished your model should look like the one shown in the figure below. 4. Mesh the plate Finite Elements Action: Object: Type: Create Mesh Seed Uniform Number of Elements Number=: MSC.Nastran 104 Exercise Workbook

131 WORKSHOP 6 Radiation Enclosures Curve List: Surface Mesh the solids to create Quad8 element with global edge length 1.0. Action: Object: Type: Finite Elements Global Edge Length: 1 Element Topology: IsoMesh Create Mesh Quad8 Surface Surface List: Surface 1:3 6. Create the isotropic material properties using the material constants specify in figure. Materials MSC.Nastran 104 Exercise Workbook 6-9

132 Action: Object: Method: Material Name: Input Properties... Constitutive Model: alum Thermal Conductivity: 204 Create Isotropic Manual Input Solid properties 7. Create the model s element properties assigning the material type to the correct region of the model. Action: Properties Dimension: Type: Property Set Name: Input Properties... Material Name: alum Create 8. Define the radiation enclosures by defining two cavities for radiation exchange. This will save a lot of time attaining a temperature solution within MSC NASTRAN. Basically, to identify the TOP and BOTTOM surfaces appropriately, each independent 2D Shell m:alum Thickness: Select Members: Surface 1:3 Add 6-10 MSC.Nastran 104 Exercise Workbook

133 WORKSHOP 6 Radiation Enclosures surface within an enclosure will have a distinct SET NAME. Consistent use of the ENCLOSURE ID with each SET NAME ensures that the elements are included in the appropriate enclosure. Action: Object: Type: Options: Load/BCs New Set Name: Target Element Type: Input Data... Surface Option: Enclosure ID: 1 Create Radiation Element Uniform Enclosures enl_1 2D Top Top Surf Emissivity: 1.0 Surface Can Shade Surface Can Be Shaded Select Application Region Geometry Filter: Geometry Select Surfaces or Edges: Surface 1 Add New Set Name: Input Data... Surface Option: Enlosure ID: 1 Bottom Surf Emissivity: 1.0 encl_1a Bottom MSC.Nastran 104 Exercise Workbook 6-11

134 Select Application Region Geometry Filter: Geometry Select Surfaces or Edges: Surface 2 Add New Set Name: encl_2 Input Data... Surface Option: Top Enlosure ID: 2 Top Surf Emissivity: 1.0 Select Application Region Geometry Filter: Geometry Select Surfaces or Edges: Surface 2 Add New Set Name: encl_2a Input Data... Surface Option: Bottom Enlosure ID: 2 Bottom Surf Emissivity: 1.0 Select Application Region 6-12 MSC.Nastran 104 Exercise Workbook

135 WORKSHOP 6 Radiation Enclosures Geometry Filter: Geometry Select Surfaces or Edges: Surface 3 Add 9. a Heat Flux on the Top Surfaces of the chip. Load/BCs Action: Create Object: Applied Heat Type: Element Uniform Options: Normal Flux New Set Name: heat_flux Target Element Type: 2D Input Data... Surface Option: Top Top Surface Heat Flux 2000 Select Application Region Geometry Filter: FEM Select 2D Elements or Edges Elm Add MSC.Nastran 104 Exercise Workbook 6-13

136 10. Perform the analysis.since radiation heat transfer, by definition makes our problem highly nonlinear, we need to consider the Default Initial Temperature setting if we hope to achieve a converged solution with the MSC.Nastran thermal solver Action: Object: Method: Analysis Job Name: Solution Type... Solution Parameters... ex6 Default Init Temperature=: 500 Radiation Parameters... Stefan-Boltzmann Constant: Analyze Entire Model Analysis Deck e-8 An MSC.Nastran input file called ex6.bdf will be generated. This process of translating your model into an input file is called the Forward Translation. The Forward Translation is complete when the Heartbeat turns green MSC.Nastran 104 Exercise Workbook

137 WORKSHOP 6 Radiation Enclosures Submitting the Input File for Analysis: 11. Submit the input file to MSC.Nastran for analysis. 11a. To submit the MSC.Patran.bdf file, find an available UNIX shell window. At the command prompt enter nastran ex6.bdf scr=yes. Monitor the run using the UNIX ps command. 11b. To submit the MSC.Nastran.dat file, find an available UNIX shell window and at the command prompt enter nastran ex6 scr=yes. Monitor the run using the UNIX ps command. When the run is completed, edit the ex6.f06 file and search for the word FATAL. If no matches exist, search for the word WARNING. Determine whether existing WARNING messages indicate modeling errors. MSC.Nastran 104 Exercise Workbook 6-15

138 12. MSC.Nastran Users have finished this exercise. MSC.Patran Users should proceed to the next step. 13. Proceed with the Reverse Translation process, that is, attaching the ex6.xdb results file into MSC.Patran. To do this, return to the Analysis form and proceed as follows: Analysis Action: Object: Method: Select Results File... Select Results File Attach XDB Result Entities Local ex6.xdb 14. Display the Results. Object: Results Select Results Cases: Quick Plot Default, A1:Non-Linear: 100. % of Load Select Fringe Result: Temperatures 6-16 MSC.Nastran 104 Exercise Workbook

139 WORKSHOP 6 Radiation Enclosures Your Viewport will appear as follows. The viewport may now be reset by clicking on the broom icon in the main window. File/Quit... MSC.Nastran 104 Exercise Workbook 6-17

140 6-18 MSC.Nastran 104 Exercise Workbook

141 WORKSHOP 7 Axisymmetric Flow in a Pipe MSC.Nastran 104 Exercise Workbook 7-1

142 7-2 MSC.Nastran 104 Exercise Workbook

143 WORKSHOP 7 Axisymmetric Flow in a Pipe Model Description: In this example we will analyze an axisymmetric structure for its temperature distribution. We will use the MSC.NASTRAN CTRIAX6 axisymmetric element (in its 3 node configuration) as the heat conduction element. The basic geometry is detailed in the figure above. A section of pipe consisting of composite materials is divided into two different material regions. Region A is from radius 1.5 feet to 3.5 feet. Region B is from radius 3.5 feet to 4.75 feet. The overall pipe section is 5.0 feet long with an inside diameter of 3 feet and an outside diameter of 9.5 feet. Oil flows through the interior with an inlet temperature of 100 o F and a mass flow rate of 2.88E6 lb m /hr. The forced convection heat transfer coefficient between the oil and wall is calculated by MSC.NASTRAN using the following relationship: Nu = Re 0.8 Pr Thermal conductivity properties for Region A and Region B are 0.2 and 0.5 Btu/hr-ft- o F. Volumetric internal heat generation occurs in the subregion of Region B (Specifically from radius 3.5 feet to feet), and varies based on Z location. The heat generation is 1200 * (1-Z/5) Btu/hr-ft 3, where Z is given in units of feet. Free convection to an ambient temperature of 100 o F is applied to the exterior surface of the structure through a heat transfer coefficient of 3.0 Btu/hr-ft 2 - o F. Figure 7.1 Z Fluid Region A Region B q = q vol (z) = 1200 (1 - Z/5) Btu/hr-ft ft h = 3.0 Btu/hr-ft 2 - o F T amb = 100 o F T. in = 100 o F m = 2.88E6 lb m /hr µ oil = lb m /ft-hr 1.5 ft Oil Flow 3.5 ft ft 4.75 ft Nu = Re 0.8 Pr K oil = Btu/hr-ft- o F C p oil = 0.44 Btu/lb m - o F ρ oil = 56.8 lb m /ft 3 X K A = 0.2 Btu/hr-ft- o F K B = 0.5 Btu/hr-ft- o F MSC.Nastran 104 Exercise Workbook 7-3

144 7-4 MSC.Nastran 104 Exercise Workbook

145 WORKSHOP 7 Axisymmetric Flow in a Pipe Suggested Exercise Steps: Create a new database called ex7.db Using thermal analysis, create a geometry representing a pipe divided up into two region. Perform meshing on the Fluid Curve and Pipe Surfaces using one way bias mesh seed. Mesh the rest of the solid. Merge all coincident nodes using Equivalence action in patran. Define all material properties accordingly. Using 2D Axisym Solid to define the element s properties and 1D solid to represent the Flow Tube. MSC.Nastran 104 Exercise Workbook 7-5

