Using
PATRAN
(a tutorial with an engineering attitude)
by
Herbert A. Koenig
Copyright ©1999 Herbert A. Koenig. All rights reserved. Printed in the United States of America. Except as permitted under the United States Copyright Act of 1976, no part of this publication may be reproduced or distributed in any form or by any means, or stored in a data base or retrieval system, without prior written permission of the author.
Library of Congress
Registration Number: TXu 895-105
PATRAN
PATRAN is a robust software package that is capable of modeling a part for both structural and thermal finite element analyses. It can be used to design the part using the CAD portion of the software. The part may then be converted to a solid model and meshed for analysis by an external Finite Element Analysis (FEA) package. Finally, the results of the FEA may be analyzed to calculate the values of all the state variables that are connected to the physical processes that are being considered. Each of the aforementioned sections of the PATRAN code will now be delineated, in detail.
The usual approach of the design engineer is to construct a part and then analyze this part using an FEA package. The construction phase of the process is generally conducted using a CAD tool such as PRO-E or CADKEY. However, the procedures that are involved with structural construction, using a CAD package, will be reserved for other tutorials that will be part of the current series of documents.
The designer would create all of the geometric entities that are associated with the desired part and create a model and/or a set of design drawings. If the design of the part is where the process is to end, then using a CAD tool is probably the best approach. However, since the goal of the engineer is to continue this design process with the construction of an FEA model, the ease or difficulty in converting a CAD model into a solid or FEA model must be seriously considered. Contrary to popular thought, the process of converting a CAD model into its next step is difficult and hardly seamless, as is advertised by CAD software manufacturers. Therefore, unless there is a compelling reason to use a CAD tools, the CAD portion of PATRAN is the best way to create a model and have it directly available for meshing into an FEA model. PATRAN has strong CAD capabilities and can be used to create almost any geometry. If, on the other hand, an exist ing CAD file is already in existence, then a procedure must be established which will link it with PATRAN even though the procedure may be cumbersome.
Once the CAD portion (also called the geometric modeling phase) is complete (preferably using PATRAN itself), the model is then converted into an FEA model, which would then be used for analysis. This phase of the development process is called meshing or FEA modeling. PATRAN does this job very well. The user has a wide choice of element types that can be used for both structural and thermal analyses of the relevant part.
The FEA model is then converted to a data file that is compatible with the type of FEA package that is available. Currently, at the University of Connecticut, PATRAN can produce a data file (deck) for MARC, ABAQUS, and NASTRAN. These three FEA packages along with the software called ANSYS (not available at the present time) are some of the more popular FEA software tools that are used in academe and industrial environments at the present time.
The next step in the design process is the execution of the Finite Element Analysis itself. This is the actual calculation of all of the state variables that are associated with the physical process that is being modeled. All of the variables that were requested in the FEA phase of PATRAN are now written to an output file for further processing. This output file is the actual "guts" of the design process and is the single important event that characterizes the entire process as a physically important procedure rather than just the drawing of parts, which may be unkindly, be considered "cartoon drawing".
Once the FEA output file is produced, PATRAN may once again, be used to study the results and to display these results graphically. This phase will be described, in depth, in section III of this tutorial.
Before the author launches a full description of PATRAN, some philosophical ideas, which formed the production of this tutorial, will now be presented. This author has not written the tutorial in a manner that is similar to those that are usually written by the manufacturers of the software. Using his experience of 30 years in modeling, the author has decided to write this document using thought processes that an engineer would undergo if that person were performing the desired analysis. It is important for the reader to understand that the engineer using this tutorial must be familiar with the general concepts and ideas of modeling, FEA, and the particular physical processes of his application. IN this light, the author has no desire to solve a particular problem in this tutorial. Instead, he has chosen an unusually difficult part for geometric and FEA modeling and he demonstrated how this model is used to create an actual FEA data stream. This model will not be analyzed once it is created.
The author has chosen a simpler FEA model (constructed and analyzed elsewhere) to produce the output file that will be postprocessed by PATRAN. The output file will be used to display the results of the FEA graphically. In this way, the author hopes to present this phase of the design process in a manner that can evenly be understood by the most novice users of Finite Element Analysis.
The reader should now have a "road map" for the design process that will be used in this tutorial while studying PATRAN. The actual descriptions of the various components of this software now begin.
This tutorial was written using PATRAN VERSION 7.5. Some of the figures in this tutorial were taken from Version 7.6 which is not yet available at the University of Connecticut. This use of various versions of PATRAN should not cause the reader any difficulty since the versions are very similar.
Before any description of PATRAN can be attempted or any consideration of modeling can be made, the user must be able to "launch" the software. At the University of Connecticut, PATRAN resides on only a few machines. Therefore, in order to use this computer tool, the user must first logon to the machine on which it resides. This machine is known as "merlin". Thus, the user must issue the following command at his console,
rlogin merlin
The user must then supply his password. This is the same password that the user needs to login his own machine. If the model that he wants to create is in the user's home directory, he need do NOTHING. However, if the model is in another directory, the user must now cd to that directory.
Since the user will be running PATRAN on merlin, but would like the display to be shown on his own machine, he must redirect this display to the machine which he is currently using. For instance, if the machine that he is currently logged is called hemo, then the user must issue the following command to redirect the display
setenv DISPLAY hemo:0.0
The above command is case sensitive.
The user is now ready to "fire up" PATRAN by simply issuing the command patran. This will cause the screen to start initializing the files. The following sequence of events will now occur. The responses to these events are listed after their descriptions.
Message --> OK
A - If this is a new file, issue the command
File --> New
B - If this is an existing model, issue the command
File --> Open
A list of existing files will appear on the right. Just click on the model that is currently desired.
