USER MANUAL FESAWIN 4.0
Revision 4.0.0

Table of Contents

1.0 Introduction

> > 1.1 General
> > 1.2 Description of Finite Element Analysis
> > 1.3 Description of FesaWin
> > 1.4 Technical Information

> > > 1.4.1 Elements
> > > 1.4.2 Stress Convention
> > > 1.4.3 Files

2.0 Controls

> > 2.1 Mouse actions
> > 2.2 Main Menu

> > > 2.2.1 File
> > > 2.2.2 Edit
> > > 2.2.3 Select
> > > 2.2.4 Add
> > > 2.2.5 Define
> > > 2.2.6 Setting
> > > 2.2.7 View
> > > 2.2.8 Analyze
> > > 2.2.9 Post-Process
> > > 2.2.10 Info

> > 2.3 Command line

3.0 Creating and Analyzing a model

> > 3.1 Analysis setup

> > > 3.1.1 Units
> > > 3.1.2 Type of analyses
> > > 3.1.3 Declare workspace

> > 3.2 Placing elements

> > > 3.2.1 Defining element groups
> > > 3.2.2 Single element placement
> > > 3.2.3 Patching and Meshing

> > 3.3 Defining boundary condition
> > 3.4 Analyzing model
> > 3.5 Post-processing

4.0 Element description

> 4.1 BARDTwo Nodal Axial rod element
> 4.2 BEAM Two Nodal Beam Bending Element
> 4.3 TRIM Three Nodal Membrane Element
> 4.5 PLARD Four Nodal Thin plate bending element
> 4.6 QUARS Four Nodal Stress based Membrane Element
> 4.7 TPLRS Four Nodal Thick plate bending element
> 4.8 SPRING One node user defined Flexible support element

1.0 Introduction

> 1.1 General

> This manual describes how to use FesaWin for Finite Element Analysis (FEA).
> The Manual is divided in four chapters.

> Chapter 1, INTRODUCTION
> This chapter will give the user a general description of FEA and FesaWin, and some technical information on the available elements and numerical method used.

> Chapter 2, CONTROLS
> To be able to work with the program, the user needs to know how to communicate with the program. Read this chapter or use it as quick reference.

> Chapter 3, CREATING AND ANALYZING A MODEL
> This chapter will tell you how to built a model and how to analyze and post-process it.

> Chapter 4, Element description
> Here all elements are described.

> The different controls of the program are referred to as follows:

> - Main menu [File,save…]
> - Button <left mouse button>
> - Frame or Form Title -Title-
> To get a general idea on how FesaWin works run the built-in model building and analyses demonstration. Start FesaWin, click on 'Info' and 'Run demo', [Info, Run demo...] .

> 1.2 Description of Finite Element Analysis

> The Finite Element method is an approximate numerical method in which an arbitrary shaped structure is divided up into small elements of various shapes, sizes and types which are assembled together to form an approximate mathematical model. In this method, a large number of equilibrium equations are formulated which are solved to obtain stress and displacement distributions.

> In order to do this, the engineer has to prepare the mathematical model and data which consists of model co-ordinates, material properties, loading and constraint conditions and types of elements adopted.

> 1.3 Description of FesaWin

> FesaWin is a Linear Static Finite Element stress analysis program, which includes modeling, analyzing and post-processing.

> In FesaWin a model is defined with the following components:

> 1) Elements
> 2) Nodes
> 3) Element property groups
> 4) Boundary condition

> The FesaWin interface also includes Graphical elements to help to built the model.

> Results of an analysis are presented in terms of:

> 1) Stresses
> 2) Displacements

> The program can handle more multiple loadcases and load combinations.

> The Graphical pre-processor enables the user to define a model by simple mouse clicks and/or by direct entering co-ordinates. There is also a numerical interface available taht enables the user to direct enter coordinates, element definitions and other data.

> The basis of FesaWin is that what you see is what you have. Elements need to be placed by the user either by direct placement of single elements or by generating patches from graphically defined surfaces.
> Modeling can start by dividing the structure into several four or three sided patches using graphical lines or circles. When this is ready the patches can be meshed with elements. These elements are assigned to a group. Each group of elements has one set of material and element properties. When this is done, the constraint condition should be applied by fixing some of the nodes of the model. Finally the required loadcases are created and nodal loads, element loads or extra masses are defined for each loadcase.

> Note: it is very important for the numerical solver of the equations that rigid body movements of the model are constraint. If not properly constraint the solver will stop and give you the following message: "The construction has a Mechanism".

> The analysis can be started. The model will be solved and the results are written in the database for each loadcase.

> After the analysis, load combination can be defined which are constructed from the previously defined loadcase. Each loadcombination can be reviewed graphically or written into a report file. Loadcombinations can be changed and modified without rerunning the analysis.

> The results of the whole model or a selection of elements can be visualized by contour plots of the stresses and deformations.

> 1.4 Technical Information

> 1.4.1 Elements

> The following elements are available:

> BARD Two Nodal Axial truss element
> BEAM Two Nodal Beam Bending Element
> TRIM Three Nodal Membrane Element
> QUA4D Four Nodal Membrane Element
> QUARD Four Nodal Rectangular Membrane Element
> PLARD Four Nodal Rectangular Plate bending Element
> TPLRS Four Nodal Rectangular Stress Based Thick Plate bending Element
> QUARS Four Nodal Rectangular Stress based Membrane Element
> SPRING One node user defined Flexible support element

> The following table presents the Degrees of Freedom (DOF) of the FesaWin elements:

> Name | Nodes | 2-D Analysis | 3-D Analysis
> |  | Local DOF | Global DOF | Local DOF | Global DOF
> BARD | 2 | x | x y | x | x y z
> BEAM | 2 | x y rz | x y rz | x y z rx ry rz | x y z rx ry rz
> TRIM | 3 | x y | x y | x y | x y z
> QUA4D | 4 | x y | x y | x y | x y z
> QUARD | 4 | x y | x y | x y | x y z
> PLARD | 4 | Not Valid | Not Valid | x y z rx ry | x y z rx ry rz
> TPLRS | 4 | Not Valid | Not Valid | x y z rx ry | x y z rx ry rz
> QUARS | 4 | x y | x y | x y | x y z
> SPRING | 1 |  | x y (rz) |  | x y z (rx ry rz)

> Table 1.4.1 Element Degrees of Freedom

> Chapter 4 presents the full description of the elements.

> The elements local axis are defined as follows:

> The order in which the nodes of an elements are defined determine the local axis of that element. The axis system is defined as follows:

> - The X-axis is defined from node 1 to node 2 for all elements types.
> - For three or four nodal finite elements the z-axis is pointing away from the viewer if the nodes are defined clockwise. The Y-axis is defined using the right hand rule.
> - For line elements the local Y-axis is perpendicular to the global x-y plane. If the element x-axis is paralel to the global z-axis, than the element local y-axis is parallel to the global y-axis.
> 1.4.2 Stress Convention

> > Line element stress convention:

> >     Sx     Axial stress (tension is positive)
> >     Sby    Bending stress  around local y-axes (Positive when outer fiber in local z-direction is in tension)
> >     Sbz    Bending stress around local z-axes (Positive when outer fiber in local y-direction is in tension)
> >     Sxy    Shear stress x-y plane
> >     Sxz    Shear stress x-z plane
> >     Stx    Tortional shear stress around x-axes

> >     Finite Element stress convention:
> >     Sx     Membrane stress x-direction (Positive for tension)
> >     Sy     Membrane stress y-direction (Positive for tension)
> >     Sbx    Bending stress around local x-axes (Positive when outer fiber in local z-direction is in tension
> >     Sby    Bending stress around local y-axes (Positive when outer fiber in local z-direction is in tension
> >     Sxy    Shear stress x-y plane
> >     Syz    Shear stress y-z plane
> >     Sxz    Shear stress x-z plane
> >     Stz    Shear stress x-y plane for plate elements due to bending

> >     Combined stress formula
> >     Combined stress has been based on the Von Mises formula, which is a yield criterion.
> >     For line elements the combined stress is calculated at the for corners of a square cross section, and
> >     the highest is reported.

