Gerber files

Ivan, There should be no reason that GC-Prevue or Viewmate won't display your Gerber files, I have used both programs intermittently to view Gerbers generated from Protel.

Now maybe just because of variations in your wording (Altium/Protel) but I can't be sure which version of Protel/Altium software you are using. Is it P98, P99SE, DXP, AD or some other version? Which Protel program reads them in fine, Camtastic or directly into Altium Designer (AD, which is also Camtastic but just integrated into the package?

Now the only variable that I can see which may interfere with either program reading in your Gerbers, is what is your Gerber format? RS274? RS274-X (embedded apertures)? Data format, 2.3, 2.4, 2.5 or some other (image too large or image too small and you just don't see it)? Leading zeroes removed/included or trailing zeroes removed/included?

The most likely suspect is that you are outputting RS274 data (no embedded apertures) and you haven't read in an aperture file. Although this will usually still display very thin zero width lines of your circuit.

Or am I maybe getting way ahead of the problem, you just don't see the correct file extensions appear in either GC-Prevue or Viewmate? Don't worry about the preset extensions, set the file open type to *.* and load your Gerbers.

--
Sincerely,
Brad Velander.

"Ivan Sedneff"  wrote in message 
news:d5vof2plma4lnr8igat306mvv4afdl4bm3@4ax.com...
> Hello
>
> I have just outputted a complete series of Gerber files using Altium
> Protel.
> They show up fine in the Protel program, however GC Preview and
> Viewmate will not display the files.
> The extensions are: GBL, GBO, GBP, GBS, etc.
> Shouldn\'t these generic viewers be able to view these files?
>
> Ivan
>
> -- 
> Posted via a free Usenet account from http://www.teranews.com
>

GC-Prevue expects .gbr extensions. Perhaps you can persuade Protel to use them, or just rename the files.

Leon

Thank you Brad and Leon,

I am using Altium 2004 DXP with Service pack 2, which has Camtastic and a host of other modules integrated.

Everything looks good-to-go but as a precaution I wanted to preview the Gerber files with a stand alone viewer.

ViewMate gives me an error 28: "Cannot determine file type C:\\path.....GTS", etc.

Now here's where it gets weird..... In some instances when I try to regenerate the files, ViewMate will view them.

First I will get a warning message Zero length of draw detected at (1.51 1.2). Convert to pad?

I have not yet been able to identify the anomaly, but almost always all the file extensions given by Protel can't be viewed.

I am using embedded apertures (RS274X).

Hope this may help narrow down my problem,

Thank you again,, Ivan

--
Posted via a free Usenet account from http://www.teranews.com

Take a look at the Gerber files with an ASCII text viewer. See if they look like Gerber files and the files actually contain the embedded apertures. If they do, perhaps your viewing program requires a certain type of extension. You can experiment with one file and change the extension to something your viewer expects.

Your zero length draw is usually a some junk left behind when you fiddled with a trace. That can create little pieces of junk. Go to that area in your PCB editor and delete the traces in that area (do a windowed delete if you have that capability) and redo the routes. It's a shame that PCB editors allow zero length traces.

--
Mark

We use them to make round copper spots on the board. Great for as-hoc test pads.

Hello Mark,

As you instructed, I concentrated on two files, both of the same .GBL and looked at them with EditPlus. Surely enough, the one that could be viewed was in ASCII and the other un viewable, in blocks and squares (binary).

I have to clear out all my Camtastic documents (Gerber files) and the Camtastic.CAM files and start fresh.

I assume a boardhouse will be looking for GBL, GTO files and the Camtastic.CAM file will not be of any use to them, correct?

Thank you,

Ivan

--
Posted via a free Usenet account from http://www.teranews.com

Mark,

I seem to have finally generated useful Gerber ASCII files for the board. Will a board house be able to interpret the files that contain the zero length errors that ViewMate found and be able to generate the correct photoplots? I locked into the various coordinates, but no matter how much I zoom in, I cant see anything and I don't know how to tell Protel to delete these zero length spots...

Thanks,

Ivan

--
Posted via a free Usenet account from http://www.teranews.com

I'm sure the board house will be ok with the zero length trace. They will get back to you if they have a problem.

--
Mark

Just out of curiosity, why are you running Altium Designer 2004 with SP2? SP4 has been available for that version (Altium Designer 2004) for some time now.

The associated download is on the heavy side (hundreds of megabytes), which could be problematic for anyone who uses dialup connections and/or is billed heavily for large downloads. But assuming you're a registered user of AD

2004 and ask the people at Altium nicely, then maybe they would be prepared to mail you a CD-ROM containing SP4.

Regards, Geoff Harland. g snipped-for-privacy@optum12net.cos.au (Transpose m & s in address provided - then also remove cuberoot of 10^3 + 9^3 - 1^3.)

Ivan, "qrk" is probably bang on the money regarding the one specific error you mentioned. The error has shown up in my files previously and it was either a zero length line or a zero radius arc at the locations mentioned. Routing or drawing lines with arcs in Protel was always infamous for creating either zero length lines or zero radius arcs at every interface between an arc and a straight length of trace ( I assume it may still be prevalent in AD versions). In this case it would be at coordinates 1.51 X and 1.2 Y. Not precisely sure where that may be in your actual PCB database because when generating Gerber you can set the Gerber for Absolute coordinates or the PCB database's coordinates. But in the Gerber viewer you would find it at the mentioned coordinates if it wasn't deleted or skipped completely during importing. But those coordinates would give you the visual location in the Gerber program to check back in your PCB database and find the origina offending detail.