Next, click on the button Enable NFS Access. This is extremely important. If this is not done PATRAN will not allow the user to do any modeling.
If the user has chosen the NEW option for the database, then PATRAN will ask
New Database Name --> soup.db
The name soup.db was chosen here since this will be the name of the initial example that is presented later in this tutorial.
Other messages and warnings will appear. The user should click on OK in all cases. Finally, the program will ask (with the following responses)
New Model Preferences --> Analysis Code --> MARCK6 --> OK
Here the author has chosen MARCK6 to be the eventual Finite Element Analysis for the model called soup.db. If the user desires another FEM code, he should choose it from the available menu at this time (e.g. ABAQUS).
As soon as the user "launches" PATRAN in the manner that is described above, the screen will appear with several graphical areas. There will be a large black area, which we will label the "Viewport". This is the region in which the reader will use to construct and view his model. At the top border of the viewport area should be a series of text that read "temp.db default_viewport default group Entity". PATRAN is informing the user that (at this time ) the database (.db) is named temp, the default viewport is being displayed, and a default group (which will be explained below) is currently active. Just above the viewport appears a large series of icons. Above the icons are words of text and a few more icons.
PATRAN is an extremely complex program that has multiple menus, sub-menus, and icons to do a powerful job of creating a model for use in Finite Elements and/or CAD. Therefore, the program tends to be complicated to use. Navigating through all of the features of PATRAN can be difficult. This tutorial has been written to explore most of the features in the software and to provide a basis upon which the user can expand his modeling capabilities. This document cannot and will not use all of the strengths that are contained herein. Instead, two complex problems will be presented which expose most of the features of PATRAN and bring the modeling process from the mind of the designer to the computer for the purposes of performing Finite Element Analysis (FEM).
Figure 1 shows the portion of the screen that is displayed above the viewport. Unless one becomes familiar with the use of these menus and icons, the use of PATRAN is impossible. Therefore, an extensive description of these items and their usages is presented before attempting to use them in the examples, which appear below. The user is strongly urged to carefully read the following descriptions and experiment with these tools prior to attempting the example problems and any modeling that the user wants to accomplish.
In the discussion that follows, and in the entire contents of this document, we will refer to the top portion of the screen as follows. The top of the screen where the menus File, Group, etc. appear will be referred as the Top Line. The icons that appear on the right of that line will be specified the Top Line Icons. The next line, which displays Geometry, Finite Elements, etc., will be described as the main menu line or simply the Main Line. Finally, the line on which the series of icons are displayed will be simply called the Icon Line. This categorization of the individual lines is solely that of the authors and may not coincide with the names that are given in the official PATRAN user's guide. However, the author feels that his description is a natural outgrowth of the use of these features and that the user is most likely to remember their functions by the names that are given by this writer.
Figures 2, 3, and 4 are magnified versions of portions of figure 1 and will be used to describe these items below. Each item will, when feasible, be denoted (in the description below) in three ways. When referring to the icons, the name of the icon will be given. A brief description of the symbol on that icon will be given. Additionally, letters have been placed on figures 2, 3, and 4 for the purposes of identifying each feature.
The Top Line
The top line of the display has the following items that are useful in creating a geometric and a Finite Element model of the user's choice.
A - File:
This item performs some of the following functions.
B - Group:
This item allows the user to create, modify and manipulate items in the database. This feature allows the user to separately define various parts of his model both from a geometric and from a Finite Element (FEM) perspective.
C - Viewport:
D - Viewing:
This feature is useful in changing the display and the parameters when postprocessing the solution to a particular application.
E - Display:
F - Preferences:
This feature is used when the user wishes to change the type of finite element analysis that will be performed on the model (e.g. MARC --> ABAQUS)
G - Tools:
Icons on the Top Line
The icons on the top line to the right of the above items are used, in
general, make the display during model development appear more "user-friendly". They
also inform the user as to progress of the tasks. In order to familiarize one's self with any
of the icons within PATRAN, the user should place the cursor on that icon which will
then display its function. These icons are used for:
H - Help:
I - Refresh Graphics (Paint Brush):
While creating a model, the display may get "cluttered" with extraneous lines and entities. This feature refreshes the graphically display and allows the user to constantly use a "clean" display.
J - Default Window Layering:
K - Reset Graphics (Broom):
This feature acts in a manner that is similar to the "Refresh Graphics" icon. The user should use both features in order to evaluate the differences.
L - Interrupt (Hand):
This feature can be used to stop all action of the program. It should not be used, except in an emergency.
M - Red/Blue/Green Button:
This button requires NO action from the user. It informs the user as to the progress of the modeling. When the button is Green, the user may perform the next task and proceed with the modeling. If the button is either Blue or Red, then the system is unavailable to the user and no tasks should be attempted.
N - Undo (Eraser):
This button is the PATRAN modeler's "best friend". When a specific task is performed which the user would like to withdraw, the application of the Undo button restores the model to its previous state, which the user last accepted. Once many tasks have been accomplished, the user cannot return to a previous state and must undo his errors by using the delete functions within PATRAN.
O - Information:
This is a useless button that merely serves to publicize PATRAN and its developer, MSC.
The Main Line
This line on the screen contains the sub-menus that constitute the main features within PATRAN. In general, the Main Line is utilized from "left to right" in the construction of a model. Upon "clicking on each of the items that are listed below, a sub-menu or a family of sub-menus may appear in order to accomplish the desired tasks. Each item will now be described.
Geometry:
This is the main menu for creating and manipulating all of the geometric entities within PATRAN. In many ways this feature acts much like any CAD tool and negates the necessity (except in the most complex cases) for using a CAD tool. In other words, unless the part which the user designs has complex geometric features or geometric interdependencies, PATRAN is the only software package that is necessary in modeling the part and transforming it into a form for FEM analysis. Most of the features within this item will be described, in depth, during the actual creation of the example that forms the basis for this tutorial.
