PATRAN/ABAQUS PRACTICE

Transcription

1 UNIVERSITY OF ILLINOIS AT URBANA-CHAMPAIGN College of Engineering CEE570/CSE551 Finite Element Methods (in Solid and Structural Mechanics) Spring Semester 2014 PATRAN/ABAQUS PRACTICE This handout provides idea and guidelines how to tackle the project. All the students are strongly recommended to practice the following example before starting the actual project. 1. Introduction In this exercise you will conduct finite element analyses of the 2-D link bar shown in Fig. 1 using a triangular element (T3). The bar has a unit thickness, is constructed of a steel alloy and is subjected to a unit axial stress applied over the left end. A plane-stress idealization is adopted for the 2-D model. The right end is supported on vertical rollers as shown in Fig. 2 to allow vertical contraction or 'breathing'. The link bar, loading and boundary conditions are all symmetric about the X-axis. Consequently, we need to consider only that portion of the link bar with Y 0. The analyses focus on convergence of key displacement and stress values as the mesh is uniformly refined into more elements. You will start the modeling and solution process by copying a Patran database, previously created for this problem. The database contains the geometry definition for the link-bar (plane surface entities). By starting with the predefined geometry, you can focus on the mesh generation, analysis and results evaluation. Fig 1 Link Bar Geometry

2 Fig Preparation Typical Half-Symmetric Model, Loading and Constraints This exercise introduces the Patran and Abaqus software. To prepare for this exercise, you should: - Read through the Abaqus tutorial handouts (see the class web-page). Become familiar with main features of the input (.inp) and output (.dat) files. - Read lab class notes which cover general features of Patran. Detailed explanation and hands-on practice regarding Patran will be provided on February 15, 17, 20 and Become familiar with the workstations: login and logout, create X-terminal windows, edit text files (vi, pico, emacs), and print files. A page with common Unix C-shell (or TCshell) commands is attached at the end of this manuscript for your convenience. 3. Overview of Steps in This Assignment This assignment involves a number of steps for completion. The major ones are as follows: 3.1) Copy an existing Patran database containing the geometry model for the link bar. Start up the Patran software. 3.2) Create a complete finite element model for the link bar using specific finite elements. The model contains the incidences, nodal coordinates, material properties, element properties, displacement boundary conditions and the nodal forces applied over the left end. The nodes are renumbered during the model building to minimize the bandwidth of the assembled stiffness matrix. 3.3) Create an Abaqus input file for the finite element model. This is an ASCII file of text lines that describe the generated model. This file can be examined with any text editor; it can be printed if necessary; it can be ed to someone for their use in Abaqus, etc. 3.4) Run the Abaqus program to analyze the model and to create Patran compatible results files of: (1) nodal displacements, (2) averaged strains at the structure nodes and (3) averaged stresses at the structure nodes. Abaqus also provides the capability to produce nicely formatted output of displacements, strains and stresses. While Abaqus is running in one window, Patran continues to run in the other window.

3 3.5) With the files of nodal results available, Patran is then used to examine the deformed shape and to examine fringe plots of the different stress-strain components. 3.6) Hardcopy output of the finite element mesh, deformed shape, fringe plots, etc. can all be sent to local PostScript printers. 3.7) The cycle now repeats by modifying the mesh characteristics, generating a new input file, etc. 4. Getting Started Login to a workstation and bring up an X-terminal window. 4.1) Change to (or create) your personal CEE570 class workspace directory. To create your personal CEE570 work directory for the semester, enter the command mkdir cee570 at the command prompt in the X-terminal window. From now on, to access this directory, you can use the command cd cee ) Download the sample starting Patran database file from the CEE 570 class website (zipped 2D_Link_Bar.db file) into your personal work directory. This is a 'binary' file and cannot be examined with a text editor nor can it be printed. However, the Unix commands rm, mv, and cp may be used to delete the file, rename the file or copy the file if desired. Unzip the file in the terminal with the command unzip 2DLinkBar.zip 4.3) Start the Patran software by entering the command patran at the X-terminal command prompt. The Patran software creates a large, main window. For the EWS users: you can minimize or lower the vertical EWS menu bar in the right side of the screen by clicking the lower edge of the bar with the middle button of the mouse and then by selecting any of the options like move, resize, lower, close. 5. Open Database and Examine Geometry Model Perform the following sequence of actions: 5.1) Select File Open from the top line, left side of the main menu. This creates a window form the database name. 5.2) A 'box' listing existing database names is shown on the right side of this form. Use the mouse to select 2D_Link_Bar.db. Then click the OK button. 5.3) A graphics window opens to display the geometry model. A message window may appear with a warning. Just click the OK button to dismiss it. 5.4) The geometry model for the top half of the link bar appears in the graphics window as shown in Fig. 3.

