I sent a set of Gerber files from EasyPC v8.0.8 to Advanced Circuits (
formatting link
), and was told that the "dimensions" file contained improper information ("only two small dashes"). This resulted in my pcb design being put on "CAM Hold", which delayed its processing.
I ended up having to create a PDF for them, with a drawing showing a marked reference point and the dimensions to each side of the PCB outline from the reference point, so they could make a Gerber dimensions/outline file, for me, from that.
This was the first time that I had had someone else make boards for me. This was for a 2-sided board, 9.75" x 2.9375". I did use
4pcb.com's very nice "FreeDFM" check, first, which showed NO errors. And all of the PDF drawings of the copper layers, silkscreen, and soldermask layers, which their FreeDFM automatically creates from uploaded Gerber files and emails back, looked fine.
Using Windows Notepad, I looked in the Gerber "dimensions" file that EasyPC had created. Here is the whole thing:
I'd never seen the inside of a Gerber file, before this, and don't have a Gerber file viewer (YET). So I don't know if this looks reasonable, or not. But apparently it's not, or else there was a problem while transmitting it.
I'm also wondering if maybe there is some setting, within EasyPC, that I need to change. If not, what could be the problem and what could I do about it? Anyone? Or maybe it's time to upgrade to EasyPC v10.
The Gerber file you posted is just a stripe 0.57mm long and 0.026mm wide according to GCPrevue
formatting link
This is worth downloading and using to check out your Gerbers before sending.
Where did the "dimensions" Gerber come from? It's not part of the usual set, and there's an option in PCB plot to include the board outline in the plot.
The Gerber is valid- it's just nonsense as a manufacturing file.
Version 8 was just fine. So is version 10. I can't remember when they introduced it, but the big thing for a while has been 3D view, which I don't use being a sad git. The copper pour has also got a lot more reliable.
I'm sorry of two of these are posted. It looks like my first attempt has vanished.
On Mar 16, 4:42 am, Paul Burke wrote:
Thanks, Paul! I have downloaded it.
The "dimensions" file was produced by EasyPC, with no special action on my part. (It does appear to be part of the standard set of Gerbers, in my EasyPC setup.)
Oddly, maybe, when I highlight the "Dimensions" plot name and click on the "Layers" tab, the "Board Outline" line has its "Selected" column set to "No", by default. (But there is a "Dimensions" line that has "Selected" set to "Yes", by default.) Next time, I'll try also setting "Board Outline" to "Yes", for the Dimensions file, since the board outline is what the "CAM Hold" guys seemed to be wanting, from that file. I must have been too sleep-deprived to think to check that, at the time.
I also don't know if a separate Dimensions file would have been required, if I'd simply included the board outline on some or all of the other plots. But I had just used the default settings that EasyPC had, which didn't include the board outline on ANY of the other plots, and did include the Dimensions plot.
One thing that I did change, after my first "freeDFM" check, was to select "Hardware Fill" and "Hardware Arcs", in the "Output" tab's "Device Setup" dialog, under "RS-274-X (Extended Gerber)", because without "Hardware Fill", the poured copper areas were filled using _lines_, which, only in certain cases, caused freeDFM to complain about lots of very thin tracks. I could actually see them, too, on the PDFs of the artwork that were emailed back to me (at least at magnifications above something like 1200X). The Gerber files were also significantly larger, without "Hardware Fill". Using "Hardware Arcs" is apparently a good idea, too, since, otherwise, arcs are rendered using multiple line segments.
You should try their free FreeDFM service! (
formatting link
, or,
formatting link
) It's not just a Gerber syntax checker. It checks (apparently) ALL sizes and clearances, etc etc, and also automatically "thickens" all silkscreen artwork to meet their minimum line-thickness requirement. Then, usually within a few minutes, it emails back a fairly-well-detailed report, which includes a nice price quote with both prototype and production pricing, PDFs of the artwork for each layer (a free on-line Gerber viewer, in essence), and, an Error Summary, with the number (quantity) of each type of error found, and five samples of each type of error it found. Each error-sample includes three zoom views of artwork showing the error, with a text description giving the error margin/measurement and its coordinates, plus a description of the relevant manufacturing requirement that was not met. It seems like it probably saves their CAM engineers and their customers a ton of time and aggravation, at least for inexperienced customers like me. (But apparently they need to start also checking the Dimensions file, if it's used.)
Aside: I didn't take advantage of any of their pricing "specials". But my prototypes' pricing seemed pretty good, although maybe a bit weird: They wanted $54 each for qty 5 ($270), but $30 each for qty 10 ($300), for a three-day turnaround. I took the 10! But now I'm kicking myself for not checking the price for 20. (In the emailed price quote that's included with the freeDFM report, you can simply change a quantity and click to update the list of quotes versus turn- times, and can click on any unit-price to place an order.) Those prices, for 2.94" x 9.75" 2-sided .031" FR4, included lead-free solder plating, green solder mask on both sides, white silkscreen on top, board dimensions cut within .01", and other stuff. They must use lasers to do the drilling, because I didn't see anything at all about pricing versus number of drill sizes, or anything like that. And I also had some non-standard hole sizes, which were never mentioned. All-in-all, it was a relatively-painless first-timer experience (and, probably largely thanks to their freeDFM check, would have been almost- completely uneventful, had it not been for my Dimension file problem). I also liked being able to go to their website to track the progress of the boards' processing. (This is starting to sound like an advertisement. But no, I am not affiliated with Advanced Circuits or their people in any way. I just enjoyed their nicely-automated setup, and their very-attentive service.)
Yes, I love EasyPC v8. The 3D and better-rendering stuff was just starting to be hinted-at, in my v8, but was only in a few of the examples, as far as I could tell, not being too interested at the time, as I was first learning it. I would actually like to have 3D, now, so I could more-easily check component clearances, etc. But I don't know if it could do what I need, since I'd like to be able to see the clearances between components on two boards that are at a right angle to each other. If they could provide that, I'd upgrade tomorrow, even though that would mean paying more, to also raise my pin limit above 1000, since one of the six boards I'd like to simulate in 3D together, at the moment, has something like 975 pins. I'll email them and try to find out more about the 3D capabilities.
I'm REALLY glad to hear that the copper pouring is more reliable, in v10! That's one of the (few) main things in v8 that is fairly-often quite aggravating.
I did just go to
formatting link
, and looked at a list of some of the improvements in v10. One that caught my eye was something about showing clearances on-the-fly, while editing tracks. I'd probably have given them my car, for that, a while back. I'm definitely going to upgrade, now.
I suspect there is a 'glitch' with this particular installation of easypc since this is- and has been for a very long time - a well known, capable, and respected pcb layout package.
from the sample gerber given - it ain't all there!!
I suspect that the 'dimensions' the pcb house was asking for is the aperture dimensions file - generally just referred to as the apertures file - in days of old, but not so oftennow, it was called the D codes sizing file (or similar). Normally easypc (and just about every other pcb package) produces 274X gerbers - they do not have a seperate apertures file. If the output is set to 274D gerbers then there must be a seperate aperture file. Since the pcb house could make no sense of the gerber file provided I guess they may have asked for the aperture dimensions file to see if that was the problem since this is the only other 'gerber' file there is. On the other hand it could be nothing to do with it.
ElectronDepot website is not affiliated with any of the manufacturers or service providers discussed here.
All logos and trade names are the property of their respective owners.