> >     For Finite Elements (Membrane and plate bending) the combined stress is calculated at top and the bottom
> >     of the element, and the hightes is reported.

> >     The following formula is used:

> >     sc = (SX ^ 2 + SY ^ 2 + SZ ^ 2 - SX * SY - SX * SZ - SY * SZ + (SXY ^ 2 + SXZ ^ 2 + SYZ ^ 2) * 3) ^ 0.5

> 1.4.3 Files

> The following program files are used:

> > > Fesawin.exe Finite Element analysis Pre and Post Processor
> > > FesaWin.ico Icon
> > > Fesawin.htm User manual readable with internet Browser
> > > Eltyp.dat Element data file
> > > Eldes.dat Element description file
> > > Plat.elm Plate element data file
> > > Matsol.exe Model Solver (Can also run without Fesawin)
> > > Matsol.ico Icon
> > > License.dat License agreement Code
> > > Decmem.dat Memory settings
> > > Defaults.dat Saved program setting
> > > Section.dig Digital database with section property data
> > > Name.obj Object file containing definition of a standard object

> The following model files are used:

> > > Root.tek Model file with nodal co-ordinates, element definition and view settings
> > > Root.mlt Group file containing all the group; data material and element data
> > > Root.gra contains the graphic element definitions
> > > Root.vpl The constraint
> > > Root.knk The applied nodal loads
> > > Root.ell The applied element loads
> > > Root.lcd Loadcase information
> > > Root.lco Loadcombination information
> > > Root.rot Element Local Axis definition

> The following analysis files are used:

> > > Root.DAT Geometrical data file
> > > Root.MAT Upper triangle of unconstrained stiffness matrix
> > > Root.MAS Nodal Mass data
> > > Root.EMS Element Mass Data

> The following result files are used:

> > > Root.RVP Displacement data
> > > Root.KRT Reaction force data
> > > Root*.rpt Analysis report file

> > > Finite Element stresses;
> > > Root.NSR Global Nodal stress data
> > > Root.NSA Global Nodal stress average plot file
> > > Root.RSA Global Nodal stress average data
> > > Root.NSL Local Nodal stress data
> > > Root.NLA Local Nodal stress average Plot file
> > > Root.RLA Local Nodal stress average data

> > > Line Element stresses
> > > Root.LES Local nodal stress report

> 2.0 Controls

> This chapter presents all the controls the user has over the program.

> Figure 1 presents the look of the program interface. The interface is divided in a main menu, the views, the command line, the status line, the snap button and the selection box. The three fields next to the selection box are used for the x, y and z co-ordinates of a selected point. Each view has scroll bars, a zoom in <+> and zoom out <-> button, and an autoscale button <Auto> to fit the complete model into the view.

> > > > Figure 1: User Interface of Pre and Post-Processor.

> The main program controls are:

> > > Mouse actions
> > > Main menu or toolbar
> > > Command line

> The next sections describe these controls in detail.

> 2.1 Mouse and Key actions

> General,
> In most cases the mouse buttons will do:

> - Left button is select, do or perform
> - Right Button gives context sensitive pop-up menu
> - <ESC> is deselect, stop or go back
> - <Enter> will stop selecting and switch directely to the move mode
> The mouse action depend on the active mode of the program. At the status line, which is located at the left bottom of the main window, the model and the object on which the mode works is displayed.

> Select mode
> By default the program is in the select mode. What you select, is defined by the check marks on the selection menu .

> > During editing and adding objects it is important to realize what the active selections are. Some times when you want something to happen and it does not work, check the active selections, as this may be the source of your trouble.

> How you select it, is defined by the SELECTION box at the bottom of the screen. The following methods are available:
> - Single : Each item is selected by clicking on it
> - Window : All items inside the window are selected
> - Group : All items within one group are selected
> - All : All items are selected
> When the selection method is "Single", pointing at the objects and clicking with the <left mouse button> does the selection of the node or element.

> When the selection method is "Window", clicking once with <left mouse button> for the first corner of the window and another time for the opposite corner does the selection of the nodes and elements. Do not drag the window.

> When the selection method is "Group", clicking on one element which is part of the group of elements that needs to be selected does the selection.

> It is allowed to switch between selection methods during one selection session.

> The following table presents the possible selection methods per item:

> Table 2.1 Possible Selection combinations

> | Nodes | Elements | Graphics
> Single | + | + | +
> Window | + | + | +
> Group |  | + |
> All | + | + | +

> An item can be selected with <Left mouse Button>. Click <Right mouse Button> once to stop selecting and to select an option from the pop-up menu.

> To deselect a selection do <ESC> several time.

> Clicking on an item, which is already selected, will remove that item from the selection list.

> Always look at the Status Line at the bottom of the screen to see in which mode the program is.

> Move mode
> When the selection of nodes eloements or graphics is ready and move has been selected from the pop-up menu, the program will go into the Move Mode.

> Selected items can be moved either by mouse action or by the "command line".

> > Move by mouse action.
> > A selection can be moved by defining a reference node and a location to move to. All selected items will be moved by the vector spanned by the reference point and move to point. Look at the Status Line at the bottom of the screen for guidance with this feature.

> > When Drag/Drop is enabled [edit, drag/drop], nodes can be moved by holding down the <left Mouse Button> and dragging the selection to the new location.

> > The program can be forced to snap to the nearest node or graphic point. Use the <Snap on/off> button at the bottom of the main window to control the snapping during editing. When snap is on and a mouse click is too far from a node, snapping will not occur.

> > Move by Commands.
> > See section 2.3.

> Add mode
> The program is in the add mode when one of the items of the Add menu has been selected.
> During adding, existing nodes or graphics can be used to snap on.

> 2.2 Main Menu

> This chapter describes the options of the main menu.

> 2.2.1 File

> [New]
> This option will delete the model from memory and present a new empty work field.

> [Open...]
> This option will delete an existing model from memory and load a new model from disk into the memory of the program.

> [Import Model...]
> This option allows you to import another model or a CAD drawing and merge it with the current model in memory.

> To import another FesaWin model select *.tek in the filetype selection box.

> To import a CAD drawing select *.dxf in the filetype selection box.

> The imported model will be placed in the working memory of the current model as a pasted object. This means that after importing, the new part is still selected and can be moved, scaled, mirrored or deleted as any selection of elements and nodes.

> [Save...]
> This option will save the current model in memory on disk.

> [Print...
> The print option will send a plot of view 1 to the printer.

> [Save Settings]
> Program and view settings will be saved on disk in the file; defaults.dat .

> [Get Settings]
> To retrieve the saved settings

> [Model Size]
> This option presents a form that enables the user to define the maximum memory size that the program should reserve. These settings can be changed during a session. It is advised to check the declared sizes regularly as the program will crash when the model becomes bigger than the reserved memory allows. Use Main Menu: [INFO, Model Info...] to review the memory use of your model.

> Do not reserve too much space as this could reduce the speed of the program.

> [Exit]
> This will exit the Fesawin session.

> 2.2.2 Edit

> [Undo]
> The undo option is only available to undo moving of Finite Element nodes when they are still selected.

> [Delete]
> This option will delete the selected FE elements, nodes or graphic elements.

> [Cut]
> This option will copy and delete the selected FE elements, nodes or graphic elements.

> [Copy]
> This option will copy the selected FE elements, nodes and graphical elements.

> [Paste]
> This option will paste the copied elements and nodes and place them at the same locations as where they were copied from. As the pasted elements and nodes are still selected they can be moved by mouse action or by entering move commands at the command line .

> To deselect and accept the pasted elements and nodes press <ESC>. When "check node merge and element merge" is on, see [SETTINGS, OPTIONS…] , each node and element from the selection will be checked and doubles will be deleted.

> [Drag/Drop]
> When this option is Checked, graphic nodes and FE Nodes can be dragged and dropped.

> Note: Only begin and end nodes of the graphic elements can be dragged.

> [Modify Selection]
> This option can be used to modify or edit the properties of the selected items.

> It is advised to select one type of item for modification. Depending on the active selection the following modification can be done:

> Modify Finite Elements:
> This option presents a form, which allows modification of the group name and/or element type of a selection of elements. The definition of the local co-ordinate system can also be modified on this form.The local coordinate system can be rotated around the local z-axis or mirrored in the local x-y plane.

> > > - First select the elements which should be modified.
> > > - Do: [EDIT, MODIFY SELECTION…]
> > > - Set the selection criteria "element type" and "group name". Only the elements which meet these criteria will be modified.
> > > - Define the change action to be performed in the lower half of the form by choosing an option in the "element type", "group name" boxes or one of the axis modification options.
> > > - When ready press <APPLY> and the change will be performed.

> Modify Graphic Elements.

> This option presents a form, which allows modification of the graphic element properties of one or more graphical element. The fields on the form are described as follows:

> > > "Element ID"
> > > This field presents the identification number of the selected graphical element. If more than one graphical element is selected, this field will be a drop down box. The drop down box allows you to select one of the selected elements or the whole selection.

> > > "Element Type"
> > > This field can not be modified and presents the type of the selected element, which could be:

> > > - Line
> > > - Arc
> > > - Circle
> > > - Various (This appears when different types of graphics are selected)
> > > "Radius" or "Length"
> > > This input field allows you to modify the radius of a circle segment or the length of a line element.

> > > The selected end node of the line element will move when length is changed.

> > > The beginning, end point and plane in which the circle lies will not change.

> > > Note: if the is radius is chosen 20 times larger than the distance between the begin and end node, the element type will be changed to line. This is done to avoid confusion on the definition of the circle plane.

> > > 'Various' will appear in this field if multiple elements are selected with different radius

> > > "Nodes"
> > > This field controls the number of nodes on the graphical element. Minimum value is two, which are the beginning and end nodes. The intermediate nodes on a graphical element are snapable but can not be moved or edited individually.

> > > 'Various' will appear in this field if multiple elements are selected with different number of nodes.

> > > "Spaces"
> > > This field does basically the same as "Nodes", except that the input is number of spaces between the nodes, in stead of number of nodes. Minimum value is 1 (one). Relation with "Nodes" is: "Spaces" = "Nodes" – 1

> > > 'Various' will appear in this field if multiple elements are selected with different number of spaces.

> > > "Distribution Factor"
> > > This factor controls the distribution of the nodes over the graphical element. The factor is defined by the ratio between the first and last spacing between the nodes.

> > > 'Various' will appear in this field if multiple elements are selected with different distribution factors.

> [Refine Elements]
> This options refines the selected finite elements. Be careful as the refining can not be undone.
> [Numerical Interface]
> This options allows the user to direct enter the data for the model. The right window can be used to enter or edit the data. The left part of the window can be used as reference only.
> - All changes are directly written to the database in the program memory
> - To edit dubbel click and enter new value. Close by <Enter> or clicking on another cell.
> - To add a new record, dubbel click on cell at the NEW line, enter value and close cell.
> - Multiple selections is not yet available

> 2.2.3 Select

> The selection process, using the mouse is described in chapter 2.1

> This menu option controls which items are active for the selection process.

> [Nodes]
> This option should be checked when you want to select Finite Element Nodes.

> [Elements]
> This option should be checked when you want to select Finite Elements.

> [Graphic]
> This selection allows you to select graphic elements or nodes for editing.

> When checked, graphical elements can be selected. To modify a graphical element double click with the <left mouse button>, and a form will appear which allows you to modify the graphic element or select a graphic and do [EDIT, MODIFY SELECTION,...] .

> [Snap]
> This option will toggle snap on or off.

> 2.2.4 Add

> [Free Node]
> This option enables the user to place free finite element nodes.

> - Use <left mouse button> to place Finite element nodes
> - Use <ESC> to stop.
> - Direct entering the co-ordinates using the command line can also be used to place nodes.
> [Elements,…]
> This option enables the user to place individual elements.
> When selected, a form will appear which allows you to choose the element type you want to use and to which group these elements should be assigned.
> - Press <Add> to start placing elements.
> - <Left mouse button> to place element nodes.
> - <ESC> to stop placing elements.
> The element nodes can be placed by clicking with the mouse in the free space, by clicking on existing nodes, (Switch on Snapping !!) or by direct input of the coordinates using the command line .

> The order in which the nodes of an elements are defined determine the local axis of that element. The axis system is defined as follows:

> - The X-axis is defined from node 1 to node 2 for all elements types.
> - For three or four nodal finite elements the z-axis is pointing away from the viewer if the nodes are defined clockwise. The Y-axis is defined using the right hand rule.
> - For line elements the local Y-axis is perpendicular to the global x-y plane. If the element x-axis is paralel to the global z-axis, than the element local y-axis is parallel to the global y-axis.
> [Mesh]
> This option starts the mesh generation module.

> The first form is used to select between 2-D meshes or 3-D meshes.

> > Note: 3-D solid meshes are not included in this version of FESAWIN.

> The next form presents the 2-D mesh generator.

> The generator uses graphical elements as edges to define the borders of the mesh. Before using the generator define a closed area using graphical elements with three or four sides. A side may be constructed from several graphic elements as long as it is one closed string.

> Activate mesh generator

> - The first field defines the mesh type to be generated, the types are:

> > Quad
> > Four sided area which will be filled by four nodal elements, opposite sides should have equal number of nodes.

> > Triang
> > Three sided area which will be filled by three nodal elements, all sides should have equal number of nodes.

> > Line
> > Line which will be meshed with two nodal elements.

> > Transit
> > Four sided area which will be filled by four nodal elements. This option is not available.

> - The second field defines the element type to be used.

> - The third field defines to which group these elements should be assigned.

> The drawing in the second frame shows the order in which the edges should be defined.

