Did you tell the fabricator that your job’s 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 I’ve 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 don’t tell him what the netlist is?
1 Like
Thanks again for sharing your settings I will use them + including netlist for electrical test
You don’t 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+?) It’s 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 “Use auxiliary axis as origin”. 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 don’t have a crack for any never version or don’t 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 don’t always choose the cheapest option. The problem is the customer who always want’s 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 “Use auxiliary axis as origin” option and he was happy with the new files. Maybe the “Use auxiliary axis as origin” has nothing to do with the bug but i don’t 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: “You must do some electrical test, but what you test, I dont care.”
- 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.
Hi all,
sorry for the late update.
I have exported the latest file with these settings and they haven’t complained about the circles anymore.
This is good news. Are they also OK if you include the Gerber job file, use extended X2 attributes and include the netlist?
The whole point of this thread was that X2 format was not compatible with their CAM software.
but was the circles due to x2 or due to the accuracy setting?
JLC have had issues with x2 GERBERS in the past, more specifically the aperture macro’s resulting in rounded rectangle pads having their corners cut
The unexplained circled however was more todo with the precision setting ( 4.6 vs 4.5) which can result in odd rounding if they are using old CAM software
The fact you have it working is great, but the settings chosen potentially mitigate two different errors and only one is x2 related.
in short, buggy CAM but this might not be x2 related
1 Like
The aperture macro bug has nothing to do with X2 either. The macro definitions have not changed since at least 1997, probably earlier. Neither have the circle definitions. These are very old bugs in CAM350, long since fixed. Of course, if one continues to use old software of doubtful legality it will never be fixed. Well, I should not complain, these bugs are there since only 30 years, it is understandable that JLC has had no time yet to fix them.
X2 has changed nothing in the image definition. X2 defines 4 new commands to define attributes. If you don’t like the attributes, just ignore the commands. And indeed JLCPCB has developed a script to remove these attributes.
Use X2, to help those that can use the attributes.
Exactly, hence pushing for this conciceness. It is “fake news” that this is an X2 issue rather than a cheap fab house issue just perpetuates the lie.
Fact is X2 is a “comment extension” to X1 so if some CAM software is bugging out when X2 is used they are non-compliant and if they are non-compliant to a simple comment, what else are they non-compliant to. would you trust such fabhouses?
Using UK/US fab-houses I have never had any issues with X2,Aperture or precision and if a Fab houses started blaming my GERBER (gerbers cross-checked with multiple viewers) and the GERBERS are compliant, I change FABhouse, its not worth the risk dealing with other fab issues
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.