Finite Elements:
This feature converts the geometric description of the model that was developed above into an FEM model for analysis. The main features of this item will be described in the example.
Loads/BC:
This feature allows the user to apply both thermal and structural loads and boundary conditions to the model that has been constructed up to that point. All types of loads and constraints are available with this feature.
Materials:
This feature is one of the most misunderstood aspects of PATRAN. This feature allows the user to define his material name, material properties, and unusual features, such as anisotropy. This feature is NOT used to apply material properties to the model. All of the materials that will eventually constitute the model are defined here. The actual definition of the elements, which possess these properties, is reserved for the next feature.
Properties:
This feature aids the user in applying the aforementioned materials to specific parts of the current FEM model. One can assign certain materials to parts of the model and other materials to other parts of the model. Additionally, if geometric entities are required in the model (such as area and moment of inertia in beam elements) they are specified within this feature.
Load Cases:
This feature allows the user to specify the name and the nature of his loading case. He may specify which of the previously defined loads, constraints, etc. are to be used in this current analysis, thereby excluding the remaining items that have been defined herein. In other words, the user, within PATRAN, may define a large set of loads, constraints, materials, etc. He may then selectively use some of them to create various loading cases.
Fields:
Analysis:
This feature is used to create the remaining details of the modeling process before having PATRAN convert the model into an actual Finite Element data stream, which is then sent to an existing FEM code. In this feature the type of analysis is specified. The load case is chosen. The FEA bandwidth optimizer is chosen. The state variables that are to be calculated and displayed are chosen. Finally, the FEM code of choice (MARC or ABAQUS) is selected.
Results:
Once the Finite Element analysis has been completed (external to PATRAN), the results of that analysis may be imported and the state variables in the solution may be displayed and evaluated. This feature then completes the usability of PATRAN as a model developer and a solution evaluator.
Insight:
XYPlot:
The Main Icon Menu
As in the description of the top icon menu, the user may illustrate the
function of each of the following icons by placing the cursor upon that icon.
AA - Polygon Pick (Polygon):
When the program requires the user to select either a region or set of nodes or a set of elements and that region is rectangular, the selection process by using the cursor and the mouse is simple. However, when the region to be selected is irregular, the use of this icon makes the process of selection tractable. The use of this feature and rectangular mouse picking will be described in the example, which is presented at a later portion of this tutorial.
BB - Mouse Rotate XY (X Y):
There are times when the user would like to rotate the display of the model for better viewing or in order to apply loads and/or boundary conditions. If the rotation that is desired is about either the X axis or about the Y axis, then this icon is to be used in the following way. Click on the icon with the left mouse button. Move the cursor to the display. Hold the middle mouse button and drag the mouse until the figure is in the desired orientation.
CC - Mouse Rotate Z (Z):
Using the same strategy as the previously described button, rotate the figure about the Z-axis.
DD - Mouse Translate XY (Up Arrow and Right Arrow):
Using the above procedures, the use of this icon allows the user to translate the display within the X-Y plane.
EE - Mouse Zoom (Two Arrows and a Box):
Clicking on this icon and following the above procedures, the display may be zoomed in or out by moving the mouse cursor.
FF - Zoom Out (Block + Left/Down Arrow):
Clicking this icon with the left mouse button causes the display to zoom out (i.e. get smaller).
GG - Zoom In (Block + Up/Right Arrow):
Clicking on this icon with the left mouse button causes the display to
zoom in (i.e. get larger).
HH - View Corners (Corners as in a Picture Frame):
The use of this icon is to obtain a full screen view of only part of the display in order to obtain a more detailed view of that area. Click on the icon with the left mouse button. Bring cursor to the region of the model that is desired. Hold the left mouse button and drag the mouse to form the rectangular region to be magnified. This icon is used when applying loads and/or boundary conditions. This icon is very useful and will be used often during the construction of the model.
II - Fit View (Multiple Arrows):
Clicking on this icon resets the display so that the entire model fits in the viewport.
JJ View Center (A Circle with a Cross):
Clicking on this icon sets the center of the viewing area. This icon is seldom used.
KK - Wireframe (Box with Hidden Lines Showing):
When constructing a model, it is sometimes desirable to see all of the lines so that even lines that normally would be hidden are displayed. Clicking on this icon will produce this result.
LL - Hidden Line (Box with Lines Hidden):
This icon does exactly the opposite of the previous icon by producing a display where all of the hidden lines do not show. This makes the display easier to understand than when using the previous icon. Click on this icon to produce a hidden line plot.
MM - Smooth Shading (A box that is crosshatched):
For display purposes, clicking on this icon produces a display that is color filled and shaded for easy viewing. This use of this icon is usually reserved to produce a plot for presentation, but is not very useful in model construction.
NN - Model Center (Box with a cross inside):
OO - Front View (Normal X-Y-Z Arrangement):
Clicking on this icon shows the front view of the model in the default X-Y-Z coordinate system.
PP - Rear View (Reversed X-Y-Z Arrangement):
Clicking on this icon displays the rear view of the model.
QQ - Top View:
Clicking on this icon produces a top view of the model.
RR - Bottom View:
Clicking on this icon produces a bottom view of the model.
SS - Left Side View:
Clicking on this icon produces a left side view.
TT - Right Side View:
Clicking on this icon produces a right side view.
UU VV- WW XX - ISO View 1 2 3 4 (Isometric Views of the axes):
The next four icons (moving left to right) produce various isometric views of the model. The user is encouraged to use these views to evaluate their differences. The orientation of the axes will inform the user as to which view is being produced.
