| Author |
 Topic  |
|
jlawton
United Kingdom
108 Posts |
|
|
Iain Wilkie
United Kingdom
1015 Posts |
 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
|
 |
|
|
edrees
United Kingdom
779 Posts |
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
United Kingdom
1015 Posts |
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
|
|
|
|
Iain Wilkie
United Kingdom
1015 Posts |
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 |
Edited by - Iain Wilkie on 25 Feb 2014 10:02:07 |
|
|
|
jlawton
United Kingdom
108 Posts |
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 |
Edited by - jlawton on 25 Feb 2014 11:30:28 |
|
|
|
edrees
United Kingdom
779 Posts |
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.
|
|
|
|
Iain Wilkie
United Kingdom
1015 Posts |
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
United Kingdom
779 Posts |
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
United Kingdom
1015 Posts |
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 |
|
|
|
JMCLAY
Ireland
1 Posts |
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 |
|
|
|
Topic |
|
Gerber Errors