Suggested Technique for Verifying IDF Contours in Pro/ENGINEER Wildfire 3.0

Pro/ECAD is an optional module providing a platform for data exchange between Pro/ENGINEER and systems for Electrical Computer Aided Design (ECAD). These systems produce data in Intermediate Data Format (IDF). This tip is concerned with the import of a printed circuit board outline in IDF format. The ECAD data for the printed circuit board (PCB) can be analyzed for errors if the imported PCB outline does not match that created in an ECAD system. Below are two techniques for this analysis.

Figure 1 illustrates a sample board outline file, imported into Pro/ENGINEER in an IDF 3.0 format.

For longer or more complicated files, there is another method for verifying the IDF contours. This involves the manipulation of the ECAD data file. The board outline file for Figure 2 is used in this example.

Create a copy of the ECAD data file and rename it to "<part>.pts"

• Remove all text in the file that appears above and below the data
• Next, delete the first column of numbers
• Change the last column of numbers to all zeros
• This transforms the board outline file to a space delimited point file in the form "X Y Z"
• The resulting file is:

10000.00000             0.00000             0.00000

10000.00000          2000.00000             0.00000

 7000.00000          5000.00000             0.00000

    0.00000          5000.00000             0.00000

    0.00000             0.00000             0.00000

10000.00000             0.00000             0.00000

 4200.00000           320.00000             0.00000

 7000.00000          3200.00000             0.00000

 8200.00000          2000.00000             0.00000

 8200.00000          1200.00000             0.00000

 4200.00000          1200.00000             0.00000

 4200.00000          3200.00000             0.00000

Click File > New and a new dialog box opens. Then:

• In the Type box, select Part
• In the Name field enter a name for the new part
• Click OK to create the new part.

Datum points can be created using the point file you created from the ECAD board outline file in step two.

• Click Insert > Model Datum > Point > Offset Coordinate System
• The Offset CSys Datum Point menu opens
• Select the default coordinate system
• In the Type field, select Cartesian
• Click Import
• The Open dialog box opens
• Browse to the filename of the point file created in step two
• Click Open
• The Offset CSys Datum Point menu will be populated with the point information from the file
• Click OK to place the points 

Datum curves are used to connect the points.

• Click Insert > Model Datum > Curve
• The Menu Manager CRV OPTIONS menu opens
• Select Thru Points > Done
• The CURVE: Through Points window opens
• Select Curve Points as the Element
• Select Define
• In the Menu Manager CONNECT TYPE menu
• Select Single Rad, Whole Array, and Add Point
• Pick any point from the data file that is displayed in the main window
• The Message Window prompts for a bend radius
• Type '0' to generate the allowable limits
• Type the value returned for the minimum bend radius
• This will produce approximately straight lines between the points
• Select Done from the CONNECT TYPE menu
• Select OK from the CURVE: Through Points dialog box

The output from this operation using the sample file is shown in Figure 4.

Note that point six seems to be in the wrong place. An examination of the point data file reveals that this was the point in question from the quick check in step one.

If the data file was correct, the output would resemble Figure 5.

Download Example Files for this Technique