Hmmmm, with regards to your overall problem maybe this is something that is only found in newer versions of Viewmate or GC-Prevue. I haven't used them in the past year or two, used to use particularly GC-Prevue religiously and Viewmate quite often for years. Otherwise the only thing that I can suggest is addressing specific error messages and trying to bypass the preset file extensions when loading the files. Using the preset extensions rather than *.* just leads me to believe that possibly with the preset extensions the import format could also look for particular details of the Gerber format that it might not find in all various CAD gerber outputs (certain header strings, declaration statements, specific ways of coding specific Gerber details, etc.).

Most Gerber import error reports either give you the X,Ycoordinates of the problematic Gerber element or the line number where it was found in the imported file. So all errors should be able to be found and addressed with minimal detective work.

--
Sincerely,
Brad Velander.

"qrk"  wrote in message 
news:4vhrf25j551lq40uvvgkl581u0tjraiepi@4ax.com...

>
> Take a look at the Gerber files with an ASCII text viewer. See if they
> look like Gerber files and the files actually contain the embedded
> apertures. If they do, perhaps your viewing program requires a certain
> type of extension. You can experiment with one file and change the
> extension to something your viewer expects.
>
> Your zero length draw is usually a some junk left behind when you
> fiddled with a trace. That can create little pieces of junk. Go to
> that area in your PCB editor and delete the traces in that area (do a
> windowed delete if you have that capability) and redo the routes. It\'s
> a shame that PCB editors allow zero length traces.
>
> ---
> Mark

Ivan, You are right about the CAM file, not much use to most fabricators.

I am beginning to wonder about your Gerber generation setup. I don't currently use DXP/AD but I know it is quite different than with the older P99SE. Check carefully to make sure that your Gerber generation is actually generating (and storing no a drive somewhere) the actual Gerber files generated before Camtatstic opens and tries taking over. Then again, if it opens proerly in Camtastic (even automagically within AD) then you can still within Camtastic export all the original Gerber layers again from Camtastic. Check the File, Export, Gerber options, sorry don't know the precise menus/key-strokes in AD or the newer Camtastic.

--
Sincerely,
Brad Velander.

"Ivan Sedneff"  wrote in message 
news:p9krf2hhjtri27v7s8ogvnpol38u353mga@4ax.com...
> Hello Mark,
>
> As you instructed, I concentrated on two files, both of the same .GBL
> and looked at them with EditPlus. Surely enough, the one that could be
> viewed was in ASCII and the other un viewable, in blocks and squares
> (binary).
>
> I have to clear out all my Camtastic documents (Gerber files) and the
> Camtastic.CAM files and start fresh.
>
> I assume a boardhouse will be looking for GBL, GTO files and the
> Camtastic.CAM file will not be of any use to them, correct?
>
> Thank you,
>
> Ivan

Thanks to one and all,

I have gotten rusty, since I last used Protel over a year ago. Previous to that I worked exclusively with PADS PCB in the days of DOS, way back in the twentieth century :)..... (boy does that date me!)

With all your help, I was able to overcome the obstacles and have a fine set of Gerber files.

Thanks again for everyone's dedicated and prompt help.

Sincerely,

Ivan

--
Posted via a free Usenet account from http://www.teranews.com

Uh huh. I go back to hand taping boards 2:1 with crepe tape on frosted mylar.

The gauntlet has been thrown.

-- mike elliott

Hi Mike, So your roots have some sticky fingers as well. Damn, I can still vividly remember the tape and donut hell that once was the norm. Seems your getting used to the AD recently. The posting volume has been dropping on the AD list and the typical post is not such a desparate plea for assistance any longer. 8^> Good on yah.

-- S>

Good times, man.

Yep, AD is making more sense. I've sorted out how to perform the routine things that I need to so, while I am certain that there are better ways to do them lurking under the hood.

That said, it is troubling that the very problem with the old Protel Client (routine Windows exceptions in module ADVPCB.EXE) that forced me to spend the Big Bucks to upgrade to Designer 6 /still/ has not been fixed: 6.3 crashed pretty frequently, too, with the same error.

Yet, there has been some improvement: while Client cheerfully corrupted open files when it crashed, Designer does not seem to. Even better, 6.5 seems to be much stabler: I've not had a crash yet(searches for a piece of wood to tap), even on the moon!

-- mike elliott

Sounds good Mike, So things are getting better for some. This has always been a problem for Altium (other companies as well I am sure). You see a group of users having problems fairly consistently, the other group doesn't see the same issues. Then a new release comes along, some of the problem group get more stable and some of the stable group start to experience instabilities. It has been the way with Altium/Protel for the past 7 years that i have observed. I was interested in reading the recent comments from Altium regarding crashes (video related, NVIDIA desktop in particular) on the forum. The one support/programmer was pursuing questions to determine if some of those experiencing the problems were running any desktop programs like Yahoo task/search bars, etc.. With the problems experienced with Nvidia desktop manager, I can see that other similar programs may be similarily causing problems. Hopefully something is found from those enquiries. Similar to the way it was with AV software, those programs could be causing problems not previously realized and understood.

-- Sincerely, Brad Velander.

"Mike Elliott" wrote in message news:KsOdnbq2y8nAXJzYnZ2dnUVZ snipped-for-privacy@adelphia.com...

In discussion with a senior support tech, he opined that AD's instability is totally environmental, as some users experience no instability whatsoever, while others pull their hair out dealing with them constantly. I don't doubt that something subtle is going on. I have my share of crashes and am running Designer on a stock Fujitsu notebook with its built-in video card, no nVidia fancy-pants graphics stuff here.

Given that I experienced the same kind of exception error in the same module in 6.3 that I experienced with 3.x, my wild-ass guess is that some bit of code in that module has not been modified since The Olde Days and it is within that code that the instability lies.

-- mike elliott