Missed traces while importing gerber

[Noir47]

Hello.

There is one missed trace on PCB plane when i have done import of BOTTOM gerber file, which was made in Diptrace.

FlatCAM version is 8.3. OS is Win 10 x64. Application runned with administrator privilege.

Screenshot with coordinates of missed trace and gerber file (it's already mirrored with Diptrace) are attached.

Thank you.

[Noir47]

When i loaded an gerber file to FlatCAM v8.2 - everything is ok.

Are there any major difference between those versions (i.e. better tool path optimization, more usable option, etc.)?

[Juan Pablo Caram]

Increasing priority as it is an unrecoverable error.

[Juan Pablo Caram]

This is the minimal Gerber causing the problem:

%MOMM*%
%ADD14C,1.5*%
%FSLAX53Y53*%
G01*
D14*
X8250Y25820D2*
X3200Y20770D1*
X1410Y9850D3*
M02*

There is a diagonally-drawn line and a circular flash. FlatCAM is not showing the line. Is the flash (D3) is removed, then the line is shown.

[Juan Pablo Caram]

Cause found: When a flash (D3) was encountered, the path drawn so far was discarded:

# Flash
elif current_operation_code == 3:

    # --- BUFFERED ---
    flash = Gerber.create_flash_geometry(Point([current_x, current_y]),
                            self.apertures[current_aperture])
    if not flash.is_empty: poly_buffer.append(flash)

    path = [[current_x, current_y]]  # Reset path starting point

[Juan Pablo Caram]

Create polygon for path drawn so far when D03 is encountered. Fixes #150.

→ <<cset 1942fe3bed07>>