Ucamco looks also fine
I will re generate the files with the option you mention and ask the fab again.
I will re generate the files with the option you mention and ask the fab again.
Another unrelated issue I see on your PCB is that you (apparently) have lots of Silk Screen text on top of pads. This is not done.
There are a few different ways that PCB fab houses handle this.
- Some just refuse your PCB.
- Others print the Silk screen directly on the pads, which make them unsolderable, but it is what you specified.
- Others point you to this, and ask you if you want to change this, or want to make the PCB as is.
- Yet others simply clip the text to keep the pads clean.
Another unrelated issue I see on your PCB is that you put a bunch of via’s inside pads. This does not matter much for hand soldering, but if you use a solder stencil, then a fixed amount of solder is available for each joint, and most of that solder will wick into the via’s and this leads to bad solder connections and rework. You have plenty of available space to put the via’s elsewhere.
These are pretty common mistakes beginners make.
It probably is a good idea to do a more thorough review before you attempt to manufacture this PCB.
3 Likes
Hi,
thanks for you feedback on the pcb. regarding the silk on pads, I thought that the solder mask had preference over the silk, so there wont be silk and no problems so far with this. I guess most of them went for option 4. I put them there to get them out of the way. Regarding the via on pad, fab has confirmed that they can do it and so far its the 4 spin of the pcb with no issues related to vias on pads. I don’t do it unless Its necessary, there is not that much space as it may seem. I will take into consideration your advice for future designs, thanks a lot.
Fab reached out and unticking that setting didn’t fix the problem. Do you happen to have a link to the original thread with JLCpcb you mention ?
typing jlcpcb in the search box of this forum, gives:
https://forum.kicad.info/search?q=jlcpcb
And the first link is:
I did not read the tread (again), but I did see the screenshots with the wrongly parsed rounded corners in the pads.
I did not imply you have the same issue though, I just meant it as an example of PCB manufacturers using buggy software.
I have vague memories of some popular program as interface between the Gerber files and the actual plotters that apparently gets pirated frequently and has known bugs / issues or otherwise does not work correctly.
What you can do is find some online viewer that does show these circles, then simplify your PCB and upload again. Iterate till you have a small file that still shows the error, and then look at the gerber file what is the root cause of these discrepancies.
You can also determine the center point of those circles, and then search for those coordinates in the gerber file. You may get lucky and find the right lines quickly.
1 Like
From this old threads, it seems to be a old bug from cam350, there are a couple of workarounds that you could try:
Good find der.ule.
The “Strange circles in the gerber” describes much closer picatostas’s problem, and also provides (seemingly working) workarounds.
The CAM 350 circle bug never goes away. Circles in the silkscreen triggered the bug and the workaround was to use two half circles
I do have indeed circles in the silk. And in the latest screenshot I got from the fab they are using CAM 350 v9.5. Thanks a lot @paulvdh @davidsrsb and @der.ule for the threads. Really interesting reads for sure. I wish kiCAD had cam output presets like eagle used to have. I read through the threads shared and try the posibilities described.
1 Like
You can have KiCad clip the silkscreen when you generate the gerbers. Look at the screenshot of the plot dialog provided by @paulvdh and you can see that he has Exclude pads from silkscreen selected. I suspect that you don’t have that selected, thus the silkscreen over pads in your gerber rendering from Ucamco.
1 Like
I have exported the files like this:
and when I open it with www.ucamco.com still says Gerber X2
Board outline doesn’t appear and there are still silks on pads.
Try ticking “subtract solder mask from silkscreen” this should at least remove silk from the pads. Whether it is still too close for your fabricator based upon how fine they can print is a different question
1 Like
Yup, that worked, thanks!
My bad for pointing to the wrong setting. Thanx for the correction.
One would expect fabs to read files that comply the Gerber specification. Point.
Of course, bugs happen. That is OK, but something must be done about them.
This bug is there forever, and is in a feature that is at least 30 year old, but those fabs simply make no attempt to have it fixed. I results in confusion, waste of time and scrap over and over again. JLCPCB, for one, is a repeat offender, as attested by numerous posts in this forum.
Is it too much to ask that fabs handle 30 year old features correctly?
1 Like
yes as it is “good enough” and to be compliant to the spec costs money. This is one reason I always tick the X2 box because if a fab house preview or their CAM engineer comes back with oddities I do not use them because if they are unable to parse X2 in a setup that only does X1 they have some serious problems and thus what else do they not do?
Nope. It’s not “good enough”.
I find it quite astounding that there is still no standard way of specifying simple things such as for example V-grooving in Gerber files.
Many man-hours are wasted with double and triple checking Gerber files, and ambiguity in standards cause many delays in PCB manufacturing. For some kind of reason I do not understand most people seem to accept this as “normal” and the cost of human hours wasted seems to be not a part of the equation.
[Edit:]
Accidentally bumped into this post from a few weeks ago again today, and did some reading about Gerber in the time in between.
There is a possibility to specify V-grooving and a lot of other features in the latest Gerber standard. Real pads can be defined for flying probe tests for example and lots more, and those may have been there for some time too. So now it’s already time to implement those things in the software and start using them 
1 Like
This whole discussion demonstrates it is not ‘good enough’.
As a trade, we want to become better and more efficient, one supposes. By sticking to 20 year old, maybe cracked, software JLC etc block progress.
1 Like
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 “Ultiboard”. 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. I’m not even sure whether “Gerber” was already a de facto standard back then.
I’m 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 it’s 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.