ME/AE446 Finite Elements in Structural Analysis

[ U_N_I_V_E_R_S_I_T_Y___o_f___N_O_T_R_E___D_A_M_E ]

Models with Multiple Element Types

Thus far you have used ALGOR to model an object with a single type of element. You have used rods (truss elements), beams, membranes, plates, or solid bricks or tetrehedron elements but in every case the model has been composed of one type of element. The composition of real-world structures is such that many different parts of the structure carry "stress" in a different fashion and modeling the entire structure with a single element type is inappropriate. A variety of types of elements may be needed to accurately model a structure either "geometrically" or in the manner in which it deforms or both. In this tutorial you will develop a model composed of different element types, analyze the model, and view the results. Again, you should be familiar enough with ALGOR by now that step-by-step commands are not necessary in most instances. Therefore, general directions will be given and specific menu directions will be used only when necessary. Don't be afraid to ask questions, or experiment on your own, in order to learn how to do something if you get stuck or lost. Also, don't forget the always helpful "F2" key or UNDO command.

Modeling the Object:
The object you will model is a stiffened thin-walled "box". This is representative of many types of lightweight structures such as aircraft wings, automobile bodies, etc. This type of structure can be modelled with a box whose skeleton is formed using axial force, or truss members, and whose walls are formed with plane stress membranes. Bending stiffness for this "box" is due to a combination of the effect of the in-plane stress in the membrane elements and the axial force carried in the truss elements. ALGOR allows one to develop "submodels" using each type of element independently and then these submodels are combined to form the final model used for the analysis. In order to develop a model composed of different element types in ALGOR you need to develop a number of initially independent models and then "combine" them after you have established the basic finite element data in decods. One important issue is that the initially independent models must be based upon the same node point geometry. The approach used in this tutorial will involve establishing the basic geometry of a stiffened, thin-walled box and then customize it to satisy the information required for each component of the combined structure. One of the models will be referred to as the "root" and the other is the "graft". It is recommended that the boundary conditions and loads be applied to the "root" which in this example will be the internal stiffening elements (truss elements) and the "graft" will be the external skin. The following describes how to build the two models and then combine them for subsequent analysis using the linear, stress analysis option, ssap0.
- Drawing the box: Draw a rectangle in the xy plane
  Change the view so you see the side of the rectangle lying down (view (2) XZ fro)(a horizontal line)
  Modify:Copy:Join:select all: F3 :Keyboard input
  Hit return to set the origin as your move start
  Set the move end so that a box will be created (for example if z is your vertical direction, set the move end to 0,0,Z where Z is some on the same order as a side of your rectangle).
  Copy:last move - this will perform the same copy:join function on the new rectangle (it should be highlighted)
  Changing to an isometric view, you should see that you have created a box with 3 rectangular cross sections similar to that shown in the sketch below.
  
  Though you now have an image that looks like a "box," what you have actually done is establish the locations of the nodes which will be shared by all of the elements.
- Customizing and saving the models
  You want to now create two different models using this basic geometry information:
  The first model to be saved will be the "skin". The skin will be made of membrane elements (two dimensional plane stress) and in order to help keep the element types differentiated we want to save this model using a different "color" element. Under the menu item Modify:Update select all of the lines and under Color change them all to "2" or red. Then proceed to "Files" and "Save As" a file named "boxskin."
  Now you have to go back and form a second model, the truss or stiffening elements, but these must be formed from the "green" or original color. So repeat the process indicated above and convert the lines back to color "1".
  The section of the model with the truss elements is to be the "root" model and it is this part of the model to which you will apply the loads and BC's.
  Fully constrain the 4 nodes at one end of the box, you may want to change the view to a side view to facilitate the application of the boundary conditions.
  Apply forces to any of the unconstrained nodes. This may be done more easily with the isometric view. Try a set of loads that will "torque the box" or one that will bend it as if it were a thin walled beam.
  Now "Save As" this file with the name "boxtruss" and quit SuperDraw.
Decoding the models:
Each file (boxtruss and boxskin) must be decoded separately as if they were separate models.
- decods boxtruss
  Enter the following information:
  - Elements
    - Type - truss
    - Info - no info can be entered for truss members
    - Group - enter steel from the library or enter values manually and be sure to enter a cross sectional area for the truss elements. You may want to make this on the order of 0.02 square inches.
    - Color - Tref=0
  - Global
    Load case - Press=0,Accel=0,Disp=1,Therm=0
  - Run
  - Make sure no errors come up.
- decods boxskin
  Enter the following information:
  - Elements
    - Type - membrane
    - Info - leave as 0)incompatible (esc)
    - Group - enter steel from the library or enter values manually
    - Color - Thickness=.05, Tref=0 (recall that you made the skin elements out of color "2" - and this is a place where we still have some confusion about the manner in which ALGOR operates so it is advised to provide both colors 1 and 2 with the same input information.
  - Global
    Load case - Press=0,Accel=0,Disp=1,Therm=0
  - Run
  - Make sure no errors come up.
Combining the decoded parts into a single input data file. This is the "new stuff" and requires using another utility which combines the files with the .sst extensions that have been created by decods.
- Type "combsst" to bring up the menu to combine decoded files. (Again you have to click in the window to transfer control)
- Enter "c" then enter a name for the combined file (e.g. "stiffbox") and then a Return
- Enter "r" then enter "boxtruss" since this is our root file, and it contains boundary conditions and loads.
- Enter "g" then enter "boxskin" which is the file to graft to the root
- Enter "p" to process the combination
Processing the model:
ssap0 filename - where filename is the name of your combined file (stiffbox)
run - watch out for any errors
Reviewing the Results
Use sview to review the results. You should be familiar enough with this post-processor that you can view displaced shape and stress contours and also inquire about information for certain elements and nodes. If you inquire about stress information for truss elements then you will see the loads in those elements. If you inquire about stress in the membranes, that is the information that will be displayed.