Next: Error Messages Up: Load Definition Previous: Boundary Data

Load Data

The association of a FEMGEN load with an ABAQUS step is achieved via the FEMGEN loadcase number argument in the 'PROPERTY LOAD' command. All loads with loadcase number 1 will be associated with the first ABAQUS step and so on.

All FEMGEN load commands have the following form:

PROPERTY LOAD load_type [load_name] [loadcase_no] part1_name/ALL 
                        [part2_name] args

**Table 7.3:** FEMGEN load command arguments.
Argument	Meaning
load_type	Load type (e.g. PRESSURE).
load_name	Optional load name identifier (for reference purposes).
loadcase_no	Optional FEMGEN loadcase No. (ABAQUS step).
part1_name/ALL	Geometric part to which load is applied.
part2_name	Optional second part to specify which side of part1 is loaded (element faces loads only).
args	Varying arguments depending on load_type

Notes:

1.: The part name may be either a single part in the model geometry or a set of such parts. In either case the interface expands the geometry-based load definition into a series of nodal, element face, or whole element loads. The user does not need to consider node/element numbers or element face identifiers; the interface derives these automatically.
2.: The use of ALL for the part name is only valid in circumstances where all parts of the model have a valid geometry for the load in question. For example a pressure load applied to ALL of a model which contains FEMGEN bodies would be invalid. A temperature load applied to the same model would be valid.
3.: The optional second part is only for loads that are applied to element faces. There may be an ambiguity over which elements are loaded, when part1 is attached to more than one part with a next higher order, e.g. a line used by two surfaces. Specifying part2 can resolve such ambiguity. The command is restricted to only allow certain combinations of parts i.e. point/line, line/surface and surface/body. In the case of sets, a similar relationship is required between the parts in the set.
4.: The command arguments vary with the load type and are described in the following sections. For all loads types, the actual load values (be it per unit depth, area, or circumference) must be entered correctly by the user. The interface, for example, does not attempt to multiply load values by element thicknesses or areas.

Notes on advanced loading:

Load Masks, Local Coordinate Systems, Space Curves and Time Curves, defined with FEMGEN 'CONSTRUCT' command, can be attached to loads using the FEMGEN command 'PROPERTY ATTACH'. The interface program supports these new features for most loads. More detailed information on advanced loading may be found in the FEMGV Users Manual.
When a time curve is attached to a load, the program adds the ABAQUS 'AMPLITUDE' parameter to the load card wherever applicable. The FEMGEN command 'CONSTRUCT TCURVE' will create a '*AMPLITUDE' card in the ABAQUS input deck. The FEMGV Users Manual gives more detailed information on the construction of time curves. If the data for the '*AMPLITUDE' definition is large, the Interface Program writes it in a separate file which takes the name of the time curve 'timecurve_name.ins'. Furthermore, the 'SMOOTH STEP' option can be allocated to '*AMPLITUDE' when the time curve name starts with 'SMO'.

The following load types are supported:

**Table 7.4:** ABAQUS Load Types Supported
Generic Load Type	FEMGEN Load Type	Application
Uniform Pressure	PRESSURE	Element faces.
Concentrated Force	FORCE	Nodes.
Prescribed Displacement	DISPLACE	Nodes.
Gravity or Body Force	GRAVITY	Whole elements.
Temperature	TEMPERAT	Nodes.
Surface Flux	HEAT	Element faces.
Forced Convection	HEAT	Element faces.
Hydrostatic Pressure	HYDROSTA	Element faces.
Centrifugal Force	CENTRIFU	Whole elements.
Coriolis Force	CENTRIFU	Whole elements.
Rotary Acceleration	CENTRIFU	Whole elements.
Distributed Seepage	DFLOW	Element faces.
Seepage Coefficients	FLOW	Element faces.
Fluid Mass Flow Rate	MFLOW	Nodes.
Concentrated Electric Charge	CECHARGE	Nodes.
Distributed Electric Charge	DECHARGE	Element faces.
Concentrated Heat flux	CFLUX	Nodes.
Radiation	RADIATE	Element faces.
Interface Contact	C-INTERF	Contact Element Set
Model Change	MODEL-CH	Whole Elements.
Velocity	VELOCITY	Nodes.