146 7-6 MSC.Nastran 104 Exercise Workbook

147 WORKSHOP 7 Axisymmetric Flow in a Pipe Exercise Procedure: 1. Open a new database. Name it ex7.db File/New... New Database Name: ex7 The viewport (PATRAN s graphics window) will appear along with a New Model Preference form. The New Model Preference sets all the code specific forms and options inside MSC.PATRAN. In the New Model Preference form set the Analysis Code to MSC.Nastran Tolerance: Analysis Code: Analysis Type: Based on Model MSC/NASTRAN Thermal 2. Create the Geometry. Geometry Action: Create Object: Curve Method: XYZ Vector Coordinates List: <0 0 5> Origin Coordinates List: [0 0 0] Click on the Bottom View icon for working with axisymmetric geometries. Bottom View Geometry MSC.Nastran 104 Exercise Workbook 7-7

148 Action: Create Object: Surface Method: XYZ Surface ID List: 1 Vector Coordinates List: <2 0 5> Origin Coordinates List: [ ] Surface ID List: 2 Vector Coordinates List: < > Origin Coordinates List: [ ] Surface ID List: 3 Vector Coordinates List: < > Origin Coordinates List: [ ] Your model should look like the following figure. 7-8 MSC.Nastran 104 Exercise Workbook

149 WORKSHOP 7 Axisymmetric Flow in a Pipe 3. Mesh the Fluid Curve and Pipe Surfaces. Finite Elements Action: Create Object: Mesh Seed Type: One Way Bias Number: 10 L2/L1: 2.0 Curve List: Curve 1 Surface Finite Elements Action: Create Object: Mesh Type: Surface Global Edge Length: 0.25 Element Topology: Tria3 Surface List: Surface 1:3 Finite Elements Action: Create Object: Mesh Type: Curve Global Edge Length: 0.25 Element Topology: Bar2 Curve List: Curve 1 MSC.Nastran 104 Exercise Workbook 7-9

150 4. Remove Coincident Nodes. Finite Elements Action: Equivalence Object: All Type: Tolerance Cube Equivalencing Tolerance: Your model should look like the following figure. 5. Specify Material Properties. Materials Action: Create Object: Isotropic Method: Manual Input Material Name: mat_a Input Properties... Constitutive Model: Solid Properties Thermal Conductivity: MSC.Nastran 104 Exercise Workbook

151 WORKSHOP 7 Axisymmetric Flow in a Pipe Cancel Material Name: mat_b Input Properties... Constitutive Model: Solid Properties Thermal Conductivity: 0.5 Cancel Material Name: oil Input Properties... Constitutive Model: Fluid Properties Thermal Conductivity: Specific Heat: 0.44 Density: 56.8 Dynamic Viscosity: Cancel 6. Define Element Properties. Properties Action: Create Object: 2D Type: Axisym Solid Property Set Name: Input Properties... Material Name: pipe_a m:mat_a MSC.Nastran 104 Exercise Workbook 7-11

152 Select Members: Surface 1 Add Properties Action: Create Object: 2D Type: Axisym Solid Property Set Name: pipe_b Input Properties... Material Name: m:mat_b Select Members: Surface 2 3 Add Properties Action: Create Object: 1D Type: Flow Tube Property Set Name: oil Input Properties... Material Name: m:oil Hydraulic Diam. at Node: 3.0 Select Members: Curve 1 Add 7-12 MSC.Nastran 104 Exercise Workbook

153 WORKSHOP 7 Axisymmetric Flow in a Pipe 7. Define a Spatial Field. Fields Action: Create Object: Spatial Method: PCL Function Field Name: Scalar Function: qvol_z 1200*(1.0- Z/5.0) 8. a Volumetric Heat Load. Load/BCs Action: Create Object: Applied Heat Type: Element Uniform Option: Volumetric Generation New Set Name: qvol Target Element Type: 2D Input Data... Volumetric Heat Generation: f:qvol_z Select Application Region... Geometry Filter: Geometry Select Surfaces: Surface 2 Add MSC.Nastran 104 Exercise Workbook 7-13

154 Your model should look like the following figure. 9. Free Convection. Load/BCs Action: Create Object: Convection Type: Element Uniform Option: To Ambient New Set Name: conv Target Element Type: 2D Input Data... Surface Option: edge Edge Convection Coef: 3.0 Ambient Temperature: 100 Select Application Region... Geometry Filter: Geometry 7-14 MSC.Nastran 104 Exercise Workbook

155 WORKSHOP 7 Axisymmetric Flow in a Pipe Click on the Edge View icon. Edge Select Surfaces: Surface 3.2 Add 10. Define Inlet Temperatures of the Fluid. Load/BCs Action: Create Object: Temp (Thermal) Type: Nodal New Set Name: Input Data... Boundary Temperature: 100 Select Application Region... Geometry Filter: 11. Define Coupled Flow Tube. inlet_temp Geometry Select Geometry Entities: Point 1 Add a fluid-structure coupling between the oil and inner wall of the pipe. Load/BCs Action: Create MSC.Nastran 104 Exercise Workbook 7-15

156 Object: Convection Type: Element Uniform Option: Coupled Flow Tube New Set Name: coup_ftube Target Element Type: 1D Region 2: 2D Input Data... Form Type: Advanced Mass Flow Rate: 2.88e6 Heat Transfer Coefficient: Formula Type Option: h=k/d*coef*re**expr*pr** Reynolds Exponent: 0.8 Prandtl Exponent, Heat In: Select Application Region... Geometry Filter: Geometry Select Curves: Curve 1 Add Active List Select Surfaces or Edges: Surface 1.4 Click on the Edge View icon. Edge Add 7-16 MSC.Nastran 104 Exercise Workbook

157 WORKSHOP 7 Axisymmetric Flow in a Pipe Your model should look like the following figure. 12. Perform the Analysis. Analysis Action: Analyze Object: Entire Model Method: Analysis Deck Job Name: ex7 An MSC.Nastran input file called ex7.bdf will be generated. This process of translating your model into an input file is called the Forward Translation. The Forward Translation is complete when the Heartbeat turns green. MSC.Nastran 104 Exercise Workbook 7-17

158 7-18 MSC.Nastran 104 Exercise Workbook

159 WORKSHOP 7 Axisymmetric Flow in a Pipe Submitting the Input File for Analysis: 13. Submit the input file to MSC.NASTRAN for analysis. 13a. To submit the MSC.Patran.bdf file, find an available UNIX shell window. At the command prompt enter nastran ex7.bdf scr=yes. Monitor the run using the UNIX ps command. 13b. To submit the MSC.Nastran.dat file, find an available UNIX shell window and at the command prompt enter nastran ex7 scr=yes. Monitor the run using the UNIX ps command. 14. When the run is completed, edit the ex7.f06 file and search for the word FATAL. If no matches exist, search for the word WARNING. Determine whether existing WARNING messages indicate modeling errors. MSC.Nastran 104 Exercise Workbook 7-19

160 15. MSC.Nastran Users have finished this exercise. MSC.Patran Users should proceed to the next step. 16. Proceed with the Reverse Translation process, that is, attaching the ex7.xdb results file into MSC.Patran. To do this, return to the Analysis form and proceed as follows: Analysis Action: Object: Method: Select Results File... Select Results File Attach XDB Result Entities Local ex7.xdb 17. Display the Results. Results Select Results Cases: Select Fringe Result: Default, PW Linear: 100. % of Load Temperatures 7-20 MSC.Nastran 104 Exercise Workbook

161 WORKSHOP 7 Axisymmetric Flow in a Pipe Your model should look like the following figure. The maximum temperature occurs near the internal heat generation region with a temperature of o F. The fluid temperature remains constant at 100 o F because of the massive flow rate at 2.88E6 lb m /hr. We can check the energy balance on this model as follows: Total heat = E4 Btu/hr (from the OLOAD RESULTANT of the F06 file) Sum of the heat on the column under Free Convection = E4 Btu/hr Sum of the heat on the column under Forced Convection = 3.297E3 Btu/hr Sum of the heat on the above two columns = E4 Btu/hr, which is equal to the input heat of E4 Btu/hr. An assumption of a 1-D fluid element is that temperature gradients within the fluid are only significant along the axial direction. With such a large diameter flow tube, this assumption is probably being misused in this particular problem. The application of the flow tube boundary convection relationship also implies fully developed flow, yet, over only a 5 foot section and with a 3 foot diameter, this is also a very crude approximation. In essence, what we are saying, is that this example serves to illustrate coupled convection in an axisymmetric environment, application of spatial heat loads, and use of convection correlation equations, rather than fluid physics. MSC.Nastran 104 Exercise Workbook 7-21