YY - Show Labels (Box, Number and an arrow, which faces Northeast):
When constructing the model, especially the geometry phase of the construction, it is often useful to have the points, the lines, and the surfaces shown using their numerical labels (assigned by PATRAN). Clicking on this icon produces the revelation of these labels.
ZZ - Hide Labels (Box, Number and an arrow, which faces Southwest):
This icon reverses the effects of the previous icon when activated.
AAA - Plot/Erase form (Display Menu) (Pencils):
This icon is extremely useful. The purpose of this icon is to temporarily erase portions of the display so that the remaining part of the model is accessible for applying loading conditions, adding elements, etc. For example, suppose one had a closed vessel such as a bowl. The user desires to apply internal pressure to this model. When the entire model is shown, this pressure cannot be applied to the nodes on the faces of the inner surface of the bowl since they are not visible. With the Plot/Erase icon, the user can hide some of the model so that he may then look inside the bowl and apply the loads. The erasing or "hiding" is only temporary for display purposes only. The user may restore his entire model a t any time. This icon is one of the most useful features of PATRAN and makes this software one of the most robust of its kind. Specific use of this icon will be described in the example problems that follow below.
BBB - Label Control (Large L):
CCC - Point Size (A Large and a Small cylinder):
DDD - Node Size (Large and Small Diamond with a Cross):
EEE - Display Lines (Box with a Grid and one without):
Part I
The Soup Cup
You have now launched PATRAN, have studied the menus and the icons and are ready to do the important work of designing your part in order to perform a Finite Element Analysis.
Before using PATRAN, you should make a sketch of your part so that the modeling will proceed in an efficient manner. The design goal in this tutorial is to model a COFFEE CUP, convert the geometric description into an FEM and create a data file that can be used by a particular code (e.g. MARC). Since the geometry of the cup is somewhat complex due to the existence of the handle, the part will be designed in two stages. First, a soup cup will be created. Subsequent ly, a handle will be added to convert this part into the coffee cup.
We begin the design process with a sketch of the overall cup (see figure 5). The dimensions of the desired cup are shown. It should be noted here that, since this tutorial is for demonstration purposes only, some license will be taken with the design. In other words, when feasible, some of the dimensions may be modified. In an actual design, this cannot be done since the design will depend on the exact dimensions.
The creation of the soup cup has two aspects to be considered. There is the geometric consideration, in which the shapes and the sizes of the various components of the part are created. Secondly, this geometry will have to be converted into Finite Elements for analysis. It is, therefore, the opinion of this author that the user ought to keep the geometric entities separate from the FEM components. In this light, we begin our journey by creating a group that will contain only geometry. We do this by
Group --> Create
A menu will appear on the right side of the screen. In that menu you should delineate
New Group Name --> soup_geom --> Apply --> Cancel
You have created a group called soup_geom. This name should appear at the top of the display screen. This indicates that this is the group that is currently active and will accept the geometric description.
It becomes easier to work in this environment if the labels are visible. Thus, you want to "click" on the icon that will SHOW LABELS. You are now ready to create the geometry of the cup. Thus, please click on the item GEOMETRY on the main menu. A sub menu will now appear that looks like figure 6.
You are going to create the geometry of the base of the cup. This will entail the creation of two circles. The outer circle will, eventually, be the outer surface of the cup while the inner circle will be the inner surface. One of the ways of creating a circle is to denote the center of the circle and the radius. There are many other ways of specifying a circle, but the aforementioned technique will be employed. Using the menu that is shown, values must be assigned to their proper location in the menu. The steps to be executed are:
Action: Create
Object: Point
Method: XYZ
Point Coordinate List: [0 0 0]
Apply
In this tutorial, the chosen method of displaying these commands shall be
Create --> Point --> XYZ --> [0 0 0] --> Apply
Most of these parameters are defaulted in the existing menu. Only the values that deviate from the above need to be changed. When the Apply button is pressed, the display should show a point with the number 1. You have now created your first geometric entity, a point, and it is the first point in the model. With this point, you can now create the two circles. A circles is considered a CURVE by PATRAN. Thus, the entities that must be activated are
Create --> Curve
Also, where the word POINT appears, the user should click on that button and select
2D Circle
from the next menu that appears. The radius of the first circle should be set to 1.75, the center point should be set to [0,0,0]. The button called Apply should now be pressed. A circle should appear in the display. The inner circle is created in the same manner except for the radius, which is now set to 1.525. Pressing the Apply button yields an inner circle. Your display should now look like figure 7.
PATRAN cannot mesh these curves until the region between these curves is converted to a series of surfaces. Basically, we desire to create two surfaces that can be meshed. In order to accomplish this task, we will "break" each curve (inner and outer circles) into two distinct curves, respectively. From the same GEOMETRY menu that we have been using, choose EDIT instead of CREATE. Choose CURVE. Choose BREAK. Another menu will now be displayed from which you choose
POINT --> PARAMETRIC--> 0.5
We are subdividing the circles into two parts and telling PATRAN to do it parametrically instead of using a point that we may specify. The user should now
Touch the outer circle with the cursor --> YES to the delete question.
Touch the inner circle with the cursor --> YES to the delete question.
You have now created four arcs from the original two circles and have deleted the original curves. To see the four individual arcs, the user can touch each arc with the cursor and watch the color of the display for that entity. In order to facilitate the next tasks, let us refer to these four arcs as, outer left, outer right, inner left, and inner right. We now wish to convert these curves into edges of surfaces so that they can be "meshed". Figure 8 shows the GEOMETRY menu with the proper parameters to accomplish this task.
CREATE --> Surface --> Curve
Starting/Ending Curve --> Touch the outer left arc and then touch the inner left arc.
