Gerbv

Anyone using Gerbv as a Gerber viewer?  I'm having a problem where a few drill locations in a drill file look out of location.  I seem to have narrowed the problem to the use of trailing zero suppression.  I can verify the drill file (which contains only line feeds it appears, so not so easy to view) has a few entries with the trailing zero suppressed.  In Gerbv these are all being interpreted as if zero suppression were off.  In fact, it tells me when it translates automatically, it is using no zero suppression.  If I manually turn on trailing zero suppression it so munges the drill file that no drill show up on the screen at all and if I click the zoom to extents button it takes me far off the board and shows me a small area with no visible features.

Is this broken in Gerbv?  I'm going to ask the fab house to turn off zero suppression and see if that fixes the problem at my end.

Rick C.

On 17/08/2018 5:22 am, gnuarm.deletethisbit@gmail.com wrote:
> Anyone using Gerbv as a Gerber viewer?  I'm having a problem where a few drill locations in a drill file look out of location.  I seem to have narrowed the problem to the use of trailing zero suppression.  I can verify the drill file (which contains only line feeds it appears, so not so easy to view) has a few entries with the trailing zero suppressed.  In Gerbv these are all being interpreted as if zero suppression were off.  In fact, it tells me when it translates automatically, it is using no zero suppression.  If I manually turn on trailing zero suppression it so munges the drill file that no drill show up on the screen at all and if I click the zoom to extents button it takes me far off the board and shows me a small area with no visible features.
> 
> Is this broken in Gerbv?  I'm going to ask the fab house to turn off zero suppression and see if that fixes the problem at my end.
> 
> Rick C.
> 

FWIW, I only ever send the drill ident.gbr map and never checked the 
.drl file.

What I see is similar to you: that gerbv seems to be interpreting values 
at 1/10 of what they should be. For example:

In the original .drl file a coordinate such as X07904Y02588 is being 
interpreted as X = 790.4mil Y = 258.8mil instead of 7904mil & 2588mil resp.

If I manually edit the drl file to remove the leading zeros and add a 
trailing one then it comes good.

This is with Gerbv v2.6A. Like I said: FWIW.
-- 
Chris.

On Thursday, August 16, 2018 at 9:52:10 PM UTC-4, Chris wrote:
> On 17/08/2018 5:22 am, gnuarm.deletethisbit@gmail.com wrote:
> > Anyone using Gerbv as a Gerber viewer?  I'm having a problem where a few drill locations in a drill file look out of location.  I seem to have narrowed the problem to the use of trailing zero suppression.  I can verify the drill file (which contains only line feeds it appears, so not so easy to view) has a few entries with the trailing zero suppressed.  In Gerbv these are all being interpreted as if zero suppression were off.  In fact, it tells me when it translates automatically, it is using no zero suppression.  If I manually turn on trailing zero suppression it so munges the drill file that no drill show up on the screen at all and if I click the zoom to extents button it takes me far off the board and shows me a small area with no visible features.
> > 
> > Is this broken in Gerbv?  I'm going to ask the fab house to turn off zero suppression and see if that fixes the problem at my end.
> > 
> > Rick C.
> > 
> 
> FWIW, I only ever send the drill ident.gbr map and never checked the 
> .drl file.
> 
> What I see is similar to you: that gerbv seems to be interpreting values 
> at 1/10 of what they should be. For example:
> 
> In the original .drl file a coordinate such as X07904Y02588 is being 
> interpreted as X = 790.4mil Y = 258.8mil instead of 7904mil & 2588mil resp.
> 
> If I manually edit the drl file to remove the leading zeros and add a 
> trailing one then it comes good.
> 
> This is with Gerbv v2.6A. Like I said: FWIW.

What program is generating your file?  

I'm also using v2.6a.  Gerbv seems to have manual controls but defaults to automatic.  I tried setting trailing zero suppresion and it didn't work.  You seem to be using both trailing and leading zero suppresion which won't work anywhere.  If you lop off a zero at the beginning and one at the end, who could you figure out where the zeros were lopped off?  In your case I would have the generating software not trailing zero suppress (it doesn't save so much in the file anyway).  Or if there is nothing in the 0.1 mil digit, you can tell Gerbv there are only 3 bits past the decimal point.  Don't know if this will work since this feature seems to be less than tested. 

In my case I found I needed a command, INCH,LZ which says work in inches and leading zeros are included which means missing digits are assumed to be trailing zeros. 

Rick C.

On Friday, August 17, 2018 at 6:58:58 AM UTC+2, gnuarm.del...@gmail.com wrote:
 
> I'm also using v2.6a.

