| Author |
 Topic  |
|
Iain Wilkie
United Kingdom
1015 Posts |
 Posted - 30 Dec 2013 : 13:55:42
|
Ed ... no the drc would not have picked it up .... cause it would not have been there in the design .... it was only there in the gerber. This is the point of this software, its comparing the netlist of the layout tool with a generated netlist from the gerber output. This would have caught the gerber output errors in Johns posts.
After a bit of reading it does appear that gerber outputs may not be as reliable as we would like them to be.
Iain |
 |
|
|
edrees
United Kingdom
779 Posts |
Posted - 30 Dec 2013 : 14:39:05
|
Yes I realised this Iain,- after posting! Duuuuuh!
This is really bad news if Gerber generation is prone to errors. Even if we used a third party Gerber checker, -there may be "bugs" in that software too that appear under "exceptional" circumstances! So we still cannot put hand to heart.
We need a way of being 100% confident in the Gerbers, and in my mind that is the responsibility of the original software source, in this case No.1.
Maybe the "Gerber" format is now too long in the tooth or too frail for modern designs ? |
|
|
|
Iain Wilkie
United Kingdom
1015 Posts |
Posted - 30 Dec 2013 : 14:45:24
|
Ed,
If you google some of this you will find that gerber importers can struggle with variations in gerber data. Does seem to be a common issue, not just with EPC.
I think your right gerber is a bit long in the tooth and has been altered so many times in the past it may be a bit of a mess, and this is really the problem. There is nothing in GenCad that pertains to netlist so I think that's no good, as is ODB++ output
Iain
|
|
|
|
Iain Wilkie
United Kingdom
1015 Posts |
Posted - 30 Dec 2013 : 21:36:15
|
Taking this further, I note we can output ODB++ from EPC.
Reading here http://forums.numericalinnovations.com/post/i-want-to-see-if-the-netlist-embedded-in-odb-checks-against-the-odb-artwork-5975257
You will see FAB 3000 can extract and construct an IPC -D 356 netlist. I think this can be used as a comparison netlist against the gerber output netlist that FAB 3000 can also generate and the comparison of the two netlists to show any errors. If this works then there would be no need to wait for Numberone to hopefuly include an IPC-D-356 netlist output.
I will give this a try and if it seems to work, it would be handy if JohnB could try it out on his problem designs to see if this would trap his errors.
Iain |
|
|
|
John Baraclough
United Kingdom
129 Posts |
Posted - 30 Dec 2013 : 21:53:45
|
Unfortunately I don't have FAB 3000. I just downloaded the free version (DFM) but I have to request a board quote from one of the signed-up companies (all US based AFAIK) to get the unlock code to do any more than just use it as a Gerber viewer.
I'm happy to send you the Gerber files and an ODB++ netlist from Easy PC if you want to try it yourself.
-------------------------------------------------------
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
United Kingdom
1015 Posts |
Posted - 30 Dec 2013 : 22:15:50
|
John,
You can download a 15 day full trial version. You need to register and they will send an unlock code. I have already done this. I will give this a test run tomorrow. I will let you know how that goes and if it looks promising and you want to send me one of your faulty files, I can try that and see what the outcome is.
Iain
You can download the trial version 7 here
http://www.numericalinnovations.com/pages/download-page |
Edited by - Iain Wilkie on 30 Dec 2013 22:21:26 |
|
|
|
John Baraclough
United Kingdom
129 Posts |
Posted - 02 Jan 2014 : 11:38:11
|
After extended Hogmanay celebrations, I now have DFM Free! up and running and there are some interesting results already. It doesn't seem to like the first Gerber block in the Drill Ident Drawing output from Easy PC. Ticking the "End Gerber Block at Newline" checkbox when loading the file seems to get rid of the errors but leaves a warning about an invalid block at byte 5 being ignored. As it's only in the Drill Ident Drawing, I'm not too concerned as my Chinese board manufacturer doesn't use that file.
DFM Free! looks very promising so I'll have to send off a request for a board quote to some of these US companies so I can get the unlock code for the more advanced features.
-------------------------------------------------------
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
United Kingdom
1015 Posts |
Posted - 02 Jan 2014 : 12:25:15
|
John,
See my previous post ..... Don't even bother with DFM free, you can download a 15 trial version of FAB 3000 on the link in my post.
Iain |
|
|
|
edrees
United Kingdom
779 Posts |
Posted - 02 Jan 2014 : 12:58:21
|
But what happens after 15 days free trail period of FAB 3000?
How much does FAB 3000 cost to double-check EPC output? I bet it's not cheap!
