Number One Systems Forum

Australia
124 Posts

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?

edrees

United Kingdom
779 Posts

Posted - 14 Jun 2013 : 09:27:47

Mike, I've been using Viewmate for many many years, and occasionally I too get a "self intersecting polygon at xxx,yyy" This point usually refers to a corner of my pcb and I also plot the board outline on all layers, so I get the same error on all plotted errors. However, the finished pcb has always been OK and I have utmost faith in Viewmate.

Does Viewmate show your bottom layer as a complete flood? If not then it's more likely that your manufacturer/photoplotter screwed up!

The drl files can be opened in any text editor, and Viewmate will import the drill.gbr file.

Another option to gain confidence is to use EuroCircuits.com. Upload your gerbers suitably zipped up, and put them into your Basket and then click on their free View PCB Image facility. In a few moments you can preview your completed pcb and inspect every layer individually. You can then cancel your basket or place an Order with them.

Australia
124 Posts

Posted - 14 Jun 2013 : 12:15:26

Thanks for the reply.

I found another viewer today. Gerberlogix. It's not free for commercial use, but at least I can try it out for a week or 2 to see if it's any good. And it's pretty cheap, anyway.

Just like GC-Prevue and Viewmate, Gerberlogix has been written without any sensible thought being put into the UI, but Gerberlogix at least allows me to load all my layers at once, or even a zip file containing all the layers.

Anyway, all three programs display the Gerbers fine*, both from my current project and the previous one that had the problem, so I've sent the files off. At least, like last time, it's only 1 prototype panel down the drain if something goes wrong.

[*] Viewmate will not show either of the drill files (plated or unplated) and I don't understand enough about Excellon files to pick what the syntax error actually is.

I couldn't work out how to use EuroCircuits.com without creating an account.

United Kingdom
1015 Posts

Posted - 14 Jun 2013 : 18:50:28

There have been problems in the past where copper fills have flooded over tracks within EasyPC, however this was noticeable from within the EasyPC PCB editor and indeed if you didn't notice it the DRC checks would show it up. If your gerber output looked ok then I think its your PCB manufacturer that has screwed up. I have used GC-Preview for years and I have produced many hundreds of layouts and NEVER had a gerber problem from EasyPC .... what I see in the PCB editor is what I get in the gerber.
There was another viewer I used to use called Gerbmagic ... don't know if its still a contender. GC-Prevue is the kinda free industry standard I think, so if using that I would have confidence in your gerbers if they look ok in GC-Preview

Iain

Australia
124 Posts

Posted - 15 Jun 2013 : 00:08:06

Thank for the reply, Iain.

Yes, I've had the dreaded copper fill problem in the past, though fortunately, not for a few years.

GC-Prevue is actually giving me problems on my current Win7/64 computer. The import dialog keeps failing to open. Sometimes, if I leave it for a couple of minutes and then press Esc I can open it again, but this is happening so often that it can take me 20 minutes to import a set of Gerbers.

As for the recent faulty boards, the manufacturer replaced the panel for free, so they were obviously admitting it was their fault. I'm still nervous, though, since I've had other Gerber weirdness in the past.

Edited by - Mike Warren on 15 Jun 2013 00:36:31

jlawton

United Kingdom
108 Posts

Posted - 17 Jun 2013 : 14:25:51

Something similar happened to me a few years ago. I had ticked 'Hardware Arcs (G74, G75) in the Gerber Setup dialogue in order to reduce the resulting file size. The result was a pile of scrap boards.
I have never used this since, so I don't know whether there is a problem or not. I work in Linux so use the Gerbv gerber viewer which works quite well as a final check.

John Lawton Electronics

Australia
124 Posts

Posted - 20 Jun 2013 : 00:36:40

Curiously, "hardware arcs" is checked automatically when RS-274-X is clicked, and the manufacturers I deal with always specify 274X format. Maybe your manufacturer required 274D.

