Panel to nodes, edges and beams
Each sub type of the panel has a separate function for input; however, the type can be changed, if required, in the property dialogue of the panel.
Common properties:
Load transfer direction
- X (LCS panel) – load is distributed to nodes, edges and beams which are perpendicular to local axis x
- Y (LCS panel) – load is distributed to nodes, edges and beams which are perpendicular to local axis x
- all (LCS panel) – load is distributed to all nodes, edges and beams
- self-explanatory (the same as for standard plate)
LCS Angle [deg]
- self-explanatory (the same as for standard plate)
Layer
- self-explanatory (the same as for standard plate)
Selection of entities
- All – all panel nodes or edges which are supported and the beams that are located in the panel plane are selected for the load generation
- User selection – only selected panel nodes or edges which are supported and the beams that are located in a panel plane are selected for load generation
Weight of loaded nodes/edges/beams
– displays all members which are included to load generation, in the right column the user can define the weight factors for individual members.
Unloaded nodes/edges/beams
– displays the rest of members belonging to panel which are not included to the load generation.
To nodes
Load is distributed only to “outer” (structure) nodes of the panel. The nodes have to be supported by another member.
Example 1
1. Define a simple steel hall.
2. Run Structure service > Load panel > Load to panel nodes and input panels to each span of the hall.
3. Select both gable panels and change Load transfer direction to All (LCS panel).
4. Run View parameter setting dialog using the icon at the bottom of a graphical window or using the (right-mouse-button-click) context menu.
5. Tick option Members 2D on the Structure tab in the Local axes group. Local axes of panels will be displayed. This indicated the orientation of the local z-axis, which is very important as it must “go outward” from the building. Select panels which have the z axis oriented inward into the hall and select item Swap orientation in the Property window.
6. Tick option Highlight supporting edges/nodes in the Structure tab, group Panel. Nodes which are considered for the generation of load are marked.
7. If some nodes of panel are not marked and should be, select the panel and press the action button Update node selection (just for the selected panel) or Update all panels (for all panels).
8. Go to service Load and define two permanent load cases of type - Standard.
9. Input Free surface load with geometry system – Member LCS around the hall in LC1.
10. Input Surface load on 2D members on all panels in LC2.
11. Select e.g. one of gable panels and press the action button Generate loads in its properties. Point forces are generated In all its nodes.
12. Run Calculation to generate point forces in the whole structure.
To edges
Load is distributed only to “outer” edges of panels. The edges have to be supported by another member.
Selection of entities
- All – see above
- Auto selection - all edges which are supported by a beam or 2D member edge, except 2D member edge which belongs to a member which is in the same plane as the panel (with tolerance +/-5 deg), are selected for the load generation. In other words it is the same as type All only edges from 2D members which are in the same plane as the panel are excluded.
- User selection – see above
Load transfer method
- Standard – the sum of defined load is recalculated to members using the weight factors
- Tributary area - the input load is recalculated based on panel and its supporting members geometry. There is used Voronoi algorithm for it.
Tributary area method
Tributary area method uses Voronoi algorithm for created the areas. It has a limitation so there is no support of curved edges, free point and line load. There also is not support for variable free surface load, load from soil and water pressure yet.
Note:Panel edge which is of type linestrip or is supported by 2D member with edge of type linestrip is also unsupported as linestrip edge is considered as a curve.
Generated areas can be divided into two or more if on the supported line is a structural node.
Generation of line load is based on a perpendicular to the supported edge in each point where is a change of tributary area geometry or the supporting element. If there is a part of area which could not be assigned by the perpendicular to the supported edge a sum of load is done and it is recalculated into line load in the edge. The length of load is 1/10 of the length of the edge or the minimal length 0,3m is used in case the supporting edge is very short. The load is variable with the value in the end of the edge and zero value in the other end.
Note: In case of a panel with an opening when the opening has a curved edge or divides a tributary area into two or more parts when the part of the area is not supported by any beam ot 2D member edge the opening is ignored for the area and load generation. See the pictures below. In the left one the opening is taken in account as each part can be distributed to a beam. In the right one there is a small triangle of the area which could not be transfered to the edge hence the opening is ignored.
Example 2
1. Create a simple steel hall.
2. Run Structure service > Load panel > Load to panel edges and input panels to each span of the hall.
3. Select both gable panels and change Load transfer direction to All (LCS panel).
4. Run View parameter setting dialog using the icon at the bottom of a graphical window or using the (right-mouse-button-click) context menu.
5. Tick option Members 2D on the Structure tab in the Local axes group. Local axes of panels will be displayed. This indicated the orientation of the local z-axis, which is very important as it must “go outward” from the building. Select panels which have the z axis oriented inward into the hall and select item Swap orientation in the Property window.
6. Tick option Highlight supporting edges/nodes in the Structure tab, group Panel. Nodes which are considered for the generation of load are marked.
7. If some edges of a panel are not marked and should be, select the panel and press the action button Update edge selection (for the selected panel) or Update all panels (for all panels).
8. Go to service Load and define two permanent load cases with type Standard.
9. Input Free surface load with geometry system – Member LCS around the hall in LC1.
10. Input Surface load on 2D members on all panels in LC2.
11. Select e.g. one of side panels and press the action button Generate loads in its properties. Line forces are generated along all its supported edges.
