This is exactly why one should always verify everything and communicate how things are, even if things are “standard”. We always maintain our own libraries just so they are all under one convention and all the assembly files contain short description of the convention. We follow 0 rotation as in the datasheet/reel orientation. It’s really easy to control in production, harder if one assembles only 5 and don’t bother about exact PN. 3D renderings of PCBs help. I’ve been using PCBGogo/PCBWay and JLCPCB for assembly and never had issues on the assembly levels, only my own mistakes.
I suppose it’s not really convenient to check every little thing all the time, but it guaranties that what you get is what you actually want.
I think that Gerber X3 includes pick-and-place information, but I don’t think anyone’s using it yet.
It does and very few are. Most are using ODB++ as it solves all these problems. Ipc-2581 is starting to replace this proprietary file format
Gerber X3 should be simpler for cam software to use as they all speak Gerber. Ipc-2581 is gaining traction as it is built from GenCAD
I think you know this already, but…
After getting more familiar over some years with gerber format I think the newer formats don’t solve many problems which gerber doesn’t solve, too. The real problem with gerber is that there are old and partial, even buggy, implementations everywhere. The last time I checked, Altium CircuitMaker exports ODB++ and adds net information to copper items, probably because it’s part of that standard. Surprise surprise: gerber spec has that information, too, and KiCad can export it, but Altium CM can’t. On the other hand manufacturers who use ODB++ more probably can actually use that information. Small cheap manufacturers who use old gerber sw probably can’t use that information.
The problem isn’t in the file format or standard, it’s in the implementations. Unfortunately it’s impossible to change that situation, and adding features to gerber doesn’t help when they are not used. It would help immensely if even some of the biggest cheap manufactures would update their systems so that they would use modern gerber features without hiccups.
I actually have yet to encounter a fab that wants ODB++ on the millions of qty of PCBs we order yearly…I’m sure there are fabs out there that do but 
This question came time-by-time here:
Basically, there is A/B standard and direct rotations can by applied. To do that, you can use the follow plugins:
- For KiCad 5.1.x https://github.com/essele/kicad_jlcpcba
- For 5+ (next v6 and Nightly) https://github.com/hildogjr/kicad_jlcpcba/
1 Like
That is only partially true because the real thing to consider is assembly houses and this is where file format is critical not in its completeness but in its adoption
It really does not matter if latex is a superior way to deal with documents if people will only accept MS-doc.
Same here… If you are dealing with purely fabrication then GERBER is all that is needed and X2 closed the gap with the missing build (layer order etc…)
But assembly ? All that was offered was pos file… That’s great, it provides (hopefully) the centre and the rotation but zero datum for the rotational frame of reference and the result is assembly houses the. Have to line up the orientation of a part from the tape with the orientation that you (as the designer) states. Time consuming and error prone.
GERBER-X3,. ODB++ and IPC-2581 fill this hole
That however is an aside because all that matters is what someone accepts and more assemblers are asking for these
Fab’s won’t but assemblers will…
These rich data formats can cut the setup time by a factor of 8 and significantly reduce human error. To stay competitive with the cheap assemblers in China these will become a pre-req and already are for places like Celestica
There is indeed a lot of talk of IPC-2581, now called DPMX. However, is anybody really using this format in reality? Does anyone know of a PCB fabricated with it, or any fabricator getting it routinely? The vast majority of fabs don’t even accept it.
On component zero orientation: http://ohm.bu.edu/~pbohn/__Engineering_Reference/pcb_layout/pcbmatrix/Component%20Zero%20Orientations%20for%20CAD%20Libraries.pdf
2 Likes
That document is very much like the KLC. It also has some examples that show that the idea of “whatever is in the tape” as zero rotation does not work.
The only standard for Pick an Place and assembly in general should be the KiCad PCB file itself. Period.
We require for all our customers to provide the KiCad PCB file as it is the only way to obtain all necessary information which are required for the assembly process. I don’t get why KiCad users are forced to use wired export file formats etc. to somehow communicate information which is included in the source file.
On the backend we use a mix of python scripts to gather pin one / orientation, rotation, position, side, MPN and so on. This enabled users to basically have “drag and drop” assembly.
4 Likes
I did consider you guys and the upload of the KiCad files was so much smoother than fiddling with Gerber files. Thanks a lot for that. Unfortunately this time I wanted to try out parts assembly and your quote was 156 € vs $12 in far east. But for boards-only I’ll definitely use you in the future.
First, this is a question of the library and not of CAD. If library does not have unique orientation of components, pick and place machine has to fix the rotations individual for all parts. If there is a unique orientation like the IPC recommendations, it is usually possible to fix the setup by automatic offsets. Formerly we used a Excel script to do this, later we wrote own Qt tool therefore. If orientation is fixed, 0 and 180 degree could fit but not 90 and 270 degree. This comes from mirror and the way the angles count CW or CCW. Some CAD change this from front to back side and others not. Anyway, our selfmade tool also adapts this and can use presets for some widely used cad outputs.
As feeders are usually possible to attach from more than one side of the assembly machine, rotation offsets are typically intrinsic for the software what comes with the machine. Anyway, the tape feed length and feeder position to component assignments needs to be setup manually by the machine operator why this step is probably never completly automatic.
On this note, I find that this Tape and Reel info is not readily available in most datasheets. It must be frustrating to have to adjust after you get the reel delivered!
Check out TI. This is how its meant to be done!
TI have there own package and test factories. Many makes don’t and use sub-contract for this. The result is lack of control of the tape and reel.
I don’t see this as the “lack of control” as in this case you could expect random orientation of individual parts.
It’s more “we don’t care” attitude if the manufacturer allows that one contractor does it consistently one way, and the other one another way. And if they can do it consistently their way, it could be done consistently right. If only someone would care about it/communicate this.
It seems that there is an opportunity to become a bearer of standards in this way. Maybe Kicad can lead at the front with regard to standards for Pick and Place and TR.
Perhaps a way to select orientation at any point and everything update accordingly. Probably more complicated than Im thinking with whats involved but hey… making standards is never easy 
It’s not the EDA thing, it’s the EMS and components manufacturers thing.
There are standards for “Pin1 orientation” EDA notation (IPC-7351C).
However there’s no standard for the interpretation of the given data (some EMS do interpret rotation in relation to component orientation in the tray/reel [WRONG imo] instead of IPC-7351C). Parts manufacturers also do not seem to follow any rules when it comes to packaging in tapes/trays.
1 Like