> The buttons on the third frame can be pressed to select the graphical components of the edges.
> Each edge may consist of more than one graphical element. The order in which the graphics are selected is not important, but the edge should be continuously.

> When all edges are selected, the mesh can be generated by pressing <Generate Mesh>. Press either <Accept> to accept the proposed mesh or <Reset> to reject. The generator is ready to generate a new mesh after <Reset> or <Accept>. The proposed mesh is only showed in view 1.

> [Object...]
> Objects are predefined models (e.g. beam, plate or tubular), which can be sized using variables and merged into the model.

> <Load new Object>
> This button will allow the user to load a new object from file. The extention of the object file is .obj .

> When the object is loaded, the available parameters which define the object and the default values are shown on the form.
> Modify the values of the variables by selecting the variable and changing the value in the edit box below.

> <Show Object>
> Press this botton to show the object.
> You may change the variables and press this button again to see the effect.

> <Autoscale>
> To fit the whole model and object into the view press this button.

> <Accept>
> This will paste the object into the model at the default location of the object and will return you to the edit mode of the program.

> The position and orientation of the inserted object can be changed using normal edit functions.

> <Cancel>
> This will close this form without merging the object.

> [Constraints...] or [Loads,...]
> These options presents a form to modify or review the boundary conditions.

> The loads menu option also allows the user to choose for element loads or nodal loads.

> The first frame controls which nodes of the selection should be modified. If all nodes of the selection should be modified then choose "Selection". If you want to modify or review one of the nodes of the selection, select the node from the pull down box.

> Note: The numerical values of the boundary conditions are presented, when you select one individual node or element from the pull down box.

> The second frame present six or three fields to enter the values of the boundary conditions. For constrains the following rules apply:

> > > > - No constrain : Empty input field
> > > > - Fixed : Fill in a 0
> > > > - Prescribed displacement : Fill in value of displacement

> For loads the following rules apply:

> > > > - No Load : Empty input field
> > > > - Prescribed load : Fill in Value of load or mass

> If the active loadcase is an inertia loadcase than the numerical values will be interpreted as point masses.

> > > Loads can be defined per loadcase. Loadcases should be defined first before loads can be assigned. Use [Define, Loadcases...]to define the loadcases.

> > > When <APPLY> is pressed the boundary conditions of the selected nodes will be replaced by the entered values of the input fields.

> Constraints and nodal loads are both defined relative to the global coordinate system. Element pressure loads are defined relative to the element coordinate system. Do [Settings, Local axis] to see element local coordinate system.

> [Graphics, line]
> This option activates the adding line mode. Use <left mouse button> or command line to define the nodes of the line. By hitting <Enter> a new line string can be started. Use <ESC> to stop the adding line mode.

> A line is defined by one begin and one end node.

> To snap on existing nodes, switch on the snapping mode and be sure that the active select mode is correct. Any visible node can be snapped on.

> [Graphics, Circle]
> This option activates the adding circle section mode. Use <left mouse button> or command line to define the nodes of the circle section. By hitting <Enter> a new circle section can be started. Use <ESC> to stop the adding circle mode. Note: a full circle can not be made by one element, you should define two half circle sections to define a full circle.

> A circle section is defined by three nodes that may not coincide. The three nodes span the plane in which the circle section is situated. The first node is the starting point, the second node is the end of the circle segment and the third node defines the radius and the plain and lies on the circumferential of the circle between the begin and end node. Use [Edit, Modify selection,…] to change the radius of the circle segment.

> The third node can be selected and relocated by mouse action or command line.

> To snap on existing nodes, switch on the snapping mode and be sure that the active select mode is correct. Any visible node can be snapped on.

> [Graphics, Intersection]
> This function will construct an intersection of two non parrallel lines. If the two lines are not in one plane, than a line will be added at the shortest distance between the two line.

> [Graphics, Extend]
> This function will extend one or both lines to the intersection point or the point at the shortest distance between the two line.

> 2.2.5 Define

> [Group]
> This form is used to define the element group names and properties.

> -Group Name-
> To define a new group, press <Add> and enter the new name in the group name field. After modifying the group name field <Update> should be pressed to save the change. To delete a group press <Delete>.

> The element groups are also used as nodal stress average groups. This means that nodal stresses averages are calculated per element group.

> When "All Groups" is selected, any edit will be applied to all groups.

> To define Beam cross sectional properties use <section tool>. This tool calculates the cross sectional properties of tubulars and several other beams. Also a database of standard beams is provided. It should be remembered that only the results of these calculations are saved in the database. No reference to the database is saved.

> -Properties-
> The following properties are to be defined:

> - E modules : young modules of elasticity
> - Poisson ratio : Contraction coefficient
> - Specific Mass of used material.
> - Thickness | Area : Thickness for membranes and plate elements, Area for line elements
> - Select : Plane strain or plane stress: Valid for membrane elements
> - Local rotation : Angle between local z-axis and global z-axis for 3-D beam elements
> - I, W : Cross sectional properties of Beam elements on local co-ordinate system
> Use <Section Tool> to calculate the geometrical properties of various cross sectional area's.

> Press <Update> to save the new properties. If "All Groups" is selected, values entered in the property fields will be applied to all groups.

> Element properties of the Spring support element can be defined on this form after pressing <Spring>. The 6 x 6 stiffness matrix can be filled out on this form. The spring element only uses the properties of this matrix all other data of this group are ignored. Other elements will ignore the stiffness matrix.

> Table 1.4.1 presents the global degree of freedom that should be filled out for the spring support element. For instance, if a 2-D analysis is performed with only BARD of membrane elements, (Only x and y are included in the analysis), than the 2 x 2 upper part of the stiffness matrix should be filled out, see also table 2.2.1. Table 2.2.1 and 2.2.2 presents the stiffness matrix entries are used for each type of analysis.

> XX | XY |  |  |  | XRZ
> | YY |  |  |  | YRZ
> |  |  |  |  | RZRZ

> Notes: Only the upper triangular has to be filled out

> > > The green entries are only included in the analysis when a beam bending element is used.

> Table 2.2.1 Spring support matrix for 2-D analysis.

> XX | XY | XZ | XRX | XRY | XRZ
> | YY | YZ | YRX | YRY | YRZ
> |  | ZZ | ZRX | ZRY | ZRZ
> |  |  | RXRX | RXRY | RXRZ
> |  |  |  | RYRY | RYRZ
> |  |  |  |  | RZRZ

> Notes: Only the upper triangular has to be filled out

> > > The green entries are only included in the analysis when a beam bending or a plate bending element is used.

> Table 2.2.2 Spring support matrix for 3-D analysis.

> [Loadcase]
> This form will be used to define the loadcases.

> Loadcase number and loadcase name
> These fields presents the names and number of the defined loadcases. The name of the loadcase can be changed by entering the new name in the name field and pressing <update>.

> Loadcase type
> This field allows the user to choose the type of loadcase required. The following types are available:

> > Applied Loads
> > This loadcase type will allow the user to define nodal loads only. The loads should be defined using [Add, loads..] .

> > Intertia loadcase; Acceleration x,y,z
> > This loadcase type will allow the user to define acceleration loads in the global x,y or z direction. The acceleration value, as specified in the acc. field, will be used to calculate nodal loads based on the masses in the model. If "Element mass ON" is selected the element specific density, as defined for the element groups are included, multiplied with the specified acceleration and applied on the model as nodal forces for this loadcase. Additional point masses can be defined for this loadcase type by using the [Add, Loads...] option of the main menu.

