| T O P I C R E V I E W |
| Mike Warren |
Posted - 14 Jun 2013 : 01:38:32
EPC Version 16.08
I have been using GC-Prevue to do a sanity check on my Gerbers for the last couple of years, but the last board I had made came back from manufacturing with copper fill all over the bottom layer, obliterating tracks.
See this picture: http://mike-warren.net/play/M20130509093716-web.jpg
This board looked fine in GC-Prevue and the board manufacturer was able to correct the problem at their end and resupplied for free, so the only problem was the extra delay.
They didn't tell me what the problem was, but other people I've been talking to say this can come about because of rounding errors in the Gerber.
I'm about to get another board made and thought I'd use a second program to double-check the Gerbers.
To that end, I installed Viewmate, which I have used previously, several years ago.
GC-Prevue loads the Gerbers fine, but Viewmate comes up with all sorts or errors, and won't display the drill files.
When importing the bottom copper:
---WARNING---
Input contains a self-intersecting polygon
at location (1.217409 2.195509) in layer 4.
When importing the drill files:
---WARNING---
Syntax error:
G81M48INC?HT10C00.050T11C00.080T12C00.126%.
This makes me nervous that there may be errors which will cause more failed boards.
It seems unlikely to me that Viewmate, being a mature program, would have bugs in the one and only thing it does.
Does anyone have any ideas? Perhaps another Gerber viewer that works well?
|
| 30 L A T E S T R E P L I E S (Newest First) |
| JMCLAY |
Posted - 25 May 2015 : 13:44:53
I would try loading your gerbers into the Eurocircuits checker. It is by far the best viewer on the planet. I do not work for Eurocircuits.
PCB Nerd |
| Iain Wilkie |
Posted - 03 Mar 2014 : 12:20:08
quote:
Judging by the lack of feedback from No1, I only hope that they must be busy getting to the bottom of this issue that they haven't had the opportunity to keep us updated of their findings. Or they have their heads in the sand hoping that the problem will just go away.
Numberone insist that if a bug is found not to report it via the forum but directly in an email to themselves. The forum is for general discussion between users and is not constantly monitored by No1. A direct email is always the best for bugs.
Iain |
| edrees |
Posted - 03 Mar 2014 : 11:31:46
Hi Iain,
No, I've not contacted No1 directly about this issue, I'd have hoped that they would by now have taken sufficient interest about the critical issues that have been raised throughout this Posting.
The chances of a "rounding error" in the EPC plotting software and an independent Gerber reading error within the EPC Importer software in the same place on the same design are impossibly small. This might suggest non -compliant Gerber format/syntax in EPC software, as every other independent Gerber reader manifests JohnB's error.
There must be tens of thousands of Gerber files created using the default 2.3 (inch) precision and flood pours in pre V17 release software, - and not one single faulty Gerber has been reported.
I'm now loosing confidence in the Gerber 3.5 (mm) precision all-embracing-fix. I still suspect that there is something more sinister lurking underneath all the issues that have been discussed in this Post.
Judging by the lack of feedback from No1, I only hope that they must be busy getting to the bottom of this issue that they haven't had the opportunity to keep us updated of their findings. Or they have their heads in the sand hoping that the problem will just go away.
|
| Iain Wilkie |
Posted - 03 Mar 2014 : 10:37:15
Hi Ed,
I agree that there is still a problem in that the EPC gerber importers do not import the bad gerber properly.
Have you reported this to No1 ?
Iain
|
| edrees |
Posted - 02 Mar 2014 : 13:53:11
I've now loaded JohnBs Gerbers in to various readers and they all indicate the same problem.
It's a shame that both EPC Gerber (intelligent and plain flavours) Importers FAIL to show this problem.
|
| jlawton |
Posted - 25 Feb 2014 : 11:25:32
Ucamco say in the document I referenced earlier:
Warning: "We strongly recommend using 6 decimal places in imperial and 5 decimal places in metric. A lower number of decimal places can lose vital precision. The option to use a lower number of decimal places is a simplistic compression method introduced in the 1950’s, when saving a few bytes was of paramount importance and computers were too feeble for proper compression algorithms. Nowadays the few bytes saved are irrelevant. Modern compression methods far outperform this simplistic method, without loss of accuracy. If the extra digits are not significant, they will be compressed away; if they are significant they should not be blindly removed. The benefits of a small number of decimal digits are long gone. The disadvantages remain. It is a source of endless confusion."