Next, click the "smooth shaded" icon on the icon menu to produce figure 9.
Starting/Ending Curve --> Touch the outer right arc and then the inner right arc
Next, click the "smooth shaded" icon to produce figure 10.
We now want to create a surface within the inner circle.
Starting/Ending Curve --> Touch the inner left arc and then touch the inner right arc
PATRAN will warn of a degenerate surface --> OK
Click the "smooth shaded" icon to produce figure 11.
Click on the icon "wireframe" on the icon menu to produce figure 12.
You have produced surfaces on the region that will eventually become the bottom of the cup.
You are now finished with the geometry of the bottom of the sup cup. We will use this geometry as the basis for constructing the rest of the bowl.
We will now desire to mesh the constructed geometry to produce a 2D finite element mesh (and eventually a 3D mesh). Thus, in keeping with our philosophy of keeping the geometry and the FEM separate, we must now create a new group by
Group Create --> New Group Name --> soup_fem --> Apply --> Cancel
The top of the display should indicate that the group "soup_fem" is the active group. The user will note that the geometry is still visible. This is because both the soup_geom group and the soup_fem group are posted, although only the soup_fem group is active at this time. It is at this point that the point, curve, and surface labels are no longer required. In fact, they tend to confuse the user in subsequent tasks. Thus, click on the icon to HIDE LABELS. The labels will no longer be visible. We are now ready to create a finite element mesh.
From the main menu, click on FINITE ELEMENTS. A menu will appear on the right side of the screen. You do not want to create a MESH SEED. You want to create a MESH. Therefore, you must obtain the menu that will allow you to create a MESH. Thus,
Create --> Mesh --> Surface
Will activate a menu that looks like figure 13. Since we only have a 2D surface at this point, you must choose the following options from the menu.
Element Topology: QUAD 4
Mesher: PAVER
Global Edge Length: 0.2
You have chosen to create quadrilateral elements that have 4 nodes. You will be using the PAVER meshing option since this seems to create a nicer mesh than the ISOMESHER when circular boundaries are present.
You must now choose the surface(s) that are to be meshed. Click the mouse in the "Surface List" box on the menu to prepare PATRAN to accept the chosen surfaces. Highlight the entire screen by "Pressing and holding the left mouse button while dragging the mouse over the entire display. The color of the display will change. Next, click the Apply button on the menu to produce figure 14.
You have now created a 2D finite element mesh of the bottom of the cup. We will now convert this mesh into a 3D solid element mesh to form the actual bottom of the cup. We do this by "extruding" the 2D mesh into a 3D mesh. Click on the following buttons
Action: Sweep
Object: Element
Method: Extrude
A small menu will become active to the left of the menu that you have been using. What is now visible is a menu that is similar to, but not exactly like, figure 15. The number of extrusions will be 1 (to be chosen on the left menu). On the right menu, choose
Extrude Distance: 0.25
You have just chosen the thickness of the base to be 0.25 inches. To select which elements are to be extruded, click on the "Base Entity List" box. Highlight the display as previously described using the mouse. The color of the display will change. Then click on the Apply button. In order to see the results of this extrusion operation, activate the "1st ISO View" icon on the main icon menu and then the "Hidden Line" icon to produce figure 16. You have now created the base of the cup.
We now want to create the sides of the cup. Therefore, we must first return to the front view of the model. Click on the "Front View" icon to achieve this view. Figure 17 results. We will create the sides of the cup in a similar manner to our producing the bottom of the cup, namely extrusion. In this instance, however, we will only want to extrude the outer layer of elements in the current model. Therefore, we must "hide" the elements that will not be extruded. We come to one of the most powerful features in PATRAN, the PLOT/ERASE feature. We desire to temporarily hide the inner elements in the display so that we can work on the outer ones, only. We do not want to erase these inner elements, just hide or deactivate them. Thus, choose PLOT/ERASE from the main icon menu. Click in the Entity box to prepare the code for the elements that will be hidden. Since the region that is to be "erased" is not rectangular (it is a circle), a simple mouse action such as highlighting the region with a rectangle, will not work. Instead, we must find a means of identifying the region in a non-rectangular manner. The icon POLYGON PICKING is available for this purpose. The actions of this icon have been described in the section, which delineated the icons. Therefore, just a brief procedure will be described here. It has been the experience of the author that the following process is difficult to master initially from a dexterity point of view. However, once the user has performed this operation a few times, the process becomes simple. Please refer to figure 18 during this discussion.
Click: Polygon Pick Icon
Starting anywhere on the second layer of elements (point 1), click the left mouse button. Next, drag the mouse to the next location, as shown. A line should be produced which indicates the path (see figure 18) . When you arrive at a point where you desire to change direction, click on the left mouse button. Repeat this process, until the entire inner region of the display is chosen as in figure 18. When you arrive at the last point N, double click on the mouse button to end the picking process. The elements which you have "picked" should change color. Return to the PLOT/ERASE menu and click on the ERASE button. Choose the RESET GRAPHICS icon and then the REFRESH GRAPHICS icon before choosing the OK button to end the hiding of the elements. Figure 19 should be produced.
You now wish to extrude the resulting outer layer of elements to produce the sides of the cup. Choose
Finite Elements --> Sweep --> Element --> Extrude
Extrude Distance = 3.75
Offset 0.25
Mesh Control: Number = 10 --> OK (on the left menu)
Base Entity List --> Mouse Choose the entire visible display --> Apply
You have chosen to extrude the elements that are shown through a distance of 3.75 inches starting with an offset of 0.25 inches (since the thickness of the base was already created and must not be repeated). You have chosen to produce 10 layers of elements. After choosing ISO View 1 from the icon menu, your display should appear as in figure 20.
