Warning: Deprecated feature: Open contours

[Jonathan Katon]

Hello,

I came across your tool last week and have been testing it out. I am generating pdf's from gerber files generated by Cadence Allegro SPB16_6. I am getting the "Warning: Deprecated feature: Open contours" message on every single G36/G37 polygon commands in all of my gerber files. I have tried searching online for information about gerbers and open contours but I have been unable to find anything that could be related to this message. I was hoping you could provide some insite into what may be causing this message so I can determine if its just a feature to deal with or if I need to submit a bug report to Cadence.

Thanks
Jonathan

An example block which produced the error:
G36
G01X-2995000Y8180000D02
Y8070000D01
X-2880000Y8125000D01
X-2995000Y8180000D01
G37

I have tried updating the block to include repeated data between lines but this did not fix the error.
G36
G01X-2995000Y8180000D02
G01X-2995000Y8070000D01
G01X-2880000Y8125000D01
G01X-2995000Y8180000D01
G37

This data may be unrelated but I am including the header to the file just in case:
G04 ================== begin FILE IDENTIFICATION RECORD ==================
G04 Layout Name: 601-129-06_a.brd
G04 Film Name: zjmk_assy0001_rs274x
G04 File Format: Gerber RS274X
G04 File Origin: Cadence Allegro 16.6-2015-S069
G04 Origin Date: Wed Jul 13 20:56:39 2016
G04 *
G04 Layer: DRAWING FORMAT/SHT1
G04 Layer: BOARD GEOMETRY/ASSY1
G04 *
G04 Offset: (0.00 0.00)
G04 Mirror: No
G04 Mode: Positive
G04 Rotation: 0
G04 FullContactRelief: No
G04 UndefLineWidth: 8.00
G04 ================== end FILE IDENTIFICATION RECORD ====================
%FSLAX26Y26MOIN%
%IR0IPPOSOFA0.00000B0.00000MIA0B0SFA1.00000B1.00000%
%ADD10C,.01%
%ADD11C,.012%
%ADD12C,.024%
%ADD13C,.008%
%ADD14C,.006%
%ADD15C,.009%
G75
%LPD%
G75*

[John-Philip Taylor]

Hi,

Generally speaking you can safely ignore those warnings. You can even use
the command-line switch "-nowarnings" to stop displaying them.

I'll have a look over the weekend to make sure that the bug is not on my
end and let you know, but I suspect that Cadence is using a deprecated
Gerber file format feature.

[John-Philip Taylor]

If you'd like to know more about the warning, you can have a look at

https://www.ucamco.com/files/downloads/file/81/the_gerber_file_format_specification.pdf

Section 2.6 states that all contours must be closed. And section 4.6 gives
an example.

[John-Philip Taylor]

After closer inspection of your example I see that it is correct. I
therefore suspect a bug on my end relating to negative numbers...

Is the PDF output correct?

Are you willing to upload a complete gerber so that I can more accurately
reproduce the problem?

[John-Philip Taylor]

I fixed it and uploaded to new version to Files.

The Gerber you gave as an example contains many depricated features:

• Image Rotation
• Image Polarity
• Offset
• Mirror Image
• Scale Factor

All those are harmless and can be ignored, because the Gerber generator you're using sets them to defaults anyway. EDA tools tend to include them for compatibility with legacy PCB printing hardware.

In future, please include such code inside a "code" block so that the special characters (such as * in this case) is preserved.

[Jonathan Katon]

John-Philip thank you for the update!! I will download the files and test them out.

My PDF output did appear to be correct despite the error message.

The other warnings I didn't bug you about becuase as you mentioned I suspected they were a result of the file Cadence is generating rather than anything your program is doing. I apologize for the code not being in a block. After being a software engineer for years I have no idea how I made such a rookie mistake.

[Jonathan Katon]

It appears the issue is fixed. Thank you so much for the extremely fast response!!

[John-Philip Taylor]

My pleasure :-)