Uniform Pressure

PROPERTY LOAD PRESSURE [load_name] [loadcase_no] part_name/ALL 
                       [part2_name] args

**Table 7.5:** PRESSURE load arguments.
Argument	Meaning
load_name	FEMGEN load name.
loadcase_no	FEMGEN loadcase number (links load to an ABAQUS step).
part_name	Geometry containing element faces/edges.
part2_name	Optional second part containing the elements to be loaded.
arg1	Pressure value.
arg2	Degree of Freedom Indicator (0,1,2,3).

Notes:

1.: Valid part types are beams, plate edges, shell faces, brick faces.
2.: The degree of freedom indicator should be set to zero (normal) for all part types except beams where it should be set to 1, 2, or 3.
3.: Part type 'ALL' is supported only for shell faces.
4.: Local Coordinate System attached to Pressure load is not supported.

Example FEMGEN Command:

PROPERTY LOAD PRESSURE LO1 1 L2 100 0

Corresponding ABAQUS Input Deck:

*ELSET, ELSET=FL2  
    4    8   12   16
*DLOAD, OP=NEW
FL2   , P2 ,  100.0000

Concentrated Force

PROPERTY LOAD FORCE [load_name] [loadcase_no] part_name/ALL args

**Table 7.6:** FORCE load arguments.
Argument	Meaning
load_name	FEMGEN load name.
loadcase_no	FEMGEN loadcase number (links load to an ABAQUS step).
part_name	Any geometry containing nodes.
arg1	Force value.
arg2	Degree of Freedom Indicator (1,2,3,4,5,6).

Notes:

1.: The interface will simply apply the same force value to all nodes attached to the specified geometry ie. it will not divide the force value by the number of nodes.
2.: Part type 'ALL' is supported.

Example FEMGEN Command:

PROPERTY LOAD FORCE LO1 1 P3 100 2

Corresponding ABAQUS Input Deck:

               
*NSET, NSET=P3  
   25
*CLOAD, OP=NEW
P3   ,    2 ,   100.0000

Prescribed Displacement

PROPERTY LOAD DISPLACE [load_name] [loadcase_no] part_name/ALL args

**Table 7.7:** DISPLACE load arguments.
Argument	Meaning
load_name	FEMGEN load name.
loadcase_no	FEMGEN loadcase number (links load to an ABAQUS step).
part_name	Any geometry containing nodes.
arg1	Displacement value.
arg2	Degree of Freedom Indicator (1,2,3,4,5,6,7).

Notes:

1.: The interface will simply apply the same displacement value to all nodes attached to the specified geometry ie. it will not divide the displacement value by the number of nodes.
2.: Part type 'ALL' is supported.
3.: Prescribed displacement and more general prescribed values can be defined with the FEMGEN command 'PROPERTY BOUNDARY PRESCRIBE', see above.

Example FEMGEN Command:

PROPERTY LOAD DISPLACE LO1 1 P4 100 2

Corresponding ABAQUS Input Deck:

               
*NSET, NSET=P4  
   21
*BOUNDARY
 P4  ,   2,   2,  100.0000

Gravity and Body Force

PROPERTY LOAD GRAVITY [load_name] [loadcase_no] part_name/ALL args

**Table 7.8:** GRAVITY load arguments.
Argument	Meaning
load_name	FEMGEN load name.
loadcase_no	FEMGEN loadcase number (links load to an ABAQUS step).
part_name	Any geometry containing whole elements.
arg1	Gravitational Constant or body force value.
arg2	Degree of Freedom Indicator (1,2,3).

Notes:

1.: The interface will apply the same gravitational load to all elements on the specified part.
2.: Part type 'ALL' is supported.
3.: If the load name starts with 'BODYF', a body force will be applied instead of a gravity load. The ABAQUS load label will then depend on the degree of freedom indicator: 'BX' for 1; 'BY' for 2 and 'BZ' for 3.