I would try the newer version: 2.6.2

Bye Jack

On 17/08/2018 2:58 pm, gnuarm.deletethisbit@gmail.com wrote:
> On Thursday, August 16, 2018 at 9:52:10 PM UTC-4, Chris wrote:
>> On 17/08/2018 5:22 am, gnuarm.deletethisbit@gmail.com wrote:
>>> Anyone using Gerbv as a Gerber viewer?  I'm having a problem where a few drill locations in a drill file look out of location.  I seem to have narrowed the problem to the use of trailing zero suppression.  I can verify the drill file (which contains only line feeds it appears, so not so easy to view) has a few entries with the trailing zero suppressed.  In Gerbv these are all being interpreted as if zero suppression were off.  In fact, it tells me when it translates automatically, it is using no zero suppression.  If I manually turn on trailing zero suppression it so munges the drill file that no drill show up on the screen at all and if I click the zoom to extents button it takes me far off the board and shows me a small area with no visible features.
>>>
>>> Is this broken in Gerbv?  I'm going to ask the fab house to turn off zero suppression and see if that fixes the problem at my end.
>>>
>>> Rick C.
>>>
>>
>> FWIW, I only ever send the drill ident.gbr map and never checked the
>> .drl file.
>>
>> What I see is similar to you: that gerbv seems to be interpreting values
>> at 1/10 of what they should be. For example:
>>
>> In the original .drl file a coordinate such as X07904Y02588 is being
>> interpreted as X = 790.4mil Y = 258.8mil instead of 7904mil & 2588mil resp.
>>
>> If I manually edit the drl file to remove the leading zeros and add a
>> trailing one then it comes good.
>>
>> This is with Gerbv v2.6A. Like I said: FWIW.
> 
> What program is generating your file?

I'm using DesignSpark PCB 8.1.1 to generate the Gerbers.

> I'm also using v2.6a.  Gerbv seems to have manual controls but defaults to automatic.  I tried setting trailing zero suppresion and it didn't work.  You seem to be using both trailing and leading zero suppresion which won't work anywhere.  If you lop off a zero at the beginning and one at the end, who could you figure out where the zeros were lopped off?  In your case I would have the generating software not trailing zero suppress (it doesn't save so much in the file anyway).  Or if there is nothing in the 0.1 mil digit, you can tell Gerbv there are only 3 bits past the decimal point.  Don't know if this will work since this feature seems to be less than tested.
> 
> In my case I found I needed a command, INCH,LZ which says work in inches and leading zeros are included which means missing digits are assumed to be trailing zeros.
> 
> Rick C.

This sort of thing isn't bread and butter stuff for me so that's one 
reason I haven't paid much (any!) attention to the .drl drawing 
particularly. I just used a cheapo PCB fab found at random on the 'net 
and they didn't require/ask for .drl files.

Sorry I can't be of more help.
--
Chris.

gnuarm.deletethisbit@gmail.com wrote:
> Anyone using Gerbv as a Gerber viewer?

Yes.  I use it to laser cut mechanical templates before fab.

>  I'm having a problem where a few drill locations in a drill file look out
> of location.  I seem to have narrowed the problem to the use of trailing
> zero suppression.  I can verify the drill file (which contains only line
> feeds it appears, so not so easy to view) has a few entries with the
> trailing zero suppressed.  In Gerbv these are all being interpreted as if
> zero suppression were off.  In fact, it tells me when it translates
> automatically, it is using no zero suppression.  If I manually turn on
> trailing zero suppression it so munges the drill file that no drill show
> up on the screen at all and if I click the zoom to extents button it takes
> me far off the board and shows me a small area with no visible features.

I've used (I think) the default settings in Kicad and drill files and
gerbers match, so I haven't tried fiddling with settings in gerbv.  The
board houses (including entirely-automated-nobody-speaks-English board
houses in China) have been fine with them.  Also Altium, but I don't
remember whether I changed the settings.

It may be that Kicad is outputting a different format by default to not trip
into this.  Can you change your output settings?
 
Theo

On 17/08/2018 12:34, Theo Markettos wrote:
> gnuarm.deletethisbit@gmail.com wrote:
>> Anyone using Gerbv as a Gerber viewer?
> 
> Yes.  I use it to laser cut mechanical templates before fab.

"Mechanical template" is a space model?

And who do you use for the laser cutting?