> > Intertia loadcase; Rotation rx,ry,rz
> > This loadcase type will allow the user to define rotational acceleration loads around the global x,y or z axis. The acceleration value, as specified in the acc. field, together with the specified rotation center, will be used to calculate nodal loads based on the masses in the model. If "Element mass ON" is selected the element specific density, as defined for the element groups are included, multiplied with the specified acceleration and applied on the model as nodal forces for this loadcase. Additional point masses can be defined for this loadcase type by using the [Add, Loads...] option of the main menu.

> Important Note:
> Be consistence with the units of the model and accelerations of the defined loadcases. Table 3.1 presents examples of consistence stes of units.

> After any change press <update> to save the change.

> 2.2.6 Setting

> [Colors]
> This form allows the user to change the color settings of the program. To save the color settings for a next session, do [FILE, SAVE SETTINGS].

> [Font]
> This option allows the user to set the font properties of the node and element labels. To save the font settings for a next session, do [FILE, SAVE SETTINGS].

> [Scrollbar]
> To display the scrollbars check this option.

> [Global Axis]
> To display the global axis check this option.

> The global axis are displayed in the left lower corner of each view. The axis are color marked as follows:

> - x-axis Red
> - y-axis Green
> - z-axis Blue
> [Local Axis]
> Check this option to display the elements local axis systems. The axis are color marked as follows:
> - x-axis Red
> - y-axis Green
> - z-axis Blue
> [Options]
> This form allows the user to set various features of the program.
> File & Save
> Auto renumber before saving option can be controlled.
> After an analysis, the auto renumber option will be switched off automatically. This is done because model renumbering can make the analysis results invalid. After an Add command from the main menu, renumbering is switched on automatically again assuming that the model is changed.
> GUI
> Several auto-redraw options can be switched off. This can be usefull when workin with a large model.

> Modelling
> Option for finite element moddeling can be controlled.

> Hiddenline
> The hidden line options are presented on this form. Here the color, the intensity and the direction of the light source for shading can be set.

> [Symbols]
> This form allows the user to set the size of the symbols used by the program.
> Symbols are graphical icons used in the model.
> [Toolbars]
> This form allows the user to switch the toolbars on or off.
> The toolbars can be dragged using the mouse and placed anywhere on the screen.

> 2.2.7 View

> [View Set]
> This option shows a form, which controls the settings of the view.

> -View type-
> You can chose to display only one view or four views at the same time.
> <Copy>, <Paste>
> These functions can be used to copy and paste view settings from view to view.

> -View angle-
> These fields defines your view direction regarding the horizontal and vertical plane.
> The buttons on this frame sets four pre-defined view angle settings.

> -View point-
> These fields defines the point at which you are looking at through your view. When <AutoScale> is used the middle of the model will be set as the viewpoint.

> -View settings-
> This defines the scaling factor and your distance relative to the view point.

> The "Unit Vector Length" is a value between 0 and 2 which is used to size the graphics of the boundary conditions and the scale of the deformed shape plot relative to the view size. The view width and height is 10.

> <Autoscale>
> The autoscale routine sets the middle of your model as the view point and sets the scale to fit the model in the view.

> Click on the little views on this form to select another view.

> -Define Elements to view-
> Select one of the following options:

> * All Elements :All elements will be shown in the view
> * Group :Select one group of elements which should be shown in the view.
> * Selection :Press <Select> and select the elements that should be shown in the
> view, press <ESC> to stop selecting.

> It should be noted that Finite Element Nodes which are not connected to an element will not be visible and can not be selected when a selection of elements is shown. When <All Elements> are selected also all nodes will be shown.

> If you want to make one group invisible in a view work as follows:

> - Press <select>
> - Set selection method to "All"
> - Click in the view to select all elements
> - Set selection method to "Group"
> - Click on an element of the group which should be made invisible (This will remove that group from the selection)
> - Press <ESC>
> When ready press <OK>.

> [Redraw]
> This options redraws all views.

> [Nodes] , [Elements], …..
> This options controls if the attributes or objects are drawn.

> [Window]
> This option will allow the user to define a new view window by drawing a rectangular fence around a part of the model. The contents of the fence will be the new window. Follow the instruction in the 'Status Line' (Left Bottom of screen).

> [Hiddenline]
> Select this option to switch-on hiddenline.

> 2.2.8 Analyze

> [Check Model...]
> The check model form will help the user to find errors in the model. The following check can be performed:

> - Define elements to check -
> Here you can define which elements should be checked or modified.

> - Check local element axis -
> For the nodal stress average calculation each stress components of adjecent elements within an element group will be averaged in order to get a continues stress field. For a correct stress field it is paramount that the direction of the stress component of each element is similar or deviates only a little. The larger the angle between local axis of two elements the larger the error of the averaged stress will be.

> This check will show large differences per local axis by giving diffirent color shading to different directions.

> Press the buttons in the frame and check if any discontinuity of the element shading can be
> found within an element group which indicates that the local axis are not correctely defined.

> To correct by hand, select the element and do [Edit, Modify Element..] and change the definition of that element local axis until it fits better into the element group.

> To auto correct use the following two functions:

> <Modify>
> This option will change the element definition such that adjecant elements will have the smallest difference in local axis direction. This is done by changing the order of the element nodes.
> <Homogenize Axis>
> This option will change the local axis definition and will rotate the local axis such that adjecent element have similar local directions. This is done by offsetting the axis with an angle such that all local direction are similar.

> Figure 2.1. presents an example of a good defined mesh and a bad defined mesh.

> GOOD BAD

> Figure 2.1 Example of good local axis and bad local axis of two adjecent elements in a 2-D model.

> If it is not possible to model the local axis correctly it is advised to assign the elements to different groups.

> [Options..]
> This form controls the analysis.

> -General-,
> Chose between a 2-D or a 3-D analysis. If a 2-D analysis is chosen only the x and y co-ordinates are considered for the analysis.

> When "Clear memory before analysis" is checked, the memory used by the model is cleared to free RAM for the analysis. This is advisable when a very large model is to be analyzed. When a small model is run uncheck this option as the clearing of the memory is not needed and will probably take more time than the analysis.

> -Pre-processor-,
> When "Renumber model nodes" is checked, the model will be renumber before analysing. Since this action takes some time it can be switched off. But one should be aware that if this option is off and nodes or elements have been added, the node numbering could be far from optimal which will enlarge the bandwidth and consequently your matrix size and solving time drastically.

> "Generate Element Mass Matrix" can be switched of if no acceleration loadcases are defined. Before running an analysis the program will automatically switch this option on if any element masses are required for the defined loadcases.

> -Solver-,
> "Compile Stiffness matrix" may be switched off when no changes of the model have occurred since the last run. Boundary conditions (Constrains and loads) are not applied to the saved stiffness matrix, so a rerun with different boundary conditions without compiling the stiffness matrix is allowed. If the model is renumbered the stiffness matrix should always be recalculated

> When "Solve Displacements" is checked the compiled stiffness matrix is read from file, the boundary conditions are applied and the displacements are solved and written to file.

> -Post-Processor-,
> The options on this frame controls which stresses are calculated using the latest displacements found in file.