Will No1 "repair" the gerber generating code in 15 days time?
If they can't, can they give us a IPC -D 356 netlist utility?
We've not yet even had any input or re-assurance from No1 about this very concerning issue.
Happy New Year to all!
|
|
|
|
Iain Wilkie
United Kingdom
1015 Posts |
Posted - 02 Jan 2014 : 13:22:17
|
Ed, not sure about cost but I think it is a few hundred dollars. But the point is that it appears that even if no1 fix this particular problem that another error may come along. it seems gerber output is a bit hit and miss and hence these third party checkers emerging.
To have a dedicated third party checker seem to big step towards ensuring your files are good.
The 15 day trial allows us to see if say the netlist within the odb++ is compatible and if not could it be made to be or as you mention could we have a dedicated IPC-D-356 netlist format output.
I am looking at FAB3000 and it looks very impressive, however I still cannot generate a netlist from the odb cleanly and am in the process of getting the vendors to look at this, but holidays are still in the way.
Iain |
|
|
|
John Baraclough
United Kingdom
129 Posts |
Posted - 02 Jan 2014 : 14:48:33
|
Happy New Year to you all.
I find it disturbing that Numerical Innovations refuse to give the cost of FAB 3000 on their website, insisting that you ask for a quotation by email. As a retired design engineer who just does this for pocket money, I doubt I can afford the annual cost of the full package. I'm reluctant to download the evaluation version of FAB 3000 in case it stops DFM Free! from working.
A bit more positive information from Numerical Innovations would be welcome.
-------------------------------------------------------
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
United Kingdom
1015 Posts |
Posted - 02 Jan 2014 : 15:09:27
|
DFM doesn't do a netlist compare I don't think.
The fact they don't show prices simply means they have a flexible pricing policy, not sure if thats good or bad I am not sure.
I cannot see how installing fab3000 would stop dfm working, they are completely different programs.
I can understand the worry about the cost of a checker, but for me who is doing dense 12 layer cards with bga's, I need to be absolutey sure that my gerbers are ok, even a prototype spin of a couple of boards can cost a thousand pounds. Ok you could discover a gerber fault on protoypes but when you respin you could create another....just not worth it.
iain |
Edited by - Iain Wilkie on 02 Jan 2014 15:10:34 |
|
|
|
John Baraclough
United Kingdom
129 Posts |
Posted - 02 Jan 2014 : 21:06:59
|
Hi Iain,
I'm sure DFM Free! doesn't do a netlist compare otherwise there's not much worth paying for in FAB 3000! I might just download the evaluation copy and see what I can get out of NI in the way of a reasonable price.
-------------------------------------------------------
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 02 Jan 2014 21:07:31 |
|
|
|
edrees
United Kingdom
779 Posts |
Posted - 03 Jan 2014 : 13:26:32
|
Hi John,
I've had another look at your images,-
http://mydesk.myzen.co.uk/_Useful/EasyPc/BeltpackPcbError.jpg
http://mydesk.myzen.co.uk/_Useful/EasyPc/EasyPcGerberFaultB1.jpg
http://mydesk.myzen.co.uk/_Useful/EasyPc/EasyPcGerberFaultB2.jpg
I note that the offending track/pad (and others) has a "teardrop" feature. I wonder if this is aggravates the problem with the flood mis-pour as the Gerber viewer image clearly mis-interprets this particular teardrop?
Is it worth removing the teardrops in the design and re-checking the Gerber plot on 2.3 setting please? If you haven't the time, please email me the layer and I'll check it out and report back.
I'm not convinced that Gerber plot errors are quite as common as Iain reports, however, through some Google research I found a "n.4" or "n.5" plot setting recommendation in two Gerber Viewer/checkers totally unrelated to EasyPC,-"otherwise small plot errors may occur"!
|
|
|
|
Iain Wilkie
United Kingdom
1015 Posts |
Posted - 03 Jan 2014 : 15:45:24
|
Ed,
The gerber problems I am refering to which may be common are not all fatal. In fact I just tried running Fab3000 on one of my designs and it picked up a few "errors" that really should not be there but do not really cause any problems. For example some small copper pour areas that were unconnected whereas the copper pour had been set to remove unconnected islands. This seemed to be aggravated by the setting of the minimum pour area being set very small.
What I am trying to say is due the complexities of the gerber export it would not be uncommon to errors but only once in while it may be that one patricular error could cause a fatal error.
