This section examines how to work with the finite element data that you import from an upstream External Model system. It examines the following topics for importing mesh-based databases.
When you import an External Model source file that includes any of the finite element data listed below, Mechanical inserts an “Imported” folder (excluding Named Selections) beneath the corresponding Tree outline object. As illustrated in the example Outline pane below, this Imported folder object is a simple group folder and will contain a child object for the associated data type.

Selecting a child object of the Imported folder displays the model in the Geometry window with the imported data type highlighted as well as the Worksheet. An example of a selected imported spring is illustrated below. The Worksheet displays a summary of all imported data including column headings for the specific data associated with each data entry (connection Type, node ID, etc.). Each row of the Worksheet represents a different set of data. You can sort the table data by clicking on a column heading. The check-box for each Worksheet row enables you to deactivate (suppress) the row. And, based on the number of data items imported, the Worksheet displays 500 (default) data items per worksheet page. Use the display and/or navigational options at the bottom of the window to display more data items per page as well as to step through the available pages of data.

A graphical representation of the data is also shown in the Geometry window. You can choose which data is displayed in the Geometry window using the Show Rows property under Graphics Properties category in the Details view. The Show Rows property includes the following options:
From Current Page (default): Only display the data from the current page in the worksheet.
From All Pages: Display all of the data for the object independent of the rows visible in worksheet.
None: Do not display any data in the Geometry window.
In addition, for the following objects, you have the ability to select the color used for the displayed data in the Geometry window through a color selection property in the Details view:
Furthermore, when you select a Worksheet row, the graphical representation of the data in the Geometry window becomes highlighted, such as the green spring shown in the above image. You can also select the graphical representation directly in the Geometry window by activating the Label or Imported Objects option on the Graphics Toolbar. This selection option behaves as it does when it is used in other selection scenarios for the application. Normal mouse and key combinations for selecting, unselecting, modifying, or clearing selections act just as they do with geometry selections, etc. This selection feature is available for the following types of imported data:
In addition, for the above data types, when you select the graphical representation (Point Mass, Spring, etc.) in the Geometry window and right-click, the context menu provides the following applicable options:
> : This option navigates to attached bodies in the tree.
: This option only displays the selected objects in the worksheet. You can revert to viewing a specified number of rows in the Worksheet by editing the column headings via the right-click Show option in the Worksheet.

When the finite element data is displayed in the Worksheet, there are common options you can employ when you right-click on a Worksheet row, including:
Promote: When you promote a Worksheet entry, the data, in whichever form (Coordinate System, Element Orientation, etc.), remains linked to the external system. You can modify the data within Mechanical, however; your changes are not transfer to the external system. In addition, any changes made in the external system will overwrite any modifications you make in Mechanical.
Copy as new: When you copy a Worksheet entry, a new independent object, based on the type of data, is inserted into the Tree outline. The application assigns a default name to the object based on the data type (Coordinate System, Element Orientation, etc.).
Show: This option enables you to select which columns you wish to display on the Worksheet.
Check/Uncheck: This option enables you to deactivate (suppress) a worksheet row.
Go To Promoted: This option becomes available after you have promoted a Worksheet entry. This option takes to you the corresponding Tree outline object.
Edit Items: This option becomes available when your finite element data type has editable Worksheet content. It enables you to make changes to the associated data items, such as a node ID. You can select individual or multiple rows as well as the data type tree object. When you select multiple rows or the tree object, the application applies all changes to all of the selected rows or to all of the Worksheet content, respectively.
Note: Currently, Mechanical supports the Promote and Copy options for the following imported data:
Contacts
Coordinate Systems
Element Orientations
Point Masses (when scoped to a node of the geometry only)
Mechanical enables you to import the following finite element data types from External Model. Select a link to jump to steps for working with that data type:
For the imported FE data types listed below, Mechanical enables you to assign custom names to reference nodes in the Worksheet. This enables you to access the nodes in the solver file (through command snippets). Your name can contain only standard English letters and numbers, spaces, underscores, hyphens, and/or parenthesis characters.
Imported Point Masses
Imported Rigid Remote Connectors
Imported Flexible Remote Connectors
Imported Spring Connectors
Mechanical automatically makes the following changes to your custom name in order to prepare the new reference name for the Mechanical APDL application:
A name exceeding 32 characters is truncated.