Edited by - Mike Warren on 20 Jun 2013 00:58:11

United Kingdom
1015 Posts

Posted - 20 Jun 2013 : 10:14:43

Hey Mike .... Old Sods law has kicked in on this .... after me saying I have NEVER had a board/gerber error in years, one has just turned up !!. However its not bad news ... the output from EasyPC gerbers was ok. I ended up with two pads that should have been isolated from a copper flood connected it !. I quickly checked my EasyPC files and the gerber output I sent and they look ok.
Phoned my manufacturer, who looked into this and it appears that the gerbers at their end were also ok, however these apparently get sent to a plotting beureau and it is the plots that came back bad !!. Now as the ATE uses the gerbers to check it should have thrown an error on these boards, but it appears the operator got the error, but then looked at the plots rather than the gerbers and decided it was a problem with the ATE !!.
So bottom line is as before .... have confidence in the gerber output if the view ok .... Manufacturer very sorry
Iain

Australia
124 Posts

Posted - 20 Jun 2013 : 13:10:18

Ouch! I hope it wasn't a large number of boards.

I had a similar error in 2004 where a series of oval pads were rotated by 90 degrees, shorting a high current -40V supply to ground. 100 boards. The PCB manufacturer never noticed it. The assembler never noticed it. I took me fitting the first board to a product and doing a basic continuity check on the power supplies to find it. The assembler had to cut the shorts with a Dremel.

That wasn't the only problem with those boards. Two 2200uF 50V Electros on the +40V supply were fitted in reverse on about 20 of the boards. When the first one exploded it gave me quite a surprise. :)

My latest prototype panel is coming from China by DHL now. I should get it on Monday. Fingers crossed that the boards are good. One of them is a revision of the one I had the problem with last time.

United Kingdom
1015 Posts

Posted - 20 Jun 2013 : 14:34:15

In theory this should never happen.
All boards should be tested before the mnufacturer ships them to you.
I think some of them cut corners to keep the cost down.

Iain

Australia
124 Posts

Posted - 21 Jun 2013 : 13:37:42

Well, the boards arrived today and they are fine. :)

United Kingdom
129 Posts

Posted - 19 Nov 2013 : 17:19:08

Just bumping this topic as I have just received a batch of boards with what I thought was a manufacturing error but has turned out to be an error in the Gerber output from EasyPC version 17.

The first picture is a screendump from the EasyPC layout and the second is from GCPrevue. As you can see the problem is in the Gerber file not the manufacturing process. It's only the top copper layer that's affected.

http://mydesk.myzen.co.uk/_Useful/EasyPcGerberFault1.jpg

http://mydesk.myzen.co.uk/_Useful/EasyPcGerberFault2.jpg

Does this mean I have to visually check every pad and via in all my Gerber files before I send them away for manufacturing?

-------------------------------------------------------
Birthdays are good for you: the more you have, the longer you live.

United Kingdom
1015 Posts

Posted - 19 Nov 2013 : 20:10:45

That is very bad. I would contact NumberOne directly about this and keep us all in the loop as gerbers have to be relied upon. Its impossible to full visually check a gerber on a complex board.

I note this is on a copper pour .... did you run a "check copper pours" in your DRC ???

Iain

United Kingdom
129 Posts

Posted - 19 Nov 2013 : 23:24:10

Yes, I did a full DRC check and everything was OK. I have contacted support and got a very rapid response. Apparently the problem is a rounding error in the Gerber file. Gerber precision setting needs to be a minimum of four decimal places (preferably five) when one is using copper pours to avoid the problem.

Strangely the offending error is a large pad under the via at the end of a track and not the copper pour itself. Perhaps EPC should warn the user that four or five decimal places are required when using copper pours.

-------------------------------------------------------
Birthdays are good for you: the more you have, the longer you live.

edrees

United Kingdom
779 Posts

Posted - 20 Nov 2013 : 09:06:02

John, sorry to hear about your mis-fortune, but thanks for bringing this issue to our attention.

I have ALWAYS visually checked gerbers (with Viewmate) before shipping them out for manufacture, but that is only a very casual check. We must have every faith in the Gerbers, and cannot be expected to visually check everything, otherwise we may as well go back to using black tape.

