You can apply a pressure normal to a curved 'surface' of Beam elements using Grid Area Loads, as follows:

• Define a Grid Plane onto which the whole surface can be projected. Often a grid plane parallel to the global XY will do.
• Set the Grid Plane Tolerance such that all elements in the surface are picked up by the Grid Plane. (i.e. a large tolerance.) You may need to specify the Element List as other than 'all' if you want some elements not to attract load.
• Define a Grid Area Load applied to the whole Plane of your Grid Plane.
• Set the Axis of the Grid Area Load to 'Local' and the direction to z. The Local axis for the Grid Plane is such that the local z is normal to the 'surface' of elements (and the local x is the grid plane x projected onto the surface).
• You can then expand the Grid Area Load into equivalent Beam Loads using the 'Tools | Expand Grid Loading…' option. (This may take a while.)

There are three ways of deleting loads efficiently:

• To delete all of a particular load module (e.g. Beam Loads): right-click on the load module on the Tables tab of the Gateway and select 'Delete all…'. (In fact this option is available for all modules.)
• To delete all loads associated with a particular load case: right-click on the load case in the Load Case Titles table and select 'Delete Loads'.
• To delete loads graphically: display the loads you want to delete in a Graphic View and select 'Sculpt | Delete Displayed Loading'.

Then of course you can always delete load records explicitly in the loading tables.

Splitting elements graphically, whether using the split element, refine element or connect element commands, can be a slow process. Typically this happens when the elements that are being split have loads applied to them; - GSA takes a long time adjusting the element lists by replacing the old element reference with references to the new elements. The slow processing can be avoided by deleting the loads before splitting the elements and then re-applying the loads after the split.

Data files containing large report log strings take a long time to open (in GSA 8.0). You can overcome this problem by opening the report ('View | Open Report View') and deleting the contents ('View | Clear Report').

Models imported from DXF files often suffer from bad element connectivity. The Connect 1D Elements option ('Sculpt | 1D Element Operations | Connect 1D elements') is effective at tidying up such models. This connects selected crossing elements by splitting them and connecting the split elements to a common node at the point of intersection. It can also be used for trimming and extending elements.

GSA's Quad4 and Tri3 elements can be created from DXF files that contain corresponding polygon or polyface meshes. When importing the DXF file into GSA (via 'File | Import | AutoCAD (DXF file)') select which type of 2D element is to be created from these DXF entities by specification in GSA's 'DXF Import Options' dialog.

2D elements sometimes appear to be corrupted by using the sculpt 'Modify elements' option to convert from 'linear' to 'parabolic' (e.g. Quad4 to Quad8). In that operation, when creating the new mid-side nodal position GSA first looks for an existing node in the required position before creating a new node. This is so as to provide good connectivity at the mid-side nodes. GSA uses the current 'tolerance for coincidence' when considering whether a coincident node exists. GSA can be misled into choosing an existing corner node as the mid-side node where such a node lies within the tolerance; typically this occurs when working with small elements. This can be avoided by setting the 'Options | Preferences | Sculpting | Tolerance for coincidence' to an appropriate (i.e. smaller) value.

The GSA programming interface (i.e. COM interface) can be used to control GSA from, say, a spreadsheet or other remote program. A typical use of this is where you want to carry out structural optimisation in a spreadsheet. For example in a VBA macro you can tell GSA to:

• Open a data file.
• Analyse.
• Get results.
• Delete results.
• Get a section property.
• Set a section property.
• Analyse.
• …
• Save

Refer to the 'Programming and Command Line Interface' chapter of the GSA help for more details. Sample XLS files that demonstrate the use of this feature are installed in the …\Oasys\GSA 8.0\Samples folder. Note that the command that enables the getting and setting of individual data records (GwaCommand) is new in GSA 8.0 build 27. Revised documentation in the form of a GSA 8.1 draft of the 'Programming and Command Line Interface' chapter is available on the GSA Downloads page of the website.

The time taken to do a GSS solution depends on the way the equations are set up. GSA tries to set these up in a well ordered manner, working along the longest dimension of the structure. This normally results in a stiffness matrix clustered close to the diagonal. However, when a structure contains rigid constraints these can provide topological connection which introduces many more off-diagonal terms. This results in a much larger matrix to be solved.

An example of where this problem might arise is where a structure is longer than it is tall and rigid constraints have been used to model rigid floor plates. In this situation the automatic solution order is along the length of the structure whereas the most efficient order is in the vertical direction.

If rigid constraints seem to cause a significant increase in the analysis time it may be worth telling the solver the direction in which to build the solution matrix. This can be done by going to the Analysis Specification and selecting 'Advanced'. Then set the solution order vector to 'User defined' and set the vector components such that the direction is normal to the rigid constraints.

Where the yield stress in a user material is given a non-zero value the material is treated as 'elastic - perfectly plastic' in GsRelax non-linear static analysis. A yield stress of zero specifies an elastic material; all standard materials are elastic. (Note that ultimate stress, hardening modulus and hardening parameter are not used in any GSA analysis at present.)

Nodal forces and moments from non-linear analysis are balanced at the deformed position of the nodes. Where the displacements are large the nodal forces may appear not to be in equilibrium at the undeformed nodal positions.

In raft analysis it is not necessary to specify support stiffnesses for the nodes that interact with the soil since support stiffnesses are automatically generated during the analysis and deleted after the analysis. However, where support stiffnesses are specified these will be used as the initial soil stiffness. This can speed up the analysis if the specified stiffness is closer to the actual soil stiffness than the default initial stiffness of 1.0e10 N/m.