Example FEMGEN Command:

PROPERTY LOAD GRAVITY LO1 1 S1 -9.814 2

Corresponding ABAQUS Input Deck:

                    
*DLOAD, OP=NEW
S1   , GRAV,  -9.814000   , 0.0000000    ,  1.000000    , 0.0000000

Temperature

PROPERTY LOAD TEMPERAT [load_name] [loadcase_no] part_name/ALL args

**Table 7.9:** TEMPERAT load arguments.
Argument	Meaning
load_name	FEMGEN load name.
loadcase_no	FEMGEN loadcase number (links load to an ABAQUS step).
part_name	Any geometry containing nodes.
arg1	Temperature value.

Notes:

1.: The interface will apply the same temperature value to all nodes attached to the specified geometry.
2.: Part type 'ALL' is supported.

Example FEMGEN Command:

PROPERTY LOAD TEMPERAT LO1 1 L4 100

Corresponding ABAQUS Input Deck:

     
*NSET, NSET=L4  
   21   16   11    6    1
*TEMPERATURE, OP=NEW
L4   ,   100.0000

Surface Flux

PROPERTY LOAD HEAT [load_name] [loadcase_no] part_name/ALL [part2_name]
                   args

**Table 7.10:** HEAT load arguments (for surface fluxes)
Argument	Meaning
load_name	FEMGEN load name.
loadcase_no	FEMGEN loadcase number (links load to an ABAQUS step).
part_name	Geometry containing element faces.
part2_name	Optional second part containing the elements to be loaded.
arg1	Reference flux.
arg2	0
arg3	Reference flux for S2 side of shells.

Notes:

1.: The interface will apply the reference flux to all element faces on the specified part.
2.: Arg2 must be set to zero; non-zero values will trigger the forced convection load type.
3.: Part type 'ALL' is supported only for shell faces.
4.: Parameter arg3 is used only for shell elements where it is desired to apply different flux values to either side of the shell. arg1 is applied to the 'S1' side of the shell and arg3 to the 'S2' side.

Example FEMGEN Command:

PROPERTY LOAD HEAT LO1 1 L3 123 0

Corresponding ABAQUS Input Deck:

  
*ELSET, ELSET=FL3  
   13   14   15   16
*DFLUX, OP=NEW
FL3   , S3 ,   123.0000

Forced Convection

PROPERTY LOAD HEAT [load_name] [loadcase_no] part_name/ALL [part2_name] 
                   args

**Table 7.11:** HEAT load arguments (for forced convection)
Argument	Meaning
load_name	FEMGEN load name.
loadcase_no	FEMGEN loadcase number (links load to an ABAQUS step).
part_name	Geometry containing element faces.
part2_name	Optional second part containing the elements to be loaded.
arg1	Reference film coefficient.
arg2	Reference sink temperature.
arg3	Reference film coefficient for S2 side of shells.
arg4	Reference sink temperature for S2 side of shells.

Notes:

1.: The interface will apply the reference film coefficient and sink temperature to all element faces on the specified part.
2.: Arg2 must be non-zero; zero values will trigger the surface flux load type.
3.: Part type 'ALL' is supported only for shell faces.
4.: Parameters arg3 and arg 4 are used only for shell elements where it is desired to apply different values to either side of the shell. arg1 and arg2 are applied to the 'S1' side of the shell and arg3 and arg4 to the 'S2' side.

Example FEMGEN Command:

PROPERTY LOAD HEAT LO1 1 L2 123 456

Corresponding ABAQUS Input Deck:

                   
*ELSET, ELSET=FL2  
    4    8   12   16
*FILM, OP=NEW
FL2   , F2 ,   456.0000     ,   123.0000

Hydrostatic Pressure

PROPERTY LOAD HYDROSTA [load_name] [loadcase_no] part_name/ALL 
                       [part2_name] args

**Table 7.12:** HYDROSTA load arguments.
Argument	Meaning
load_name	FEMGEN load name.
loadcase_no	FEMGEN loadcase number (links load to an ABAQUS step).
part_name	Geometry containing element faces.
part2_name	Optional second part containing the elements to be loaded.
arg1	Pressure at point name1.
arg2	Degree of Freedom Indicator (0).
arg3	Point name1.
arg4	Point name2.
arg5	Pressure at point name2.