12. Run Calculation to generate line forces on the whole structure.
To edges and beams
If the load transfer direction is set to X or Y the following option is available:
Max. Angle for transfer [deg]
– defines an allowed inclination of a 2D member edge or beam from the axis. The angle is measured in the direction that is perpendicular to the selected axis.
If the load transfer direction is set to all, the following options are shown:
Transfer in X/Y
– defines the percentages of load distribution for x and y axis
Available only for Load transfer method set to Accurate (FEM).
It says which percentage is distributed in which direction. The direction is defined by the local axis of the panel. If different percentage is defined in each direction, the calculation is based on the calculation of an orthotropic plate.
Load transfer method
- Standard – the sum of defined load is recalculated to members using the weight factors
- Accurate (FEM), fixed link with beams - an accurate FEM-based calculation assuming rigid links between panel and beams (see explanation below)
- Accurate (FEM), hinged link with beams - an accurate FEM-based calculations assuming hinged links between panel and beams
- Tributary area - the input load is recalculated based on panel and its supporting members geometry. There is used Voronoi algorithm for it.
Note: Tributary area method has some limitation yet. It is unsupported in case of curved edges, variable free surface load, free point and line load, load from soil and water pressure.
Max. eccentricity of members [m]
only for Selection of entities set to “all”, defines a distance of members from load panel plane
Selection of entities
- All – see above
- Auto selection - all edges which are supported by a beam or 2D member edge, except 2D member edge which belongs to a member which is in the same plane as the panel (with tolerance +/-5 deg), are selected for the load generation. In other words it is the same as type All only edges from 2D members which are in the same plane as the panel are excluded.
- User selection – see above
- By type – group Selection of elements is shown, where user selects beams for load generation by type .
Note: The tolerance of an inclination of members or 2D member edges from panel plane is 1%. If the inclination is larger than 1% members and 2D member edges are not included in the selection, i.e. no load is transferred to them.
FEM method
The FEM method allows to determine a load distribution on underlying elements based on the FEM response of an auxiliary plate with finite stiffness. The plate response is determined prior to the analysis of the 3D structure (upon pressing the "Generate loads" action button).
Load transfer from a panel to adjacent elements and nodes is affected by the boundary conditions of this auxiliary plate. Panels may be assumed to be rigidly connected to underlying beams at the panel edges, or to be connected to these via hinges. The user may chose between two options: "fixed link with beams" or "hinged link with beams", which result in different final load distribution. The resulting reactions of the background calculation of auxiliary plates are converted to the loads generated on the actual structure. In the case of "rigid link with beams," moment reactions are ignored, as these do no originate in the structural response.
The generator of loads uses the following parameters:
Thickness is set to 1m.
The orthotropic material uses the following parameters:
E modulus = 1 GPa
Poisson coefficient = 0.25
D11 = 44.44 MN/m
D22 = 44.44 MN/m
D33 = 16.67 MN/m
D44 = D55 = 13 000 MN/m
D12 = 11.11 MN/m
For load transfer direction set to X or Y, the E1:E2 ratio is taken as 80:20% and E = E1 + E2 = 100%.
Note: If you model two identical cases, but one with a load panel and the other with an orthotropic plate with the parameters set as above, the shape (result graph) of the generated load and intensity in supports should be the same. The values depend on the mesh size which is automatically generated for the load panels as 10% of the shorter edge (the distance between two adjacent supports).
Note: In some cases this method may give unexpected results. It is caused by material properties which are necessary for the FEM calculation with an orthotropic material. For example:
case 1 – a panel is supported only with one member – generated load can have the opposite direction then the input one. It is caused by the stiffness, etc.
case 2 – a panel is subject to free surface load (with a geometry system set to projection) – the load is also generated in the direction which is perpendicular to the direction of the effectiveness of the input load. It is caused by the nonzero Poisson coefficient.
Example 3
1. Create a simple steel hall.
2. Run Structure service > Load panel > Load to panel edges and beams and input panels extending through all the spans of the hall.
3. Select both gable and roof panels and change Load transfer direction to All (LCS panel).
4. Select both roof panels and set Selection of entities – By type. Then select only some types, e.g. beam, purlin, truss chord.
5. Select both gable panels and set Selection of entities – User selection. Then select one by one, press the action button Update edge/beam selection and select some 1D members, e.g. columns and upper truss chords.
6. Run View parameter setting dialog using the icon at the bottom of a graphical window or using the (right-mouse-button-click) context menu.
7. Tick option Members 2D on the Structure tab in the Local axes group. Local axes of panels will be displayed. This indicated the orientation of the local z-axis, which is very important as it must “go outward” from the building. Select panels which have the z axis oriented inward into the hall and select item Swap orientation in the Property window.
8. Tick option Highlight supporting edges/nodes in the Structure tab, group Panel. Nodes which are considered for the generation of load are marked.
9. If some members are not marked and should be, select the panel and press the action button Update edge/beam selection (for the selected panel) or Update all panels (for all panels).
10. Go to service Load and define two permanent load cases of type Standard.
11. Input Free surface load with geometry system – Member LCS around the hall in LC1.
12. Input Surface load on 2D members on all panels in LC2.
13. Select e.g. one of the side panels and press the action button Generate loads in its properties. Line forces are generated in all its supported edges/beams.
14. Run Calculation to generate line forces on the whole structure.
15. Select all panels and change Load transfer method to Standard.
16. Run Calculation again.