> If "Line element stresses" is selected the stresses of all two nodal line elements will be calculated.

> If "Finite Element stresses" is selected, the stresses of all three or four nodal finite elements will be calculated.

> [Analyze]
> This menu entry will start MatSol, which is the FesaWin Finite Element analyzer. MatSol can also be started outside FesaWin, which allows you to continue working on a model while another model is running. Do not work and run at the same model at the same time. And do not run more then one MatSol analysis at the same time as they may interfere with each other.

> For large problems it is advised to run MatSol outside FesaWin as FesaWin will continue to use processor time and thus slow done MatSol.

> Note: If Matsol will be executed outside FesaWin it is advised to run renumber within FesaWin first, do [Analyze, Option...] switch on the renumber option and switch off all other options, close the form and do [Analyze, analyze]. That way a optimal node numbering will be set which will minimize the size of the global stiffness matrix, which will reduce the execution time of Matsol significantly.

> 2.2.9 Post-Process

> [Load combinations...]
> This form will be used to define and select the load combination.

> Load combination name
> This selection box presents the names of the defined load combinations. The name of the load combinations can be changed by entering the new name in the box and pressing <update>. For post-processing the active load combination will be used which is the selected load combination in this box.

> Loadcase Name
> This selection box presents all available loadcases of the model.

> Multiplier
> This field present the loadcase multiplier for this loadcase and load combination. Change the multiplier and press <Update> to save.

> - Equation of Load Combination: ...." -
> This frame will show the equation of the active load combination as defined using the multipliers.

> After any change press <update> to save the change.

> [Displacement]
> When checked, the deformed shape of the active load combination will be plotted. The displacement will be scaled relative to the view size using the "Unit Vector Length" value as maximum displacement. By changing this value the deformations can be altered for clarity, do [View, view set..] .

> [Contour Plot]
> When checked, the active contour plot of the active load combination will be plotted. To view a different loadcombination, use the selection box on the Stress index frame. To select the type of contour plot do: [Post-Process, Option..] .

> [Mode Shapes]
> Frequency domain analysis is in development.

> [Element Stress]
> When checked, the line element stresses of the active load combination will be color plotted. To view a different loadcombination, use the selection box on the Stress index frame. To select the type of stress component do: [Post-Process, Option..] .

> [Report..]
> This entry will activate the report generator.

> Check the reports you want to write into your report file and do "Write".
> Choose a filename and save the report. The report is an unformatted ASCII file. To print the report, use another utility to do so.

> To browse through the report select "View". Select the file with extension .rpt and the browser will be opened.

> [Options..]
> `This form present the options for post processing.`

> -Select Contour Plot Type-
> Filled contour or contour lines can be chosen.

> -Select data for contour plot-
> Nodal stresses or nodal displacements can be chosen.

> `-Select Stress Component for post processing -`
> `The following stress components are available:`
> `Direct stresses.`
> `Sx`
> `Sy`
> `Sz`
> `Shear stresses`
> `Sxy`
> `Sxz`
> `Syz`
> `Bending stress around axis`
> `Sbx`
> `Sby`
> `Sbz`
> `Torsion stresses around axis`
> `Stx`
> `Sty`
> `Stz`

> `Combined stress (Von Mises)`
> `VM`

> `-Select stress coordinate system-`
> `This frame allows the user to choose between a local coordinate system or global system.`
> `It should be noted that for the calculation of local nodal stress averages it is required that two adjacent elements within the same element group should have the same local coordinate system. If not, stresses of different directions are averaged which will give wrong results. If local coordinate systems within a group of elements are not uniform use global stresses. The combined stress component (Von Mises)is direction independent and will therefore be correct and similar for both local or global.`

> -Select stress Type-
> This frame allows the user to select element nodal stresses or nodal stresses averages. if element stresses are selected the nodal stresses of each individual element is used. The contour plot will not be smooth as the stress field is not continuos between elements. This is a characteristic of the displacement based finite element method. To smoothen the stress field, the element stresses of one node are averages for each connected element and used for post processing. Only elements which are from the same group are included to calculate the nodal stress average value. This implies that discontinuity of the stress field between two element groups can be observed.

> -Select displacement component for contour plot-
> Chose a global direction or the x y z displacement which will show the length of the total displacement vector in each node.

> `-Define Elements to Post-Process-`
> Select one of the following options:

> * All Elements :All elements will be shown in the view
> * Group :Select one group of elements which should be shown in the view.
> * Selection :Press <Select> and select the elements that should be shown in the
> view, press <ESC> to stop selecting.

> `-Stress Index Scale-`
> `This options allows the user to control the range of stress values to be plotted.`
> `Select <Auto> to plot the full range of stresses found in the database of the selected elements`

> `Select <Manual> to define a range of stresses to be plotted.`

> 2.2.10 Info

> [User manual..]
> This option displays the user manual in ASCII format. It is advised to use your internet browser to view the manual. Filename = manual.htm.

> [About..]
> General information about FesaWin can be found here.

> [Model Info..]
> This option presents the size of the model and the size of the declared space for the different model arrays. Perform a regular check and declare more space if needed. Warning; the program will crash if the model gets greater than declared for!

> [License..]
> This form presents your licence level and allows you to change your license.

> [Run Demo...]
> This option will start the demonstration which will show you how to built a model and perform an analysis.

> 2.3 Command line

> The command line, located at the bottom of the main window, can be used to edit the co-ordinates of a selection of nodes during editing or moving and to enter the numerical values of node co-ordinates during adding of nodes or graphics.

> The commands should be typed in lower cases and are activated by pressing Enter on your key-board or the <Enter> button left of the Command Line.

> The pull down button at the right of the command line shows the previous commands, which can be selected for re-use.

> The following commands are available.

> dx=dx; dy; dz

> - to move the selected nodes by the vector (dx;dy;dz) relative to the previous or last selected location
> ax= x; y; z
> - to move the selected nodes to the absolute location (x,y,z).
> - To fix a co-ordinate use * .Example: ax=12 ;* ;-5.2 This command will set the x co-ordinate of all selected nodes at 12 and the z co-ordinate of all selected nodes at -5.2. The y co-ordinates will not be changed.
> rx= angle
> - to ro tate the selected nodes by "angle" degree around the global X axis
> - Note: Rotations are performed around the center point of the selected nodes.
> ry=angle
> - to rotate the selected nodes by "angle" degree around the global Y axis
> - Note: Rotations are performed around the center point of the selected nodes.
> rz=angle
> - to rotate the selected nodes by "angle" degree around the global Z axis
> - Note: Rotations are performed around the center point of the selected nodes.
> sc=scx ;scy; scz
> - to multiply each co-ordinates of the selected nodes by the factor scx, scy and scz.
> mxy z
> - to mirror the selected nodes in the X-Y plane.
> - z defines the z co-ordinate of the mirror plane.
> Note: If z is omitted or z = * the center point of the selected nodes is used to define the plane.

> myz x

> - to mirror the selected nodes in the Y-Z plane.
> - x defines the x co-ordinate of the mirror plane.
> Note: If x is omitted or x = * the center point of the selected nodes is used to define the plane.

> mxz y

> - to mirror the selected nodes in the X-Y plane.
> - y defines the y co-ordinate of the mirror plane.
> Note: If y is omitted or y = * the center point of the selected nodes is used to define the plane.