162 Quit MSC.Patran when you have completed this exercise MSC.Nastran 104 Exercise Workbook

163 WORKSHOP 8 Directional Heat Loads MSC.Nastran 104 Exercise Workbook 8-1

164 8-2 MSC.Nastran 104 Exercise Workbook

165 WORKSHOP 8 Directional Heat Loads Model Description: Figure 8.1 In this example we will apply a directional heat load on cylinder. We will orient the surface normal from the surface such that the normal vector (Right hand rule) will point away from the surface. This allows the incoming directional heat flux to see the normals, and project the correct energy by forming a dot product with this vector. A typical application of this directional heat load process is in an orbital heating environment. The dimension of the cylinder is 1.5 inch in diameter with a length of 6 inches. The material is aluminum with a thermal conductivity of 3.96 W/in- o C. The absorptivity and emissivity of the cylinder surface are 0.8. The directional heat load is 30 W/in 2. The exterior surface of the cylinder looses heat by radiation to space. The radiation view factor is 1.0 and the ambient temperature is 20 o C. 6.0 in 1.5 in q = q vec = 30 Radiation Boundary Condition View Factor = 1.0 T amb = 20.0 o C Y Aluminum Cylinder k = 3.96 W/in- o C α = ε = 0.8 Z X Thickness = in MSC.Nastran 104 Exercise Workbook 8-3

166 8-4 MSC.Nastran 104 Exercise Workbook

167 WORKSHOP 8 Directional Heat Loads Suggested Exercise Steps: Create a new database called Create the Surfaces of Printed Circuit Board and Electric Components. Extrude the Surfaces to Create Solids. Mesh the Solids. Specify Materials. Define Element Properties. Merge the Common Nodes. Verify the Free Edges. a heat load on each device. a convection boundary condition on the PCB. Perform the Analysis. Read the analysis results. Display the results. MSC.Nastran 104 Exercise Workbook 8-5

168 8-6 MSC.Nastran 104 Exercise Workbook

169 WORKSHOP 8 Directional Heat Loads Exercise Procedure: 1. Open a new database. Name it ex8.db File/New... New Database Name: ex8 The viewport (PATRAN s graphics window) will appear along with a New Model Preference form. The New Model Preference sets all the code specific forms and options inside MSC.PATRAN. In the New Model Preference form set the Analysis Code to MSC.Nastran Tolerance: Analysis Code: Analysis Type: Based on Model MSC/NASTRAN Thermal 2. Create the geometry. Geometry Action: Create Object: Point Method: XYZ Point ID List: 1 Refer. Coordinate Frame: Coord 0 Point Coordinates List: [ ] Geometry Action: Create Object: Curve Method: Revolve MSC.Nastran 104 Exercise Workbook 8-7

170 Curve ID List: 1 Total Angle: Auto Execute Point List: Point 1 Geometry Action: Create Object: Surface Method: Extrude Translation Vector: <0 0-6> Curve List: Curve 1 Click on the Iso 1 View icon to obtain a 3D view of the cylinder. Iso 1 View Your model should look like the following figure. 8-8 MSC.Nastran 104 Exercise Workbook

171 WORKSHOP 8 Directional Heat Loads The surface normal direction is important in this problem, because the incoming heat flux vector will form a dot product with the normal vector for the surface generating the correct projected surface area for application of the heat load. Therefore, when we created the cylinder using geometry, we should verify that the normal vector points outward. This is accomplished by using: Geometry Action: Show Object: Surface Method: Normal Auto Execute Surface List: Surface 1 Click on the Front View icon. Front View Select Surface 1 to make sure that the normal vector indicated by the red arrow points outward from the cylinder. If the normal vector is pointing inward, then you can reverse the surface normal by using the following command: Geometry Action: Edit Object: Surface Method: Reverse Auto Execute Surface List: Surface 1 MSC.Nastran 104 Exercise Workbook 8-9

172 3. Create Finite Elements. Finite Elements Action: Create Object: Mesh Type: Surface Global Edge Length: 0.1 Element Topology: Quad4 Surface List: Surface 1 Click on the Iso 1 View icon. Iso 1 View 4. Remove Coincident Nodes. Finite Elements Action: Equivalence Object: All Type: Tolerance Cube Equivalencing Tolerance: MSC.Nastran 104 Exercise Workbook

173 WORKSHOP 8 Directional Heat Loads Your model should look like the following figure. 5. Specify Material Properties. Materials Action: Create Object: Isotropic Method: Manual Input Material Name: alum Input Properties... Constitutive Model: Solid properties Thermal Conductivity: 3.96 Cancel 6. Define Element Properties. Properties Action: Create Object: 2D MSC.Nastran 104 Exercise Workbook 8-11

174 Type: Shell Property Set Name: Input Properties... Material Name: 7. a Directional Heat Load. alum m:alum Thickness: Select Members: Surface 1 Add Load/BCs Action: Create Object: Applied Heat Option: Directional Fluxes Type: Element Uniform New Set Name: Target Element Type: Input Data... vector_flux 2D Surface Option: Top Top Surf Absorptivity: 0.8 Top Surf Heat Flux: 30 Incident Thermal Vector: <-1 0 0> Select Application Region... Geometry Filter: Geometry Select Surface or Edges: Surface 1 Add 8-12 MSC.Nastran 104 Exercise Workbook

175 WORKSHOP 8 Directional Heat Loads 8. a Radiation Boundary Condition. Load/BCs Action: Create Object: Radiation Type: Element Uniform Option: Ambient Space New Set Name: Target Element Type: Input Data... rad_space 2D Surface Option: Top Top Surf Emissivity: 0.8 Top Surf Absorptivity: 0.8 Ambient Temperature: 20 View Factor: 1.0 Select Application Region... Geometry Filter: Geometry Select Surface or Edges: Surface 1 Add MSC.Nastran 104 Exercise Workbook 8-13

176 Your model should look like the following figure. 9. Specify Radiation Parameters and Perform the Analysis. Analysis Action: Analyze Object: Entire Model Method: Analysis Deck Job Name: ex8 Solution Type... STEADY STATE ANALYSIS Solution Parameters... Radiation Parameters... Absolute Temperature Scale: Degree Celsius Stefan-Boltzmann Constant: e-11 WATTS/IN2/K MSC.Nastran 104 Exercise Workbook

177 WORKSHOP 8 Directional Heat Loads An MSC.Nastran input file called ex8.bdf will be generated. This process of translating your model into an input file is called the Forward Translation. The Forward Translation is complete when the Heartbeat turns green. MSC.Nastran 104 Exercise Workbook 8-15

178 Submitting the Input File for Analysis: 10. Submit the input file to MSC.Nastran for analysis. 10a. To submit the MSC.Patran.bdf file, find an available UNIX shell window. At the command prompt enter nastran ex8.bdf scr=yes. Monitor the run using the UNIX ps command. 10b. To submit the MSC.Nastran.dat file, find an available UNIX shell window and at the command prompt enter nastran ex8 scr=yes. Monitor the run using the UNIX ps command. 11. When the run is completed, edit the ex8.f06 file and search for the word FATAL. If no matches exist, search for the word WARNING. Determine whether existing WARNING messages indicate modeling errors MSC.Nastran 104 Exercise Workbook

179 WORKSHOP 8 Directional Heat Loads 12. MSC.Nastran Users have finished this exercise. MSC.Patran Users should proceed to the next step. 13. Proceed with the Reverse Translation process, that is, attaching the ex8.xdb results file into MSC.Patran. To do this, return to the Analysis form and proceed as follows: Analysis Action: Object: Method: Select Results File Select Results File Attach XDB Result Entities Local ex8.xdb 14. Display the Results. Results Select Results Cases: Select Fringe Result: Default, PW Linear: 100. % of Load Temperatures MSC.Nastran 104 Exercise Workbook 8-17

180 Your model should look like the following figure. Example 8 demonstrates an aluminum cylinder in radiative equilibrium. The heat source is directional (light source oriented), and the radiation boundary condition is equal for all directions. The cylinder s maximum temperature (~473 o C) is attained on the side subject to the solar heat load. The minimum temperature (~424 o C) occurs in the shadow region. The high conductivity of the cylinder helps to equilibrate the temperatures. If the conductivity were very low, the maximum temperature would approach 740 o C with the minimum approximately 20 o C. Quit MSC.Patran when you have completed this exercise MSC.Nastran 104 Exercise Workbook

