Hey Folks, I can't say I've been doing layout for long, but I did have a couple comments. For the designs we send for fabrication, Gerber review is an absolute necessity. It is very seldom that the first set of Gerbers we generate is correct. You might argue that a "good" designer wouldn't make a mistake at this level, but we routinely push the boundaries of what Protel is capable of and so it becomes paramount to review the design in a WYSIWYG viewer. In fact, to avoid reviewing things twice I basically do the entire final layout review in a Gerber viewer. Unfortunately this results in some small amount of time spent regenerating the files, but I find this review to be far more effective as the layer control is way easier than Protel's. Rather than just verifying each layer one by one, I've developed a system of verifying the interactions between layers etc.
As for the original plane connection problem, I've never used DXP, but if it were me I'd do the following. If subsequent regenerations of the gerber files results in the same effects, I would copy the design to a new directory and then start deleting parts of the layout and regenerating until you can distill it down to the smallest part of the layout that still exhibits the problem. If the problem is not apparent at this point, at least there is less "stuff" to check. Once you've deleted everything, you could consider posting the layout for others to inspect (if you've deleted enough that IP/confidentiality concerns no longer exist). Hopefully in doing so you/we will find whatever protel bug caused the issue so we can avoid it in the future. Darcy Davis Design Engineer, Dynastream Innovations, Inc. -----Original Message----- From: [EMAIL PROTECTED] [mailto:[EMAIL PROTECTED] Behalf Of Abd ulRahman Lomax Sent: March 21, 2005 6:47 AM To: Protel EDA Discussion List Subject: Re: [PEDA] HELP!! Gerber Output Contains Random Subtle ErrorsWith Plane Connects! At 01:02 AM 3/20/2005, Matt Polak wrote: > As you can clearly see, when viewing the power plane connections > in the layout editor, the interconnects show fine. When viewing the > verbatim generated Gerbers, however (RIGHT IN DXP!) there are missing > plane connections! The entire top set of 7 vias are not connected to ANY > planes, whilst the bottom row are connected just fine where appropriate. > I looked at the properties of all of the top-row vias, and they're just > fine - nothing out of the ordinary. Surprisingly most of the other vias > on the board (including the bottom row) connect just fine!! This example is an object lesson in why one should always inspect the Gerbers. Now, it might seem that it would be difficult to detect this particular problem; after all, examining one layer at a time, nothing would be obviously out of place. But there is an old trick. If you look at all layers at once, it is fairly easy to detect pads and vias with no connection. A via with no connection is almost certainly an error. As for pads, I used to generate no-connect lists so I could verify every no-connected pad. This will catch a very large percentage of errors. We don't yet know why this problem occurred, or at least it is not obvious to me. One thing I would do, and perhaps Mr. Polak has already done it, is to regenerate the gerbers. Are they still bad? Could the gerbers seen be from a prior plot run? If the problem is reproducible, I would then send the file to Altium. A reproducible bug should be worth its weight in gold.... That is, in a rational system, there should be a reward for finding such a bug, to the first user to report it and provide clear evidence. This reward should be substantial enough to cover a modest prototype run. Of course, with a large board with many layers, that might be pretty expensive.... > Honestly, this is bringing me to an absolute last straw in > continuing to use Protel if we can't even be guaranteed consistent > WYSIWYG output. Someone PLEASE tell me we did something wrong? I'm > starting to lose patience with Altium's little "features" in the software. Every CAD system of which I am aware has bugs. Yes, they can be enormously frustrating. However, this is one reason why a Gerber viewer is included with Protel. It is Gerber which is truly WYSIWIG, or at least it used to be: flashes and draws are phenomenally simple; if something goes awry, usually what the fabricator will see will be such a complete mess, or will at least be so obviously suspect, that the fabricator will squawk. But a fabricator is not likely to notice disconnected pads; a really awake fabricator might notice that the flash used for vias results in unconnected pads, which is almost certainly an error; the fabricator might even have software to look for this. But I wouldn't blame the fabricator here. Plane layers are calculated layers in Protel. What is displayed is thus inferred, not explicit. I have long argued that positive-negative merges are far more reliable for plane layers than simple negative layers. I developed this process working as a contractor for a company with a $500,000 CAD system (about twenty years ago) which did not check plane layers for opens caused by the formation of moats around pads when blowouts touch. The solution was to generate the negative only as the blowouts. The negative layer has no connections at all, just a plane flood that is clear of all pads and vias. Then the connections are made with track on a positive layer. This is plotted over the negative, easy for the photoplotters. Necessarily, every connection is explicit. If you want spoked thermals, the extra track is added crossing the basic connecting track. And both clearance and connection are DRCd. (The only caveat was that in the simple implementations I used, if there was a split plane, the connecting track could cross the split thus shorting the sections. However, this would be easy to check for: a connecting track should not cross a split line; it should not even contact a split line without generating at least a warning.) An autorouter could easily generate the connecting track, respecting plane splits as keepouts. The irony here is that Protel is quite reliably WYSIWYG, and we are thus lulled into a false sense of security, and so skip a careful review of the Gerbers. This might even seem rational; after all, if it takes an hour for a careful review, and only one out of a hundred designs has a problem (it is likely more reliable than that), Gerber review will cost 100 hours for every error found. That well exceeds the cost of a normal prototype. >Frustrated as hell, >-- Matt If one misses a market opportunity because of the need for another turn, the cost of the problem could easily exceed that 100 hours. Ironically, again, we would be likely to be in a rush in this case, and thus more tempted to skip the cautious review. However, one can review the Gerbers after sending them, so the review need not delay the process more than a little, and only if an error is found. ____________________________________________________________ You are subscribed to the PEDA discussion forum To Post messages: mailto:[email protected] Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/[email protected] Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/[email protected] ____________________________________________________________ You are subscribed to the PEDA discussion forum To Post messages: mailto:[email protected] Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/[email protected] Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/[email protected]
