This section describes how to use the ACT API to automate the creation of worksheets in Mechanical. ACT enables you to create and populate worksheets by entering commands into the ACT Console and executing them in Mechanical. For more information, see ACT Console.
The following examples are used to illustrate worksheet capabilities in ACT:
This section describes how to use the ACT API to automate the creation of a named selection worksheet in Mechanical. It assumes that the Scoping Method for your named selection is already set to Worksheet.
ACT supports all available actions for named selection worksheets, as described in Specifying Named Selections Using Worksheet Criteria in the ANSYS Mechanical User’s Guide. This example focuses on the Add Row action to add new geometric entities to a named selection.
To create the named selection worksheet, execute the following commands in the ACT Console:
model = ExtAPI.DataModel.Project.Model sel = model.AddNamedSelection() sel.Name = "Pipe" selws = ExtAPI.SelectionManager.CreateSelectionInfo(SelectionTypeEnum.WorksheetSpecific) sel.Location = selws pipews = sel.Location
This creates the named selection object, renames it Pipe, and creates the worksheet for your named selection.

Data in the named selection worksheet defines the criteria based on geometric or meshing entities. Each row of the worksheet performs a calculation for the specified criteria.
The command AddRow adds worksheet rows according to
the standard behavior of the Add option in Mechanical
named selection worksheets. It adds the information defined in the current
row to information in the previous row, provided that the Entity
Type is the same for both rows.
To add the first row in your worksheet, you execute these commands:
pipews.AddRow() pipews.SetEntityType(0,NamedSelectionWorksheetEntityType.Body) pipews.SetCriterion(0,NamedSelectionWorksheetCriterion.Size) pipews.SetOperator(0,NamedSelectionWorksheetOperator.GreaterThan) pipews.SetValue(0,3.8e-5) pipews.Generate()
This example uses set methods to define a Body with a Size value greater than 3.8e-5.

The method Generate generates the body. After
executing this method, the pipe body is selected in the
Graphics view. In Details, the
property Total Selection is set to 1
Body.

Next, you define and generate another body:
pipews.AddRow() pipews.SetEntityType(1,NamedSelectionWorksheetEntityType.Body) pipews.SetCriterion(1,NamedSelectionWorksheetCriterion.Size) pipews.SetOperator(1,NamedSelectionWorksheetOperator.LessThan) pipews.SetValue(1,8e-6) pipews.Generate()
In this row, set methods define a Body with a Distance value less than 3.8e-6. When there are no locally defined coordinate systems, you don’t need to set the Coordinate System value. It is set to Global Coordinate System by default.

After executing the method Generate, the bolt body
is now selected in the Graphics view, along with the
pipe body. In Details, the property Total
Selection is set to 2 Bodies.

This section describes how to use the ACT API to add rows to an existing mesh worksheet, specifying the order in which meshing steps are performed in Mechanical.
ACT supports most of the functionality available for mesh worksheets, which is described in Using the Mesh Worksheet to Create a Selective Meshing History in the ANSYS Meshing User’s Guide. The following exceptions apply:
The named selections must have Entity Type set to Body. Other entity types are not supported.
The Start Recording and Stop Recording buttons are not supported.
This section assumes that you have already defined two or more named selections in Mechanical. In your sample Static Structural analysis, you’ve defined three named selections, as shown in the following figure:

To display the mesh worksheet, perform the following steps:
Select the Mesh node in the tree.
Click the toolbar button.
The empty worksheet is displayed in the Worksheet tab.

Next, you need to define variables for the mesh worksheet and the named selections to use in the worksheet rows:
model = ExtAPI.DataModel.Project.Model msh = model.Mesh mws = msh.Worksheet nsels = model.NamedSelections ns1 = nsels.Children[0] ns2 = nsels.Children[1] ns3 = nsels.Children[2]
Finally, you add new rows to the mesh worksheet. Each row in the worksheet corresponds to a step in the meshing sequence.
To add the first row to your worksheet, you execute these commands:
mws.AddRow() mws.SetNamedSelection(0,ns1) mws.SetActiveState(0,True)
The command AddRow adds an empty
row.
The command SetNamedSelection sets the
Named Selection value to your named
selection object ns1.
The command SetActiveState sets the
property Active State at the row index (enables
the row, as indicated by the check mark in the left column).
The following image shows the mesh worksheet after the execution of these commands.