So the clear recommendation is 2:6 imperial or 3:5 metric.
An explanation of Gerber accuracy problems is explained in the section 4.4.2 on Arc Definition.
The Gerber standard now states that up to 7 decimal places (imperial) may be used although not all software will work with this.
They also explain why the Gerber RS-274D standard is deprecated and obsolete.
I've just noticed that 2:6 is not a valid setting in EPC so maybe an internal accuracy upgrade is desirable?
John Lawton Electronics |
| Iain Wilkie |
Posted - 25 Feb 2014 : 09:59:42
To try and conclude.....
Increase your resolution to 2.5 (at least) to prevent gerber output problems .... simples !
If you want to double check your gerbers this can be done using a package like FAB3000.
If you can use ODB++ for your boards do so.
Iain |
| Iain Wilkie |
Posted - 25 Feb 2014 : 09:41:40
To save any confusion arising here.
John B's gerber error is a true error in the gerber and can be seen in ANY viewer. Moving from 2.3 to 2.5 solves this problem.
John L's gerber error is NOT a gerber error as such as it only manifests itself in one particular viewer. In all other viewers it appears ok and I have checked that the gerbers on that one are ok.
Iain
|
| edrees |
Posted - 25 Feb 2014 : 09:30:54
JohnB's problem is also present when read by Viewmate, although the actual error is not as obvious as that highlighted in GC-Prevue.
Any netlist re-constructed from this Gerber will include this short and therefore the error will not be picked up by flying probe ATE unless an independent netlist was also supplied (and used to verify the re-constructed netlist).
I think its ODB++ for me from now on! |
| Iain Wilkie |
Posted - 25 Feb 2014 : 07:59:54
Numberone have already admitted that the default setting of 2.3 appears to have caused JohnB's problem and to increase this to 2.5 at least a fix.
I believe that for those that have adopted the 2.5 that these has been no problems. JohnL's problem was due to a viewer problem
Iain
|
| jlawton |
Posted - 24 Feb 2014 : 19:42:11
Take a look at the documents on this site: http://www.ucamco.com/downloads
Very interesting information about Gerber files and more. With the information it might be possible to validate the Gerbers that EPC produces.
This document http://www.ucamco.com/files/downloads/file/3/the_gerber_file_format_specification.pdf pages 53/54 and 74/75 stress the importance of using high accuracy settings, 6 decimal places for imperial and 5 for metric - even more than No.1 suggest.
John Lawton Electronics |
| Iain Wilkie |
Posted - 24 Feb 2014 : 19:17:46
Again Ed .... That is what not to do. You must ensure the same plots are used. I think you can ask for them if you move to another supplier.
Iain |
| edrees |
Posted - 24 Feb 2014 : 18:07:11
There is off course another sting in the tail of the gerber only plot route. Having "proven" the gerbers by puchasing a few pcbs as a first spin from a supplier specialising in express turn around of small quantity orders, you then place a production order for a large quantity of pcbs from another supplier who specialies in larger quantities. There are now two front end fiddlers, so the second run of pcbs could still be different!
Makes one wonder why we have got away with this for so long! |
| John Baraclough |
Posted - 24 Feb 2014 : 17:41:17
quote:
Originally posted by edrees
.
.
I would be only too happy to view JohnB's original Gerbers in Viewmate too, (to compare results against GC Prevue).
.
.
An email has been sent.
-------------------------------------------------------
Birthdays are good for you: the more you have, the longer you live ... and I've had lots of them so I should know! |
| Iain Wilkie |
Posted - 24 Feb 2014 : 15:19:11
Lot of folks use PCBTrain for boards ... just checked with them and they accept ODB++
Iain
|
| edrees |
Posted - 24 Feb 2014 : 14:44:30
JohnB/Iain,
I was not aware that the original native file had been found and I was under the impression that only the Gerbers were available.
I would be only too happy to view JohnB's original Gerbers in Viewmate too, (to compare results against GC Prevue).This is most likely down to the 3 decimal place "Gerber rounding error" explanation offered by No1, and it would be interesting if Viewmate "auto-corrected" this error whilst GCPrevue displayed the problem.
Even if you used the regenerated Gerbers from FAB3000 you must still include an IPC netlist for the Front End Fiddler to check his tweaks against.
Presently, not all my PCB suppliers accept ODB++, but yes, I believe it will become the defacto standard given time. |
| Iain Wilkie |
Posted - 24 Feb 2014 : 13:59:17
I have just opened up JB's ODB++ file in FAB3000 and looking at the plots ... the error is not there. This kinda indicated that the ODB++ output is good. I could actually then re-generate good Gerbers from this from within FAB3000 in if required.
It looks maybe like we should be submitting ODB++ files instead of gerber ?
Iain
|
| Iain Wilkie |
Posted - 24 Feb 2014 : 13:52:18
Ed ... you can also get the Valor free viewer from Mentor here ...
http://www.mentor.com/pcb/downloads/odb-plus-plus-viewer
Iain
|
| edrees |
Posted - 24 Feb 2014 : 13:25:38
Your understanding of ODB++ is the same as mine, -but I'm not too familiar with it.
I understand that it is more robust. It may not eliminate all the "manual front-end fiddling about", but at least there's an encapsulated design netlist for the P/Plotter to check against.
Viewmate (free) viewer imports ODB++
Is a now a case of the devil you know?
|
| Iain Wilkie |
Posted - 24 Feb 2014 : 12:50:41
Ed, what you say is all correct as I have always understood it.
The request for an IPC-D-356A output is already logged into EPC as a new feature, that was done right at the beginning of all this.
However I believe that ODB++ was specifically designed to supply ALL the info to manufacturers in one file ... this I believe includes the plotting info and the netlists but I would need check, but if so it may be that it is the ODB++ files we should be sending ?
Iain
|
| edrees |
Posted - 24 Feb 2014 : 12:18:33
I have now discussed this issue with some Contract pcb designers, plottoplotters, pcb manufacturers and sub-contract assemblers.
The common theme is that Gerber error plots are extremely rare and that the Gerber standard is generally robust. However, there is a great deal of "manual front end fiddling about" undertaken by the photoplotter. This is when the gerbers are checked/edited for obvious plot errors (like 0.5 metre wide tracks), checked for manufacturability and unterminated tracks etc. (but not mis-interpreted Gerber data). A "corrected" "secondary" set of Gerbers may even be produced from the Gerbers supplied to plot the final artwork!
The netlist is then constructed from the set of Gerber plots. Any two intersecting tracks will be (erroneously) treated as one net. Without an IPC netlist, this re-constructed netlist becomes the default netlist used by the flying probe ATE which checks for pcb manufacturing faults such as under etch, track-track shorts etc. Without an independently generated netlist to compare the re-constructed Gerber netlist with, the (intersecting track) error is undetectable.
The solution for Gerber only plots appears to be to supply the pcb manufacturer/photoplotter with the set of Gerbers along with an IPC netlist. Unfortunately at present there is no facility within EPC to do this. It may be done via FAB3000 interpreting the ODB++ output from EPC as Iain suggests, but it's imperative that it's also sent along with the Gerber set to the plotter. The chances of a corrupt ODB++ file/FAB3000 producing the same error as the "front end fiddling about" will be incredibly rare, so this should be failsafe method although it may generate "false positive" errors.
So No1, when can we have an IPC nelist output feature please and is the syntax of your Gerber output fully compliant? |
| Iain Wilkie |
Posted - 24 Feb 2014 : 09:52:20
quote:
Iain, Its not uncommon for me to order 50+ pcbs as the first spin. Some of my Clients need a "one time only" product quickly (which is why I self etch my protos wherever possible) and there is no time for a production quality proto evaluation before ordering bulk pcbs. I need to get it right first time.
Ed .... I would never do this ! .... All customers are informed that the first spin is prototype and 2nd spin production. Anyway up to 4 layer can be expressed (3 days I think from PCBTrain) only copper though but that's what needs checking anyway ! ... so it doesn't need to run away with time.