Notes:

1.: Valid part types are plate edges, shell faces, brick faces.
2.: The degree of freedom indicator should be set to zero (normal) for all part types.
3.: Part type 'ALL' is supported for shell faces.
4.: ABAQUS does not support a hydrostatic head in an arbitrary direction; it must be either in the global Y or Z directions depending on the element types used. For 2D models, the interface will use the Y coordinate of point name1 to define the position where pressure = arg1, and the Y coordinate of point name2 to define the position where pressure = arg5.
For 3D models, the interface will use the Z coordinate of point name1 to define the position where pressure = arg1, and the z coordinate of point name2 to define the position where pressure = arg5.

Example FEMGEN Command:

PROPERTY LOAD HYDROSTA LO1 1 L2 100.00 0 P3 P2 0

Corresponding ABAQUS Input Deck:

*ELSET, ELSET=FL2  
    4    8   12   16
*DLOAD, OP=NEW
FL2   , HP2 ,   100.0000     ,  0.0000000     ,   100.0000

Centrifugal Force, Coriolis Force, Rotary Acceleration

PROPERTY LOAD CENTRIFU [load_name] [loadcase_no] part_name/ALL args

**Table 7.13:** CENTRIFU load arguments.
Argument	Meaning
load_name	FEMGEN load name, determines ABAQUS load label.
loadcase_no	FEMGEN loadcase number (links load to an ABAQUS step).
part_name	Any geometry containing whole elements.
arg1	Magnitude.
arg2	Degree of Freedom Indicator (for display purposes only).
arg3	Point name1 (first point on rotation axis).
arg4	Point name2 (second point on rotation axis).

Notes:

1.

The FEMGEN load name is used to determine the ABAQUS load label.

If the name starts with 'CNTRF', a centrifugal load with label 'CENTRIF' is applied and the magnitude is specified as ${\omega^2}$ .
If the name starts with 'ROTA', a rotary acceleration load with label 'ROTA' is applied.
If the name starts with 'CORIO', a Coriolis load with label 'CORIO' is applied and the magnitude is specified as ${\omega}$ .
If the name does not start by 'CNTRF' nor 'ROTA' nor 'CORIO', a centrifugal load with label 'CENT' is applied and the magnitude is specified as ${\rho\omega^2}$ .

2.

The interface will apply the same load to all elements on the specified part.

3.

The degree of freedom indicator is not used in the load definition but is used for display purposes in FEMGEN.

4.

Part type 'ALL' is supported.

Example FEMGEN Command:

PROPERTY LOAD CENTRIFU LO9 1 S1 100.00 1 P5 P6

Corresponding ABAQUS Input Deck:

*DLOAD, OP=NEW
 S1   CENT  100.0 -10.00 0.0000 0.0000 0.0000 1.000 0.0000

Distributed Seepage

PROPERTY LOAD DFLOW [load_name] [loadcase_no] part_name/ALL 
                    [part2_name] args

**Table 7.14:** DFLOW load arguments.
Argument	Meaning
load_name	FEMGEN load name.
loadcase_no	FEMGEN loadcase number (links load to an ABAQUS step).
part_name	Geometry containing element faces.
part2_name	Optional second part containing the elements to be loaded.
arg1	Reference seepage magnitude.

Notes:

1.: The interface will apply the reference seepage magnitude to all element faces on the specified part.
2.: Part type 'ALL' is not supported.

Example FEMGEN Command:

PROPERTY LOAD DFLOW LO10 1 L1 100.00

Corresponding ABAQUS Input Deck:

                   
*ELSET, ELSET=FL1  
    1    2    3    4
*DFLOW, OP=NEW
FL1   , Q1 ,   100.0000

Seepage Coefficients

PROPERTY LOAD FLOW [load_name] [loadcase_no] part_name/ALL 
                   [part2_name] args

**Table 7.15:** FLOW load arguments.
Argument	Meaning
load_name	FEMGEN load name.
loadcase_no	FEMGEN loadcase number (links load to an ABAQUS step).
part_name	Geometry containing element faces.
part2_name	Optional second part containing the elements to be loaded.
arg1	Reference pore pressure.
arg2	Reference flow coefficient

Notes:

1.: The interface will apply the reference pore pressure and flow coefficient to all element faces on the specified part.
2.: Part type 'ALL' is not supported.

