Engineering Solutions

Pressure Load on Beam Elements

Pressure Load on Beam Elements

 Previous topic Next topic No expanding text in this topic  

Pressure Load on Beam Elements

 Previous topic Next topic JavaScript is required for expanding text JavaScript is required for the print function  

HyperMesh 11.0 supports pressure load on bar and rod elements, which means you can now import the pressure load [SFBEAM] applied on ANSYS BEAM elements. The following items are supported under this feature:

•Import pressure load applied on BEAM3, BEAM4, BEAM23, BEAM44 elements. Import restrictions are explained below.
•Use the Pressure panel to apply SFBEAM load on beam elements.
•Export pressure load applied on BEAM elements in HyperMesh as SFBEAM load in ANSYS solver deck. The Export feature is explained in detail below.

 

Importing pressure load

SFBEAM is the key word command in ANSYS decks to apply pressure load on BEAM elements. This command line has following arguments:

SFBEAM,ELEM,LKEY,Lab,R5.0,DIOFFST,DJOFFST

 

ELEM is element ID and Lab is always pres(pressure). LKEY is load key number which determines the face of the beam where the pressure load is applied. You need to refer to the ANSYS solver documentation to know the face of the beam and corresponding LKEY number as it changes from BEAM to BEAM.

 

Restrictions

1.The HyperMesh-ANSYS interface presently supports following LKEY values for each BEAM element. You can import SFBEAM load with these LKEYs.

ELEMENT TYPE

SUPPORTED LKEYs

BEAM3

1, 3, 4

BEAM4

1, 2, 4, 5

BEAM23

1, 3, 4

BEAM24

1, 2, 4, 5

BEAM44

1, 2, 4, 5

BEAM54

1, 3, 4

BEAM188

1, 2, 4, 5

BEAM189

1, 2, 4, 5
2.In the above arguments, DIOFFST, DJOFFST which define offset values for pressure value at node I and J are not supported in HyperMesh.
3.SFLOAD also allows you to apply pressure load that varies across the length of the beam. But this type of load is not supported in HyperMesh 9.0. Only pressure load with constant value can be imported.

 

Applying pressure on BEAM elements in HyperMesh for the ANSYS interface

•You can apply pressure load in HyperMesh on any bar2, bar3 and rod, elements. But you can export only those pressure loads which are applied on BEAM element types that have been mentioned earlier as supported elements.
•By default if no option for direction is selected, pressure is applied on ‘element – y’ direction. You can use different options available in pressure load panel to specify the direction of the load.
•The ANSYS solver allows pressure on beam elements in only specified faces of the elements (as mentioned by LKEYS). In other words, pressure on beam elements is applied in element co-ordinate system.  You should keep this in mind before determining the direction of the pressure.
•You cannot apply pressure load that varies across the length of the BEAM even though it is allowed in the ANSYS Solver.
•Load offsets at node I and J are not supported.

 

Exporting pressure load on BEAM elements from HM for Ansys interface

•Pressure on Beams is exported as SFBEAM cards.
•Pressure only applied on BEAM3, BEAM4, BEAM23, BEAM44, BEAM54, BEAM188, BEAM189 elements will be exported.
•Pressure applied in any arbitrary directions is resolved in to corresponding element systems and relevant LKEYs will be assigned while exporting. Hence when you import the deck back to HyperMesh, you will see resolved loads.