181 WORKSHOP 9 Thermal Stress Analysis from Directional Heat Loads MSC.Nastran 104 Exercise Workbook 9-1

182 9-2 MSC.Nastran 104 Exercise Workbook

183 WORKSHOP 9 Thermal Stress Analysis from Directional Heat Loads Model Description: This example demonstrates how to apply the thermal results of Example 8 to perform a stress analysis. We will create the temperature loading for the stress run by using the Create-Spatial- FEM command under the Fields Application. You can also use the include punch file option to get the thermal load. The diameter of the cylinder is 1.5 inch with a length of 6 inches. The material is aluminum. The heat transfer problem solved in Example 8 resulted in a temperature solution which we would now like to apply to a thermal stress analysis. Figure in Y 1.5 in Aluminum Cylinder E = 1.0E7 lb/in 2 ν = 0.34 α = 1.3E-5 in/in- o C Thickness = in Z X MSC.Nastran 104 Exercise Workbook 9-3

184 9-4 MSC.Nastran 104 Exercise Workbook

185 WORKSHOP 9 Thermal Stress Analysis from Directional Heat Loads Suggested Exercise Steps: Create a new database called ex9. Create Spacial FEM based on the Temperature Profile. Specify the material properties after changing the Analysis Type to Structural. Define element properties using 2D shell. Create new load case and applyed fixed boundary conditions on the end of the cylinder. boundary conditions to the structural load case and define temperature load to the model. Analyze the model Read and display the results. MSC.Nastran 104 Exercise Workbook 9-5

186 9-6 MSC.Nastran 104 Exercise Workbook

187 WORKSHOP 9 Thermal Stress Analysis from Directional Heat Loads Exercise Procedure: 1. Open the database ex8.db from the previous exercise. File/Open... Existing Database Name: ex8 2. Create a Spatial FEM based on the Temperature Profile. Fields Action: Create Object: Spatial Method: FEM Field Name: tempload FEM Field Definition: Continuous Field Type: Scalar Mesh/Results Group Filter: Current Viewport Select Group: default_group 3. Change the Analysis Type to Structual. Preferences/Analysis... Analysis Type: Structural 4. Specify the Structural Materials. Materials Action: Create Object: Isotropic Method: Manual Input MSC.Nastran 104 Exercise Workbook 9-7

188 Material Name: Input Properties Assign Element Properties. When asked, Surface 1 already has been associated to an element property region. Overwrite the association?, answer Yes. 6. Create a New Load Case. alum_st Constitutive Model: Linear Elastic Elastic Modulus: 1.0e7 Poisson Ratio: 0.34 Thermal Expan. Coeff: Reference Temperature: 0.0 Cancel Properties 1.3e-5 Action: Create Object: 2D Type: Shell Property Set Name: Input Properties... Material Name: alum_st m:alum_st Thickness: Select Members: Surface 1 Add Yes 9-8 MSC.Nastran 104 Exercise Workbook

189 WORKSHOP 9 Thermal Stress Analysis from Directional Heat Loads We will create a new load case consisting of the structural thermal loading and apply the fixed boundary conditions on the ends of the cylinder. Load Cases Action: Create Load Case Name: 7. the Clamped Boundary Conditions. Click on the Curve or Edge icon. struct_load Load Case Type: Static Load/BCs Action: Create Object: Displacement Type: Nodal Analysis Type: Structural Current Load Case: New Set Name: Input Data... Load/BC Set Scale Factor: 1.0 struct_load clamp_bc Translations <T1 T2 T3> < 0., 0., 0.> Rotations <R1 R2 R3> < 0., 0., 0.> Select Application Region... Geometry Filter: Curve or Edge Geometry Select Geometry Entities: Curve 1 Surface 1.3 MSC.Nastran 104 Exercise Workbook 9-9

190 Add 8. Define a Temperature Load. Load/BCs Action: Create Object: Temperature Type: Nodal Analysis Type: Structural Current Load Case: struct_load New Set Name: temp_load Input Data... Load/BC Set Scale Factor: 1.0 Temperature: f:tempload Select Application Region... Geometry Filter: Geometry Click on the Surface or Face icon. Surface or Face Select Geometry Entities: Surface 1 Add 9-10 MSC.Nastran 104 Exercise Workbook

191 WORKSHOP 9 Thermal Stress Analysis from Directional Heat Loads Your model should look like the following figure. 9. Perform the Analysis. Analysis Action: Analyze Object: Entire Model Method: Analysis Deck Job Name: Subcase Select... Subcases For Solution Sequence:101 Subcases Selected: ex9 struct_load Default An MSC.Nastran input file called ex9.bdf will be generated. This process of translating your model into an input file is called the Forward Translation. The Forward Translation is complete when the Heartbeat turns green. MSC.Nastran 104 Exercise Workbook 9-11

192 Submitting the Input File for Analysis: 10. Submit the input file to MSC.Nastran for analysis. 10a. To submit the MSC.Patran.bdf file, find an available UNIX shell window. At the command prompt enter nastran ex9.bdf scr=yes. Monitor the run using the UNIX ps command. 10b. To submit the MSC.Nastran.dat file, find an available UNIX shell window and at the command prompt enter nastran ex9 scr=yes. Monitor the run using the UNIX ps command. 11. When the run is completed, edit the ex9.f06 file and search for the word FATAL. If no matches exist, search for the word WARNING. Determine whether existing WARNING messages indicate modeling errors MSC.Nastran 104 Exercise Workbook

193 WORKSHOP 9 Thermal Stress Analysis from Directional Heat Loads 12. MSC.Nastran Users have finished this exercise. MSC.Patran Users should proceed to the next step. 13. Proceed with the Reverse Translation process, that is, attaching the ex9.xdb results file into MSC.Patran. To do this, return to the Analysis form and proceed as follows: Analysis Action: Object: Method: Select Results File Select Results File Attach XDB Result Entities Local ex9.xdb 14. Display the Results. Results Select Results Cases: struct_load, Static Subcase Select Fringe Result: Stress Tensor Result Position: At Z1 Result Quantity: von Mises Select Deformation Displacements, Translational Result: MSC.Nastran 104 Exercise Workbook 9-13

194 Your model should look like the following figure. For output we plot the von Mises stress for the fixed end cylinder undergoing the directional thermal load. Peak stresses occur near the fixed end points (recall the points are fixed in X, Y, and Z directions). Thermal expansion causes growth in the axial and radial directions with a circumferential variation due to the directional nature of the thermal load. Near the cylinder mid-plane, in an axial sense, we find the maximum stress at the location which is normal to the directional load vector. The minimum is on the opposite side of the cylinder in the shadow. Quit MSC.Patran when you have completed this exercise 9-14 MSC.Nastran 104 Exercise Workbook

195 WORKSHOP 10 Thermal Stress Analysis of a Bi- Metallic Plate MSC.Nastran 104 Exercise Workbook 10-1

196 10-2 MSC.Nastran 104 Exercise Workbook

197 WORKSHOP 10 Thermal Stress Analysis of a Bi-Metallic Plate Model Description: Figure 10.1 In this example we will perform the thermal stress analysis of a bimetallic strip. We will build the entire model from geometric construction so that we can apply loads directly on the geometry. The dimension of the bi-metallic strip is one inch by one inch. The thickness for the solder type material is 0.05 inch, and the thickness of the Ge material is inch. Thus the assembly thickness is inch. The top surface temperature boundary condition is -30 o C, and the bottom surface temperature boundary condition is 70 o C. We will determine the temperature distribution by running a steady-state thermal analysis. Y 1.0 in K Ge = W/in- o C K solder = 1.27 W/in- o C 1.0 in Z Ge: in T = o C X E Ge = 1.885E7 lb/in 2 G Ge = 0.933E7 lb/in 2 α Ge = 5.8E-6 in/in- o C E Solder = 1.3E7 lb/in 2 ν Solder = 0.4 α Solder = 2.47E-5 in/in- o C Solder: 0.05 in X T ref = -30 o C T = 70.0 o C Prior to the development of the MSC.Patran MSC.Nastran Heat Transfer interface, one would request: TEMP(PUNCH)=all in the MSC.Nastran Case Control section of the thermal run. The temperature load is then created and saved inside the punch file. In the subsequent thermal stress analysis one can access this file by defining TEMP(LOAD)=1 in the Case Control section of the ensuing stress analysis run. MSC.Nastran 104 Exercise Workbook 10-3

198 However, using MSC.Patran you can use the Create-Spatial-FEM command after you have postprocessed the thermal result in the viewport. We will use this technique to apply a thermal load for the stress analysis. Also, we will analyze the thermal stress analysis for the free-free expansion by enforcing a minimum number of constraints to fix-rigid body motion MSC.Nastran 104 Exercise Workbook