4 5.5) The model consists of 16, 4-sided 'surfaces' in Patran terminology. The points and surfaces are not numbered sequentially but this is not an issue. We can ask Patran for the area of these surfaces. Fig 3. Geometry Model for Link Bar. Point and Surface Entity Numbers are shown. 6. Get Some Properties of Previously Defined Surfaces (OPTIONAL) Perform the following sequence of actions: 6.1) On the main menu across the top of the screen (on the row of diamond buttons), select the one for Geometry (push the diamond button using the mouse and left mouse button). 6.2) This brings up a new Geometry menu form on the right side of the screen. In that form, use the left mouse button to pick the following entries-. Action: Show Object: Surface Info: Attributes 6.3) Click the Auto Execute button to turn it off (out). Click on the Surface List box. This will enable the list of surfaces to be entered. Use the mouse to define a rectangle selection box in the graphics window which encloses all 16 surfaces. The box will show the list of surfaces selected. 6.4) Click on the Apply button at the bottom of the Geometry menu form. A 'spreadsheet' type window will appear showing data for each of the selected surfaces. Click the Cancel button on this form to dismiss the surface area information. (PATRAN might crash) 6.5) To dismiss the Geometry menu, click the Geometry button on the main menu (clicking the diamond button makes the Geometry menu go away). 7. Create Layout of Elements With Fixed Side Length Perform the following sequence of actions: 7.1) On the main menu across the top of the screen, on the row of diamond buttons, select the one for Elements (push the diamond button using the mouse and left mouse button). 7.2) This brings up a new Elements menu form on the right side of the screen. In that form, use the left mouse button to pick the following entries: Action: Create Object: Mesh Seed

5 Type: Uniform The mesh seed defines the node layout along the edges of each surface. In this case, our initial mesh will have elements of side length 0.2 in. 7.3) Push the Element Length button to select it. Click the Length box and type the value 0.2 (Do not hit carriage return!!). 7.4) Click on the Auto Execute box to deselect it. 7.5) Click on the Curve List box to select it. Then use the mouse to create a rectangular selection box that encloses the entire model (must get all the curves defined in the model). The list of curves is displayed in the box. 7.6) Click on the Apply box to actually create the mesh seeds (open circles defined along the curves that make up the surface edges). The graphics image should appear as shown below. Fig 4 Mesh Seeds to define Elements Along Each Edge of Each Surface for the Link Bar Model. 8. Create Elements Perform the following sequence of actions: 8.1) On the Finite Elements menu form, use the left mouse button to pick the following entries: Action: Create Object: Mesh Type: Surface 8.2) Examine the Element Topology box. It has a slider bar to select the element type. Use the slider to find element type and select it (Elem Shape: Tria, Mesher: IsoMesh, and Topology: Tria3). 8.3) Make sure the IsoMesh button is selected. 8.4) Click on the Surface List box to select it. Then use the mouse to create a rectangular selection box that encloses the entire model (must get all the surfaces defined in the model). The list of surfaces is displayed in the box.

6 8.5) Click on the Apply box to actually create the elements. This takes a few seconds to happen. The graphics image should appear as shown in Fig. 5. For the sake of illustration, a mesh with CST elements is provided in Fig. 5. Fig. 5 Very Coarse Mesh of CST Elements for Link Bar Model 9. Cleanup Graphics Window At this point, the graphics window has become cluttered with the various geometry and mesh labels. Patran provides a simple tool to control this aspect of the appearance. 9.1 On the main Patran menu, locate the long horizontal row of icons. The L icon (near the right end) controls labeling. Click on this icon. 9.2 A box of 9 icons appears on the left side of the display. These are 'smart' icons in that a simple message appears to describe the icon as the mouse is slowly moved over them. 9.3 Select the top, left icon All Entity Labels and click on that icon. All the labels are immediately erased (or turned back on; these are toggle switches). 9.4 Close the 9 box of icons. 10. Eliminate Duplicated Nodes, Optimize Node Numbering and Align Element Normals The mesh generation process creates nodes for each surface independently and as a result, duplicate nodes are created along the shared edges between the surfaces. These are eliminated by a geometric search which 'zips-together' the shared edges. 10.1) On the Finite Elements menu form, use the left mouse button to pick the following entries: Action: Equivalence Object: All Method: Tolerance Cube 10.2) Click the Apply button. As a result of the equivalencing process, the node numbers are no longer numbered sequentially and the nodes are not necessarily associated with elements to minimize the bandwidth of the assembled stiffness matrix. A node numbering optimization step solves both issues.

