Modeling, Processing, and Analyzing Three-Dimensional Solid Bodies:
An ALGOR Application

• Modeling the Object:

  The object you will model is a simple I-beam. You will do this by drawing the cross section, extruding it, applying surface meshes to all of the sides, and then meshing the entire solid. Each of these steps is described below.

  • Drawing the cross section:
    Using lines, draw a cross section of an I-beam (Add:line)
    - just keep adding lines end to end until you have closed the cross section (it does not have to be perfect)
    Divide the top and bottom edges of the flange into 3 line segments.
    This can be done using either the Construct:Divide or you can also try the Modify:Intersect command which will allow you to determine the points at which the sides of the web would "intersect" the top of the flanges, this is very convenient.
    - just make sure you divide the top and bottom of the flange into 3 line segments, it may help to turn on the "x end Pt" option (under F6) in order to actually see where you have constructed line segments
    Draw lines between nodes to section off the cross section so that the top and bottom flanges are composed of 3 quadrilaterals (possibly rectangles) and the center web is a quadrilateral

    

  • Extruding the cross section into an I-beam modify:copy:join, select all, F3 Keyboard input Hit return to set the origin as your move start set the move end to 0,0,Z where Z is some appropriate value for the length of the beam you wish to model
    Look at the isometric view

  • Applying surface meshes
    Save the file (under Files)
    Transfer:SSURF - this is the surface generator
    Construct:Gpatch, select all, Gpatch, Esc
    Quick msh: Test, this mesh is rather dense and may take too long to process so change the density under Number-u to 3 and test it again. If it looks fine then File msh. Hit return to accept the default filename which is your original name with an "m" (for mesh) added to it.
    F9:Transfer:Mesh-sd2(save work when asked)

  • Adding a 3-D mesh to the solid
    (you should be in sd2 now) Automesh:Hypergen:Hypergen
    watch your command tool as it displays the building of the solid out of tetrahedra (when it is finished sd2 will load) (at some point in the future you may also wish to mesh a model with Hexagen - which as you might expect models the solid with hexahedron elements - it too requires that the external surface of the solid be meshed with four sided regions (quadrilaterals))

  • Apply forces and boundary conditions
    Change the view to YZ right (or whatever is appropriate to allow you to see the model edge upon which you wisht to apply the boundary conditions
    Fully constrain one end of the beam (add:FEA add) by box applying to the very bottom nodes
    Apply forces in the negative y direction by box applying to all the nodes on the right edge (in this view)
    Save the file and quit
    

• Processing the model
  The model must be set up in decods as usual and run through the ssap0 processor.
  Enter decods (remember your new filename has an extra "m" added to it)
  Enter the following information:
  • Elements
    • Type - Tetrahedron
    • Info - 4 nodes
    • Group - enter steel from the library or enter values manually
    • Color - Tref=0
  • Global Load case - Press=0,Accel=0,Disp=1,Therm=0
  • Run
  Make sure no errors come up.
  Run the file through ssap0 - it should take a few minutes to run

• Reviewing the Results

  This section describes some of the more exciting, flashy (and potentially confusing) post processing options. Many are not discussed in detail below and it is up to you to explore them (much information can be obtained using the Inquire option).

  sview the model
  View the displaced with the undisplaced (calc scale also) You may or may not want to change the perspective
  There are some very neat ways to view this solid model:

  Under Stress-di, you can view a shaded version of the model by selecting Light and then Do dither.
  Under Light you can select other options such as the color of shading, the number of colors to use in the shading, etc. But the default settings for this are usually the best. This option is intended to help you orient yourself as you inspect both the external and internal stress or strains which exist under this loading condition.

  You can view the stress results as usual under Stress-di:Post (there are several choices for the type of stress you want to view)
  Also under Post, select disp Vec:Magnitude and Esc out and Do dither to see a color illustration of the displacement of the beam.
  There is also an option called "Shrink" under Options:General. Select this option and go back and do a dither (either light or post). Actually, an alternative and sometimes better way to view this is in bitmap form, so instead of "Do dither", select Bitmap and Preview (if you select Do bitmap, a bitmap file of this image will be created). Hit Esc to get out of this.
  If you ever want to unshrink it you must return to this menu and deselect this option. This option is most useful if you have actually made errors in the modeling for now you can see the location of "holes" which might have been unintentionally built into your model.
  The final option to be discussed is under Options:sLice.
  Using "slice" you can see "inside" the solid by defining a cutting plane. You will probably find that it is difficult to know exactly how you are cutting it in the isometric view, so change to another view (YZ rig) and under Options:slice:Define pl choose 2pt & eye and simply choose the 2 endpoints of the cutting plane and then select Cut. Now you can change views and do light or post(stress) dithers and bitmaps. At any time you can return to this menu and choose uncut to return it to normal and/or select a new cutting plane. You can even do multiple cuts.
  Sometimes you may have to go to F10:Redraw to update the drawing according to the new options chosen.