5.1
FORK WRENCH WITH PLANE STRESS ELE. NO.7
Copy the example files B1_*
into Z88 entry files Z88* (has been already carried out on the Z88 CDs
or
Internet packages for your immediate start):
B1_X.DXF ---> Z88X.DXF
input file for CAD converter Z88X
B1_2.TXT ---> Z88I2.TXT boundary conditions for Cholesky solver Z88F
B1_3.TXT ---> Z88I3.TXT header parameters for stress processor Z88D
Simply
proceed with the following steps to get familiar with Z88:
CAD:
As for this
first example, you should only look at the CAD super structure without
producing it. This comes with later examples. Import Z88X.DXF into your
CAD
program and view it. Usually you would draw or model the super
structure in
your CAD system. Do not change anything and leave your CAD program
without
saving, converting etc. If you do not have any suitable CAD system,
then drop
this step.
Z88:
Z88X,
conversion from Z88X.DXF to Z88NI.TXT.
Windows: Press button Z88X in
the Z88 commander, Button DXF --> Z88NI,
Run Button.
Close program Z88X.
LINUX/UNIX: In the Z88
commander press button DXF --> Z88NI.
Z88O, looking at the super structure.
Windows: In the Z88
commander press button Z88O. If you
press now the Run button, don't worry
about the error message because Z88O wants to load the file Z88I1.TXT
as a default
which does not exist at the moment. However, you want to load now
Z88NI.TXT: Proceed
as follows: Diskette button >
Z88NI.TXT, Run button. Then
switch to Wireframe by the appropriate
button and show the nodal numbers and the element numbers by Menu > Labels > All. Zoom in with
the Prior key. Close Z88O.
LINUX/UNIX: In the Z88
commander press button Z88O. If you
press now the Run button, don't worry
about the error message because Z88O wants to load the file Z88I1.TXT
as a default
which does not exist at the moment. However, you want to load now
Z88NI.TXT: Proceed
as follows: File button >
Z88NI.TXT, Run button. Then
switch to Wireframe by the appropriate
button and show the nodal numbers and the element numbers by Menu > Labels > All. Zoom in with
the Prior key. Close Z88O.
Z88N, mesh generator, reads
Z88NI.TXT and produces Z88I1.TXT.
Windows: In the Z88 commander
button Z88N, Run button. Close Z88N. Hint:
You should always close the unneeded Z88 modules to have a maximum
of
memory.
LINUX/UNIX: In the Z88 commander
press button Z88N.
Z88O, looking at the finite elements
structure. Proceed
as follows:
Windows: In the Z88
commander press button Z88O, Run Button.
LINUX/UNIX: In the Z88
commander press button Z88O, Run Button.
Z88F, calculates displacements. Proceed as follows:
Windows: In the Z88 commander
press button Z88F, CD Button (is
default), Run Button.
LINUX/UNIX:
In
the Z88 commander press button Z88F -C.
Z88D, calculates stresses. Proceed as follows:
Windows: In the Z88 commander
press button Z88D, Run Button.
LINUX/UNIX:
In
the Z88 commander press button Z88D.
Z88O look at the deflected finite
element structure. Proceed
as follows:
Windows: In the Z88 commander
press button Z88O, Run Button, Wireframe Button,
Deflected Button. As a default, the deflections are multiplied by 100. This is too
large
for this example. Thus: Menu
> Factors > Deflections
> enter for FUX and FUY 10 . You
may also look at the reduced stresses because Z88D was run before. Try
the
buttons Reduced stresses in corner nodes,
Reduced stresses mean values per element
and Reduced stresses in Gauss points
(this feature for undeflected structures only).
LINUX/UNIX: In the Z88 commander
press button Z88O, Run Button, Wireframe Button,
Deflected Button. As a default, the deflections are multiplied by
100. This
is too large for this example. Thus: Menu
> Factors > Deflections > enter for FUX
and FUY 10 . You may also look at the reduced stresses
because Z88D was run before. Try the buttons Stresses
Corner Nodes, Stresses
per Element and Stresses Gauss Points
(this feature for undeflected structures only).
Z88E, nodal forces calculation. Proceed as follows:
Windows: In the Z88 commander
press button Z88E, Run Button.
LINUX/UNIX:
In
the Z88 commander press button Z88E.
Your
task:
A fork wrench should be loaded with the screw's tightness torque. A
couple of
forces are applied in the wrench's mouth according to the torque and
the fixed
points are assumed to be at the locations where the mechanic's hand
grips the
wrench. In fact, these clever boundary conditions are doing the same
task as
(in reality !) the fixed points in the mouth and the forces applied to
the
grip, but are much easier to handle.
The fork wrench should be
modelled by 7 super elements Plane Stress No.7.
The mesh generator should produce 66 finite
elements from the super elements. The element thickness is 10 mm each.