Iain |
| edrees |
Posted - 24 Feb 2014 : 09:45:46
JFI.
I've loaded JohnL's Gerbers (all four flavours) into Viewmate with no error visible.
It seems to me that if various "industry standard" Gerber viewers/plotters are producing different outputs, it may be because the Gerber syntax may be incorrect and the resultant plots are a result of how the different packages interpret the incompatible file data.
Viewmate sometimes gives me (and Mike W) a,-
quote:
When importing the bottom copper:
---WARNING---
Input contains a self-intersecting polygon
at location (1.217409 2.195509) in layer 4.
It then asks whether I want to auto correct this problem, -and I allow it to do so!
This is always on a flood pour layer. Now it's impossible to manually construct a self-intersecting polygon, but EPC manages to do it within it's flood pour algorithm, or the Gerber syntax is incorrect and is being mis-interpreted by Viewmate as such!
I will try and phone around some of my Contract pcb designers and also some major sub contract pcb suppliers/manufacturers today, and get a feel for just how many bad Gerbers there are out there. I suspect it is going to be very very rare.
Iain, Its not uncommon for me to order 50+ pcbs as the first spin. Some of my Clients need a "one time only" product quickly (which is why I self etch my protos wherever possible) and there is no time for a production quality proto evaluation before ordering bulk pcbs. I need to get it right first time.
|
| Iain Wilkie |
Posted - 23 Feb 2014 : 19:28:14
Ed ... I think your missing one important point here. On complex multilayer boards the first spin would only mean making 1 or 2 boards. I agree we don 't find anything wrong till the boards are on our desk, but thats life. Initial testing will discover errors in design and build and of course any gerber error. If there is a gerber error then we would try to modify the prototype boards but this could be difficult especially on complex multilayer. However if the pcb is ok .... Then the plots for that board would be used to produce production batches of boards in the knowledge that the gerber data was plotted correctly. If there is a gerber error this would be reported back to the manufacturer who will investigate and a fix would be worked out and new plots produced and checked. The whole reason for first spin prototypes is to find any problems wherever they lie and then feed what is discovered back into the second spin an subsequent production batches. Internal board faults are the worst to put right to get your prototype working hence the need to get the gerbers correct first time especially on 6 layers and above.
Iain
|
| edrees |
Posted - 23 Feb 2014 : 18:33:40
Iain, if a plotting /manufacturing error has occurred, the first we will be aware of it is when we bench test the first off, and unless the manufacturer makes the bare pcb and the assembly, no-ne (apart from the Designer) will take responsibility for the consequential loss and inevitable delays. Your Post on 20th June 2013 testifies that ATE bare board testing is still prone to human error,- even though the Gerbers are fine! But this is a different matter.
There are precious few UK based pcb manufactures left in the UK, and even fewer that offer sub contact manufacture as well. I'm fortunate in that I've a local one, but usually my pcb assemblies come from a combination of an independent pcb manufacturer and an independent sub-contract assembler.
My concern is that different Gerber viewers/photoplotters appear to interpret the same EPC generated Gerber file differently and whether this is a result of EPC Gerbers not being fully complaint to the relevant Gerber Specifications -see RVpilot post,- quote:
"....does No1 plan on updating the output format to meet the current specification. i.e. Add D01 and D02 codes to the end of all relevant lines ? which by Ucamco's own admission can currently cause unpredictable issues in manufacturing machines depending on how the parsing of the files is handled"
-to which No1 has yet to reply!
FAB3000 may be smart enough to interpret the (non-conforming) data as intended, but that's no re-assurance that the pcb manufacturer/plotoplotter will. And if they can prove that the Gerber is not 100% compliant then they will be vindicated in supplying bad pcbs. |
| Iain Wilkie |
Posted - 23 Feb 2014 : 17:18:08
quote:
This is concerning, as if I'd invested in FAB3000, verified my Gerbers OK, and then instructed my Sub-Contractor to order the (12 layer) pcbs and manufacture several pcb assemblies comprising very expensive semis, the fault still would not come to light until the day I bench tested the first off, and then who pays for the subsequent re-work? I am no better off and my sleepless nights continue to haunt me!
