14.3 The session

14.3 The session

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 =>

! COMPONENT NEWISH( 2 ) NAME =>

! COMPONENT NEWISH( 3 ) NAME =>

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