Tim

On Friday, August 17, 2018 at 7:34:23 AM UTC-4, Theo Markettos wrote:
> gnuarm.deletethisbit@gmail.com wrote:
> > Anyone using Gerbv as a Gerber viewer?
> 
> Yes.  I use it to laser cut mechanical templates before fab.
> 
> >  I'm having a problem where a few drill locations in a drill file look out
> > of location.  I seem to have narrowed the problem to the use of trailing
> > zero suppression.  I can verify the drill file (which contains only line
> > feeds it appears, so not so easy to view) has a few entries with the
> > trailing zero suppressed.  In Gerbv these are all being interpreted as if
> > zero suppression were off.  In fact, it tells me when it translates
> > automatically, it is using no zero suppression.  If I manually turn on
> > trailing zero suppression it so munges the drill file that no drill show
> > up on the screen at all and if I click the zoom to extents button it takes
> > me far off the board and shows me a small area with no visible features.
> 
> I've used (I think) the default settings in Kicad and drill files and
> gerbers match, so I haven't tried fiddling with settings in gerbv.  The
> board houses (including entirely-automated-nobody-speaks-English board
> houses in China) have been fine with them.  Also Altium, but I don't
> remember whether I changed the settings.
> 
> It may be that Kicad is outputting a different format by default to not trip
> into this.  Can you change your output settings?

I'm not generating the file.   The assembly house has redone the array going from 4 up to 5 up to get better utilization of the full PWB panel size.  In the process they rotated the gerbers which makes it a *LOT* harder to verify the coordinates of any given feature.  Instead of a simple translation by X,Y now you have to swap the coordinate, add to the offset X and subtract from the offset Y.  I can't do that in my head so easily.  Couple that with their use of LF rather than LF/CR and that is why it was rather hard to figure out what was wrong.  

The problem with the current state of PCB design documentation is that it is very similar to SPI ports.  The documentation covers one original implementation and there are many permutations on that which are not very compatible.  Excellon files in particular are a real PITA.  IPC had a good idea, but the industry was too lazy and complacent to make a change that would require work.  They'd rather continue with the confusion because it is only a constant low level of irritation. 

Rick C.

Tim <tim@bugblat.invalid> wrote:
> On 17/08/2018 12:34, Theo Markettos wrote:
> > gnuarm.deletethisbit@gmail.com wrote:
> >> Anyone using Gerbv as a Gerber viewer?
> > 
> > Yes.  I use it to laser cut mechanical templates before fab.
> 
> "Mechanical template" is a space model?

Yes.  A piece of cardboard of the same thickness, shape and with the same
holes as the PCB, to 1:1 scale.

> And who do you use for the laser cutting?

Ourselves.  We have a GCC Laserpro Spirit 40W laser cutter.

The flow is:
Kicad export to gerber
Gerber opened in gerbv
only display the layers to be cut.  The GCC allows one raster layer and
multiple vector layers - my usual flow is raster for images to etch like
tracks, one layer for holes, another layer for edge cuts.  Give each layer a
distinct colour (black=raster, red=holes, green=edge)
Export as EPS, load into Adobe Illustrator CS3 (the laser cutter only plays
nicely with a few programs)
Tidy up the EPS to keep the laser cutter happy (line thickness = 0.01pt,
make sure objects have the right line colours)
'Print' to the laser cutter, setting appropriate powers for the different
colours.  The red (holes) layer is cut before the green (edge) layer.

It works quite well, and is handy for debugging mechanical issues before
going to fab.

Theo

On 17/08/2018 19:15, Theo Markettos wrote:

<snip>

>> And who do you use for the laser cutting?
> 
> Ourselves.  We have a GCC Laserpro Spirit 40W laser cutter.
> 
> The flow is:
> Kicad export to gerber
> Gerber opened in gerbv
> only display the layers to be cut.  The GCC allows one raster layer and
> multiple vector layers - my usual flow is raster for images to etch like
> tracks, one layer for holes, another layer for edge cuts.  Give each layer a
> distinct colour (black=raster, red=holes, green=edge)
> Export as EPS, load into Adobe Illustrator CS3 (the laser cutter only plays
> nicely with a few programs)
> Tidy up the EPS to keep the laser cutter happy (line thickness = 0.01pt,
> make sure objects have the right line colours)
> 'Print' to the laser cutter, setting appropriate powers for the different
> colours.  The red (holes) layer is cut before the green (edge) layer.
> 
> It works quite well, and is handy for debugging mechanical issues before
> going to fab.


Sounds great. And only "from $21,995" :) Until I'm a millionaire I'll 
keep getting semi-routed double sided boards from China...

Tim