Pro/INTRALINK can accurately track changes to Pro/ENGINEER files including the version, revision, and lifecycle, but cannot capture the types of changes within the Pro/ENGINEER model files. For example, there may be meta-data, geometry, drawing, or cosmetic changes between two file versions that is not tracked at all. To determine the difference between two Pro/ENGINEER file versions, you can either manually compare the Pro/ENGINEER models or ask the designer who made the changes to point out the differences between the two models. Both of these methods are time consuming and risky.
Pro/ENGINEER Wildfire 2.0 has the ability to compare two part files and provide a fast, precise, error-free report identifying the differences. Part comparison and difference reporting allow you to understand exactly what has changed between two Pro/ENGINEER part files.
What’s more, with Pro/ENGINEER Wildfire 2.0 and Pro/INTRALINK 3.4, you can achieve even better part comparison and difference-reporting to highlight and detail the differences between two parts. You can compare:
- A part from a Workspace with a part in the Commonspace
- A part from disk with a part in the Commonspace
- A part from a Workspace with a part from disk
You can also compare two versions of the same part or two different parts. When you compare two versions of the same part, it is necessary to enter a replacement name when opening the comparison part, since Pro/ENGINEER does not allow two models with the same name in session.
You can format the difference report to show any combination of the following types of changes:
The steps for comparing two versions of the same part in Pro/ENGINEER Wildfire 2.0 with Pro/INTRALINK are as follows:
1. Start Pro/ENGINEER Wildfire 2.0 linked to a Pro/INTRALINK workspace either by:
o Launching Pro/ENGINEER, then registering Pro/INTRALINK as your server.
o Set Pro/INTRALINK as Primary Server and choose the Active Workspace you want to work with.
o Launching Pro/ENGINEER from a Pro/INTRALINK browser with the workspace you want to work with.
2. Retrieve a part into Pro/ENGINEER. The first part will be referred to as the Base Model. For example, in Figure 1, the base model is “0001_COMP_4.PRT”.
3. In Pro/ENGINEER Wildfire 2.0, click Analysis > Compare > By Feature. The File Open dialog box opens.
4. Choose File | Open or select the Pro/INTRALINK cabinet icon in the Folder Navigator to browse your Pro/INTRALINK Commonspace for the comparison model. Locate and retrieve the second part you want to compare.
o If you want to compare the same part, select the latest version of the part that is currently in session and click Open.
o Because the part that you are opening has the same name as the object in session, the Version Conflict dialog box opens. Enter a replacement name for the part and click OK. The system saves the comparison model under the specified file name.
In Figure 2, we compare the latest version of the same part, “0001_COMP_4.PRT”, and give it a replacement name of “PRT0001.PRT”.
Note: Each of the two Pro/ENGINEER parts will appear in a separate window. The Base Model will be in the active Pro/ENGINEER window.
5. Pro/ENGINEER will generate and display the Model Comparison report in the Pro/ENGINEER Wildfire browser as shown in Figure 3.
The Model Comparison report displays the name of the base model and its version, and the name of the comparison model and its version. If you provide a replacement name for the comparison model, the Model Comparison report will display the original name of the comparison model. In Figure 3, the Base Model name and the Comparison Model name are the same, “0001_COMP_4.PRT”, as shown in Figure 3.
By default, the Model Comparison report will display all the change types. The Filter Change Types option in the difference report allows you to configure the report to display only the change types you want to see. Check the box next to each Change Type of interest, choose Apply, and the Model Comparison report will display only the selected changes types.
A difference in the value of a system or user defined parameter
Addition or removal of a feature or a difference in a feature’s dimensions
Differences related to views, geometric tolerances, notes, or sections
A change in a cosmetics, such as color
For further information about a Geometry change, you may:
· Highlight an affected feature by clicking the triangle icon in the column under the Base Model or the Comparison Model. Selecting the triangle icon will cause the affected feature to be highlighted in the window of the affected model.
· See feature information on an affected feature by clicking the info icon and the feature information will be displayed in the browser.
Note: If you want to compare an earlier version of a part with the latest version of the part, you must first retrieve the earlier version into Pro/ENGINEER as your base model. Then you can retrieve the latest version of the model for comparison.
Summary. Pro/ENGINEER Wildfire part difference analysis currently supports comparing two parts. Comparison of assemblies, drawings, and family tables is not supported with Pro/ENGINEER Wildfire 2.0 but is planned to be available with the next release of Pro/ENGINEER Wildfire.
When choosing the comparison model, Pro/ENGINEER Wildfire will retrieve the latest version of the selected file. This is useful when trying to identify the changes you made to a model that you checked out and worked on in Pro/ENGINEER.
Pro/ENGINEER Wildfire part difference analysis is also available with Windchill PDMLink.
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