Mesh
generation: Local and global axises are not the same direction in this
example:
Local x direction at super element 1 defines by the local nodes 1 and 2
which
correspond to the global nodes 1 and 3. The local y direction of SE 1
is determined
by local nodes 1 and 4 which correspond to the global nodes 1 and 7.
Further
take into account: Super elements which have a joint side must have an
absolutely identical subdivision at this side. Thus, SE 1 and SE 2
share the
line 3-4-5: The subdivisions in y direction must be exactly the same.
Here 3
subdivisions, respectively.
Now calculate this example
as indicated above. After that, one can experiment: Subdivide the SE 7
in Z88NI.TXT as a meaningful variation as
follows:
7 7 ("Super
element 7 is of type 7, i.e.
Plane Stress Element No.7")
6 L 3 E (
"Subdivide SE 7 into finite elements Plane Stress No.7 and subdivide
into
x direction 6 times geometrically ascending and in y direction 3 times
equidistant") Of course, the SE 1 to SE 5 as well could each be
condensed in direction of the screw:
1 7
3 L 3 E
2 7
3 L 3 E
.... continue ....
Note: As it is obvious for the input
files, you can add comments after all required data are entered in
every line.
Separate the last date from the comment by at least one blank. You can
do this
just the same in your own files. A maximum of altogether 250 characters
per
line is permitted.
5.1.1
Input
This example works
with a super structure, i.e. a very rough FE mesh. The mesh generator
should
generate a FE structure from the super structure. Thus, the first task
is to
design the mesh generator input file Z88NI.TXT.
Chapter 2.6 outlines the procedure
if working with CAD. If you work without a CAD system, you design the
file
Z88NI.TXT by editor or word processing program. The super structure
shall look
as follows:
With
CAD program:
Follow the description of chapter 2.7. Do not forget to write the super
element information on the layer Z88EIO by TEXT function. Thus
SE 1 7 7 3 E 3 E ( 1st
SE, SE type 7, FE type 7, subdivide into x 3 times equid., into y 3
times
equid. )
SE 2 7 7 3 E 3 E ( 2nd SE, SE type 7, FE type 7, subdivide into X 3
times
equid., into y 3 times equid. )
SE 3 7 7 3 E 3 E
SE 4 7 7 3 E 3 E
SE 5 7 7 3 E 3 E
SE 6 7 7 1 E 3 E
SE 7 7 7 6 E 3 E
...and write the general
information and material information onto the layer Z88GEN :
Z88NI.TXT 2 38 7 76 1 0 0 0
0 0 ( 2-DIM, 38 nodes, 7 superelements, 76 DOF, 1 mat info, flags 0
)
MAT 1 1 7 206000 0.3 3 10 ( 1.mat info from SE 1 to SE 7: Young's
modulus,
Poisson's ratio, INTORD, thickness, )
Export the drawing as DXF
file with the name Z88X.DXF and start the CAD converter Z88X with the option "from Z88X.DXF
to Z88NI.TXT" (DXF -> NI). Z88X will produce the mesh generator
input
file Z88NI.TXT. You should have a look at it with Z88O.
With
editor:
Write the mesh
generator input file Z88NI.TXT (cf.
chapter 3.3) with an editor:
2 38 7 76 1
0 0 0 0 0
(2-DIM, 38 nodes, 7 superelements,
76 DOF, 1 mat info line, flags 0)
1 2 22.040 32.175
(Node 1, 2 DOF, X and Y coordinates)
2 2 31.913 28.798
(Node 2, 2 DOF, X and Y coordinates)
3 2 43.781 24.826
4 2 43.880 32.373
5 2 43.980 39.424
...... (Coordinates for nodes 6... 36 not represented)
37 2 202.847 27.507
38 2 144.905 42.403
1 7 (SE 1 of the type Plane Stress
No.7)
1 3 5 7 2 4
6 8 (Coincidence
for 1st SE)
2 7 (SE 2 of the type Plane
Stress No. 7)
3 10 12 5 9 11
13 4 (Coincidence
for 2nd SE)
..... (Coincidence for elements 3 .. 6 droped here)
7 7
30 35 37 32 34 36 38 31
1 7 206000 0.3
3 10 (mat
info from SE 1 to SE
7:Young,Poisson,INTORD,thickness)
1 7 (Subdivide 1st SE into FE type 7
and
3 E 3 E subdivide
into x 3 times equidistant + into y 3 times equidistant)
2 7 (Subdivide 2nd SE into FE type 7
and
3 E 3 E subdivide
into x 3 times equidistant + into y 3 times equidistant)
3 7
3 E 3 E
4 7
3 E 3 E
5 7
3 E 3 E
6 7
1 E 3 E
7 7
6 E 3 E
With
CAD program and editor:
Start the mesh generator
Z88N for producing
the final Z88 structure file Z88I1.TXT.