It is now time to "unhide" the elements. Choose PLOT/ERASE and click on the PLOT ALL POSTED FEM --> OK. After choosing to return to the front view, you should see figure 21. If you choose the ISO 1 View and choose the Hidden Line icon, you will produce figure 22. You have now produce a three dimensional finite element representation of the soup cup. However, you now have both quad4 elements and solid hex elements coexisting. This cannot be allowed to remain in the model. Therefore, it is now time to delete the quad elements since they have served their purpose and are now longer needed. To do this, activate the following sequence
Finite Element --> Delete --> Element
On the left menu, click on the icon that represents quad elements
Element List --> Choose the entire display. Only the quad elements will be highlighted.
Apply
In order to complete the model creation, several more details remain. First, we will choose the physical constraints on the cup. In any finite element analysis, rigid body motion must be eliminated or a singular matrix will be created. In order to suppress the rigid body motion, we now go to the main menu and activate the Load/BC menu. Also, by clicking on the 4th isometric view icon, figure 23, which shows the bottom of the cup, is produced. Since we only want to "tie down" a few nodes on the bottom surface of the cup, and the actual nodes are not important, we will choose several nodes arbitrarily. In order to do this, activate the Zoom icon menu and then use the mouse to highlight the region that will be relevant (see figure 24). We must now invoke the following series of events
Action: Create
Object: Displacement
Type: Nodal
New Set Name: Fixed
on a menu that looks like figure 25. To set the data that is associated with the "fixed" data set, click on the Input Data icon, which will activate a left menu. On this new menu, choose
Translations --> <0 0 0>
OK
You have chosen the displacements to vanish in all 3 coordinate directions. You must now Select Application Region to specify which nodes belong to the "fixed" data set. From a small menu that appears at the left, choose FEM . This tells the code that you will be selecting finite element quantities (instead of geometric quantities) for your set. You may now choose several nodes (say 8) on the bottom of the cup. After each selection, hold the SHIFT key so that the next node is added to the previously chosen nodes.
Select Nodes
Add
OK
Apply
Fit View
Figure 24 shows these results.
The materials and the material properties must now be selected. First, reset and refresh the graphics. Next, choose the Materials menu from the main menu. The submenu that is shown should look like figure 26. Choose
Create --> Isotropic --> Manual Input
Material Name: Ceramic
To specify the material parameters, click on Input Properties which will activate a menu that looks like figure 27. Choose
Elastic Modulus: 10E+06
Poisson's Ratio: 0.3
Coeff Thermal Expansion: 0.3E-06
Reference Temperature: 70
Apply
Cancel
You have now created a material called Ceramic with the properties above. You must now apply this data to the actual model. From the Main menu choose PROPERTIES. A menu that is similar, but not exactly like figure 28 appears. Then the following sequence of events must be initiated
Properties --> Create --> 3D --> Solid
Property Set Name --> Ceramic
Input Properties
Click on Ceramic --> OK
Select Members --> Solid Element (Menu on the left)
Choose entire model with the mouse (display will change color)
Add
Apply
Choose the Hidden Line icon if the display does not exhibit hidden lines.
It is now time to create a Load Case by selecting this item from the Main menu. Figure 29 shows the resulting submenu. Follow the procedure
Load Cases --> Create
Load Case Name: Soup
Assign/Prioritize Loads/BC:
A new menu appears (on the left) that has all of your loads and/or boundary conditions that were selected to this point. In our case, only the fixed displacement has been chosen.
This will appear as Displ_fixed in the left menu. Choose it by clicking on the item.
OK
Apply
You have modeled the part, have applied boundary conditions, and have selected material properties and are ready to produce a finite element data file for MARC. First, however, we must clean up our model. The following set of steps should always be done in any modeling case before taking the final step of creating a finite element data file. We are now about to equivalence all of the nodes and the elements in the model to eliminate the possibility of having create " loose" quantities that are not associated with any other quantity. Also, we will renumber both the elements and the nodes so that they are in sequential order starting from 1 until the maximum number of that quantity. This must always be done.
Returning to the Finite Elements menu, choose the parameters that are shown in figure 30, namely
Finite Element --> Equivalence --> Apply
If a message occurs that tells the user that the default tolerance is too large and will result in elements being "fused" together, then a smaller tolerance (see figure 30) must be chosen.
In order to renumber the elements and the nodes, please refer to figure 31.and do the following
Finite Element --> Renumber --> Node --> Nodal List --> Highlight entire model with the mouse --> Apply
The results of this operation should be # of Nodes = Total in Model =1784
Finite Element --> Renumber --> Element --> Hex Element (on left menu) -->
Element List --> Highlight entire model with the mouse --> Apply
The results of this operation should be # of Elements = Total in Model = 903
The user should now refresh and rest the graphics. We are now ready to produce an analysis deck for MARC. This is done by choosing Analysis from the Main menu. You must now tell PATRAN what you want to be included in the data set that is to be produced. Figures 32 33, 34, 35, 36, 37, and 38 are relevant to this task. Please refer to the appropriate figure when carrying out the following steps
Analysis --> Entire Model --> Analysis Deck
Solution Type: Linear Static --> OK
Select Load Cases --> soup --> OK
Solution Parameters --> Optimize Bandwidth --> Cuthill-McKee --> OK --> OK
Output Requests --> Element Output Requests -->
Stress
Stress Equivalent Von-Mises
Temperature, Element --> OK --> OK
Apply
A message "Generating input for MARCK6" will appear and the use of PATRAN will be suspended as indicated by RED light on the top line. During this process, several warnings may be issued. Just click OK in the warning box . When the data creation process is finished, the light will turn GREEN and the display will be restored. You have now created a soup cup and produced a MARC finite element file. At this point, the user should exit from PATRAN and open the data file that was produced. We will return to the code later to add a handle to the soup cup which will convert it to a coffee cup. To exit, use the FILE menu and click on QUIT.
