kicad-developers team mailing list archive

[jp charras <jp.charras@xxxxxxxxxx>]

Le 20/09/2017 à 17:32, Maciej Sumiński a écrit :
> On 09/20/2017 05:29 PM, jp charras wrote:
> [snip]
>> After tests with 2 schematics I found a rounding issue in coordinates (especially wires and pins):
>> Many coordinates are very near (1 mil, therefore one Eeschema unit) the 50 mils grid but not exactly
>> on grid (for instance 499 instead of 500 mils)
>> The a few values I checked are smaller (one mil) than the grid coordinate, so I am thinking this is
>> a rounding issue.
> 
> Would you share an example schematic file, so we could investigate the
> problem?
> 
> Regards,
> Orson

I made more tests on a schematic (attached the eagle file and the converted kicad files).

I have 2 different issues.

1 - "Rounding" issues:
Attached a .sch from Eagle, and the same after conversion to eeschema file.
In the Eeschema file, many (most of?) wires are on the 1 mil grid (see for instance lines 51, 53,
55), not on the 25 or 50 mils grid.
Same in the .lib file for many pins (see lines 129, 130 ... for instance in cache lib)

2 - Library is broken (see the cache lib) after written on disk and cannot be loaded:
 - some empty texts are in library (see line 108)
 if a text is empty the dummy char ~ must be used in file as text string.
 - some symbols ( I am thinking they could be multi units symbols) are incorrect.
for instance see ELECTRON_SMT
especially pins are broken: a pin like:
X A2 10A 10B 10C -400 -100 100 R 50 50 1 0 U
is perhaps a pin multi unit pin
But the pin number (10A 10B 10C) cannot have spaces in string (space is not allowed in pin names and
pin numbers).
This line is broken.

-- 
Jean-Pierre CHARRAS

Attachment: eagle_asset-tracker-v008.zip
Description: Zip compressed data