199 WORKSHOP 10 Thermal Stress Analysis of a Bi-Metallic Plate Suggested Exercise Steps: Create a new database called ex10.db Create a geometry representing a bi-metallic strip. Mesh the solid using Uniform Mesh Seed for solid 1 and Mesh using HEX8 for both solids. Merge all coincident nodes using Equivalence action in the Finite Elements menu Specify thermal material properties. Define properties using 3D solid for each individual parts. temperature boundary conditions to the solid. Analyze, perform, and read the results. Define a spatial FEM Field based on the temperature Profile. Define the new material properties using structural analysis. different loads and boundary conditions for the solid Perform the structural analysis and read the results. MSC.Nastran 104 Exercise Workbook 10-5

200 10-6 MSC.Nastran 104 Exercise Workbook

201 WORKSHOP 10 Thermal Stress Analysis of a Bi-Metallic Plate Exercise Procedure: 1. Open a new database. Name it ex10.db File/New... New Database Name: ex10 The viewport (PATRAN s graphics window) will appear along with a New Model Preference form. The New Model Preference sets all the code specific forms and options inside MSC.PATRAN. In the New Model Preference form set the Analysis Code to MSC.Nastran Tolerance: Analysis Code: Analysis Type: Based on Model MSC/NASTRAN Thermal 2. Create the Model. Geometry Action: Create Object: Surface Method: XYZ Vector Coordinates List: <1 1 0> Origin Coordinates List: [0 0 0] Geometry Action: Create Object: Solid Method: Extrude Translation Vector: < > MSC.Nastran 104 Exercise Workbook 10-7

202 Auto Execute Surface List: Surface 1 Click on the Solid Face icon. Solid Face Translation Vector: < > Surface List: Solid 1.6 Your model should look like the following figure. 3. Mesh the Solids. Finite Elements Action: Create Object: Mesh Seed Type: Uniform 10-8 MSC.Nastran 104 Exercise Workbook

203 WORKSHOP 10 Thermal Stress Analysis of a Bi-Metallic Plate Number: 4 Click on the four corners of Solid 1. Hold shift key down while you click. Curve List: Solid Number: 2 Click on the four corners of Solid 2. Hold shift key down while you click. Curve List: Solid Finite Elements Action: Create Object: Mesh Type: Solid Global Edge Length: 0.1 Element Topology: Hex8 Solid List: Solid Remove Coincident Nodes. Finite Elements Action: Equivalence Object: All Type: Tolerance Cube Equivalencing Tolerance: MSC.Nastran 104 Exercise Workbook 10-9

204 Your model should look like the following figure. 5. Specify Thermal Material Properties. Materials Action: Create Object: Isotropic Method: Manual Input Material Name: Ge Input Properties... Constitutive Model: Solid properties Thermal Conductivity: Cancel Material Name: Solder Input Properties... Constitutive Model: Solid properties Thermal Conductivity: MSC.Nastran 104 Exercise Workbook

205 WORKSHOP 10 Thermal Stress Analysis of a Bi-Metallic Plate Cancel 6. Define Element Properties. Properties Action: Create Object: 3D Type: Solid Property Set Name: Ge Input Properties... Material Name: m:ge Click on the Bottom View icon. Bottom View Select Members: Solid 2 Add Property Set Name: Solder Input Properties... Material Name: m:solder Select Members: Solid 1 Add 7. temperature boundary conditions. Load/BCs Action: Create MSC.Nastran 104 Exercise Workbook 10-11

206 Object: Temp(Thermal) Type: Nodal Analysis Type: Thermal New Set Name: temp_bottom Input Data... Boundary Temperature: 70 Select Application Region... Geometry Filter: Geometry Click on the Surface or Face icon. Surface or Face Select Geometry Entities: Surface 1 Add New Set Name: temp_top Input Data... Boundary Temperature: -30 Select Application Region... Geometry Filter: Geometry Select Geometry Entities: Solid 2.6 Add MSC.Nastran 104 Exercise Workbook

207 WORKSHOP 10 Thermal Stress Analysis of a Bi-Metallic Plate Your model should look like the following figure. 8. Perform the Thermal Analysis. Analysis Action: Analyze Object: Entire Model Method: Analysis Deck Job Name: ex10 An MSC.Nastran input file called ex10.bdf will be generated. This process of translating your model into an input file is called the Forward Translation. The Forward Translation is complete when the Heartbeat turns green. MSC.Nastran 104 Exercise Workbook 10-13

208 Submitting the Input File for Analysis: 9. Submit the input file to MSC.Nastran for analysis. 9a. To submit the MSC.Patran.bdf file, find an available UNIX shell window. At the command prompt enter nastran ex10.bdf scr=yes. Monitor the run using the UNIX ps command. 9b. To submit the MSC.Nastran.dat file, find an available UNIX shell window and at the command prompt enter nastran ex10 scr=yes. Monitor the run using the UNIX ps command. 10. When the run is completed, edit the ex10.f06 file and search for the word FATAL. If no matches exist, search for the word WARNING. Determine whether existing WARNING messages indicate modeling errors MSC.Nastran 104 Exercise Workbook

209 WORKSHOP 10 Thermal Stress Analysis of a Bi-Metallic Plate 11. MSC.Nastran Users have finished this exercise. MSC.Patran Users should proceed to the next step. 12. Proceed with the Reverse Translation process, that is, attaching the ex10.xdb results file into MSC.Patran. To do this, return to the Analysis form and proceed as follows: Analysis Action: Object: Method: Select Results File Select Results File Attach XDB Result Entities Local ex10.xdb 13. Display the Results. Results Form Type: Select Results Cases: Default, PW Linear: 100. % of Load Temperatures Click on the Iso 1 View icon to change the view. Iso 1 View MSC.Nastran 104 Exercise Workbook 10-15

210 Your model should look like the following figure. 14. Define a Spatial FEM Field based on the Temperature Profile. Fields Action: Create Object: Spatial Method: FEM Field Name: t_load FEM Field Definition: Continuous Field Type: Scalar Mesh/Results Group Filter: Current Viewport Select Group: default_group 15. Change the Analysis type to Structural. Preferences/Analysis... Analysis Type: Structural MSC.Nastran 104 Exercise Workbook

211 WORKSHOP 10 Thermal Stress Analysis of a Bi-Metallic Plate 16. Specify Structural Material Properties. Materials Action: Create Object: Isotropic Method: Manual Input Material Name: Solder_st Input Properties... Constitutive Model: Linear Elastic Elastic Modulus: 1.3e7 Poisson Ratio: 0.4 Thermal Expan. Coeff: 2.47e-5 Reference Temperature: Cancel Material Name: Ge_st Input Properties... Constitutive Model: Linear Elastic Elastic Modulus: 1.885e7 Shear Modulus: 0.933e7 Thermal Expan. Coeff: 5.8e-6 Reference Temperature: Cancel 17. Assign Element Properties. Properties Action: Create Object: 3D MSC.Nastran 104 Exercise Workbook 10-17

212 Type: Solid Property Set Name: Ge_st Options: Standard Formulation Input Properties... Material Name: m:ge_st Select Members: Solid 2 Add When asked, Solid 2 already has been associated to an element property region. Overwrite the association?, answer Yes. Yes Property Set Name: When asked, Solid 1 already has been associated to an element property region. Overwrite the association?, answer Yes. 18. Create a New Load Case. Solder_st Options: Standard Formulation Input Properties... Material Name: m:solder_st Select Members: Solid 1 Add Yes Load Cases Action: Create MSC.Nastran 104 Exercise Workbook

213 WORKSHOP 10 Thermal Stress Analysis of a Bi-Metallic Plate Load Case Name: Load Case Type: struct_load Static 19. Define a Temperature Load. Load/BCs Action: Create Object: Temperature Type: Nodal Analysis Type: Structural Current Load Case: struct_load New Set Name: temp_load Input Data... Load/BC Set Scale Factor: 1.0 Temperature: f:t_load Select Application Region... Geometry Filter: Geometry Click on the Solid icon. Solid Select Geometry Entities: Solid 1 2 Add 20. constraints on the four corner points of the top surface. Load/BCs MSC.Nastran 104 Exercise Workbook 10-19

