Step 1 |
Start FEMGV and read in the results file.
UTILITY READ VIEWDATA TUTLUG.FVI |
(If the results file is available from chapter 5 then this should be used in preference) |
Step 2 |
Access the lug model within FEMVIEW
FEMV TUTLUG |
Step 3 |
Confirm that two loadcases exist
UTILITY TABULATE LOADCASES |
Step 4 |
Select the type of results attribute to be considered
RESULTS LOAD LC0001 RESULTS NODAL DISPLACE ALL |
Step 5 |
Perform the combination
RESULTS CALCULATE COMBINE CMB1 (CMB1 is the name for the combined loadcase) LC0001 (Source loadcase) 1.5 (Scaling factor) LC0002 2.5 GO (Perform the scaling and the combination and store the results) 1.5*L1 + 2.5*L2 (Up to 20 characters are available to describe the combination) CURRENT (Select the attribute to be combined) |
It is worth noting at this stage that in addition to combining individual attributes of a loadcase it is also possible to combine all the attributes for the source loadcases. It is left to the user to make sure that all the combinations performed are meaningful.
Step 6 | Confirm that a third loadcase has been created |
The third loadcase should be shown as a combination loadcase containing only
displacements.
UTILITY TABULATE LOADCASES |
Step 7 | Select a loadcase and nodal stresses |
Note that because the combination loadcase becomes the current loadcase it
is necessary to re-select one of the original loadcases before the stresses
can be selected.
RESULTS LOAD LC0001 RESULTS NODAL ST SXX |
Step 8 |
Perform the combination
RESULTS CALCULATE COMBINE CMB1 Note that because the combination definition already exists for CMB1 it will automatically be used to combine the stresses. |
Step 9 |
Confirm that nodal stresses have been added to the combination loadcase
UTILITY TABULATE LOADCASES |
Step 10 |
View the mesh and present contours for the combination loadcase
VIEW MESH RESULTS LOADCASE CMB1 RESULTS NODAL ST SYY PRESENT CONTOUR LEVELS 10 |
Step 11 Calculate and present the Von Mises stresses for the combination loadcase.
Before the next two calculations can be performed a stress attribute must be selected.
RESULTS CALCULATE VONMISES
DRAWING DISPLAY
Step 12 |
Now calculate the principal stresses for this loadcase and present the resulting
principal stress vectors.
RESULTS CALCULATE P-STRESS P1 2DSORT PRESENT VECTORS |
Note that in the general case there will be three principal stresses available at a node (P1, P2 and P3). The sort feature allows the maximum principal stresses at each node to be associated with P1, the minimum principal stress to be associated with P3 and the remaining value to be P2. For three dimensional models, this is achieved with the 3DSORT option. For two dimensional models when one of the principal stresses is zero, this is omitted from the sort (when 2DSORT is specified) and the minimum principal stress is associated with P2.
Step 13 | Now you can calculate TRESCA (the difference between the maximum and minimum principle stress) stress using the RESULTS CALCULATE EXPRESSION command. |
First, you need to save the principle stress results in a new loadcase.
RESULTS CALCULATE EXPRESSN LC3 (new loadcase name) ! 20 Character Ref => pr stress P-STRESS NEWISH (this is the expression) 2DSORT LOADCASE LC0001 1 NODAL STRESS (define NEWISH) ! SCALE FACTOR (1.0) =>
! OUTPUT ATTRIBUTE NAME => NEWISH ! COMPONENT NEWISH( 1 ) NAME => P1 ! COMPONENT NEWISH( 2 ) NAME => P2 ! COMPONENT NEWISH( 3 ) NAME => P3
View the principle stress results.
RESULTS LOADCASE LC3 RESULTS NODAL NEWISH P1 PRESENT CONTOUR LEVELS RESULTS NODAL NEWISH P2 PRESENT CONTOUR LEVELS
Next, is to calculate another expression to define TRESCA stress.
RESULTS CALCULATE EXPRESSN LC3 (or you can use a new loadcase name) MAXP SUBTRACT MINP (this is the expression) LOADCASE LC3 NODAL NEWISH P1 (define MAXP) ! SCALE FACTOR (1.0) =>
LOADCASE LC3 NODAL NEWISH P2 (define MINP) ! SCALE FACTOR (1.0) =>
! OUTPUT ATTRIBUTE NAME => TRESCA
View TRESCA stress results.
RESULTS LOADCASE LC3 RESULTS NODAL TRESCA PRESENT CONTOUR LEVELS
|