Example FEMGEN Command:

PROPERTY LOAD FLOW LO12 1 S1 100.00 200.00

Corresponding ABAQUS Input Deck:

                   
*ELSET, ELSET=FS1  
    1,    2,    3,    4,    5,    6,    7,    8,    9,   10,   11
*FLOW, OP=NEW
FS1   , Q1 ,   100.0000     ,   200.0000

Fluid Mass Flow Rate

PROPERTY LOAD MFLOW [load_name] [loadcase_no] part_name/ALL args

**Table 7.16:** MFLOW load arguments.
Argument	Meaning
load_name	FEMGEN load name.
loadcase_no	FEMGEN loadcase number (links load to an ABAQUS step).
part_name	Any geometry containing nodes.
arg1	Mass flow rate per unit area (x)
arg2	Mass flow rate per unit area (y)
arg3	Mass flow rate per unit area (z)

Notes:

1.: The interface will apply the mass flow rates to all nodes on the specified part.
2.: It is not necessary to enter all three mass flow rates.
3.: Part type 'ALL' is not supported.

Example FEMGEN Command:

PROPOPERTY LOAD MFLOW LO13 1 P2 1 2 3

Corresponding ABAQUS Input Deck:

 
*NSET, NSET=P2  
    5
*MASS FLOW RATE, OP=NEW
P2   ,   1.000000     ,   2.000000     ,   3.000000

Concentrated Electric Charge

PROPERTY LOAD CECHARGE [load_name] [loadcase_no] part_name/ALL args

**Table 7.17:** CECHARGE load arguments.
Argument	Meaning
load_name	FEMGEN load name.
loadcase_no	FEMGEN loadcase number (links load to an ABAQUS step).
part_name	Any geometry containing nodes.
arg1	Reference magnitude for electric charge.

Notes:

1.: The interface will apply the same reference electric charge to all nodes attached to the specified geometry.
2.: Part type 'ALL' is supported.

Example FEMGEN Command:

PROPERTY LOAD CECHARGE LO14 1 P4 100.00

Corresponding ABAQUS Input Deck:

     
*NSET, NSET=P4  
   21
*CECHARGE, OP=NEW
P4   , ,   100.0000

Distributed Electric Charge

PROPERTY LOAD DECHARGE [load_name] [loadcase_no] part_name/ALL 
                       [part2_name] args

**Table 7.18:** DECHARGE load arguments.
Argument	Meaning
load_name	FEMGEN load name.
loadcase_no	FEMGEN loadcase number (links load to an ABAQUS step).
part_name	Geometry containing element faces.
part2_name	Optional second part containing the elements to be loaded.
arg1	Reference magnitude for electric charge.

Notes:

1.: The interface will apply the reference electric charge to all element faces on the specified part.
2.: Part type 'ALL' is not supported.

Example FEMGEN Command:

PROPERTY LOAD DECHARGE LO16 1 L4 100.00

Corresponding ABAQUS Input Deck:

                   
*ELSET, ELSET=FL4  
    1    5    9   13
*DECHARGE, OP=NEW
FL4   , ES4 ,   100.0000

Concentrated Flux

PROPERTY LOAD CFLUX [load_name] [loadcase_no] part_name/ALL args

**Table 7.19:** CFLUX load arguments.
Argument	Meaning
load_name	FEMGEN load name.
loadcase_no	FEMGEN loadcase number (links load to an ABAQUS step).
part_name	Any geometry containing nodes.
arg1	Flux value.
arg2	Degree of Freedom Indicator (1,2,3).

Notes:

1.: The interface will simply apply the same flux value to all nodes attached to the specified geometry ie. it will not divide the flux value by the number of nodes.
2.: Part type 'ALL' is supported.