214 Action: Create Object: Displacement Type: Nodal Analysis Type: Structural New Set Name: fix_x Input Data... Load/BC Set Scale Factor: 1.0 Translations <T1 T2 T3> <0.,, > Select Application Region... Geometry Filter: Geometry Click on the Point icon. Point Select Geometry Entities: Point 9 10 Add New Set Name: fix_y Input Data... Load/BC Set Scale Factor: 1.0 Translations <T1 T2 T3> <, 0., > Select Application Region... Geometry Filter: Geometry Select Geometry Entities: Point 11 Add MSC.Nastran 104 Exercise Workbook

215 WORKSHOP 10 Thermal Stress Analysis of a Bi-Metallic Plate New Set Name: fix_z Input Data... Load/BC Set Scale Factor: 1.0 Translations <T1 T2 T3> <,, 0.> Select Application Region... Geometry Filter: Geometry Select Geometry Entities: Point 9:12 Add Your model should look like the following figure. MSC.Nastran 104 Exercise Workbook 10-21

216 21. Perform the Structural Analysis. Analysis Action: Analyze Object: Entire Model Method: Analysis Deck Job Name: ex10_st Subcase Select... Subcases For Solution Sequence:101 Subcases Selected: struct_load default MSC.Nastran 104 Exercise Workbook

217 WORKSHOP 10 Thermal Stress Analysis of a Bi-Metallic Plate Submitting the Input File for Analysis: 22. Submit the input file to MSC.NASTRAN for analysis. To submit the MSC.PATRAN.bdf file for analysis, find an available UNIX shell window. At the command prompt enter: nastran ex10_st.bdf scr=yes. Monitor the run using the UNIX ps command. 23. When the run is completed, edit the ex10_st.f06 file and search for the word FATAL. If no matches exist, search for the word WARNING. Determine whether existing WARNING messages indicate modeling errors. 24. Read in the Analysis Results. Analysis Action: Read Output2 Object: Result Entities Method: Translate Job Name: Select Results File... ex10_st.op2 25. Display the Results. Results Select Results Cases: Select Fringe Result: ex10_st Result Quantity: von Mises Select Deformation Displacements, Translational Result: struct_load, Static Subcase Stress Tensor MSC.Nastran 104 Exercise Workbook 10-23

218 Your model should look like the following figure. The reference or zero stress state for the assembly is initialized at - 30 o C. The thermal coefficient of expansion for the solder is approximately four times that of Ge. When the temperature gradient associated with the temperature boundary conditions is applied, the solder layer wants to grow significantly more than the Ge layer due not only to the higher coefficient of thermal expansion, but also because of the higher temperature relative to TREF. The Ge layer ends up with a more complex stress pattern due to its four corner points being constrained, the distribution of temperature through the layer, and the growth enforced by the solder layer. The free surface of the solder layer exhibits the low stress levels. Quit MSC.Patran when you have completed this exercise MSC.Nastran 104 Exercise Workbook

219 APPENDIX A Transient Thermal Analysis of a Cooling fin Objectives: Create a new database. Create the surface. Assign the thermal loads Submit the model for analysis MSC.Nastran 104 Exercise Workbook A-1

220 A-2 MSC.Nastran 104 Exercise Workbook

221 APPENDIX A Transient Thermal Analysis of a Cooling Fin Suggested Exercise Steps: Create a new database and name it fin.db. Create a surface model of the cooling fin Generate the finite elements using mesh seeds Define material and element properties. the convection conditions to the model. Submit the model to MSC.Nastran for analysis. Review results. MSC.Nastran 104 Exercise Workbook A-3

222 A-4 MSC.Nastran 104 Exercise Workbook

223 APPENDIX A Transient Thermal Analysis of a Cooling Fin Exercise Procedure: 1. Open a new database called fin.db. File/New... New Database Name fin In the New Model Preferences form set the following: New Model Preference Tolerance Analysis Code: Analysis Type: Default MSC/NASTRAN Thermal Whenever possible click Auto Execute (turn off). 2. Create the surfaces of the cooling fin Geometry Action: Create Object: Surface Method: XYZ Reference Coordinate Frame Coord 0 Vector Coordinates List [0.5, 2, 0] Origin Coordinates List [0, 0, 0] Repeat the previous step to create the remaining surface. Vector Coordinates List [0.5, , 0] Origin Coordinates List [0.5, , 0] MSC.Nastran 104 Exercise Workbook A-5

224 3. Generate the mesh seed for the surfaces created: Action: Object: Method: Finite Element Element Edge Length Data Number = 9 Create Mesh Seed Uniform Number of Elements Curve List Surface Number = 4 Curve List Surface Number = 3 Curve List Surface 2.3 Using the mesh seed generated in the previous step, mesh the geometry and create finite elements. Action: Object: Method: Finite Element Create Mesh Surface Surface List Surface 1 2 Use equivalence function to make sure all the overlapping nodes are connected. Finite Element Action: Object: Equivalence All A-6 MSC.Nastran 104 Exercise Workbook

225 APPENDIX A Transient Thermal Analysis of a Cooling Fin Method: Tolerance Cube 4. Next, define a material using the specified thermal conductivity, specific heat, and density. Action: Object: Method: Materials Material Name: Input Properties Create Isotropic Manual Input mat_1 Thermal Conductivity 6e-4 Specific Heat Density MSC.Nastran 104 Exercise Workbook A-7

226 5. Next, reference the material that was created in the previous step. Define the properties of the cooling fin. Action: Object: Type: Properties Property Set Name Input Properties Material Name Thickness 1 Create 6. Since this is a transient analysis problem, a transient load case needs to be defined before loads and boundary conditions are applied. 2D Shell fin m:mat_1 Select Members Surface 1 2 Add Load Cases Action: Load Case Name Load Case Type: Create transient Time Dependent 7. Assign the convection properties to the cooling fin. 7a. The convection on the left edge is defined as follows: Loads/BCs Action: Object: Type: New Set Name Create Convection Element Uniform conv A-8 MSC.Nastran 104 Exercise Workbook

227 APPENDIX A Transient Thermal Analysis of a Cooling Fin Target Element Type: Input Data Surface Option: 7b. The right hand side of the fin undergoes a different type of convection. 2D Edge Edge Convection Coef Ambient Temperature 2500 Select Application Region Geometry Filter Geometry Select Surfaces or Edges Surface 1.1 Add Action: Object: Type: Loads/BCs New Set Name Target Element Type: Input Data Surface Option: Create Convection Element Uniform conv_right 2D Edge Edge Convection Coef Ambient Temperature 1000 Select Application Region Geometry Filter FEM MSC.Nastran 104 Exercise Workbook A-9

228 Select 2D Elements or Edge Element 37: :12: :48: : Add 8. Click on the Analysis radio button on the Top Menu Bar and complete the entries as shown here: Action: Object: Type: Analysis Translation Parameters Data Output: Solution Type Solution Type Solution Parameters Default Init Temperature 70 Subcase Create Available Subcases Subcase Parameter Initial Time Step = 0.1 Number of Time Steps = 20 Cancel Analyze Entire Model Analysis Deck XDB and Print TRANSIENT ANALYSIS transient A-10 MSC.Nastran 104 Exercise Workbook

229 APPENDIX A Transient Thermal Analysis of a Cooling Fin An MSC.Nastran input file called fin.bdf will be generated. This process of translating your model into an input file is called the Forward Translation. The Forward Translation is complete when the Heartbeat turns green. MSC.Nastran 104 Exercise Workbook A-11

230 Submitting the Input File for Analysis: 9. Submit the input file to MSC.Nastran for analysis. 9a. To submit the MSC.Patran.bdf file, find an available UNIX shell window. At the command prompt enter nastran fin.bdf scr=yes. Monitor the run using the UNIX ps command. 9b. To submit the MSC.Nastran.dat file, find an available UNIX shell window and at the command prompt enter nastran fin scr=yes. Monitor the run using the UNIX ps command. 10. When the run is completed, edit the fin.f06 file and search for the word FATAL. If no matches exist, search for the word WARNING. Determine whether existing WARNING messages indicate modeling errors. A-12 MSC.Nastran 104 Exercise Workbook

231 APPENDIX A Transient Thermal Analysis of a Cooling Fin 11. MSC.Nastran Users have finished this exercise. MSC.Patran Users should proceed to the next step. 12. Proceed with the Reverse Translation process, that is, attaching the fin.xdb results file into MSC.Patran. To do this, return to the Analysis form and proceed as follows: Analysis Action: Object: Method: Select Results File Select Results File Attach XDB Result Entities Local fin.xdb 13. When the translation is complete and the Heartbeat turns green, bring up the Results form. Choose the Default result case, and plot the result by selecting Temperature in the Select Fringe Result. Action: Object: Results Create Quick Plot Select Result Cases Default, A1:Time = 1.02 Select Fringe Result Temperature MSC.Nastran 104 Exercise Workbook A-13