7 10.3) On the Finite Elements menu form, use the left mouse button to pick the following entries: Action: Optimize Object: Nodes Method: Both 10.4) On the list of buttons for Minimization Criterion, select Profile. This option minimizes the fill-in during the Choleski factorization of the assembled stiffness. 10.5) Click the Apply button. A spreadsheet window appears to show the 'before' and 'after' properties of the node numbering sequences. Click OK to dismiss this window. We also renumber the finite elements at this point in case they are not numbered sequentially. This can happen due to various sequences of commands to mesh and remesh surfaces with different mesh refinement. 10.6) On the Finite Elements menu form, use the left mouse button to pick the following entries: Action: Optimize Object: Elements Method: Both 10.7) On the list of buttons for Minimization Criterion, select Profile. 10.8) Click the Apply button. A spreadsheet window appears to show the 'before' and 'after' properties of the element numbering sequences. Click OK to dismiss this window. We have to verify also that all elements have their positive surface normals pointing outwards. This is a very important step. 10.9) On the Finite Elements menu form, use the left mouse button to pick the following entries: Action: Verify Object: Element Test : Normals 10.10) Click Draw Normal Vectors and then click Apply. You should see red arrows being plotted ) Click on the Iso 1 View icon (at the top 3rd level menu) or click on the middle button of the mouse and without releasing it move the mouse. You will have a good view of the element normals. Click on reset graphics to get the previous view. To change the normal directions: 10.12) Click the Display only icon under test control, so it changes to Reverse Elements icon.

8 10.13) Click in Guiding element databox. Use the left mouse button and pick one element from the surface which is pointing in the correct or 'outward' (positive z) direction. (Select such that all normals of the surface are in the same direction.) 10.14) Click the Apply button ) Click on the Front View icon. 11. Create Material and Element Properties In this section, we define a named material then a named set of element properties (material, plane stress vs. plane strain, element thickness). The properties are then assigned to all elements in the model. The material model here is simple linear-elastic, isotropic with properties of Young's modulus equal to 30,000 ksi, and Poisson's ratio of 0.3. The element property is the thickness (1.0) and the type of model is plane-stress (not plane-strain). 11.1) On the main menu across the top of the screen (on the row of diamond buttons), select the one for Materials (push the diamond button using the mouse and left mouse button). 11.2) This brings up a new Materials menu form on the right side of the screen and dismisses the Finite Elements menu form. In the new form, use the left mouse button to pick the following entries: Action: Create Object: Isotropic Method: Manual Input 11.3) Click on the Material Name box, and type Steel (the name is user definable). 11.4) Push the Input Properties.. button. This brings up an Input Options form in which we enter values for the material. Enter 30,000 in the Elastic Modulus and 0.3 in the Poisson's Ratio boxes. 11.5) Click on the OK button. 11.6) Click on the Apply button in the Materials menu. Steel will now appear in the box of Existing Material. 11.7) On the main menu across the top of the screen (on the row of diamond buttons), select the one for Properties (push the diamond button using the mouse and left mouse button). 11.8) This brings up a new Element Properties menu form on the right side of the screen and dismisses the Materials menu form. In the new form, use the left mouse button to pick the following entries: Action: Create Type: 2D Solid Object: 2D Options: Plane stress 11.9) Click on the Property Set Name box and type Link Bar (the set name is user definable).

