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
diskettes
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: Compute > Z88X > Type
Conversion
> 6 from Z88X.DXF to Z88NI.TXT > Compute > Go, UNIX:
pushbutton DXF <-> Z88 with radiobutton DXF -> NI
(Z88-Commander) or z88x -nifx (console or X-term).
Z88P, looking at the super structure.
The error message should not disturb you, because Z88P still has no
.STO file
and therefore expects Z88I1.TXT to load (which is not yet present).
However,
you want to load Z88NI.TXT: Windows: Plot > Z88P
> File
> Structure File > Z88NI.TXT, UNIX: with the
Z88-Commander
pushbutton Plot feature and radiobutton Z88P or enter
from an
X-term z88p, enter z88ni.txt
in textfield Struc., press Return. Now try Z88O.
Z88N, mesh generator, reads
Z88NI.TXT and produces Z88I1.TXT. Windows: Compute >
Z88N >
Compute > Go. UNIX: pushbutton Z88N
(Z88-Commander) or z88n
(console or X-term).
Z88P, look at the finite element
structure. Z88P now has a Z88P.STO file from the former Run and expects
Z88NI.TXT to load. Now you want to load Z88I1.TXT. Windows: Plot
>
Z88P > File > Structure File > Z88I1.TXT, UNIX:,
with the
Z88-Commander pushbutton Plot feature and radiobutton Z88P
or
enter from an X-term z88p,
enter z88i1.txt
in textfield Struc., press Return. This could have been avoided
if you
would have deleted the file Z88P.STO before start of Z88P, because
Z88P.STO
stores all parameters of the last Z88P run. If Z88P.STO does not exist,
Z88P
works with default values, for example Z88I1.TXT as structure file.
Z88F, calculates displacements. Use the
Compactmode: Windows: Compute > Z88F > Mode >
Compactmode,
> Compute > Go, UNIX: pushbutton Z88F with
radiobutton Compact
M (Z88-Commander) or z88f -c (console or X-term).
Z88D, calculates stresses. Windows: Compute
> Z88D > Compute > Go,
UNIX: pushbutton Z88D (Z88-Commander) or z88d
(console or
X-term).
Z88P, look at the deflected finite
element structure. Z88P has a .STO file and thus features correct
parameters. The
displacements are multiplied per default by the factor 100, which is a
bit too
large for this example. Windows: Plot > Z88P >
Factors >
Deflections > enter 10 for FUX and FUY
each,
> Structure > Deflected UNIX: Z88-Commander:
pushbutton Plot
feature and radiobutton Z88P or enter from an X-term z88p, enter 10 into both textfields FUX
and FUY,
press either a Return for each textfield or pushbutton Regen.
Click
radiobutton Deflected. Because Z88D has been already run, you
can
display the von Mises stresses right now. Go to Undeflected
structure. Windows:
> Mises Stresses > Show von Mises stresses. UNIX:
Togglebutton Mises . Furthermore you could produce a plotter
file,
perhaps undeflected and without von Mises stresses. Windows: >
Output > Plotter. UNIX: Pushbutton Plot. The
resulting
plot file Z88O6.TXT contains HP-GL commands.
Z88E, nodal forces calculation. Windows:
Compute > Z88E > Compute > Go, UNIX:
pushbutton Z88E
(Z88-Commander) or enter z88e from a console or X-term.
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 ( 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 Z88P.
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 (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 Z88P.
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 should
choose for Z88F the flag -c (Compactmode) because
only one set of boundary conditions is available cf. section 2.1.
Basically, z88f
-c (Compactmode) is always correct. 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 following picture of
the plot program shows the deflected structure for FUX and FUY = 10
each
(magnifications of the deflections):
The nodal force processor Z88E
uses internally the calculated deflections of Z88F and stores
Z88O4.TXT,
the computed nodal forces.
Z88P plots the von Mises
stresses zoomed around the area of the element 12, which features the
biggest
von Mises stresses as pointed below. The letter J corresponds to a von
Mises
stress from 647 to 718 N/mm**2. Now do the same with Z88O but
keep in mind that the maximum stresses are
somewhat lower, ref. Chp. 2.11.