Having said all that, I can catagorically state that for the hundreds of boards I have done, I have never had a fatal gerber error. The only thing close to that was actually a manufacturers plotter import error on one of my gerbers that caused a fatal error. Of course I was in the clear on that one as the gerbers were proven to be ok.
Iain |
|
|
|
Benno
Netherlands
79 Posts |
Posted - 03 Jan 2014 : 21:21:02
|
fab3000 is more then just a gerber checker. You can generate documentation with it, modify gerbers, create placement files, create panels and a lot more.
I got a quote from them in december for a named single user license. With their discount it was about $650,-. Lifelong support and update is an additional $1000,-
I think if you create and prep a lot of boards for mfg it is worth the money. It eases up making doc and prepare mfg files. Also it seems more open then epc so you can connect your own database for parts etc. fab3000 has an api for plugins.
For now I stick with dfm-now since it seems to do a lot more for me then gcprevue can. But if the number of boards I need to make stays increasing I'll definately buy fab3000. |
|
|
|
Iain Wilkie
United Kingdom
1015 Posts |
Posted - 03 Jan 2014 : 21:59:53
|
The netlist comparison is one of the key features of FAB 3000 but until we can get a handle on whether we can get a dedicated IPC-D-356 netlist output or import the ODB++ output from EPC that can be converted to IPC-D-356 [it can do this], then its still in the lap of the gods. But yes there are many other exciting features in FAB 3000 and $650 would not put me off purchasing.
Iain |
|
|
|
Iain Wilkie
United Kingdom
1015 Posts |
Posted - 20 Jan 2014 : 14:30:28
|
John Baraclough I have tried to email you..... if you don't receive
the email can you contact me at ....
iain@wilkie-electronics.co.uk |
|
|
|
edrees
United Kingdom
779 Posts |
Posted - 20 Jan 2014 : 14:48:49
|
I think that we should have heard No1's considered response to this rather concerning issue by now!
IF Gerber generation is a bit "flakey" then surely we deserve a method of independently checking (e.g. Fab3000) and a IPC-D-356 netlist output capability from EPC.
Come on No1, or are "holidays are still in the way"? |
|
|
|
Iain Wilkie
United Kingdom
1015 Posts |
Posted - 20 Jan 2014 : 17:27:36
|
Hi Ed,
I am still evaluating the FAB3000 route. The gerber output being "flakey" is not really a problem confined to Numberone, it seems that there is always an inherent possibility that something could go wrong. I have to say I have never had a gerber problem EVER with EasyPC gerber output, but after reading about gerber output potential problems, I do not want to take the risk on some of my complex boards. It seems the format is quite old and tampered with that sometimes something might not quite be right. This is the whole point of the compare facility in FAB3000.
, hence the FAB3000 evaluation.
Iain
|
|
|
|
edrees
United Kingdom
779 Posts |
Posted - 21 Jan 2014 : 09:50:05
|
Hi Iain.
I believe that the quality of the Gerber output is a function of the algorithms employed by the Developers for that particular software in question. No1 Developers or Tech Support should be in a position to give their considered opinion whether there is a potential problem or not.
Cheap (or free) pcb layout software programmes may have less complex algorithms that may not produce error free Gerbers at all times. We both may have read on the internet about Gerber errors introduced by this latter category of CAD layout programs. I have been unable to identify which CAD packages caused these Gerber errors which FAB3000 might wish to exploit. I do accept however that FAB3000 may offer additional features that some designers may find useful,- but that's another issue.
I'm of the opinion that (given a resolution of 5 decimal places) EPC is capable of producing error-free Gerbers, -after all we have designed hundreds of boards between us without one single Gerber error!
-Just would like to hear No1's considered opinion in this matter and whether IPC-D-356 netlist output capability is potentially on offer or not. |
|
|
|
Iain Wilkie
United Kingdom
1015 Posts |
Posted - 21 Jan 2014 : 10:45:14
|
Hi Ed,
I agree with everything you say. As far as FAB3000 is concerned we do not need an explicit IPC-D-356 output .... but it would be nice. This is because EasyPC has an ODB++ output and FAB3000 can reproduce an IPC-D-356 netlist format from the netlist in the ODB++ files. This is what I am messing with at the moment. Please note I am turned on by FAB3000 not simply by the fact that with netlist compare we can eliminate gerber errors, but it is a complete gerber tool in it own right offering a range of utilities that I can see myself using.
I am working along side Numerical Innovations on this one to ensure the netlist compare is going to work for us. They have been extremely pro-active and we did identify a fault in the ODB++ output in EasyPC which Numberone have now addressed. Yup I had complete faith in EasyPC's gerber output, but its just these odd problems that have arisen that have made me feel I need a gerber confirmation tool.