Figures 39 and 40 are an abbreviated (to save space here) of the MARC data file called soup.dat. It contains the finite element topology, the material properties and the fixed nodal constraints. All that would be needed to execute a finite element analysis using MARC would be the inclusion of thermal and/or structural loading data. This could have been done in PATRAN or can be included now by referring to the MARC manuals that are available.
Part II
The Coffee Cup
Hello and welcome back. We would now like to convert the soup cup of the previous example into a coffee cup by adding a handle to the above model. This seemingly simple idea requires a considerable amount of expertise when using PATRAN. To a void destroying the wonderful model of the soup cup that was created above, let us copy the file into a new file, which we shall call coffee. Please issue the following command
cp soup.db coffee.db
We now relaunch PATRAN by typing patran. The commands that follow are the same as the ones which were used in the soup example. The only exception is that now, a database (.db file) called coffee.db already exists. Thus,
Enable NFS Access (do not forget this or you will be very unhappy)
OPEN --> coffee.db
To begin the process of adding a handle, click on the Bottom View icon on the icon menu. Your display should look like figure 41. We must now create groups for the handle just as we did for the cup. Thus,
Group --> Create --> New Group Name --> handle_geom --> Apply --> Cancel
We have created a group that will contain the geometry of the handle. The top of the display screen should now show that the active group is the handle_geom. We now will pick certain nodes from the cup and have them form the basis of the construction for the handle. Using the PLOT/ERASE feature with creative use of the mouse and POLYGON PICKING, a small region of the cup is left visible with the rest of the model being hidden. Figures 42 and 43 show the portion of the cup that needs to be selected. Figure 42 is a front view while figure 43 is an isometric view. Figure 43 also shows the region of nodes (highlighted) that will serve as the basis for the handle construction. Then, after selecting the Geometry menu, the following steps are taken
Create --> Curve
There are only Nodes in the soup cup. Therefore, you will use these nodes to help create the handle. You will use some of these nodes which exist on the cup to form the curves that will eventually be the geometric envelope of the handle.
Therefore, select Node (from the menu that appears to the left)
Successively choose 2 contiguous nodes until a box of 8 lines is created. Please see figure 44. Now let us only show the selected handle geometry.
Group --> Post --> handle_geom --> Apply
Figure 44 should be on your screen. We now want to create surfaces from these lines (curves).
Create --> Surface
Touch the upper and then the lower lines to create figure 46. Figure 47 is a magnification of figure 46 that was created using the Fit View icon. By clicking the Shading icon, the surfaces that were just created are shown. We are now ready to mesh these surfaces. Thus, we must create a new group called handle_fem
Group --> Create --> handle_fem --> Apply --> Cancel
Then, after ensuring that this group is the default group at the top of the display window, click on the
Finite Elements
Create --> Mesh --> Quad4 --> Global Edge Length = 0.2
Surface List --> Highlight the entire display --> Apply
We have created a mesh. We would now like to display the handle_fem on top of the soup_fem so that we can compare the alignment of these two groups. Since the handle is to be attached to the soup cup, it must line up with the cup FEA. Choose
Group --> Post --> handle_fem and soup_fem (use CNTRL to select both)
The choice of the icon Bottom View creates a display like figure 48. We will now extrude this 2D finite element model into a 3D model. Issue the commands
Finite Elements
Sweep --> Element --> Extrude (2-D Elements on left menu)
Number = 5 --> OK (on left menu)
Direction = [0,1,0]
Distance = -1.375
Base List --> Grab the entire model with the mouse (only the new elements will highlight since these are the only quad elements that are currently in the display)
Apply
Hidden Line
ISO View 3
Will produce figure 49. We have just extruded the 2D FEM in the y direction for a distance of 1.375 inched and produced 5 layers of solid elements. In order to create the bottom portion of the handle and make it identical to the recently created upper portion, we must have only the handle FEM available to us. Thus,
Group --> Post --> handle_fem --> Apply --> Cancel
Finite Elements
Transform --> Translate --> Element
Hex Element ( on left menu)
Vector = [ 0 0 2.250 ]
Repeat = 1
Mouse pick the entire visible model --> Apply which results in figure 50.
We have translated and copied the upper portion of the handle into a lower portion of the handle. The menu that is used for this purpose is shown in figure 51. Let us now see the combined models of the cup and the presently existing handle.
Group --> Post --> handle_fem and soup_fem
Figure 52 is the result. We would like to add the vertical portion of the handle at this time. To post the handle_fem only
Group --> Post --> handle_fem --> Apply --> Cancel
We will only work with the lower portion of the handle so that we must PLOT/ERASE the upper piece of the handle (see figure 53). The vertical portion of the handle will only come from the front layer of elements in the handle. Thus, we continue to use Plot/Erase until the portion of the model that is shown in figure 54 remains. You may have to click on the Hidden Line icon to get a clear picture. Then the vertical portion of the handle is created by extrusion
Finite Elements --> Transform --> Translate --> Hex Element
Vector = [ 0 0 0.375 ]
Repeat = 5
Element List --> Highlight entire display --> Apply
Figure 55 is created. To view the entire handle model now, we post ALL FEM in the Plot/Erase menu. Figure 56 results.
We must now delete the quad elements from the model as previously explained. Then, click on
Finite Elements
Delete --> Elements --> Quad Elements (left menu)
Grab the entire model. Only the quad elements will highlight.
Apply
We now desire to view the entire coffee cup model.
Group --> Post --> handle_fem and soup_fem (remember CNTRL)
Apply
Cancel
The model is shown in figure 57.