> help

> - will show you a short reminder of the commands.
> First select the nodes then type the commands into the command line, (replace the red marked text by numerical values), and press <Enter> to activate. Always use lower case.

3.0 Creating and Analyzing a model

> This chapter describes how to create a Finite element model in FesaWin. It is assumed that the user is familiar with finite element analysis.

> 3.1 Analysis setup

> 3.1.1 Units

> The program works dimensionless. This means that any consistence set of units can be used. The following units are advised:

> Length | [L] | m | m | mm | Inch
> Mass | [M] | kg | Ton | kg | ????
> Acceleration | [a] | m/s2 | m/s2 | mm/s2 | ????
> Force | [F] | N | kN | N | Kips
> Stress | [S] | N/m2 | kN/m2 | N/mm2 | Kips/inch2

> Table 3.1 Model units

> Be consistence with the units otherwise the results are not correct, each column represents a consistence set of units.

> 3.1.2 Type of analyses

> The following two types of analysis are available:

> - Three dimensional
> - Two dimensional

> When a 2-D analysis is considered, the model should be placed in the x-y plane only. Select only one view window and set the view direction at X-Y.
> Do: [view, viewset….] ,<Single>, <X-Y>, <OK>.

- For a 3-D analysis the model may be built anywhere. It is recommended to select all four views and to look at your model through each view with an other perspective.
Do: [view, viewset….] ,<Multi>, set for each view the preferred view perspective by using <ISO>, <X-Y, <X-Z>, or <Y-Z>.

3.1.3 Declare workspace

Use the model size option on the main menu file menu to size the workspace in memory you need for your model. During modeling the workspace may be increased if required. But, if the workspace is to small for the model, errors may occur and the model in memory could be damaged. If this occurs, do not save the model but exit without saving, restart FesaWin, increase workspace, and retrieve the model from disk.

DO: [File, Model Size…] , fill in the required size and press <OK>.

Do not make the total declared size to large as this may decrease the speed of the computer.

3.2 Placing elements

To build a finite element model, elements have to be placed and the element and material properties have to be defined.

3.2.1 Defining element groups

Elements are assigned to a named group. Before you place the elements it is advisable to define the group names first. The reasons to assign elements to certain groups are as follows:

> - Material properties and element properties like thickness and section properties can be set per group of elements
> - nodal stress averages are generated per group of elements,
> - groups of elements can easily be selected and modified,
> - element groups can be switched on or off for post-processing.

To define groups use [define…]of the main menu.

3.2.2 Single element placement

When the model is small, or for any other reason you want to place elements one by onesingle elements can be placed.

The finite elements can be placed by using [add, Element…] of the main menu.

Select the type of element you want to place and the group name for the element. To define the elements, press <Add> and place the elements by clicking with <Left mouse Button> or by direct entering the node coordinates using the command line .

When finished press <right mouse button> to stop placing.

To check if elements are really placed and at the right location it is advised to switch element labeling on. This option will write the element rank number in the middle of the element. Use [view, element label, number] to switch this option on or off.

3.2.3 Patching and Meshing

When large quantities of elements are required it is more easy and faster to use the mesh generator.

The mesh generator can place line elements on a graphic line and membrane or plate elements on a surface defined by graphic elements.

Line Elements,
To place line elements like axial rods or beam elements work as follows:

- Draw the line string using straight lines or circle sections. Do: [Add, Graphics, line/circle] . To be sure that the end and beginning of each line segment is connected to each other, switch snapping on. Use the <Snap on> button at the bottom of the main window to do so.
- Define the number of finite elements to be placed on each graphic element by sub divide the graphic elements. First use [Select, Graphics] to switch to graphic element selection. Double click a graphic and the " Edit Graphic Elements " form will appear. Set the number of spaces on this form equal to the number of elements you want on this graphic. When ready press <OK>.
- Now start the mesh generator, [Add, Mesh…] , press <2_D Mesh>.
- Set the "Mesh Type" to "Line"
- Select the element type and group.
- Press <Edge 1> and select the graphic elements using <left mouse button>. When ready press <ESC>.
- Now press <Generate Mesh> and review the result as shown in view 1.
- When acceptable press <Accept> else press <Reset>.
- When ready press <Ready>

To place three or four nodal elements like membranes or plate elements work as follows:

- Define the surface to be meshed using straight lines or circle sections [Add, Graphics, line/circle] . To be sure that the end and beginning of each line segment is connected to each other, switch snapping on. Use <Snap on> at the bottom of the main menu to do so. To create a mesh with four nodal elements, the surface should be defined by four sides. To create a mesh with three nodal elements, the surface should be defined by three sides.
- Define the number of finite elements to be placed along each graphic element by sub divide the graphic elements. First use [Select, Graphics] to switch to graphic element selection. Double click a graphic and the "Edit Graphic Elements" form will appear. Set the number of spaces on this form equal to the number of elements you want along this graphic. When ready press <OK>. Note that for a four nodal mesh, opposite sides of the surface should have equal sub division. For a three nodal mesh all three sides should have equal sub division.
- Now start the mesh generator, [Add, Mesh…] , press <2_D Mesh>.
- Set the "Mesh Type" to "Quad" or "Triang"
- Select the element type and group.
- Press <Edge #> and select the graphic elements using <left mouse button>. When ready press <ESC>. Do this for each edge and mind the order of the edges.
- Now press <Generate Mesh> and review the result. See figure 3.1 and 3.2 for examples of a three and a four nodal mesh.
- When acceptable press <Accept> else press <Reset>.
- When ready press <Ready>

> > > Figure 3.1 Three nodal Mesh (Click on picture to enlarge)

> > Figure 3.2 Four nodal mesh (Click on picture to enlarge)

> > 3.3 Defining boundary condition

> > When the elements are placed the boundary conditions should be defined.

> > To define the loads work as follows:

> > > - First use [Select, Nodes] to switch to finite element nodes selection.
> > > - Select all nodes with equal loads
> > > - Do: [Add, Loads..]
> > > - Select the loadcase
> > > - Enter the values of the load components
> > > - Press <Apply>
> > > - Review the results in view 1
> > > - Press <Ready>

> > If multiple loadcases are required, define the loadcase name and type at [Define, Loadcase...]

> > Check the settings of [View, Loads,....] if loads are not shown while defined.

> > To define the constraints work as follows:

> > > - First use [Select, Nodes] to switch to finite element nodes selection.
> > > - Select all nodes with equal constraints
> > > - Do: [Add, Constraints..]
> > > - Enter the values of the constraint components
> > > - Press <Apply>
> > > - Review the results in view 1
> > > - Press <Ready>

> > Any pre-described nodal displacement will only be used in loadcase 1. For the other loadcases the pre-described displacement will be set at zero, which results in a constraint.

> > 3.4 Analyzing model

> > When the model is ready, the analyses can be performed. Save your model first! When a very large model is to be run, it is advisable not to start the analysis from FesaWin, but use MatSol instead, as this will run faster. MatSol is a separate executable which was included with FesaWin. Search in the directory of FesaWin and double click MatSol.exe to start.

> > First the options of the analysis have to be set. Within FesaWin do [Analysis, options..] or within MatSol press <Options>, and select the right options. If you are running a simple 2-D analysis set the analyses type to 2-D.

> > When this is done, press <Run> in MatSol or do [Analysis, Analysis] in FesaWin.

