I could not agree more.
Complying to existing standards, as they are, would be a good first step.
As long as JLC etc refuse to use anything else than 20 year old, maybe cracked, software we are going nowhere, however brilliant the specification.
1 Like
Lots has improved already.
The first EDA program I used was a DOS version of âUltiboardâ. It came with drivers for some 30+ different Gerber plotters, each with their own dialect, and you had to use the right driver to make gerber files that were compatible with the plotter that your fab house used. Iâm not even sure whether âGerberâ was already a de facto standard back then.
Iâm a big proponent of freely accessible open standards (and software). Too much damage has been done already by companies deliberately blocking progress out of fear to give their competition some kind of advantage. It is the single most important reason that I use Linux exclusively. Linux has itâs own issues (and therefore only about 2% of desktop users), but I simply and bluntly refuse to run along with the madness in this world.
You two did notice that âgood enoughâ was in quotes because itâs "good enough " from the fabricators perspective but not from the designers
Donât like it, dont use those fabricators because I donât like it and I dont use them
1 Like
Sorry, I missed the true intention of your posts.
No worries with the offtopic,
I still donât understand why when unticking the macros and x2 export options Ucamco still interpretes that is x2 instead of x1 
Another manufacturer reported to still see the circles after I sent them new gerbs
I think the problem with the circles has nothing to do with X1/X2 but with sloppy rounding in the fabricator CAM software.
In Gerber, a circular arc is defined by begin point, end point and center. Simple. When begin point and end point coincide it represents a full circle. I guess there are very short arcs in your Gerbers, with end point close to the end point. This is perfectly valid. The CAM software rounds these values with the care of a bull in a china shop, begin and end point land on top of one another, lo and behold, a full circle appears. Those that know what they are doing round carefully, and render the file correctly. It is all clearly explained in section 4.2 of the spec. When you change resolution rounding is different, and when you are lucky the problem does not occur on that job and that software, but in another job or other software it may re-appear.
Did you tell the fabricator that your jobâs Gerbers are perfectly OK as you checked them on the Reference Gerber Viewer, that it is his problem, and what he is going to do about it?
If so what did he say?
Not sure if this helps but Iâve successfully order boards from (JLCPCB, PCBWay, OSH Park, etc) with this settings without any hiccups so far (KiCAD v4.7, 5.1.x)
1 Like
Excellent. Pity you did not enable X2 and include netlist, though.
You probably expect the fabricator to do a serious electrical test on the boards. How is he supposed to do that if you donât tell him what the netlist is?
1 Like
Thanks again for sharing your settings I will use them + including netlist for electrical test
You donât actually need X2 for that. It certainly helps but many CAM tools can figure out the electrical connections virtually for probing.
Indeed. You do not even have to know what or where pads are. you just follow connected copper until you find a hole in the solder mask layer, and manufacturers for software for flying probe tests have been playing this game for 20+ years. (30+ or even 40+?) Itâs pretty simple to extract that data.
Several years ago, one work round was to use Coordinate Format 4.5 and not the default 4.6, for which the CAM350 version had a bug with full circles
Had the same problem. Workaround is to use 10nm instead of 1nm precision. Select format 4.5 (mm) when exporting gerber. And disable âUse auxiliary axis as originâ. This is a workaround and the CAM350 bug will not trigger.
Also, change the drill units to millimeter. This has nothing to do with the bug, but using non-metric units is a pain and there is no good reason to use inch for PCBs more than 130 years after we declared all units called inch as obsolete. You will have rounding errors when using non-metric.
1 Like
This has nothing to do with the age. The bug only occurs when you use nm precision. AFAIK most other PCB tools use a lower precision, so the bug does not occur.
And think about the situation in which they are: They have a, probably cracked, old version of CAM350, this version is older because they donât have a crack for any never version or donât want to buy a new version. Buying it is quite expensive for them, CAM350 will them probably cost more than 3500 CNY per seat, Chinese median monthly income is something like 8000 CNY. And the staff knows how to work with the current version, buying a new version would cost man hours to learn the new version. They rather do not support such formats and turn a few % of customers away than buying a newer version. If they need to buy it, there prices would increase. If you have a problem with that you should buy somewhere else and donât always choose the cheapest option. The problem is the customer who always wantâs the cheapest stuff.
First that I have heard about the auxiliary origin.
I guess this is why we still have the 4.5 option
I just read it in the other thread, here Strange circles in the gerber. Our PCB manufacturer complained about this circles, i switched to 4.5 format and disabled âUse auxiliary axis as originâ option and he was happy with the new files. Maybe the âUse auxiliary axis as originâ has nothing to do with the bug but i donât really care, as long as i know that this settings work.
You are right, fabricators will reverse engineer (= guess) the netlist from the image data. They have to. Strangely enough, it is a cultural thing. In the US the netlist is nearly always included. In Europe the netlist is nearly always omitted. Why that is I do not know.
No netlist has the following disadvantages.
- If anything goes wrong with the Gerber files - bugs do happen -, the polarity, which layer they are associated with, mirroring, etc the netlist will be changed with high probability. It is a powerful checksum on the data. US fabricators compare the supplied netlist with the reverse engineered one, and if anything goes wrong, bingo, they see it. In Europe, the problem will appear when the PCB is delivered. Which do you prefer?
- Reverse engineering is never fully accurate. Not supplying the netlist is accepting a dodgy electrical test. In effect, not supplying the netlist is telling the fabricator: âYou must do some electrical test, but what you test, I dont care.â
- If you supply a netlist, and something goes wrong, the blame is with the fabricator, unequivocally. No discussion whether the Gerbers are correct, the layer structure was clear, dadada.
Not supplying the netlist is daft. No other industry would find this normal.
Do you still have this problem? If not, how did you solve it? You may help future readers when tell use what worked for you.
