Allegro Component Outline/Terminal Issue with Chip

Hi.  When importing into Allegro and sending the Component outline, including terminals to the CAD output there is a problem with Chip parts.  I haven't noticed this issue with the other families. 

 The outline/terminal line is incomplete.   Please see the attached image comparing the PCBLEP expected output to the actual Allegro import.  Note the missing line.  There should actually be 3 separate line paths with 4 segments each, 1 for the outline and 2 for the terminals.   Can this please be corrected?

This problem is present in version 2016.10 and 2016.11

Regards,

Chris

Hi Chris.  Yes I confirmed it’s not a graphical issue.  I looked into it a little more and found the problem.  The problem is actually two fold.

The first problem is you are sharing lines at the body start/end vertex.  While your script pick points are correct Allegro will merge lines when picking the start/end of a path.

Below are the script lines in question, I’ve added the allegro command line feedback as a comment where the problem occurs (“Merged with existing line. Start next line.”) . As soon as the left terminal picks the lines start/end they merge and the line disappears.  The remaining 2 vertices are added as a new separate line. The right terminal doesn’t have a problem because it never picks the start/end point.

I believe the only way to avoid this would be to have the component body rectangle start/end away from the terminal picks, ie in the middle somewhere.  You’ll see the same issue with Oscillator, Corner Concave for example since the pins are at the corners.

Having all of that, lol, there is an allegro environment variable that can correct this:

         addline_nomerge

The default value is to have this unset.  When unset the problem described above manifests its self.   When you set this variable there will be no issue with the line drawings.  To set or unset it type the following at the Allegro  command line:

     set addline_nomerge
     unset addline_nomerge

Hope this helps.
Chris


Script snippet:

# Graphics
add line
setwindow Form.mini
FORM mini lock_direction Off
FORM mini class PACKAGE GEOMETRY
FORM mini subclass DISPLAY_TOP
FORM mini line_width 0.001
setwindow pcb
pick -1.6 -0.8
pick -1.6 0.8
pick 1.6 0.8
pick 1.6 -0.8
pick -1.6 -0.8
done


add line
setwindow Form.mini
FORM mini lock_direction Off
FORM mini class PACKAGE GEOMETRY
FORM mini subclass DISPLAY_TOP
FORM mini line_width 0.001
setwindow pcb
pick -1.1 0.8
pick -1.1 -0.8
pick -1.6 -0.8            #Merged with existing line. Start next line.
pick -1.6 0.8
pick -1.1 0.8
done

add line
setwindow Form.mini
FORM mini lock_direction Off
FORM mini class PACKAGE GEOMETRY
FORM mini subclass DISPLAY_TOP
FORM mini line_width 0.001
setwindow pcb
pick 1.1 -0.8
pick 1.1 0.8
pick 1.6 0.8
pick 1.6 -0.8
pick 1.1 -0.8
done

·         Allegro/OrCAD PCB – Added a command which turns off the line merge capabilities of Allegro during Graphic placement, and another that turns it back on when done. This should prevent component outlines from accidentally merging with terminal outlines and causing graphical issues.

A new V2016.11 pre-release is ready to test - www.pcblibraries.com/downloads