Iain |
|
|
|
edrees
United Kingdom
779 Posts |
Posted - 21 Jan 2014 : 12:30:51
|
Hi Iain,
I'm sure that I speak for a number of us Users when I say I appreciate the investigative work you have undertaken regarding this issue.
No chance of you negotiating a discount from Numerical Innovations for EPC users?
In the meantime, I'll wait eagerly for No1's comments...........
|
|
|
|
Iain Wilkie
United Kingdom
1015 Posts |
Posted - 21 Jan 2014 : 14:29:40
|
I have noe even asked NI to quote, of course it did cross my mind that if others don't want to buy, I could offer a checking service ????
Iain
|
|
|
|
Iain Wilkie
United Kingdom
1015 Posts |
Posted - 19 Feb 2014 : 20:14:28
|
I have completed my evaluation of FAB3000 and found it to be an excellent tool to verify gerber outputs and would recommend it to anyone who would take comfort that their gerber outputs are flawless. I have decided to purchase this as we are now doing boards up to 12 layers and cannot afford to take any chances with gerber faults. I am considering offering a checking service to anyone who do not want to invest but would still like to have this form of check. I still have to come to a cost for this service but it will be very affordable. We ran John Barracloughs gerber through FAB3000 and the fault was detected. If anyone thinks this type of service would be of interest, please comment.
Iain |
|
|
|
Benno
Netherlands
79 Posts |
Posted - 20 Feb 2014 : 18:56:21
|
| did you use odb++ for that check of John's files? |
|
|
|
Iain Wilkie
United Kingdom
1015 Posts |
Posted - 20 Feb 2014 : 20:37:48
|
Benno,
Yes .... What needs to be done is you generate your gerbers as normal and then an ODB++ file. In FAB3000 you can extract the netlist from the ODB++ file and convert it to an IPC-D-356A and save it as such. Then you import the gerbers into FAB3000 and extract a netlist from the gerbers alone. You now re-import the IPC-D-356D into FAB3000 and compare it to the gerber netlist. If both are the same .... great ..... otherwise FAB3000 reports the errors as either open on shorts and an indication of the affected net.
Sounds complicated but easy after a few times.
Iain |
|
|
|
jlawton
United Kingdom
108 Posts |
Posted - 21 Feb 2014 : 12:03:34
|
Okay, here's my pennyworth on this issue.
I have just seen a problem with my latest design using EPC 17.0.3 and Gerber settings of 2:3 Here are some images:
https://drive.google.com/folderview?id=0B4LwHmrN5_GHQjlsM2JnWnQ4Zkk&usp=sharing
You can see that with Gerber accuracy set to 2.3 the large pads on the left hand side are badly obscured and pads on the right hand side are slightly obscured.
At settings of 2:5 there is no problem.
These screensgrab images are from Gerbv 2.6.0 (in Linux) set to Normal or High Quality mode. Other viewing modes don't display these errors, neither does GCPreview (in Windows) 22.1.8
Curiouser and curiouser!
John Lawton Electronics |
Edited by - jlawton on 21 Feb 2014 13:15:20 |
|
|
|
edrees
United Kingdom
779 Posts |
Posted - 21 Feb 2014 : 12:37:58
|
Thanks John for sharing that with us. At least there is some hope by using 2.5. Is there a problem using 2.5 in inches though?
I'm appalled that we still haven't had a public statement from No1 regarding this serious issue. It's been going on for far too long now and complete silence from No1. You owe it to your Customers!
Neither do I think that FAB3000 is the way ahead.
Iain,-
quote:
We also double check gerbers using Numerical Innovations FAB3000 so you can be rest assured your gerbers will be error free.
I don't suppose that you offer a cast iron guarantee and full comprehensive liability for any erroneous Gerber file plot that you've checked and the subsequent cost of manufacturing?
You're too wise for that! I haven't "rest assured" for many years now, far too many important issues seem to have been taken out of our control!
|
|
|
|
jlawton
United Kingdom
108 Posts |
Posted - 21 Feb 2014 : 13:21:59
|
Hi Mike,
I amended my posting because actually when I changed from accuracy 2:3 (imperial) to 2:5 I had also ticked the mm units box and accuracy was changed automatically to 3:5.
The change in units might be confusing so I have just replotted at 2:5 imperial, and the obscuration problem disappears as before.
Plotting using metric at 3:5 would be even more accurate than imperial 2:5 but the Gerber file size is also larger.
John Lawton Electronics |
|
|
|
Topic |
|
Gerber Errors