[Solved] What resoluton does altium have for PCB and Gerber exports?

[Doctorandus_P]

Edit:
In the end it turned out there was nothing strange about the altium resolution. It was just a TQFP 144 footprint that had it's pads defined in some non regular pattern. I don't now the origin of that footprint and am still mildy curious to know whether it could have been a default altium footprint.

===================================
I use KiCad myself, and some time ago I experimented with the altium importer. I imported one of the bigger Nucleo boards, and the import was usable, but not perfect. One of the things I noticed was that the pitch of pads (I think it was a 0.5mm TQFP or QFN) was not regular. I guessed that altium may be working on a 1mil resolution natively, and that seems to become a limitation now that SMT parts get smaller and ever higher resolution PCB's are made.

I also have a vague memory about one of Dave's own video's where he states that fine pitch stuff is difficult to get "just right" in altium, and maybe there is some "special high resolution mode".

KiCad uses 32bit integers as nanometers, so resolution is plenty for any PCB. (up to 4 by 4 meters, but that may be untested and buggy).

[tszaboo]

Nonsense, the export resolution can be set to 0.01mil. And components and tracks can be moved by 0.001 mm.

[Doctorandus_P]

Nonsense, the export resolution can be set to 0.01mil. And components and tracks can be moved by 0.001 mm.

"can be set". Does this mean this is a user setting?

It's not that I would be "claiming altium is faulty in the eyes of a KiCad Fanboy". I'm just trying to understand what could be the cause. Maybe the KiCad importer of Altium files is not very good. I can imagine that at some point altium improved resolution and this is stored in the file in some intuitive way for compatibility reasons.

If someone is interested in this topic I can spend some time on re-importing such an ST nucleo board and post some screenshot of what I saw in KiCad.

[thm_w]

https://resources.altium.com/p/generate-gerber-files-altium-designer-step-step-schematic-pcb
For gerber exports you choose what resolution you want eg for inches 2:3, 2:4, or 2:5. So 1mil, 0.1mil, or 0.01mil. For that to make any sense it means Altium internally is using at least 0.01mil precision.

Fine pitch stuff is difficult because you normally work on a 1mil or 10mil grid or whatever, so if all of a sudden you have to work in smaller increments, and don't adjust the grid appropriately, it will throw you off. I'm sure kicad is the same.

It must be some issue with the import.

[Doctorandus_P]

Ok, thanks for the feedback already.
I was doubting my own tests (from about a year ago) so I went to the ST website and got another Nucleo board:

STM32 Nucleo-144 development board with STM32F413ZH MCU
https://www.st.com/en/evaluation-tools/nucleo-f413zh.html#cad-resources.
https://www.st.com/resource/en/board_manufacturing_specification/nucleo_144pins_gerber.zip

Back then I did an import of the Gerbers into a KiCad project, today I just reviewed the Gerbers in KiCad's Gerber viewer, so nothing special.
The IC has a 0.5mm pitch and the pads are 0.3mm wide, but the gaps alternate between about 182 micrometer and 207 micrometer.
Then I looked a little bit closer, and the gaps seem to be either 7.2mils or 8.2mils wide while the edges fit on a 0.1mil grid.

So I conclude it's not an Altium, nor a Kicad thing, but that just the footprint of the TQFP144 is "off".
It also does not seem to be a big issue, just a bit "weird".
Of course I do not know where ST sources it's footprints, but still, I'm curious whether this could be a native TQFP144 altium footprint or some other footprint.

I also attached the Gerbers, so everybody can be sure comparisons are made from the same source.

[Pseudobyte]

Why are you importing the gerbers? ST provides the native .pcbdoc in what they label "schematics" on their website.

[Doctorandus_P]

Why are you importing the gerbers? ST provides the native .pcbdoc in what they label "schematics" on their website.

Main reason is probably that I'm overwhelmed by the documentation.
I went back and the page for that Nucleo board does not load properly today, so I also only had the .pdf of the schematic.

I also went back to look around a bit more and found the b-g431-esc1 I downloaded all design files for that project without a hitch, and can also import the PCB into KiCad without problems (Including complete 3D view with all the parts).
This board does double or triple duty for me, as I'm interested in both STM32, motor controllers and their design, altium import in KiCad.

And I must say I'm thoroughly impressed in lots of different ways. By ST by making such boards available and amount (and quality!) of their documentation, for KiCad for their import quality.

But I'm trying to limit my KiCad raving in this altium section, so back to the original topic.
The chip footprint for the G432-ESC board has a perfect metric pitch. Pads are 0.3mm wide and with a clearance of 0.2mm, so apparently there is just something strange with that Nucleo-144 board.

... half an hour later...
I also had a look at this MB1035:
Design files available, imports into KiCad, Only two layer That other nucleo board was 6 layers) and the tqfp 100 footprint is quite differently designed. Pads are narrower, clearances are wider, and the "corner pads" are bigger then the others. But to keep on topic The pitch of this one is also nicely regular, which confirms again that the other board just had a weird IC footprint.
https://www.st.com/en/evaluation-tools/stm32-discovery-kits.html#cad-resources