Look at
it either
Enlarge the wrench's mouth
by zooming for defining the two nodes which will get the load
representing the
torque (to simplify matters it is assumed, that the screw gets only
selectively
a couple of forces as torque at the corners and that the screw itself
and not
the wrench revolves):
We find the nodes 11 and
143. The pictures printed here were produced directly by Z88O.
In the same way both the nodes for fixing the wrench are determined and
the
boundary conditions are entered in the plot program or CAD system:
In
the CAD program:
Switch to the
layer Z88RBD and write with the TEXT function into any free place:
Z88I2.TXT 16 (16
Boundary conditions altogether)
RBD 1 11 2 1 -7143 (1st BC: Node 11, DOF 2, Force -7,143 N assumed)
RBD 2 143 2 1 7143 (2nd BC: Node 143, DOF 2, Force 7,143 N assumed)
RBD 3 216 1 2 0 (3rd BC: Node 216, DOF 1, Displacement 0 (= fixed)
assumed)
RBD 4 216 2 2 0
RBD 5 220 1 2 0
RBD 6 220 2 2 0
RBD 7 227 1 2 0
RBD 8 227 2 2 0
RBD 9 231 1 2 0
RBD 10 231 2 2 0
RBD 11 238 1 2 0
RBD 12 238 2 2 0
RBD 13 242 1 2 0
RBD 14 242 2 2 0
RBD 15 249 1 2 0
RBD 16 249 2 2 0
with
an Editor:
Design the
boundary condition file Z88I2.TXT by
editing:
16 (16 Boundary
conditions altogether)
11 2 1 -7143 (1st
BC: Node 11, DOF 2, Force -7,143
N assumed)
143 2 1 7143
(2nd BC: Node 143, DOF 2, Force 7,143 N assumed)
216 1 2 0 (3rd BC: Node
216, DOF 1, Displacement 0
(= fixed) assumed)
216 2 2 0
220 1 2 0
220 2 2 0
227 1 2 0
227 2 2 0
231 1 2 0
231 2 2 0
238 1 2 0
238 2 2 0
242 1 2 0
242 2 2 0
249 1 2 0
249 2 2 0
Input for stress
calculation:
In
the CAD program:
Switch to the
layer Z88GEN and write with the TEXT function into any free place:
Z88I3.TXT 3
0 1 ( 3x3
Gauss points for stresses, KFLAG 0,
von Mises stresses)
Export the drawing as DXF
file with the name Z88X.DXF, then start the CAD converter Z88X with the
option
"from Z88X.DXF to Z88I*.TXT" (DXF -> I*). The CAD converter
produces the three Z88 input files Z88I1.TXT, Z88I2.TXT, Z88I3.TXT.
With
an editor:
Enter in the
parameter file for the stress processor Z88I3.TXT
(cf. Chapter 3.5):
3 0 1 ( 3x3 Gauss
points for stresses, KFLAG 0,
von Mises stresses)
Now launch the Cholesky
solver Z88F and
then the stress
processor Z88D. You will see
during the run of Z88F, that 14.848 memory places (8
bytes each) are needed in the total stiffness matrix GS. NKOI, i.e. memory places in the coincidence
vector KOI, is
printed as 540 (4 Bytes each). Well, this also matches Z88.DYN. Where
does the
number 540 come from? 66 finite elements of the type Plane Stress No.7
with 8
nodes each, makes 66*8 = 528. The number 540 results because Z88F
always calculates
20 nodes for security reasons for the last finite element. Thus, NKOI
becomes
here: 65*8 + 20 = 540.
You calculate the nodal
forces with Z88E.
5.1.2
Results
The Cholesky solver
Z88F provides the following output files:
Z88O0.TXT stores the processed structure data. It is mainly
intended for
documentation purposes, but also shows if your input file Z88NI.TXT for
the
mesh generator did what you meant it to do.
Z88O1.TXT stores the processed boundary conditions: For
documentation
purposes. And: Was your boundary conditions input in Z88I2.TXT
correctly
interpreted ?
Z88O2.TXT, the displacements, the main task and solution of the
FEA
problem.
The stress processor Z88D uses internally the calculated
displacements
from Z88F and stores Z88O3.TXT, the calculated stresses. The
results in
Z88O3.TXT depend on the header parameters in Z88I3.TXT.
The nodal force processor Z88E
uses internally the calculated deflections of Z88F and stores Z88O4.TXT,
the computed nodal forces.
The OpenGL plot program Z88O
can use three
methods
of view for reduced stresses: the average reduced stresses per node,
average reduced
stresses per element and the reduced stresses computed in the Gauss
points. These
three methods can give very different results depending on stress
peaks. Usually
the stresses computed in the Gauss points give the highest and most
exact
values depending on the kind of structure and boundary conditions.
Otherwise,
if you get nearly the same values for all three methods of view, then
your kind
of structure and the boundary conditions are very equable.