9 11.10) Click the Input Properties... button. This brings up an Input Properties form in which we enter values for this model ) Select Steel from Material Property Sets box and it appears in the Material Name box ) Enter 1.0 into the [Thickness] box, and then click the OK button ) Click the Select Application Region button and in the popped up window click in the Select Members box. In the picking filters window, make sure to have Tri element selected. Then select the entire model (elements) with the mouse ) Click the Add button. The element numbers appear in Application Region box ) Click the Apply button. This causes Patran to assign the material and element properties to all elements shown in the Application Region box. 12. Create a Load Case At this point in the model generation, the nodes and elements are fully defined. We now define the loading, which in Patran terminology consists of the displacement boundary conditions and applied nodal forces. There can be any number of load cases, each of which has sets of imposed nodal displacements and nodal forces. In this assignment only one load case needs to be defined. Perform the following sequence of actions: ) On the main menu across the top of the screen (on the row of diamond buttons), select the one for Load Cases (push the diamond button using the mouse and left mouse button). 12.2) This brings up a new Load Cases menu form on the right side of the screen and dismisses the Element Properties menu form. In the new form, use the left mouse button to pick the following entries: Action: Create 12.3) In the Existing Load Cases box, select the Default load case. This name will now appear in the Load Case Name box. A large form menu, Input Data, appears. Just dismiss it by clicking OK. 12.4) Click on the Apply button of the Load Cases menu form. A 'warning' box appears with a message saying that the load case already exists. Click the YES button. In the sections below, we will add displacement and nodal loading 'sets' to this default load case. Key point: the displacement and nodal loading sets defined below can be included in one or more load cases. For example, a set of nodal forces representing the dead_load could be included in all load cases. 13. Create Sets of Displacement Boundary Conditions

10 To analyze the link bar model, we need two sets of displacement boundary conditions. The set we choose to name bottom_symm enforces the displacement condition v = 0 on all nodes along Y= 0. The set we choose to name right-end enforces the displacement condition u = 0 on all nodes along X = 6. Perform this sequence of commands. 13.1) On the main menu across the top of the screen (on the row of diamond buttons), select the one for Loads/BCs (push the diamond button using the mouse and left mouse button). 13.2) This brings up a new Loads/BCs menu form on the right side of the screen. In that form, use the left mouse button to pick the following entries: Action: Create Object: Displacement Type: Nodal 13.3) Examine the New Set Name box. It has no entries at this point. Click on this box and type in the text bottom symm (the underbar character is not required). Do not hit a carriage return!! 13.4) Click on the Input Data button. This brings up a form in which we enter the values of the displacements on the Y= 0 nodes. Examine the box: Translations <Tl T2 T3>. Enter the following text: <,0.0 > The angle brackets < > must be included. The leading comma implies that there is no constraint on the u x displacement. This command indicates that u y = 0 on the yet to be selected nodes. Click on the Ok button to save the data and dismiss this form. 13.5) Click on the Select Application Region button. This brings up another window form menu over the Loads/BCs. Under the Geometry Filter section, select the FEM button. 13.6) Click on the Select Nodes box. Use the mouse to define a selection rectangle which includes all nodes along Y= 0. The list of nodes appears then in the Select Nodes box. Click on the Add button and then check on Ok. The Select Application Region window is dismissed. 13.7) Click on the Apply button to actually create the constraints. These are shown as triangle symbols on the affected nodes. The graphics window should appear now as shown in Fig.6 Fig. 6 Graphics Window Image Showing Constraints Applied Along the Bottom Edge of Model (CST elements are displayed on the above mesh). Now begin repeating the above process to define the u x =0 constraints on all nodes along

11 X=6 coordinate. 13.8) Examine the New Set Name box. It has no entries at this point. Click on this box and type in the text right_end (the underbar character is not required). Do not hit a carriage return!! 13.9) Click on the Input Data button. This brings up a form in which we enter the values of the displacements on the X= 6 nodes. Examine the box: Translations <Tl T2 T3>. Enter the following text: < 0.0 > The angle brackets < > must be included. This command indicates that u = 0 on the yet to be selected nodes. Click on the Ok button to save the data and dismiss this form ) Click on the Select Application Region button. This brings up another window over the Loads/BCs. Under the Geometry Filter section, select the FEM button ) Click on the Select Nodes box. Use the mouse to define a selection rectangle which includes all nodes along X= 6. The list of nodes appears then in the Select Nodes box. Click on the Add button and then click on Ok. The Select Application Region window is dismissed ) Click on the Apply button to actually create the constraints. These are shown as triangle symbols on the affected nodes. The graphics window should appear now as shown in Fig 7. Fig. 7 Graphics Window Image Showing Constraints Applied Along the Bottom and Right Edges of the Model. 14. Create the Applied Load Set The physical model is loaded by a 1.0 ksi axial tension stress applied uniformly over the left end of the model. With the current mesh resolution, we have 3 nodes along X = 0. The total force of 0.5 kips (0.5 in. high 1.0 in. thick 1.0 ksi stress = 0.5 kips force) applied on these three nodes is distributed from bottom to top as: 0.125, 0.25, kips. Perform the following sequence of commands to apply these forces. 14.1) Set new Loads/BCs menu values to the following: Action: Create Object: Force Type: Nodal 14.2) Examine the New Set Name box. It has no entries at this point. Click on this box and type in the text axial_tension_a (the underbar character is not required). Do not hit a carriage return