> > 3.5 Post-processing

> > After the analysis, load combination can be defined which are constructed from the previously defined loadcases. Each load combination can be reviewed graphically or written into a report file. Loadcombinations can be changed and modified without rerunning the analysis.

> > To look at the deformed shape of the model, use [Post-Process, Displacements]

> > To review the stresses in the construction use one of the stress plot options of Post-Process menu.

> > The stress plots can be controlled by using [Post-Process, Options] . Use this form to select which stress component and from which elements you want to see the stress plots.

> > Use [Post-Process, Report…] to create a numerical report of the input and output information of the model.

> > Use [File, Print...] to plot the contents of view 1.

> 4.0 Element description

> > 4.1 BARD Two Nodal Axial rod element

> > Description,
> > This element is a simple axial truss, which can only take load in the direction of the element definition line.

> > Nodes : 2
> > Local Degrees of freedom : 1 per node

> > Group Properties,
> > E modulus
> > Poisson ratio
> > Area

> > Local stress Output,
> > LSX Stress in local X direction

> > Performance,
> > This is an analytical element, which means that the exact solution of the stress and strain relation is known and used.

> > 4.2 BEAM Two Nodal Beam Bending Element

> > Description,
> > This element is a beam bending element, which can take load in all degrees of freedom.

> > Nodes : 2
> > Local Degrees of freedom :

> > - 3-D 6 per node (x,y,z,rx,ry,rz)
> > - 2-D 3 per node (x,y,rz)
> > Group Properties,
> > E modules
> > Poisson ratio
> > Area
> > Rot
> > Ixx
> > Wxx
> > Iyy
> > Wyy
> > Izz
> > Wzz
> > Note: For 2-D analysis the Ixx, Wxx, Iyy and Wyy are not used.

> > Local stress Output,
> > LSX Axial Stress in local X direction
> > LSBY Bending stress around local y-axis
> > LSBZ Bending stress around local y-axis
> > LSXY Bending stress around local y-axis
> > LSXZ Bending stress around local y-axis

> > Performance,
> > This is an analytical element, which means that the exact solution of the stress and strain relation is known and used.

> > 4.3 TRIM Three Nodal Membrane Element

> > > > Description,
> > > > This element is a displacement based triangular membrane element with two degrees of freedom per node.

> > > > Nodes : 3
> > > > Local Degrees of freedom : 2 per node
> > > > Local x
> > > > Local y

> > > > Group Properties,
> > > > E modules
> > > > Poisson ratio
> > > > Specific mass
> > > > Thickness
> > > > Plane strain or plane stress

> > > > Local stress Output,
> > > > LSX Direct stress in local X direction
> > > > LSY Direct stress in local Y direction
> > > > LSXY Shear stress in local XY Plane

> > > > Performance,
> > > > This is not an analytical element, which means that an approximate solution of the stress and strain relation is used.
> > > > The reported local stresses are constant over the element surface, which means that the performance of this element in a coarse mesh is rather poor.

> > 4.4 QUA4D and QUARD Four Nodal Membrane Element

> > Description,
> > This element is a displacement based quadrilate membrane element with two degrees of freedom per node.For rectangular element shapes the QUARD is recommended while for more irregular shapes the QUA4D performs better.

> > Nodes : 4
> > Local Degrees of freedom : 2 per node
> > Local x
> > Local y

> > Group Properties,
> > E modules
> > Poisson ratio
> > Specific mass
> > Thickness
> > Plane strain or plane stress

> > Local stress Output,
> > LSX Direct stress in local X direction
> > LSY Direct stress in local Y direction
> > LSZ Direct stress in local Z direction (For plane strain only)
> > LSXY Shear stress in local XY Plane

> > Performance,
> > This is not an analytical element, which means that an approximate solution of the stress and strain relation is used.
> > The reported local stresses vary linear over the element surface, which means that the performance of this element in a coarse mesh is rather better than the TRIM element.

> > 4.5 PLARD Four Nodal Thin plate bending element

> > Description,
> > This element is a displacement based quadrilate plate bending element with five degrees of freedom per node. The element behaves very good if rectangular shaped however irregular shapes can also be done.

> > Nodes : 4
> > Local Degrees of freedom : 5 per node
> > Local x,y z, rx, ry
> > The local rz degree of freedom has been given a dummy stiffens to prevent singularity of the stiffness matrix.

> > Group Properties,
> > E modules
> > Poisson ratio
> > Thickness

> > Local stress Output,
> > LSX Membrane stress x-direction (Positive for tension)
> > LSY Membrane stress y-direction (Positive for tension)
> > LSBX Bending stress around local x-axes (Positive when outer fiber in local z-direction is in tension
> > LSBY Bending stress around local y-axes (Positive when outer fiber in local z-direction is in tension
> > LSXY Shear stress x-y plane
> > LSTZ Not reported

> > Performance,
> > This is not an analytical element, which means that an approximate solution of the stress and strain relation is used.
> > The reported local stresses vary linear over the element surface, which means that the performance of this element in a coarse mesh is rather better than the TRIM element.

> > 4.6 QUARS Four Nodal Stress based Membrane Element

> > Description,
> > This element is a stress based quadrilate membrane element with two degrees of freedom per node.This element performs very well even in coarse and irregular shaped meshes.

> > Nodes : 4
> > Local Degrees of freedom : 2 per node
> > Local x
> > Local y

> > Group Properties,
> > E modules
> > Poisson ratio
> > Specific mass
> > Thickness
> > Plane strain or plane stress

> > Local stress Output,
> > LSX Direct stress in local X direction
> > LSY Direct stress in local Y direction
> > LSZ Direct stress in local Z direction (For plane strain only)
> > LSXY Shear stress in local XY Plane

> > Performance,
> > This is not an analytical element, which means that an approximate solution of the stress and strain relation is used.
> > This element has been developed based on stress field assumption rather than displacement field assumptions. Therefore the behavior of the element is a lot better than the displacement based elements.

> > 4.7 TPLRS Four Nodal Thick plate bending element

> > Description,
> > This element is a stress based quadrilate thick plate bending element with five degrees of freedom per node. The element behaves very good if rectangular shaped however irregular shapes can also be done.

> > Nodes : 4
> > Local Degrees of freedom : 5 per node
> > Local x,y z, rx, ry
> > The local rz degree of freedom has been given a dummy stiffens to prevent singularity of the stiffness matrix.

> > Group Properties,
> > E modules
> > Poisson ratio
> > Thickness

> > Local stress Output,
> > LSX Membrane stress x-direction (Positive for tension)
> > LSY Membrane stress y-direction (Positive for tension)
> > LSBX Bending stress around local x-axes (Positive when outer fiber in local z-direction is in tension
> > LSBY Bending stress around local y-axes (Positive when outer fiber in local z-direction is in tension
> > LSXY Shear stress x-y plane
> > LSYZ Shear stress y-z plane
> > LSZX Shear stress z-x plane

> > LSTZ Not reported

> > 4.8 SPRING One node user defined Flexible support element

> > Description,
> > This element is a spring support defined by one 6x6 stiffness matrix.

> > Nodes : 1
> > Local Degrees of freedom : None
> > Globale degree of freedom: Depending on analysis type and used elements see here for more information.

> > Group Properties,
> > Stiffness matrix

> > Local stress Output,
> > None