Gerber files

I

Ivan Sedneff

Guest
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
 
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" <ivans@scannersinc.com> 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
Click to expand...
 
Ivan Sedneff wrote:
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?
Click to expand...
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








On Mon, 04 Sep 2006 15:22:41 -0400, Ivan Sedneff
<ivans@scannersinc.com> wrote:

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
Click to expand...

--
Posted via a free Usenet account from http://www.teranews.com
 
On Mon, 04 Sep 2006 15:22:41 -0400, Ivan Sedneff
ivans@scannersinc.com> wrote:

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
Click to expand...
On Tue, 05 Sep 2006 14:36:54 -0400, Ivan Sedneff
<ivans@scannersinc.com> wrote:

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
Click to expand...
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
 
qrk <SpamTrap@spam.net> writes:
It's a shame that PCB editors allow zero length traces.
Click to expand...
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

On Tue, 05 Sep 2006 19:06:45 GMT, qrk <SpamTrap@spam.net> wrote:

On Mon, 04 Sep 2006 15:22:41 -0400, Ivan Sedneff
ivans@scannersinc.com> wrote:

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

On Tue, 05 Sep 2006 14:36:54 -0400, Ivan Sedneff
ivans@scannersinc.com> wrote:

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

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
Click to expand...

--
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








On Tue, 05 Sep 2006 15:43:45 -0400, Ivan Sedneff
<ivans@scannersinc.com> wrote:

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

On Tue, 05 Sep 2006 19:06:45 GMT, qrk <SpamTrap@spam.net> wrote:

On Mon, 04 Sep 2006 15:22:41 -0400, Ivan Sedneff
ivans@scannersinc.com> wrote:

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

On Tue, 05 Sep 2006 14:36:54 -0400, Ivan Sedneff
ivans@scannersinc.com> wrote:

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

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
Click to expand...

--
Posted via a free Usenet account from http://www.teranews.com
 
On Tue, 05 Sep 2006 15:43:45 -0400, Ivan Sedneff
ivans@scannersinc.com> wrote:

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

On Tue, 05 Sep 2006 19:06:45 GMT, qrk <SpamTrap@spam.net> wrote:

On Mon, 04 Sep 2006 15:22:41 -0400, Ivan Sedneff
ivans@scannersinc.com> wrote:

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

On Tue, 05 Sep 2006 14:36:54 -0400, Ivan Sedneff
ivans@scannersinc.com> wrote:

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

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
Click to expand...
On Tue, 05 Sep 2006 19:29:44 -0400, Ivan Sedneff
<ivans@scannersinc.com> wrote:

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
Click to expand...
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
 
"Ivan Sedneff" wrote:

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.
snip
Click to expand...

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_harland@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" <SpamTrap@spam.net> 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
Click to expand...
 
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" <ivans@scannersinc.com> 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
Click to expand...
 
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






On Wed, 06 Sep 2006 03:55:49 GMT, "Brad Velander"
<bveland@SpamThis.com> wrote:

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.
Click to expand...

--
Posted via a free Usenet account from http://www.teranews.com
 
On 9/6/2006 8:31 PM Ivan Sedneff wrote:

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!)
Click to expand...
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.

--
Sincerely,
Brad Velander.

"Mike Elliott" <j.michael.elliott@gmail.com> wrote in message
news:j-GdndvTuf9J4p3YnZ2dnUVZ_vSdnZ2d@adelphia.com...
On 9/6/2006 8:31 PM Ivan Sedneff wrote:

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!)

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

The gauntlet has been thrown.

-- mike elliott
Click to expand...
 
On 9/7/2006 10:45 PM Brad Velander wrote:

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.
Click to expand...
Good times, man.

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.
Click to expand...
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" <j.michael.elliott@gmail.com> wrote in message
news:KsOdnbq2y8nAXJzYnZ2dnUVZ_s2dnZ2d@adelphia.com...
On 9/7/2006 10:45 PM Brad Velander wrote:

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.

Good times, man.

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.


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
Click to expand...
 
On 9/9/2006 1:34 AM Brad Velander wrote:


I was interested in reading the recent comments from Altium regarding
crashes (video related, NVIDIA desktop in particular) on the forum.
Click to expand...
<snip>

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
 
You must log in or register to reply here.

Welcome to EDABoard.com

Sponsor

Back
Top