Next, you add rows for your other two named selections,
ns2 and ns3. Note that for
ns3, you use the command
SetNamedSelectionID to set the named
selection.
mws.AddRow() mws.SetNamedSelection(1,ns2) mws.SetActiveState(1,True) mws.AddRow() mws.SetNamedSelectionId(2,ns3.Id) mws.SetActiveState(2,True)
The following image shows the mesh worksheet after the two new rows have been added:

When you check the Graphics tab, you can see that no mesh has been generated yet. To generate the mesh for the named selections in the mesh worksheet, execute the following command:
mws.GenerateMesh()
When you execute this command, the steps are processed one by one in the order specified by the worksheet. For each step, the bodies identified by the named selection are meshed using the meshing controls applied to them. By watching the mesh generation in the Graphics tab, you can see the order in which each body is meshed.

To clear the generated mesh, execute the following command:
mws.ClearGenerateMesh()
To delete a single row, execute the following command:
void DeleteRow(int index)
To delete all rows, execute the following command:
mws.DeleteAllRows()
To display the row count in the ACT Console command history, execute the following command:
mws.RowCount
This section describes how to use the ACT API to access the worksheet for a layered section definition in Mechanical. It assumes that you've already created a layered section and set the property Layers to Worksheet.
To display the layered section worksheet in Mechanical, perform the following steps:
In the Project tree, expand the Geometry node and select the Layered Section node.
In the details of the layered section, select the Layers property.
To the right of the Worksheet selection for this property, click the right arrow and select Worksheet.
The layered section worksheet is displayed in the Worksheet tab.
To get to the layered section worksheet object in the ACT Console, enter:
mymodel = ExtAPI.DataModel.Project.Model geo = mymodel.Geometry ls = geo.Children[1] lsws = ls.Layers
To get and display the material property for layer index 2, enter:
lsmat = lsws.GetMaterial(2) lsmat
Assume that Structural Steel displays as the
material property.
To get and display the thickness property for layer index 2, enter:
lsthick = lsws.GetThickness(2) lsthick
Assume that 0.00253999746 displays as the thickness
property.
To get and display the thickness property for a different layer index, such as layer index 3, enter:
lsws.GetThickness(3)
Assume that 0.004 displays as the thickness
property.
To get and display the angle property for layer index 2, enter:
lsang = lsws.GetAngle(2) lsang
Assume that 45 displays as the angle
property.
To set the thickness property for layer index 2 to
0.0999999 and display this value, enter:
lsthick = lsws.SetThickness(2,0.0999999) lsthick = lsws.GetThickness(2) lsthick
The thickness property then displays as
0.0999999.
This section describes how to use the ACT API to access the bushing joint worksheet for Mechanical. A bushing joint worksheet defines stiffness and damping coefficients via symmetric matrices. This section assumes that you’ve already created a bushing joint worksheet.
To display the worksheet for a bushing joint in Mechanical, perform the following steps:
In the Project tree, expand the Connections node and then the Joints node.
Select the node for the bushing joint.
To the right of the Worksheet selection for this property, click the right arrow and select Worksheet.
The worksheet for the bushing joint displays in the Worksheet tab. The size of the matrices for stiffness and damping coefficients are fixed, which means that rows and columns cannot be added or deleted. Another aspect of these square matrices (6x6) is that they are both symmetric about their main diagonals. To ensure that these matrices are always symmetric, you cannot enter values into their upper right corners.
To get to the bushing joint worksheet object in the ACT Console, enter:
mymodel = ExtAPI.DataModel.Project.Model joints = mymodel.Connections.Children[1] bushing = joints.Children[0] bws = bushing.BushingWorksheet
The ACT API for a bushing joint worksheet enforces the fixed matrices by limiting the range of indices that can be specified to set or get the value from a particular cell. The row indices are zero-based.
For example, to get the coefficient for the stiffness per unit Y at row index 1, enter:
bws.GetBushingStiffnessPerUnitY(1)
Assume that 136073.550978543 displays as the
stiffness per unit Y.
Now, assume you’ve entered the following:
bws.GetBushingStiffnessPerUnitZ(0)
The given index of 0 (zero) produces an error because that cell lies above the main diagonal. As indicated by the error message, the valid range of indices is equal to 2 and less than or equal to 5.
The following image displays some of the many methods available for getting coefficients for damping and stiffness.