232 A-14 MSC.Nastran 104 Exercise Workbook

233 APPENDIX B Analytical Solution for a Simple Radiation to Space Problem Objectives: Create a new database. Create the solid model Assign the thermal loads Submit the model for analysis MSC.Nastran 104 Exercise Workbook B-1

234 B-2 MSC.Nastran 104 Exercise Workbook

235 APPENDIX B Analytical Solution for a Simple Radiation to Space Problem Suggested Exercise Steps: Create a new database and name it furnance.db. Create a surface of the wall and then extrude it to generate a solid model. Generate mesh seeds on the edges of the solid. Create a finite element model using the available mesh seeds. Define material and element properties. the convection conditions to front surface of the furnance wall. radiation and heat flux to the back side of the model. Submit the model to MSC.Nastran for analysis. Review results. MSC.Nastran 104 Exercise Workbook B-3

236 B-4 MSC.Nastran 104 Exercise Workbook

237 APPENDIX B Analytical Solution for a Simple Radiation to Space Problem Exercise Procedure: 1. Open a new database called furnance.db. File/New... New Database Name furnance In the New Model Preferences form set the following:. New Model Preference Tolerance Analysis Code: Analysis Type: Default MSC/NASTRAN Thermal Change to a front view by selecting the Iso1 View button on the toolbar. Iso1 View Whenever possible click Auto Execute (turn off). 2. Create the surfaces of the furnance wall. Geometry Action: Create Object: Surface Method: XYZ Reference Coordinate Frame Coord 0 Vector Coordinates List <3, 2.5, 0> Origin Coordinates List [0, 0, 0] MSC.Nastran 104 Exercise Workbook B-5

238 Extrude the surface to create a solid wall with thickness of 0.15 Geometry Action: Create Object: Solid Method: Extrude Reference Coordinate Frame Coord 0 Translation Vector <0, 0, 0.15> Surface List [Surface 1 3. Create a finite element model Generate two mesh seeds on the edge of the wall.: Finite Element Action: Create Object: Mesh Seed Method: Uniform Element Edge Length Data Number of Elements Number = 2 Choose the lower right hand curve Curve List Solid Create mesh seed on the two longer edges of the solid Element Edge Length Data Element Length (L) Number = 0.2 Curve List Solid B-6 MSC.Nastran 104 Exercise Workbook

239 APPENDIX B Analytical Solution for a Simple Radiation to Space Problem Create finite elements using the mesh seeds generated in the previous steps. Action: Object: Method: Finite Element Create Mesh Solid Surface List Solid 1 4. Define a material using the specified thermal conductivity. Action: Object: Method: Materials Material Name Input Properties Create Isotropic 5. the material properties to the furnance wall Manual Input mat Thermal Conductivity = 1.2 Properties Action: Object: Type: Property Set Name Input Properties Material Name Create 3D Solid solid mat MSC.Nastran 104 Exercise Workbook B-7

240 Select Members Solid 1 Add 6. Assign the thermal loads to the wall The front surfaces of the solid is undergoing convection. Loads/BCs Action: Create Object: Convection Type: Element Uniform New Set Name convection Target Element Type: 3D Input Data Convection Coef 20 Ambient Temperature 298 Select Application Region Geometry Filter Geometry Choose the front faces of solid Select Surfaces or Edges Surface 1.6 Add Heat flux and radiation is being applied to the back surface. Loads/BCs Action: Object: Type: Create Applied Heat Element Uniform B-8 MSC.Nastran 104 Exercise Workbook

241 APPENDIX B Analytical Solution for a Simple Radiation to Space Problem New Set Name heat_flux Target Element Type: 3D Input Data Form Type: Basic Surface Option: Bottom Bottom Surf Heat Flux 2020 Select Application Region Geometry Filter Geometry Select Solid Faces Solid 1.5 Add Specify the parameters for the radiation on the back surface. Loads/BCs Action: Create Object: Radiation Type: Element Uniform New Set Name radiation Target Element Type: 3D Input Data Top Surf Emissivity 0.8 Top Surf Absorptivity 0.8 Ambient Temperature 298 View Factor 1 Select Application Region MSC.Nastran 104 Exercise Workbook B-9

242 Geometry Filter Geometry Select Solid Faces Solid 1.6 Add 7. Click on the Analysis radio button on the Top Menu Bar and complete the entries as shown here: Action: Object: Type: Analysis Translation Parameters Data Output: Solution Type Solution Type: Solution Parameters Default Init Temperature 300 Radiation Parameters Stefan-Boltzmann Constant: Analyze Entire Model Analysis Deck XDB and Print STEADY STATE ANALY- SIS 5.67e-8 An MSC.Nastran input file called furnance.bdf will be generated. This process of translating your model into an input file is called the Forward Translation. The Forward Translation is complete when the Heartbeat turns green. B-10 MSC.Nastran 104 Exercise Workbook

243 APPENDIX B Analytical Solution for a Simple Radiation to Space Problem Submitting the Input File for Analysis: 8. Submit the input file to MSC.Nastran for analysis. 8a. To submit the MSC.Patran.bdf file, find an available UNIX shell window. At the command prompt enter nastran furnance.bdf scr=yes. Monitor the run using the UNIX ps command. 8b. To submit the MSC.Nastran.dat file, find an available UNIX shell window and at the command prompt enter nastran furnance scr=yes. Monitor the run using the UNIX ps command. 9. When the run is completed, edit the furnance.f06 file and search for the word FATAL. If no matches exist, search for the word WARNING. Determine whether existing WARNING messages indicate modeling errors. MSC.Nastran 104 Exercise Workbook B-11

244 10. MSC.Nastran Users have finished this exercise. MSC.Patran Users should proceed to the next step. 11. Proceed with the Reverse Translation process, that is, attaching the furnance.xdb results file into MSC.Patran. To do this, return to the Analysis form and proceed as follows: Analysis Action: Object: Method: Select Results File Select Results File Attach XDB Result Entities Local furnance 12. When the translation is complete and the Heartbeat turns green, bring up the Results form. Choose the Default result case, and plot the result by selecting Temperature in the Select Fringe Result. Results Action: Object: Select Result Cases Select Fringe Result Create Quick Plot Default Temperature B-12 MSC.Nastran 104 Exercise Workbook

245 APPENDIX C Printed Circuit Board Using 2 1/2 D Paved meshing method Objective: Create Geometry from MSC.Patran MSC.Nastran 104 Exercise Workbook C-1

246 C-2 MSC.Nastran 104 Exercise Workbook

247 APPENDIX C Printed Circuit Board Using 2 1/2 D Paved Meshing Method Suggested Exercise Steps: Create a new database called pcb.db MSC.Nastran 104 Exercise Workbook C-3

248 C-4 MSC.Nastran 104 Exercise Workbook

249 APPENDIX C Printed Circuit Board Using 2 1/2 D Paved Meshing Method Exercise Procedure: 1. Create a New Database and name it pcb.db. File/New... New Database Name pcb 2. Change the Tolerance to Default and the Analysis Code to MSC.Nastran in the New Model Preferences form. Verify that the Analysis Type is Thermal. New Model Preference Tolerance Analysis Code: Analysis Type Default MSC/NASTRAN Thermal Whenever possible click Auto Execute (turn off). 3. Create the surfaces representing the printed circucit board. Geometry Action: Create Object: Surface Method: XYZ Vector Coordinates List: < > Origin Coordinates List: [ ] Repeat the previous step to create the two rectangular components. Vector Coordinates List: < > Origin Coordinates List: [ ] MSC.Nastran 104 Exercise Workbook C-5

250 Vector Coordinates List: <1 1 0> Origin Coordinates List: [ ] Use the Curve object to create the two circular components Geometry Action: Create Object: Curve Method: 2D Circle Input Radius 0.75 Construction Plane List Coord 0.3 Center Point List [ ] Input Radius 0.5 Construction Plane List Coord 0.3 Center Point List [ ] Input Radius 0.5 Construction Plane List Coord 0.3 Center Point List [ ] 4. Create trimmed surfaces that will represent the components and the circuit boards. In order to create trimmed surfaces, the curves that represents the edges of the surface must be chained together. Geometry Action: Object: Create Curve C-6 MSC.Nastran 104 Exercise Workbook