Since the coffee cup was constructed in parts (soup then handle), there is no connection between the nodes of the handle and the nodes of the cup. We have to provide that connection by equivalencing the entire model. After this task, all of the nodes and the elements must be numbered so that they are in sequence.
Finite Elements --> Equivalence --> Apply
Finite Elements --> Renumber --> Nodes
Grab entire model --> Apply --> 1984 nodes
Renumber --> Elements--> Hex Element --> Grab entire model --> Apply -->
993 elements
Although the cup has material properties, the handle does not. We need to apply these properties just to the handle. However, eliminating the existing properties and applying them to the entire model is simpler. Note that we can only use this simplistic procedure because all of the materials are the same.
Group --> Post --> handle_fem + soup_fem --> Cancel
Properties --> 3D --> Solid
Input Properties --> Choose Ceramic which was created for soup.db --> OK
Erase all of the elements in the Application Region Box
Select Members --> Solid Element (Left menu)
Grab entire model --> Add --> Apply
Answer "Yes" to the overwrite question
A new load case must now be constructed.
Load Cases --> Load Case Name = coffee
Assign/Prioritize --> Loads/BC
Select Displ_fixed --> OK --> Apply
The final step in the process is the creation of an analysis data file for either MARC or ABAQUS. We follow the same steps as were previously used. These will be summarized here.
Analysis --> Analyze --> Entire Model --> Analysis Deck
Jobname = coffee
Solution Type = Linear Static --> OK
Select Load Cases --> coffee --> OK
Solution Parameters --> Optimize Bandwidth --> Cuthill-McKee --> OK --> OK
Output Requests --> Element Output Requests -->
Temperature, Element
Stress
Stress, Equivalent Mises
OK --> OK --> Apply
Once again a "generating input for MARCK6" message will appear and the light will turn RED. When completed, we can also create a data file for ABAQUS by,
Preferences --> Analysis --> ABAQUS --> OK
Analysis --> Analysis Deck --> Apply
The message will now say "generating input for ABAQUS". When completed the user may exit from PATRAN by
File --> Quit
We are done with the models. There should be two new data files in the current directory. A coffee.dat which is the MARC data file (figures 58-59) and an ABAQUS data file (figures 60, 61, 62).
Part III
Postprocessing
Now that the coffee cup has been designed and constrained, a Finite Element Analysis should be performed using either the MARC data file or the ABAQUS file that were created in the previous section. In order to do this, thermal boundary conditions would have to be added to the existing data files to simulate the liquid, the convection effects and the solid-fluid interface. This is a difficult process, which would not aid in the study of PATRAN.
Therefore, this author has decided to create a much simpler model, conduct an FEA, and create an output results file in order to discuss how PATRAN can be used to postprocess the results of the FEA. A cantilever beam that is subjected to a concentrated end load was chosen for this purpose. It is immaterial which FEA software package is used for the analysis as long as the output results file is compatible with PATRAN's requirements. Both MARC and ABAQUS satisfy these criteria. In the example that is given herein, MARC was used as the analysis tool and the resulting output file, called cantilever.t16 was produced. The actual meaning of this type of output file along with other MARC considerations will be the subject of another tutorial in this series. Let it suffice to declare that a MARC output file with an extension of .t16 or .t19 contains the values of the state variables that were requested by the user when the modeling phase was conducted. Typical output quantities that are requested in a structural problem are Von-Mises Stress, Strain, and Temperature.
In order to postprocess the results of an FEA using PATRAN, we follow several of the steps that have been used in the previous sections. Therefore, the steps that we will follow will be described in an abbreviated manner until we arrive at the actual postprocessing phase of the procedure. The following steps are now performed.
rlogin merlin
password
setenv DISPLAY hemo:0.0 (remember case sensitive)
cd to directory
patran
O.K. to warning
File --> New --> Enable NFS Access
New Database Name: results.db --> OK
OK to Warning
New Model Preferences --> Analysis Code --> MARCK6 --> OK
We have a file called model1_cantilever.t19, which exists, in the current directory. On the Main Line, choose Analysis. In the menu that appears on the right, choose the following
Action: Read Results
Object: Both
Method: Translate
Select Results File:
At the top of the menu, change the file type from .t16 to .t19
Filter
Choose model1_cantilever.t19 --> OK --> Apply
Yes (to question)
At this point, the Red and/or the Blue Button will be activated which renders PATRAN unavailable to the user. After the software reads the results file, and you answer OK to a warning message, you have arrived at the point where you can study the output results from the FEA.
You have chosen the MARC output file called model1_cantilever.t19, which was produced after the FEA. You have also instructed PATRAN to read the results so that they may be studied.
In order to display the results, return to the Main Line and choose Results. From a menu that appears on the right, choose
Cantilever
INC. = 1
TIME = 1
Select Displacement for Fringe Plot Result
Select Displacement for Deformation Result
Select Y component for quantity
Apply
You have chosen the results from FEA increment 1 and time 1. You desire to see the y deformation of the part with a color contour key to identify the values of the quantities. Figure 63 is the result of this procedure.
Finally, in order to see the stress variations in the cantilever beam, you must activate the following series of keystrokes to produce Figure 64.
Select Stress, Equivalent Mises --> Apply
If the reader is brave enough to click on Animate --> Apply then the beam will undergo a vibration in the mode shape that is compatible with the static deformation. When the user wants to stop the animation, just click on Stop Animation.
Although this section which describes the postprocessing of an FEA output file is somewhat abbreviated, it actually covers most of the keystrokes that are required to process any file. The author feels that the rest of this section is intuitive. In actual results files that are produced by complex FEA models continuos application of the above methods will lead the user to plots of all of his state variables. The user is encouraged to try several of these methods on an output file of the users choosing.