12 14.3) Click on the Input Data button. This brings up a form in which we enter the values of the forces. Examine the box: Force <F1 F2 F3>. Enter the following text: < > The angle brackets < > must be included. The negative sign denotes that the X-direction loading is to the left. Click on the Ok button to save the data and dismiss this form. 14.4) Click on the Select Application Region button. This brings up another window form menu over the Loads/BCs. Under the Geometry Filter section, select the FEM button. 14.5) Click on the Select Nodes box. Use the mouse to select the lower left node of the model and the top left node on the left end. Hold down the shift key when clicking on the nodes. This adds each selected node to the list. The list of nodes appears then in the Select Nodes box. Click on the Add button and then click on Ok. The Select Application Region window is dismissed. 14.6) Click on the Apply button to actually create the nodal forces. These are shown as yellow arrows on the affected nodes. 14.7) Examine the New Set Name box. Click on this box and type in the text axial_tension_b (the underbar character is not required). Do not hit a carriage return!! 14.8) Click on the Input Data button. This brings up a form in which we enter the values of the forces. Examine the box: Force <Fl F2 F3>. Enter the following text: < > The angle brackets < > must be included. The negative sign denotes that the X-direction loading is to the left. Click on the Ok button to save the data and dismiss this form. 14.9) Click on the Select Application Region button. This brings up another window form menu over the Loads/BCs. Under the Geometry Filter section, select the FEM button ) Click on the Select Nodes box. Use the mouse to select the middle (of 3) nodes along the left end of the model. The nodes number appears then in the Select Nodes box. Click on the Add button and then click on Ok. The Select Application Region window is dismissed ) Click on the Apply button to actually create the nodal forces. These are shown as yellow arrows on the affected nodes. The graphics window should now appear as in Fig ) Locate the 'broom' icon on the top right side of the display and click it. This cleans up the graphics window by erasing the constraint and load symbols. Fig. 8 Graphics Window Image Showing Forces Applied to Left End of Model.

13 15. Create the Abaqus Input File for Model All aspects of the finite element model are now defined. Thus the Abaqus input file can be generated. 15.1) On the main menu across the top of the screen (on the row of diamond buttons), select the one for Analysis (push the diamond button using the mouse and left mouse button). 15.2) This brings up a new Analysis menu form on the right side of the screen and dismisses the Loads/BCs menu form. In the new form, use the left mouse button to pick the following entries: Action: Analyze Object: Entire Model Method: Analysis Deck 15.3) Click the Job Name box, then type 2D_Link_Bar (the job name is user definable. The Abaqus input file will then be named 2D_Link_Bar.inp). 15.4) Click the Step Creation button. This brings up the Step Create menu. 15.5) Select the Default Static Step in the Available Job Steps box. 15.6) Click the Output Requests button. This brings up the Output Requests menu which lists various kinds of stress, strain, displacement, etc. output that can be requested. 15.7) Change the Form Type: from Basic to Advanced. 15.8) For BOTH Stress Component and Strain Component, we want to change the Element Position: from Integration Pts to Nodes. This will request that Abaqus output values at the nodes of each element. Click Ok on the Output Requests menu to save requests and dismiss the menu. 15.9) Click Apply, then the Cancel button in the Step Create menu. This saves values and dismisses the menu ) Now click on Step selection. A window will pop up. You will find Default Static step under the heading Existing job steps. Click on this option. Now you will see the Default Static step under the heading Selected job step ) Click the Apply button on the remaining main Analysis menu. This causes Patran to actually write the Abaqus input file. For larger models this can require as much as 10 seconds. During this process, the Patran graphics window disappears. When the heartbeat (at the top right corner of the screen) turns green and the graphics window reappears, the task is finished. The Abaqus input file is now named 2D_Link_.inp (based on the responses given above) ) In an X-terminal window, change to your work directory then open the input file named 2D_Link_Bar.inp with a text editor. For example, type gedit 2D_Link_Bar.inp Another option is:

14 gvim 2D_Link_Bar.inp 15.13) In order for ABAQUS (version 6.6) to generate an output file for PATRAN2006, above the line *END STEP, type as follows: *NODE FILE U, *EL FILE S, E, Hint: If you are using nano, you can press Control+W and perform a search for the keyword you are looking for. This comes in handy in large files. Emacs has the same functionality too. 16. Run Abaqus to Perform Analysis In an X-terminal window, change to your work directory then initiate execution of Abaqus using the command: abaqus *NOTE: If this throws a -bash error, type: module load abaqus into the terminal. This will load abaqus to your directory. Abaqus asks 2 questions about files associated with the analysis. Question one is: identifier : proj1 where the question answer, proj1 in this example, is a user definable name for the analysis job. Abaqus generates a number of files during the analysis; these files are named proj1.xxx. input file (w/o.inp) : 2D_Link_Bar Abaqus now starts execution to perform the analysis. The program runs in the 'background'. This enables continued use of the X-terminal window. Abaqus is a fast program for linear analysis and most jobs for our classes complete quickly. It will take around sec to finish it, although in X-terminal window it would seem like it was executed in a second. To check the status type ps in the X-term. If you see proj1.com under the list of the ps commands that would mean, the program is still running Several key files produced by Abaqus during execution (using proj1 as the identifier given above): - proj1.dat contains the printed error messages, results and other comments - proj1.log contains a very short summary (20 lines) of the starting and stopping steps in the analysis. Simply display this file to determine when your analysis is completed. Use the command: cat proj1.log

15 - proj1.fil contains the displacements, strains, stresses in a form that can be read by PATRAN for post-processing. 17. Import Results Into Patran Database In this step, we will 'import' the nodal displacements, stress and strain into the Patran database for this model and generate a graphical image of the deformed shape. Perform the following sequence of actions: 17.1) On the main menu across the top of the screen (on the row of diamond buttons), select the one for Analysis (push the diamond button using the mouse and left mouse button). 17.2) This brings up a new Analysis menu form on the right side of the screen. In the new form, use the left mouse button to pick the following entries: Action: Read Results Object: Result Entities Method: Translate 17.3) Click the Select Result File button. 17.4) Select on the proper result file in Available Files window (proj1.fil in this example). 17.5) Click OK on the Select File menu 17.6) Click the Apply button on the Analysis menu. This causes Patran to actually read the Abaqus results file into the Patran database (2D_Link_Bar.db) for this problem. For larger models this can require as much as seconds. During this process, the Patran graphics window disappears. When the heartbeat turns green and the graphics window reappears, the task is finished. 18. Generate Image of Deformed Shape This step produces a graphics image of the deformed shape superposed over the undeformed shape. Then we can generate a hardcopy output of the image. 18.1) On the main menu across the top of the screen (on the row of diamond buttons), select the one for Results (push the diamond button using the mouse and left mouse button). 18.2) This brings up the Results menu form on the right side of the screen and dismisses the previous menu. 18.3) Examine the Select Result Cases box. There should be available selections. Select the bottom one in the box. Examine the Select Deformation Result 'box'. Select the option Deformation Displacements. Click the Apply button at the bottom of this menu. 18.4) The undeformed image changes to a have blue lines, with the deformed image in white color lines for triangle elements.