A name that begins with a number, space, hyphen, or parenthesis character, is renamed to include “C_” before the character.
Spaces, hyphens, or parentheses between characters in a name are replaced with underscores.
For example, a Reference Node in the Mechanical application called "1 Edge" appears as component "C_1_Edge" in the Mechanical APDL application input file.
The Mechanical application enables you to import supported finite element data types from External Model and represents them natively through various imported objects in the tree. In addition, imported databases almost always contain additional commands that are not natively supported by the application. Mechanical exposes these commands (along with the commands natively processed in Mechanical) through the ACT extensions and console window. The following APIs enable you to access the underlying commands repository for a file specified in External Model.
commands = ExtAPI.DataModel.Project.Model.GetFECommandsRepository("Setup", "File1");
Users familiar with ACT APIs for ANSYS Mechanical will notice
that the command GetFECommandsRepository on the
Model object provides access to the commands repository. The two
arguments ("Setup" and "File1") specify the source External
Model Component Id and "File Identifier" in
the External Model Component.


The return object commands is an instance of the interface
ICommandRepository.
Once user has access to the commands database, you can access:
Processed Commands: Commands processed and natively represented in Mechanical.
Unprocessed Commands: Everything other than Processed Commands.
User can access the unprocessed commands names using the combination of following commands:
unprocessedCmdNamesCount = commands.GetCommandNamesCount(Ansys.ACT.Automation.Mechanical.FE.CommandsType.UnProcessed);
And...
unprocessedCmdName = commands.GetCommandName(Ansys.ACT.Automation.Mechanical.FE.CommandsType.UnProcessed, index);
As you might notice, the command
GetCommandNamesCount on
ICommandRepository
provides the count of the command names of type specified as first argument:
Ansys.ACT.Automation.Mechanical.FE.CommandsType.UnProcessed
Or...
Ansys.ACT.Automation.Mechanical.FE.CommandsType.Processed
And the command GetCommandName provides
the command name given the type and index (index is 1 based, therefore, if the
unprocessedCmdNamesCount = n, the valid index value are
(1,n)).
Given a command name, user can access all instances of a command with a given name as:
namedCommands = commands.GetCommandsByName(commandName);
The return value namedCommands is an
instance of the interface ICommandColl. A command can be accessed
from the namedCommands as:
namedCommand = namedCommands.Item(index);
The index argument is 1 based, therefore
valid index value are (1,namedCommands.Count()))
The return value namedCommand is a derived
instance of the interface ICommand, i.e. the
namedCommand instance exposes the methods available on the
ICommand interface:
Name(): Command name
Index(): 1 based global index of the command in command repository
And any additional methods exposed the specific instance of the
command. For example, if the namedCommand is an instance of
ICECommand (a type of processed command from CDB file), then the
following additional methods are available:
Nce(): Constraint Equation ID
Constant(): Constant Term
TermCount(): Number of Terms
GetTerm(int index): Term at Index
Similarly, if the namedCommand is an
instance of IGenericCommand (unprocessed command from CDB file),
then the following additional methods are available:
ArgumentCount(): Number of arguments
GetArgument(int index): Argument at index
Refer to the External Model CDB Commands and the External Model ABAQUS Commands section s for all the available processed and unprocessed commands from CDB and ABAQUS databases.
In addition, you can traverse the command repository by going to the next and previous commands in the database using the following APIs:
prevCommand = commands.GetCommandByIndex(currentCommand.Index()-1);
nextCommand = commands.GetCommandByIndex(currentCommand.Index()+1);
Given the information provided in the above section, let's take a look at some examples.
The following examples describe how to query the command repository.
commands = ExtAPI.DataModel.Project.Model.GetFECommandsRepository("Setup", "File1")
Example: List All Command Names
This example enables you to generate a listing all command names in the command repository.
commandType = Ansys.ACT.Automation.Mechanical.FE.CommandsType.All commandCount = commands.GetCommandNamesCount(commandType) commandsNames = [] for iCommand in range(0, commandCount): commandsNames.append(commands.GetCommandName(commandType, iCommand+1)) commandsNames
Example: List All Nodes
This example enables you to generate a listing all nodes in the command repository.
