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

- in the CAD program (from Z88I1.TXT to Z88X.DXF, I1 -> DXF) after conversion with Z88X or
- with the Z88 plot program Z88O for defining the boundary conditions:

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.

1st method of view: Reduced stresses in the corner nodes (which are in fact computed from the Gauss points around a node).

2nd method of view: Reduced stresses as a mean value per element.

3rd method of view: Reduced stresses in the Gauss points.