Copper pours have always been a bit of an issue with EPC, and a bug like this must be fixed ASAP. No1 take note please!

Peter Johnson

United Kingdom
498 Posts

Posted - 20 Nov 2013 : 10:43:46

Actually, although it looked like it, John's problem wasn't the pad. When I regenerated his files, it was clear that it was the pour profile surrounding the pad which was a complete circle rather than an arc allowing an exit route for the track from the pad. In John's file, somehow this circle had been flagged as filled, which is in itself odd, but that bit I couldn't reproduce.

Increasing the resolution to 4 decimal places cured the problem, but you'll want to know why. Well, there are two methods of outputting curves in Gerber files. The older one is a piecewise approximation to the curve using straight lines - in the same way that old pen plotters using HPGL worked. The disadvantages of rounding errors here are obvious - the curves are anything but smooth! The second one is where information is included to allow the curve to be drawn, centre, end points, etc.

The problem here is that relatively small errors mean that the points don't line up, geometrically speaking. Mostly you get away with it, as the software interpreting the data makes the right decisions, but every so often the errors stack up in just the wrong way and it gets it wrong.

That's why increasing the resolution works. it drastically reduces the chances of an arc being small enough for the rounding errors to be critical. Of course, using two extra decimals means it's a near certainty that it will always get it right.

There's already a design rule check function for identifying potential problem areas. That's what the 'Copper Verification' check does, in case you've all been wondering.

United Kingdom
1015 Posts

Posted - 20 Nov 2013 : 10:51:38

Peter,

I asked John if he had done the copper pour verification (see post above) and he indicates that he did do this and there were no errors. Does this mean the copper verification check does not work ?

Iain

edrees

United Kingdom
779 Posts

Posted - 20 Nov 2013 : 10:57:09

John,-

quote:
Yes, I did a full DRC check and everything was OK.

quote:
There's already a design rule check function for identifying potential problem areas. That's what the 'Copper Verification' check does

Does it or doesn't it, -we're all keen to find out!

Sorry, Iain/my threads crossed in the ether!

Edited by - edrees on 20 Nov 2013 11:00:44

United Kingdom
129 Posts

Posted - 20 Nov 2013 : 17:08:39

Doing a DRC check with "Copper Shape Verification" ticked definitely doesn't give an error. I have tried various settings of Gerber resolution including down to 2 decimal places and none give an error on DRC. Although on the lower resolutions the tracks do get very close to the copper pour it is ONLY on the 3 decimal places setting where this copper pour problem appears.

Incidentally, I have another board (the first one I designed using version 17) which has the same problem. At the time I blamed the manufacturer and changed suppliers because of it, but have just looked back at the old Gerbers and found that the fault is in the Gerber file. Unfortunately I didn't keep that version of the design file so can't reproduce the error. In the past I have always used the 2.3 setting for Gerber files and never had this problem, so it looks like a bug in version 17.

I suggest sticking to 5 decimal places for Gerber output until such time as the problem is resolved.

-------------------------------------------------------
Birthdays are good for you: the more you have, the longer you live.

United Kingdom
1015 Posts

Posted - 21 Nov 2013 : 11:43:09

John, Can you send your files to Numberone so that they can investigate the copper verification failure to report an error in this case if you have not already done so.

Cheers

iain

United Kingdom
129 Posts

Posted - 21 Nov 2013 : 12:34:34

Hi Iain,

Peter has all the files for this design already.

Unfortunately I don't have the design files for the fault in the first board which had this problem (around June this year) as I only realised the significance a few days ago and investigated the old saved Gerbers. However, I can send those files if it helps.

I am using Windows Vista Home Premium with SP2 on a Toshiba Satellite laptop.

-------------------------------------------------------
Birthdays are good for you: the more you have, the longer you live ... and I've had lots of them so I should know!

rvpilot

United Kingdom
51 Posts

Posted - 11 Dec 2013 : 12:21:51

On a side note, but still related to Gerber output, 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.

