Planar Gerber Data problems

Version of PI-Expert: 2.7.1.23

PI Expert Online Kernel Version: 10.7.1.23

This is basically a continuation of the "Planar transformer, Problem with pins" thread.

The comments refer to Gerber data generated in this project.

Discrepancies in the generated Gerber data will be addressed here.

First of all, I should point out that I am not an expert on the Gerber data format, but I have been forced to study it partially.

There are inconsistencies and errors in the data that cause problems in processing it.

The errors lead to the inability to use the data in production.

The inconsistencies are in the ordering and interpretation of the data.

For example, most files cannot be opened and therefore imported in Altium 17 or Altium 19. The program usually freezes and has to be hard killed.

The reason for importing into a CAD program is simple. While the Gerber generated coils are nice polygonal coils, the PCB size and hole locations are better accommodated in PCB processing software. So for me it is Altium.

Data preparation:

I don't know what the .ART extension means, but rename all of these to an extension that is digestible by the Gerber program.

For example, .CAM or, as in my case, .G. It is also possible to use directly the endings for the individual layers (.GTL, .GBL, .GTS, etc).

Data errors:

On PCB2 there is a Via connecting layers 2 and 3. However, on layer 2 it goes outside the polygon and creates a short circuit (Fig.1). This is also visible in the PI-Expert design (Fig.2).

It is necessary to either shrink it (better not!) or move it a bit.

Furthermore, there are a total of 3 buried vias on PCB2.

Via from layer 2 to layer 3.

Via from layer 3 to layer 4.

Via from layer 4 to layer 5.

The fact that the first and third Via have the same position is fine (actually it is not, corrected in the previous text).

They are above each other, but in different layers.

The problem is the middle Via. The generated data is exactly the same as the data for the first and third Via.

In PI-Expert it is positioned correctly, i.e. about 4.2 mm further to the right (Fig.3).

Discrepancies:

To check the data, I recommend this website:

gerber-viewer.ucamco.com

Not only does it display Gerber data, but it also performs syntax analysis so you have a chance to see what's wrong with the data.

Just click on the "syntax check" button (Fig.4).

If you open any generated Gerber file in a text editor, on the second line you will see this:

%FSLAX55Y55*MOMM*%

That % is the parameter delimiter. The sequencing of multiple commands when defining parameters should be fine, but somehow it is not.

If you don't want gerber-viewer to report an error, place each command separately:

%FSLAX55Y55*%

%MOMM*%

A few lines further on you will find this:

G36*

G54D10*

G36 is the start of the polygon (until terminated by G37). The data that follows and forms a closed pattern (having the same start and end coordinates) is converted to a polygon.

However, gerber-viewer does not like to change the tool/aperture inside the polygon (G54-tool/aperture-change, D10-tool/aperture-number).

The correct way is to change the tool/aperture first and then work with the polygon.

So just swap the lines:

G54D10*

G36*

However, Gerber-viewer also disagrees with the use of the G54 command. He claims that it is deprecated and that the short version of the tool/aperture change should be used.

The absolutely correct syntax should therefore be:

D10*

G36*

That's all for now.

This is my first experience with a planar transformer and so far I have to say it is a fight.

Hope this helps someone and I wish the PI Experts good luck in debugging.