About Part Comparison

In Part mode, you can compare two part files or two different versions of a part file, and obtain a graphical report on the differences between the two parts or versions. You can perform a feature comparison or a geometric comparison:

You can compare the features of two parts or two versions of the same part. For example, if you have two part files that contain the same basic part with the same basic features, but the dimensions of the features differ, you can use part comparison to analyze the difference in size between the two parts. A list of features that have been modified, along with any features that exist in only one of the part files, is displayed in the Part Comparison dialog box. Creo Parametric also displays an overlay of the second part on the first part and highlights the feature being compared. The default highlight color is red.

You can measure the geometric deviation between one part and another part. Creo Parametric performs an analysis that generates a point cloud of the first part, and then overlays it on and aligns it to the second part. Then Creo Parametric generates a shaded color display of the deviation between the two parts and displays it in the graphics window.

To perform the geometric comparison, click Analysis > Compare Part > By Geometry. The Compare Geometry dialog box opens. In the Compare Geometry dialog box, you can control the point density (how far apart the points in the point cloud will be) by typing in a measurement spacing value. The unit of measurement in this box is always the same as the default or user-defined part measurement unit. You can also control the tolerance values for the display. That is, you can choose to display only the deviations between the parts that occur above a specific value. For example, if you are interested in a deviation range of 1.0 millimeter or more, Creo Parametric displays deviations of more than 1.0 millimeter and eliminates deviations of lesser values from the display.

You can choose to export the difference report displayed in the Creo Parametric browser by clicking Export Report on the HTML report page. By default, the exported file is saved in the current working directory in the Comma Separated Value (CSV) format as <model_name>_CMPR0.csv and <model_name>_CMPR0.csv.1. Set the export_report_format configuration option to rich_text to save the exported file in the rich text format as <model name>_CMPRO.txt and <model name>_CMPRO.txt.1. You can open these saved files in Microsoft Excel.

The <model_name>_CMPR0.csv.1 and <model name>_CMPRO.txt.1 are version files. Whenever you export the same report again, new version files are created with incremented file names and the <model_name>_CMPR0.csv and <model name>_CMPRO.txt files are replaced by latest exported file.