** ABAQUS program for the truss problem discussed in the first computer assignement. 
** Every single asterisk (at left) indicate a "keyword", 
** i.e., a subroutine, that performs
** certain functions. For more information, see ABAQUS Keywords manual. All
** keywords and variables are not case-sensitive.
**
** Double asterisks (at left) indicate a comment. All such comments are
** ignored by the computer, and are inserted for clarity only.
**
*Heading
Truss problem as discussed in class
**
** The Heading title (Truss problem ...) will appear on any output files
** created by ABAQUS.
**
** The next statements give the locations of nodal points, corresponding
** in this example to the "joints" of the truss system. First entry is
** node number and the next its X1 and X2 coordinates. The absence of a
** specified X3 coordinate implies that the value is zero (plane problem). We let
** the truss structure to be a 10m*10m square in this demonstration.
**
*Node
1, 0, 10
2, 10, 10
3, 0, 0
4, 10, 0
**
** Define node sets for convenient purposes. n1 and n3 are supports, and
** nload will sustain same level of P1 and P2 on both of its nodes. We can
** add P2 on node #3 as well.
**
*Nset, nset=n1
1
*Nset, nset=n3
3
*Nset, nset=nload
2, 4
*Nset, nset=nall, generate
1,4,1
**
** Next, the elements (corresponding to truss bars in this case) are
** defined. Also, the type of element, from the library of elements
** available within ABAQUS, is defined. First number shown is the
** element number, and the next two are the two nodes which that element
** joins. The set of elements is defined as elall. Note that the
** elements are for 2D analysis; use type T3D2 for 3D truss models.
**
*Element, type=T2D2, elset=elall
1, 1, 2
2, 1, 4
3, 3, 2
4, 3, 1
5, 4, 2
6, 3, 4
**
** We now describe properties of the material, beginning with the
** cross section area (1m^2) and Young's modulus E (200GPa), in the
** units adopted. The Poisson ratio nu (0.3) is irrelevant here.
**
*Solid Section, elset=elall, material=steel
1
*Material, name=steel
*Elastic
200e+9, 0.3
**
** Next come statements about fixed boundary points. The node number is
** given first, and then the first and last degree of freedom that is
** restrained at the node -- displacements U1 & U2 are zero for node #1, and for
** node #3, U1 is restrained but U2 is not. It was not really necessary to mention
** U3, since the problem is set up as 2D.
**
*Boundary
n1, 1, 2, 0.0
n3, 1, 1, 0.0
**
** Now we describe the loading, in this case as a single "step".
** Since this involves linear elastic material and we are content to
** neglect any effects of geometry change, due to deformation, on the
** writing of the equilibrium equations, our problem is a completely
** linear one. For large deformation problems the option "NLGEOM" should
** be used after the *Step keyword.
**
*Step
**
** The parameters below *Static specifies initial increment, total
** step length, minimum increment allowed, and maximum increment allowed.
** The analysis terminates if the increment needed for solutions to
** converge is smaller than the minimum increment allowed.
**
*Static
0.2, 1., 1e-05, 0.2
**
** Following specifies that a concentrated load of 1.5MN is applied
** on node #3 in X2 direction. A concentrated load of 2MN is applied
** on both nodes #2 and #4 in X1 direction, and a concentrated load of 1MN
** is applied on both nodes #2 and #4 in X2 direction.
**
*Cload
nload, 1, 1e+06
nload, 2, 2e+06
n3, 2, 1.5e+06
**
** The follow requests to read default variables (stresses, strains,
** displacements and coordinates, etc.) to certain output files.
** *El Print and *Node Print put results in a .DAT file that you can
** type or edit, and extract results from for your lab report. *Output
** will enable user to view the results (fields and time histories) of
** default variables. Users may choose to output only desired variables
** to save disk space and time.
**
*Output, field
*element output, elset=elall
s,e
*El Print, elset=elall
s,e
*Node Print, nset=nall
u
**
** The final statement tells ABAQUS that the loading step is over
**
*End Step