Quote from the last couple of Ucamco specs : Coordinate data without D01/D02/D03 in the same data block create some confusion. It therefore has been deprecated. See 3.4.3. We urge all providers of Gerber software to review their output of coordinate data in this light.

United Kingdom
129 Posts

Posted - 27 Dec 2013 : 21:50:44

... and here's another one! This board was done back in September and the problem can be seen in this picture. The pad just to the right of the switch should be isolated from the ground plane (photo taken from the bottom side of the board).

http://mydesk.myzen.co.uk/_Useful/EasyPc/BeltpackPcbError.jpg

Here's a screendump of the bottom copper layer from Easy PC.

http://mydesk.myzen.co.uk/_Useful/EasyPc/EasyPcGerberFaultB1.jpg

This is a screendump of the Gerber data as interpreted by GC Prevue (free edition).

http://mydesk.myzen.co.uk/_Useful/EasyPc/EasyPcGerberFaultB2.jpg

As you can see the GC Prevue output bears little resemblance to the actual bottom copper layer of the finished PCB. There's definitely something weird about this.

-------------------------------------------------------
Birthdays are good for you: the more you have, the longer you live ... and I've had lots of them so I should know!

United Kingdom
1015 Posts

Posted - 28 Dec 2013 : 10:19:09

Is this output with the resolution still at 3 ?

iain

edrees

United Kingdom
779 Posts

Posted - 28 Dec 2013 : 12:12:28

John, I presume you performed a drc, which was ok?
It also "looks" to me as if some "artifact" from another layer has been plotted in parallel with your desired copper layer. Maybe check your plot settings, as this would be down to finger trouble.
Otherwise, this, and Iain's other recent post is making me very nervous about EPC, as these errors may be very expensive on a complex multi-layer pcb with no access to the inner layers.

No1 lets have some re-assurance please that in future these catastrophic bugs do not enter released "upgrades" of your software. Due care & diligence are words that spring to mind!

United Kingdom
129 Posts

Posted - 28 Dec 2013 : 12:28:13

quote:
Originally posted by Iain Wilkie

Is this output with the resolution still at 3 ?

iain

Yes Iain, this was plotted with Gerber settings at 2.3, before I discovered the bug in another board. It was back in September, the boards were made elsewhere and I have only just received samples. I have replotted this design with Gerber settings of 2.1, 2.2, 2.3, 2.4 & 2.5 and, although the coarser settings do produce strange results with copper pour, it is ONLY 2.3 that introduces these odd pads.

Since late October I have been using Gerber settings of 2.5 and checking every pad on each design (it takes about a day for each one). I haven't found any adverse effects with those settings. I have used Gerber settings of 2.3 for longer than I care to remember and never had this problem until version 17. I have been using Easy PC since the DOS versions nearly 30 years ago!

Perhaps No. 1 should change the default setting for Gerber plots from 2.3 to 2.5.

-------------------------------------------------------
Birthdays are good for you: the more you have, the longer you live ... and I've had lots of them so I should know!

Edited by - John Baraclough on 28 Dec 2013 12:31:15

United Kingdom
1015 Posts

Posted - 28 Dec 2013 : 20:55:56

John, That sounds a bit more reassuring in that I have set mine to 2.5 since this was noticed. This was a particularly bad error as it was never shown up by any drc checks. I too like you have used easypc for many years and done hundreds of layouts at 2.3 with no problem. This problem did show up a few years ago before they introduced the layan check to find pour errors. At that time there was a way of reimporting the gerbers on unused layers back into the design and if you got the colours right you would see immediately any differencies between the actual design layer and the gerber by an obvious colour change. This is quicker than visually checking the gerbers totally manually.

iain

United Kingdom
1015 Posts

Posted - 29 Dec 2013 : 14:53:44

Seems gerber output problems are not uncommon.

Have a look at this software for locating such problems.

http://www.youtube.com/watch?v=ml9IIdiA14M

Iain