Hello.
Sadly the current behaivor counting from sheet origin make useless for production.
I have 2 pick and place, and i have some suggestion about positioning file generation. If you want consider it for the future will be great, if dont, i still make it at hand.
The pick and place file is a CSV file. Is not standarized, so differents pick and places require differents files for the same PCB.
The idea of the topic is suggest some setup when KICAD generate the positioning file
The origin.
Normally the PCB editor has the coordinates origin upper left of the sheet, but is not the PCB corner. Is required allow to the user choose the right corner at starting point.
The regular point is the green, but sometimes the mounter require turn 90 degrees the PCB.
Allways we speak of positive numbers starting of origin in the sense of the arrows
Here we need the option: Origin with 4 options (one for corners)
Please note that all PNP has the origin on the bottom left point, and count possitive when move to the right and when the head go to the rear of machine.
2)Technical band
Since the PNP cant place components at the border of PCB, normally is added a “technical band” of 5mm. Sometimes the PNP allow move the origin, but if is not possible, we need the component displacement. Here we put 2 new options:
Technical band X: 2~10mm
Technical band Y: 2~10mm
PCB rotation
According point 1 is required write the coordinates considering the rotation of PCB when is placed on the PNP machine. No config needed here
Component rotation
The components rotation is not standarized too. For some PNP 90 degrees of rotation is clockwise, and for another is counter clockwise. Here we need one option:
Rotation clockwise - CCW (maybe a single checkbox)
Field order
If we can edit the field order will be great, but is not mandatory.
The origin. KiCad has PCB Editor / Place / Drill/Place File Origin and this can be used as the origin for generating Gerber, drill and placement files. This has been in KiCad for a whole bunch of years.
Technical band. It’s up to the designer where to put footprints on the PCB. There are many factors in deciding this. Many PCB’s are produced in routed out panels, and those can have footprints close to the edge, or even extend beyond the PCB (for example angled connectors). Another important factor is V-grooving. Separating V-grooved PCB’s induces a high mechanical stress in the PCB and this can break brittle ceramic SMT parts. Orientation (rotation) of SMT resistors and capacitors when close to a V-grooving line is important. If you want to enforce this on the PCB, then you can use rule area’s or custom rules.
PCB Rotation. This should not be a function of KiCad. When I create a set of files for a PCB to be made, I do not care about which brand of machines they make the PCB, or whether they put them in panels or whatever. My responsibility is that the set of files (Gerber, drill, placement, etc) are coherent to each other. Rotation is not a function that should be in the PCB design program. It is a variable for production. Adding this to the PCB program would add more confusion then it would solve problems.
Footprint rotation. It’s not standardized, and that is a big mess and a nuisance. I agree with that. KiCad itself has standardized on the rules as defined by the KLC It’s not perfect, but at least it is consistent. Some manufacturers use rotation based on how parts are oriented in the tape. This is inherently faulty, because different manufacturers may use different tape orientations for compatible parts. Sometimes a single manufacturer even has options for ordering the same part with different tape orientations. So basing rotation on tape orientation is inherently flawed. And just as with 2). It is a production parameter. Adding options in the PCB program is not the right place for such things.
Field order No comment.
Wave soldering… is another factor with overlap between PCB design and production. Sometimes footprints have extra features to improve wave soldering yield. I don’t have enough experience to have an opinion here, but thought it’s worth mentioning.
I guess that most of the things you mention can (and should be) set up in the SMT placement machine itself. There is also specialized software for PCB production that does this sort of thing and that may be worth looking into.
I have never tried to generate these files without using File Origin.
I am surprised that in Getting Started in Fabrication Outputs chapter there is no word about it and the example screenshots have this option unchecked.
When we started with KiCad live was easier…
We had at right side the Place File Origin tool while now whenever I want to use it I spend some time searching it to then find that it is hidden by the Place Grid Origin tool that I practically don’t know what it is for. May be I don’t have to place Grid Origin as it as by default at absolute origin (top left of sheet) and I work around that origin (in V4 it was the only way to have origin in your PCB center).
To be clear and not generate screen shots now (that I have then to transport here with pendrive) you can see how my PCBs are located here:
