Next: Loadcase names Up: Program Capabilities Previous: Topology and Coordinates
Next: Loadcase names
Up: Program Capabilities
Previous: Topology and Coordinates
These results go into an Elementwise Gaussian data set, the gauss points being those specified by the user in the data module `POINTS.FOR.STRESSING' in his PAFEC input data file. This specifies the number of equally spaced stressing points along the beam. If this module is omitted in the input file a default one will be generated specifying only the nodes as stressing points.
PAFEC recognises two types of beam section : rectangular and tubular, depending on the entries the user has specified in the 'BEAMS' module under the columns `INNER',`OUTER' and `THICKNESS'. All section types have 3 shear forces (SXYSHEAR, SYZSHEAR, SZXSHEAR) and 3 bending moments (MXXBEND, MYYBEND, MZZBEND).
Rectangular sections have 7 stress components : AXIAL, AVETAUY, AVETAUZ, BENSIGY, BENSIGZ, CFSTMAX and CFSTMIN, and tubular sections have 9 the extra 2 being RESBNST and TORSIGX.
In FEMVIEW, to access these results, for example SXYSHEAR for loadcase L1 one might do
RESULTS LOADCASE L1
RESULTS GAUSSIAN BEAMLOAD SXYSHEAR
and to see the results for a particular beam, number 4 for example :
PRESENT GRAPH BEAM 4
or to see the results for a particular line of beams :
PRESENT GRAPH LINE 1 etc.
These stress results are not averaged and do not contribute to the averaged nodal stress results. Beams results come for one surface only.
Diplacements and eignvectors are processed for all elements and are stored in a nodal data set. They are always returned in a global system. To access displacement results from within FEMVIEW one might enter
RESULTS LOADCASE L1
RESULTS NODAL DISP DX
and to get a contoured display PRESENT CONTOURS LEVEL 30
or to see the deformed shape VIEW MESH DEFORM DX etc.
Eigenvectors are treated in a similar manner except that to see the deformed shape one must do VIEW MESH DEFORM USE EIGN DX etc.
RESULTS LOADCASE L1
RESULTS NODAL EIGN DX
PRESENT CONTOURS LEVEL 30 etc.
The number of eigenvalues is the number of MASTERS that the user specified in the
MODES.AND.FREQUENCIES module in the PAFEC input file.
It should be noted that these results are not returned if
the pafec job didn't successfully complete to the end of phase 4, or
the user specified recovery of `GEOMETRY' or
the user specified that displacements/eignvectors should not be returned.
If these results are not recovered, natuarally they cannot be accessed from within FEMVIEW.
The attribute and component names used by the interface program in returning displacements and eignvectors are given in Table 2.3.
RESULTS LOADCASE L1
selects the attribute
RESULTS NODAL TEMP
and then to see a contoured display
PRESENT CONTOURS LEVEL 30 etc.
Beams and non-beams are treated in very seperate ways and there is no contribution from beams in the averaging process to create the nodewise data set for stresses AVSTRESS Stresses for beams are discussed in the section above on Results for beams and here we will restrict attention to plates,shells and solids.
Stresses for post-processing are stored in the file usually called 'jobname'.SS which is generated in phase 9 of a PAFEC run. They are stored in the global system but if the user specifies the local element system, stresses for isotropic elements will be transformed.
The user may select to recover the stress results for a single specified loadcase by using the command RECOVER SELECT-LOAD. It is also possible to recover only Element or Averaged stresses. These commands are discussed in Chapter 2.
STRESS is an elementwise data set containing stresses for each node and each surface in the specified axis system. To access these results one must first select the loadcase
RESULTS LOADCASE L1
and then the attribute
RESULTS NODAL STRESS SXX.
The command PRESENT CONTOURS LEVEL 30 will generate a contoured display.
Some isotropic PAFEC element types produce stresses for only one surface and others produce them for three. To look at the stresses for the middle surface for example, one might try RESULTS NODAL STRESS SXX as before and then to access the middle surface do RESULTS RANGE SURFACE 2 and then do PRESENT CONTOURS LEVEL 30.
The procedure for accessing stress results for othotropic elements is slightly different to that for isotropic elements in that stress results are obtained for the former at each of 3 surfaces for each layer specified in the PAFEC data module LAMINATES. Consequently there are 3 times as many results for each `Surface'. For presentation of stress results, each layer in an orthotropic element is represented by a surface, with a result array of 18 -
TSXX TSYY TSZZ TSXY TSYZ TSZX
SXX SYY SZZ SXY SYZ SZX
BSXX BSYY BSZZ BSXY BSYZ BSZX
6 components for each of the 3 internal stressing surfaces within the layer. So to access the top surface of the nth layer, for example, one might : select the attribute
RESULTS ELEMENT STRESS TSXX
RESULTS RANGE SURFACE n
PRESENT CONTOURS LEVEL 30 .
To access the middle surface one might select the attribute
RESULTS ELEMENT STRESS SXX
or for the bottom surface
RESULTS ELEMENT STRESS BSXX.
For example to access results for the fifth laminate :
RESULTS LOADCASE L1
RESULTS ELEMENT STRESS BSXY
RESULTS RANGE SURFACE 5
PRESENT CONTOURS LEVEL 30
will give a contoured display of the stresses on the bottom surface of the fifth laminate. Stress results for orthotropic elements are returned in the principal material directions specified in the PAFEC data module LAMINATES in the entries AXIS.SET ANG1 ANG2 ANG3. Omitting these entries will cause the default element axis to be used.
AVSTRESS is a nodal data set calculated within the interface program using the element data used to make the data for STRESS, and the material data. It calculates the data for a node by averaging the global stress contributions from all the elements connected to a node; except that averaging is not performed across a material boundary and contributions from orthotropic elements or beams are not considered. Averaged nodal stresses will be calculated for each material present at a node execpt for those represented by orthotropic elements or beams. The procedure adopted for averaging stress results for isotropic elements when a element with one surface meets one with three, is to treat the one surfaced element as if it had three surfaces but with zero results for the lower 2 surfaces.
The attribute and component names used by the interface program in returning stress results are given in Table 2.4.
Femsys Limited