Nope .... not true. The company that manufactures a lot of my boards not only manufacture the bare pcb but also do the assembly. If I issue gerbers that are correct and they manufacture the bare board that is different from the gerber, they take the hit. Remember that manufacturers will test their bare boards before supplying. They do this by generating a netlist from the gerbers and that drives the bare board tester. So their KEY information is the gerber and will be their ultimate defence in any dispute. This is why you must make sure your gerber are ok as these are the basis on which your contract hinges.
So in using FAB3000 I am better off and my sleepless nights have vanished !
I haven't heard of supplying native design files to manufactures. Not sure how that can be handled as every tool uses there own internal format I would have thought. It was because of this that ODB++ was meant to provide a solution for.
Iain
|
| jlawton |
Posted - 23 Feb 2014 : 16:49:27
Thanks Ed,
I haven't used the EPC Gerber importer. That might be interesting if it is then possible to create a netlist and compare to the original. Probably very awkward as a lot of information is lost in the process of creating Gerbers.
John Lawton Electronics |
| edrees |
Posted - 23 Feb 2014 : 12:31:29
Gentlemen,
I've just re-read this topic all over from Start again, and my conclusions are as follows,-
1) There is little evidence to indicate that EPC produces erroneous Gerber plots (especially with 2.5 inch).
2) There is little evidence to indicate that Hardware Arcs enabled is prone to producing erroneous Gerber plots.
3) Some Gerber viewers (and photoplotters) may give erroneous ouputs (**).
4) The case for FAB3000 (as a Gerber checker function only) is not justified because of 1) and 3) above.
IainW is correct in stating that with the present Gerber system there is no real "feedback loop" to ensure that the Plotoplotter output is what the Desiger intended. We are relying purely on the robustness of the Gerber Standard. Consequently, several Users report to have had bad pcbs manufactured. This is concerning, as if I'd invested in FAB3000, verified my Gerbers OK, and then instructed my Sub-Contractor to order the (12 layer) pcbs and manufacture several pcb assemblies comprising very expensive semis, the fault still would not come to light until the day I bench tested the first off, and then who pays for the subsequent re-work? I am no better off and my sleepless nights continue to haunt me! quote:
supplying faulty gerbers to manufacturers (making any errors their responsibilty)
is not the major problem!
So this problem is not necessarily of EPC doing, (** unless No1 are not abiding to Gerber Standard convention, which might result in mis-intepretation by the various Gerber readers), but rather an Industry wide matter of inconsistent Gerber plotters. Perhaps this is why some pcb manufacturers accept pcb data in "Application Source Code format" to avoid the gerber process altogether. I see pcb manufactures accepting Mentor Graphics, Altium, Boardmaker and even Eagle, but no-one I know of accepts EPC format (but one I know of accepts Design Spark!).
I've used Pentalogix "Viewmate" for many years to "visually check" my Gerbers and, touch wood, have never had bad pcbs.
I'd like to check JohnL's Gerbers too please, if you'd kindly email them to me (in strictest confidence), I'll report back what Viewmate makes of them. By the way, John/Iain, what does EPC Gerber importer (Intelligent or otherwise) think of them? |
| Iain Wilkie |
Posted - 22 Feb 2014 : 20:38:45
This just highlights the problems with gerber generally. Not only is it up to how the gerber is produced but also its interpretation by readers and viewers. I have had one instance where the gerbers were correct, but when the plotters produced their file from the gerbers it produced an error in the plot file ! In that instance the plotters took responsibility, but it does outline that the gerber format is so old and mucked about with that it is not robust.
A feature that would eliminate supplying faulty gerbers to manufacturers (making any errors their responsibilty) is to be able the generate a netlist from the outputted gerber files and comparing this with the design tool netlist. This is essentially what FAB3000 does, but might also be a future built in utility for EPC if feel they can offer this.
Iain
|
| jlawton |
Posted - 22 Feb 2014 : 20:21:58
I sent four test sets of Gerbers to Iain who has very kindly loaded them all into his FAB3000 package.
The good news is that regardless of Gerber accuracy or hardware arcs settings they all look the same, no sign of the problems I was seeing with my Gerbv viewer. So this time EPC is blameless.
John Lawton Electronics |