251 APPENDIX C Printed Circuit Board Using 2 1/2 D Paved Meshing Method Method: Chain Delete Orginial Elements Curve List Surface Curve List Surface Curve List Surface Generate the trimmed surfaces using the chained curved created in the previous steps. Geometry Action: Object: Method: Option: Create Surface Trimmed Planar Use All Edge Vertices Delete Outer Loop Outer Loop List Curve 4 Delete Inner Loops Inner Loop List Curve Click NO when the message Do you wish to delete the original curves? appears. This also applies to the following steps. Geometry MSC.Nastran 104 Exercise Workbook C-7

252 Action: Object: Method: Option: Create Surface Trimmed Planar Use All Edge Vertices Delete Outer Loop Outer Loop List Curve 2 Delete Inner Loops Be sure to delete the curve lists in the Inner Loop List box Inner Loop List Geometry Action: Object: Method: Option: Create Surface Trimmed Planar Use All Edge Vertices Delete Outer Loop Outer Loop List Curve 1 Delete Inner Loops Inner Loop List Geometry C-8 MSC.Nastran 104 Exercise Workbook

253 APPENDIX C Printed Circuit Board Using 2 1/2 D Paved Meshing Method Action: Object: Method: Option: Create Surface Trimmed Planar Use All Edge Vertices Delete Outer Loop Outer Loop List Curve 3 Inner Loop List Delete Inner Loops When you are finished your model should look like the one shown in the figure below. 5. Create the finite element model MSC.Nastran 104 Exercise Workbook C-9

254 Because the surfaces are trimmed and non-parametric surfaces, paver meshed is need to generate the finite elements. Action: Object: Method: Finite Element Create the finite elements for the components. Create Mesh Global Edge Length 0.1 Element Topology Mesher Paver Surface Quad4 Curve List Surface 4 Action: Object: Method: Finite Element Create Mesh Global Edge Length 0.1 Element Topology Mesher Paver Surface Quad4 Curve List Surface Extrude the Quad4 elements to generate solid elements to represent the epoxy layer. Action: Object: Method: Finite Element Sweep Element Extrude Direction Vector < > C-10 MSC.Nastran 104 Exercise Workbook

255 APPENDIX C Printed Circuit Board Using 2 1/2 D Paved Meshing Method Extrude Distance Offset 0.0 Delete Orginial Elements Base Entity List Elm 3044:3657:1 Mesh Control Number = 2 Repeat the previous step and create the solid elements on top of the epoxy elements to represent the components, and the circuit board. Finite Element Extrude Distance 0.4 Offset Delete Orginial Elements Base Entity List Elm 3044:3657:1 Mesh Control Number = 2 Direction Vector < > Extrude Distance 0.2 Offset 0.0 Delete Orginial Elements Base Entity List Elm 1:3657:1 MSC.Nastran 104 Exercise Workbook C-11

256 Equivalence the model to make sure all the intersecting nodes are connected. Action: Object: Method: Finite Element Equivalence Use the Verify command to make sure that the model is meshed correctly. All Equivalencing Tolerance Finite Element Tolerance Cube Action: Object: Method: Display Type Verify Element Boundaries Free Edges C-12 MSC.Nastran 104 Exercise Workbook

257 APPENDIX C Printed Circuit Board Using 2 1/2 D Paved Meshing Method 6. Create groups that represent the base component, chip, and epoxy finite elements. Group/Create... Action: New Group Name Create base_component Make Current Group Contents: Add Entity Selection Entity Selection Elm 3044:3657:1 Group/Create... Action: New Group Name Create chip Make Current MSC.Nastran 104 Exercise Workbook C-13

258 Group Contents: Add Entity Selection Entity Selection Elm 4886:6113:1 Group/Create... Action: New Group Name Create epoxy Group Contents: Make Current Add Entity Selection Entity Selection Elm 3658:4885:1 7. Post the Chip, default_group, and epoxy groups to show the finite elements in the group. Group/Post... Action: Select Group to Post Post Chip default_group epoxy Group/Post... Action: Select Group to Post Post default_group 8. Define the three different materials using the specified thermal conductivity. Materials C-14 MSC.Nastran 104 Exercise Workbook

259 APPENDIX C Printed Circuit Board Using 2 1/2 D Paved Meshing Method Action: Create Object: Isotropic Method: Manual Input Material Name: component Input Properties Thermal Conductivity 0.89 Materials Action: Create Object: Isotropic Method: Manual Input Material Name: glue Input Properties Thermal Conductivity 0.2 Materials Action: Create Object: Isotropic Method: Manual Input Material Name: circuit_board Input Properties Thermal Conductivity 0.3 MSC.Nastran 104 Exercise Workbook C-15

260 9. the material properties to the finite elements. Properties Action: Create Object: 3D Type: Solid Property Set Name pcb Input Properties Material Name m:circuit_board Select Members Elm 6114:13427:1 Add Properties Action: Create Object: 3D Type: Solid Property Set Name chip Input Properties Material Name m:component Select Members Elm 4886:6113:1 Add Properties C-16 MSC.Nastran 104 Exercise Workbook

261 APPENDIX C Printed Circuit Board Using 2 1/2 D Paved Meshing Method Action: Object: Type: Property Set Name Input Properties Material Name Create 10. the heat flux to the top surfaces of the chips Before you select the element faces, change the rectangular picking preference to Enclose Entire Entity. 3D Solid epoxy m:glue Select Members Elm 3658:4885:1 Add Action: Object: Type: Loads/BCs New Set Name Target Element Type: Input Data Form Type: Heat Flux 3 Select Application Region Geometry Filter Preferences/Picking... Create Applied Heat Element Uniform heatflux 3D FEM Basic MSC.Nastran 104 Exercise Workbook C-17

262 Rectangle/Polygon Picking entity Enclose entire Also, in the FEM Select Menu, pick the Face of element icon. Face of element Next, click on the Top View button on the main menu. Top View Now drag a rectangular box across the end of the chip elements as shonw in the following figure. Select 3D Element Faces Elm 4760:5372:1 Add C-18 MSC.Nastran 104 Exercise Workbook

263 APPENDIX C Printed Circuit Board Using 2 1/2 D Paved Meshing Method Set the boundary condition on the circuit board so it is permanetly kept at 40 degree. Action: Object: Type: Loads/BCs New Set Name Input Data Boundary Temperature 40 Select Application Region Geometry Filter FEM Create Select the right and left edges of the circuit board. Temp (Thermal) Nodal temp_edge Select Nodes Node 2 67:120 Add 11. Click on the Analysis radio button on the Top Menu Bar and complete the entries as shown here: Analysis Action: Object: Type: Translation Parameters Data Output: Solution Type Analyze Entire Model Analysis Deck XDB and Print MSC.Nastran 104 Exercise Workbook C-19

264 Solution Type Solution Parameters Default Init Temperature 70 STATIC STATE ANAL- YSIS An MSC.Nastran input file called pcb.bdf will be generated. This process of translating your model into an input file is called the Forward Translation. The Forward Translation is complete when the Heartbeat turns green. C-20 MSC.Nastran 104 Exercise Workbook

265 APPENDIX C Printed Circuit Board Using 2 1/2 D Paved Meshing Method Submitting the Input File for Analysis: 12. Submit the input file to MSC.Nastran for analysis. 12a. To submit the MSC.Patran.bdf file, find an available UNIX shell window. At the command prompt enter nastran pcb.bdf scr=yes. Monitor the run using the UNIX ps command. 12b. To submit the MSC.Nastran.dat file, find an available UNIX shell window and at the command prompt enter nastran pcb scr=yes. Monitor the run using the UNIX ps command. 13. When the run is completed, edit the pcb.f06 file and search for the word FATAL. If no matches exist, search for the word WARNING. Determine whether existing WARNING messages indicate modeling errors. MSC.Nastran 104 Exercise Workbook C-21

266 14. MSC.Nastran Users have finished this exercise. MSC.Patran Users should proceed to the next step. 15. Proceed with the Reverse Translation process, that is, attaching the pcb.xdb results file into MSC.Patran. To do this, return to the Analysis form and proceed as follows: Analysis Action: Object: Method: Select Results File Select Results File Attach XDB Result Entities Local pcb.xdb 16. When the translation is complete and the Heartbeat turns green, bring up the Results form. Choose the Default result case, and plot the result by selecting Temperature in the Select Fringe Result. Results Action: Object: Select Result Cases Select Fringe Result Create Quick Plot Default Temperature C-22 MSC.Nastran 104 Exercise Workbook

267 APPENDIX D Create Group and List Objectives: Read in the Patran session file. MSC.Nastran 104 Exercise Workbook D-1