Example FEMGEN Command:

PROPERTY LOAD CFLUX LO11 1 P2 100.00 1

Corresponding ABAQUS Input Deck:

               
*NSET, NSET=P2  
    5
*CFLUX, OP=NEW
P2   ,    1 ,   100.0000

Radiation

PROPERTY LOAD RADIATE [load_name] [loadcase_no] part_name/ALL 
                      [part2_name] args

**Table 7.20:** FLOW load arguments.
Argument	Meaning
load_name	FEMGEN load name.
loadcase_no	FEMGEN loadcase number (links load to an ABAQUS step).
part_name	Geometry containing element faces.
part2_name	Optional second part containing the elements to be loaded.
arg1	Reference sink temperature.
arg2	Radiation constant.

Notes:

1.: The interface will apply the reference sink temperature and radiation constant to all element faces on the specified part.
2.: Part type 'ALL' is not supported.

Example FEMGEN Command:

PROPERTY LOAD RADIATE LO18 1 L4 100 200

Corresponding ABAQUS Input Deck:

                   
*ELSET, ELSET=FL4  
    1    5    9   13
*RADIATE, OP=NEW, ZERO= -273.16
FL4   , R4 ,   100.0000     ,   200.0000

Interface Contact

PROPERTY LOAD C-INTERF [load_name] [loadcase_no] part_name/ALL args

**Table 7.21:** C-INTERF load arguments.
Argument	Meaning
load_name	FEMGEN load name.
loadcase_no	FEMGEN loadcase number (links load to an ABAQUS step).
part_name	Any geometry containing whole interface elements.
arg1	Reference value v.

Notes:

1.: This load type can only be applied to interface elements.
2.: Where the value of v is zero, an automatic shrink fit will be specified.
3.: Where the value of v is non-zero, a clearance will be specified.
4.: Part type 'ALL' is not supported.

Example FEMGEN Command:

PROPERTY LOAD C-INTERF LO20 1 S1 1.00000E-02

Corresponding ABAQUS Input Deck (versions 5.4 and above):

                    
*CONTACT INTERFERENCE, TYPE=ELEMENT, OP=NEW
S1   ,  0.1000000E-01

Example FEMGEN Command:

PROPERTY LOAD C-INTERF LO20 1 S1 0

Corresponding ABAQUS Input Deck (versions 5.4 and above):

                    
*CONTACT INTERFERENCE, TYPE=ELEMENT, OP=NEW, SHRINK
S1

For ABAQUS versions below 5.4, the command 'PROPERTY LOAD C-INTERF' creates a '*VALUE' card instead.

Model Change

PROPERTY LOAD MODEL-CH [load_name] [loadcase_no] part_name/ALL args

**Table 7.22:** MODEL-CH load arguments.
Argument	Meaning
load_name	FEMGEN load name.
loadcase_no	FEMGEN loadcase number (links load to an ABAQUS step).
part_name	Any geometry containing whole elements.
arg1	0=REMOVE, 1=INCLUDE

Notes:

1.: This load will either add or remove the elements on the part to which it is applied.
2.: Part type 'ALL' is not supported.
3.: Only Load Masks can be attached to the Model Change load.

Example FEMGEN Command:

PROP LOAD MODEL-CH LO19 1 S1 0

Corresponding ABAQUS Input Deck:

                    
*MODEL CHANGE, OP=REMOVE 
    1,    2,    3,    4,    5,    6,    7,    8,    9,   10,   11

Velocity

PROPERTY LOAD VELOCITY [load_name] [loadcase_no] part_name/ALL args

**Table 7.23:** VELOCITY load arguments.
Argument	Meaning
load_name	FEMGEN load name.
loadcase_no	FEMGEN loadcase number (links load to an ABAQUS step).
part_name	Any geometry containing nodes.
arg1	Velocity value.
arg2	Degree of Freedom Indicator (1,2,3,4,5,6).

Notes:

1.: The interface will simply apply the same velocity value to all nodes attached to the specified geometry.
2.: Part type 'ALL' is supported.

Example FEMGEN Command:

PROPERTY LOAD VELOCITY LO1 1 P4 100 2

Corresponding ABAQUS Input Deck:

               
*NSET, NSET=P4  
   21
*BOUNDARY, TYPE=VELOCITY
 P4  ,   2,   2,  100.0000

Next: Error Messages Up: Load Definition Previous: Boundary Data

Femsys Limited
9/9/1999