Introducing Pro/INTRALINK to Pro/ENGINEER

Well, assuming that you've worked your way through the Pro/INTRALINK 8.0 Installation Overview flowchart and have your system up and running, the next thing you probably want to do is get a look at how well it plays with Pro/ENGINEER Wildfire 2.0. There are several things you can do to make Pro/INTRALINK and Pro/ENGINEER talk fluently back and forth. These steps will allow your Pro/ENGINEER session to communicate with Pro/INTRALINK, allow you to search for CAD files based upon the Pro/ENGINEER parameters and allow your Pro/INTRALINK attributes to show up on your Pro/ENGINEER drawing title blocks.

Registering the Server and Enabling Workspaces
Before registering the server within Pro/ENGINEER Wildfire, the Workspaces must first be enabled. This can either be performed by logging into the server first via the Wildfire-integrated browser, or the administrator can enable workspaces system-wide by setting the system preferences (via Utilities>Preference Manager) such that:

/com/ptc/windchill/cadx/CadxStandAloneEnabled=true

If you enable the workspaces as a system-wide setting, all users should now be able to see the Workspaces menu item from within their Products and Libraries.

To register a server within Pro/ENGINEER Wildfire, Select Tools>Server Registry. This will bring up the dialog box where you can define the server and its URL to the Pro/INTRALINK 8.0 context root (i.e., http:///Windchill). Wildfire will ask you for a user name and password to authenticate you into the Pro/INTRALINK Server.

As a best practice, all users within an organization should use the same name for the registered server. Since the server name is used to define the search paths to any Windchill-managed start parts, formats, UDFs or libraries, using the same name for registration will allow a common config.pro file to be rolled out to all users.

Setting up Pro/INTRALINK to Understand Pro/ENGINEER Parameters
Pro/INTRALINK 8.0, like its predecessor, provides a means of viewing, modifying and searching on Pro/ENGINEER parameters. To enable this communication, first, the Pro/ENGINEER file must have the parameters defined and designated (parameters can be added and designated through the Pro/ENGINEER Wildfire Tools>Parameters menu). Next, we'll configure Pro/INTRALINK to know what parameters to look for and to which object-type they apply. This mapping of parameters to IBAs can be done either implicitly or explicitly. Today, we'll discuss the implicit method. Within Pro/INTRALINK, attributes corresponding to your Pro/ENGINEER parameters must be created within the Attribute Manager (under the Context Administrator's Utilities menu). Within the Attribute Manager, you'll want to first create an Organizer in which you will define the attributes (call it ProE or something similar). Then, create a new attribute of the same name as the corresponding Pro/ENGINEER parameter (use ALL CAPS for the name of the Attribute); ensuring that the data type is the same as defined within Pro/ENGINEER. For instance, if you have a Pro/ENGINEER designated string parameter called Material, create a Pro/INTRALINK string attribute called MATERIAL. Repeat this process for each of your designated parameters that you want to be available and searchable through Pro/INTRALINK. Next, the attribute(s) must be assigned to the CAD Document (NOT the CAD Document Master) through the Type Manager. Within the Type Manager, select the CAD Document, click the Modify icon (performing an on-the-fly checkout), then select the Template tab in the right window pane and right click on the Attribute Root column heading. From here, after selecting Add Attribute, you can then select the newly created Attributes from your Attribute Container and assign them to the CAD Document. You can also then right click on each attribute and set constraints for the permissible value that can be assigned to the attribute.

As a side note, the attributes can be assigned to the CAD Document sub-type, the Workgroup Manager CAD Document. If a future upgrade to PDMLink is likely and additional soft-typing may occur, you should probably opt for this more specific setting. In this case, the search criteria should be customized to include the Workgroup Manager CAD Document to allow attribute-based searches.

Once these changes have been made, you can then check-in the CAD Document sub-type. Any new or modified CAD documents that are checked in from that point forward will have their designated matching parameters communicated to Pro/INTRALINK and searching and bi-directional modification of those attributes can now be performed.

Adding Pro/INTRALINK Attributes to the Pro/ENGINEER Drawing Title Block
To ensure that the Pro/ENGINEER drawing formats reference the accurate value of attributes stored by Pro/INTRALINK, it is important to update the drawing formats that are in use. Some of the system attributes that can be added to the drawing format include:

Windchill Revision	&ptc_wm_revision	Revision as identified by Pro/INTRALINK
Windchill Iteration	&ptc_wm_iteration	Iteration as identified by Pro/INTRALINK
Windchill Version	&ptc_wm_version	Concatenation of the Revision and Iteration separated by a "."
Windchill Lifecycle State	&ptc_wm_lifecycle_state	Lifecycle State as identified by Pro/INTRALINK

The values listed above will be displayed on the drawing for the model file used to generate the views. If it is desired to use a drawing-specific parameter value in the field, simply append ":D" (without the quotes) to the attribute. For instance, to display the Drawing's Pro/INTRALINK Version, the following text should be added to the title block:

&ptc_wm_version:D

You'll notice that after the drawing and the model are checked into Pro/INTRALINK that the title block now reflects the correct attribute value.

This should get you started with the Pro/ENGINEER Wildfire and Pro/INTRALINK interactions. There's quite a bit more to cover and I will try to do that in future blogs. If you have any questions on these or have some specific settings you'd like to see, drop me a message in the Administration Forum.