NBLOCK,6,SOLID, 430, 10
(3i9,6e21.13e3)
421 0 0 6.3203350000000E+004-4.2985880000000E+004 6.3500000000000E+004
422 0 0 6.1696900000000E+004-4.5619000000000E+004 6.3500000000000E+004
423 0 0 5.9365700000000E+004-4.7562160000000E+004 6.3500000000000E+004
424 0 0 5.6517810000000E+004-4.8605830000000E+004 6.3500000000000E+004
425 0 0 5.3482670000000E+004-4.8603130000000E+004 6.3500000000000E+004
426 0 0 5.0634300000000E+004-4.7562160000000E+004 6.3500000000000E+004
427 0 0 4.8295410000000E+004-4.5625390000000E+004 6.3500000000000E+004
428 0 0 4.6795660000000E+004-4.2986070000000E+004 6.3500000000000E+004
429 0 0 4.6250000000000E+004-4.0000000000000E+004 6.3500000000000E+004
430 0 0 4.6795660000000E+004-3.7013930000000E+004 6.3500000000000E+004
N,R5.3,LOC, -1,
/*Commands*/
nodeIds = []
nblockCommands = commands.GetCommandsByName("NBLOCK")
nblockCount = nblockCommands.Count
for iNBlock in range(0, nblockCount):
nblock = nblockCommands[iNBlock+1]
nodeCount = nblock.NodeCount()
for iNode in range(0, nodeCount):
node = nblock.GetNode(iNode+1)
nodeIds.append(node.Id())
nodeIds
/*Output*/
[421, 422, 423, 424, 425, 426, 427, 428, 429, 430]
Example: Extract Analysis Settings
This example enables you to extract all Analysis Setting in the command repository.
ANTYPE, 2
MODOPT,LANB, 6, 0.00000000 , 0.00000000 , 0, 0, 0.00000000 , 0
/*Commands*/
antypeCommands = commands.GetCommandsByName("ANTYPE")
if(antypeCommands.Count > 0):
antypeCommand = antypeCommands[1]
if(antypeCommand.ArgumentCount() > 0):
antype = antypeCommand.GetArgument(1)
print antype
if(antype == "2"):
modoptCommands = commands.GetCommandsByName("MODOPT")
if(modoptCommands.Count > 0):
modoptCommand = modoptCommands[1]
for iArg in range(0, modoptCommand.ArgumentCount()):
print modoptCommand.GetArgument(iArg+1)
/*Output*/
2
LANB
6
0.00000000
0.00000000
0
0
0.00000000
0
This example enables you to generate a listing all nodes in the command repository.
/*Input*/
*NODE, NSET=nset_csys2
421, 6.320335E+01,-4.298588E+01, 6.350000E+01
422, 6.169690E+01,-4.561900E+01, 6.350000E+01
423, 5.936570E+01,-4.756216E+01, 6.350000E+01
424, 5.651781E+01,-4.860583E+01, 6.350000E+01
425, 5.348267E+01,-4.860313E+01, 6.350000E+01
426, 5.063430E+01,-4.756216E+01, 6.350000E+01
427, 4.829541E+01,-4.562539E+01, 6.350000E+01
428, 4.679566E+01,-4.298607E+01, 6.350000E+01
429, 4.625000E+01,-4.000000E+01, 6.350000E+01
430, 4.679566E+01,-3.701393E+01, 6.350000E+01
/*Commands*/
nodeIds = []
nodeKeywords = commands.GetCommandsByName("NODE")
nodeKeywordCount = nodeKeywords.Count
for iNodeKeyword in range(0, nodeKeywordCount):
nodeKeyword = nodeKeywords[iNodeKeyword+1]
arguments = nodeKeyword.Arguments()
for iArg in range(0, arguments.Count()):
arg = arguments.Item(iArg+1)
print arg.Key()+"="+arg.Value()
datalines = nodeKeyword.DataLines()
for iLine in range(0, datalines.Count()):
dataline = datalines.Item(iLine+1)
nodeIds.append(dataline.Item(1))
nodeIds
/*Output*/
NSET=nset_csys2
[421, 422, 423, 424, 425, 426, 427, 428, 429, 430]