16 18.5) Now we will 'animate' the result as thought the deformed shape is a 'mode' shape from a vibration analysis. Click the Animate button just above the Apply button on the Results menu. Click Apply on the Results menu. The Animate menu pops up over the Results menu and the graphics image cycles dynamically through the deformed shapes. Click the Pause Animation when desired. 19. Clean-up Image and Generate Fringe Plot of Deformed shape The graphics image is cluttered with the undeformed plot, deformed plot plus all the points, curves and surfaces from the original geometry. The following sequences clean up the image in several stages. 19.1) On the main menu across the top of the screen, select Group Modify. This brings up the Group menu form on the right side of display. Find the All Geometry line with has two buttons below the label. Click on the Remove button, then click the OK button. 19.2) Click the 'broom' (Reset graphics) icon on the top-right side of the main menu. Then return to step 18.1 to again plot the deformed shape. 19.3) Select the Object: Quick plot and Default for the Select Result Case. Click on Deformation Displacements under Select Fringe Results and under Select Deformation Result. Click on Apply. Even though the geometry items are now invisible, the undeformed mesh remains. This can be suppressed with the following sequence. 19.4) Below the Object: Quick plot scroll menu click on the Deform Attribute icon (as you move the mouse closer to these buttons the name of the button appears). This changes the menu form below. Find the Show Undeformed button. Click it 'off' (i.e. the button is out). 19.5) Click Apply on the Results form to apply this change and to dismiss the form. 19.6) Click the 'broom' icon on the top-right side of the main menu. Then return to step 18.1 to again plot the deformed shape. Now only the deformed shape is shown when requested. The 'broom' icon can be used to tidy-up the graphics image at any time. 20. Hardcopy of Graphics Image The current graphics image can be routed to the PostScript printers at any time during a Patran session. This includes the geometry model, the finite element model (with constraint and load markers), the deformed shape, etc. The sequence below may be followed at any time to send an image to the printer (or to generate a PostScript file for , ftp, sending to a remote printer, to examine in Ghostview, etc.) 20.1) On the main menu across the top of the screen, select File Print. This brings up the Print menu form on the right side of display.

17 20.2) Find the Page Setup button on the Print menu. Select this button to bring up a menu form which controls the page layout. Examine the options and select the ones you want (selecting none of these is ok). Click OK to dismiss this menu. 20.3) Find the Options button on the Print menu. Select this button to bring up a menu form which controls some additional options. In this menu, you need to select color in Format, white in Background and actual in Lines and Texts. Besides, select Print to File option. Then click Ok. 20.4) Click on the Apply button of the Print menu. This causes the hardcopy process to execute. Once the heartbeat turns green again, the plot has been sent to a file which extension is ps. 20.5) Finally, in order to print the file, type lpr Pprint_name file_name. For example, if you want to print the file named as project1.ps using the color printer (dclcolor1) available in DCL, you need to type lpr Pdclcolor1 project1.ps 20.6) Go to the web page and release your print job. 21. Generate Stress Fringe Plots This step produces a fringe plot of selected stress components on the undeformed shape. A 'fringe' plot is simply a contour plot with the colors painted in between the contour lines. Then we can generate a hard- copy output of the image, but only in shades of gray. 21.1) On the main menu across the top of the screen (on the row of diamond buttons), select the one for Results (push the diamond button using the mouse and left mouse button). 21.2) This brings up the Results menu form on the right side of the screen and dismisses the previous menu. 21.3) Examine the Select Result Cases box. There should be an available selection. Select Stress Components with the mouse in Select Fringe Result 'box'. This box lists all the stress, strain and deformation quantities available for fringe plotting. Use the vertical scroll bar to examine the full list. Select the option X component on Quantity. Click the Apply button at the bottom of this menu. 21.4) The fringe plot is shown over the model with a color scale at the right. 16 colors are used to make the plot. 21.5) To examine fringe plots of the other stress values, simply repeat the previous two steps. 21.6) To create a hardcopy, follow the instructions in Section 20.

18 22. Make More Refined Fringe Plots The fringe plots produced in the previous section use only 16 colors. Patran can also create fringe plots using more colors to give the appearance of 'smooth' fringes. This option is selected by following these steps. 22.1) On the main menu across the top of the screen, select Result. This brings up the menu form on the right side of display. Find the Fringe Attributes icon (below the Quick plot scroll menu bar, as you move the mouse closer to these buttons the name of the button appears), click on it. The menu below changes. 22.2) Click on the Spectrum button. A new form comes up. 22.3) There is a small button labeled Continuous Color. Click on it. 22.4) Click on the Apply button and the colors change to a smoother image. Use Cancel to dismiss this menu. 22.5) Use the 'broom' icon again to clean-up the image. 23. Exiting From Patran At any time, you may exit from Patran. The current database will be saved intact on disk. To exit Patran: 23.1) Select File Quit from the top line, left side of the main menu. 23.2) Alternatively, the File menu offers options to Save the existing database to disk (essentially checkpointing the session), Save As which allows the user to save the current database with a different name, and Close which saves the existing database to disk but does not exit Patran. Another database can be opened for work using the File Open sequence as before.