Gerbers and drills offset from one another...cant view properly in GC prevue

[treez]

Hi,
Our PCB layout guy sends us the PCB gerbers to check off….sometimes the drill holes are nicely on the PCB image…but sometimes the drill holes are offset from the top copper etc layers (as in attached)…also they are scaled by about two times, as shown.
Can I correct this in GC Prevue?, or does the PCB layout guy need to resend the gerbers without offsetting the drills?....he tells us that its nothing to do with him..he uses cadstar

 

[KlausST]

Hi,

I don't know whether GC prevue can correct all this.

If I remember right, then you use EAGLE.
At the CAM processor you may select wheter you want absolute coordinates or optimized values.
--> use "absolute" for all, gerbers and drill.

Btw:
We do our poduction files all automatically with a script... we don't touch a single buuton/switch/text in the CAM processor.

Klaus

 

[cadexo]

Hi
The gerber and drill file have file formats which contains informations like precision, metric/imperial, gerber type, etc... So the gerber viewer automatically interprets them and views. However if you select manual format type while loading the scaling may be 10x larger or smaller and sometime the viewer can also interpret the format in incorrect scale. To check you can try in other viewer as well like viewmate.

About drill offset, the CAD software may have two different origins one for copper layer and other one for drill layer if both are not same you may see offset. Or it is also possible that while generating nc drill, some offset is entered.

Hope this helps. If you need more details or if you want me to look at it and fix you issue please let me know.

 

[FvM]

The simple problem is that GCPrevue is able to recognize many Gerber and drill data formats automatically, but not all. In this case you need to tell the format explicitly (metric or imperial, how many fractional digits) when importing.

Another possible problem is that Gerber and drill data don't necessarily have the same offset, usually because you didn't set up the post process appropriately.

PCB manufacturers CAD operators are mostly able to align Gerber and drill data correctly. You should be too.

 

[FvM]

The drill data are apparently off by a factor of 2.54, also no correct tool sizes imported.

 

[treez]

Thanks, out by a factor of 2.54 suggests drill is in imperial and gerbers are in metric.
We have no control over this...our external pcb layout guy sends us the gerbers and we are stuck with whatever he sends us........he tells us that this problem is nothing to do with him....he uses cadstar.

I always load his gerbers/drills the same way in GC prevue....sometimes its ok and sometimnes its not.....he is adamant its our fault.

I cannot check off his gerbers properly because of this....how can i know if he has a drill hole encroaching too near a pad when i cant even see the drill hole....i suspect he is happy that we cannot inspect his work fully.

i have tried to resolve this in GC prevue but i cannot

 

[FvM]

Thanks, out by a factor of 2.54 suggests drill is in imperial and gerbers are in metric.

Not necessarily. Both can have the same unit, but one is recognized incorrectly by GCPrevue.

Not sure what you tried, but you can surely fix it in GCPrevue.

- - - Updated - - -

Is the Gerber artwork scaled correctly? If so, you only need to correct the drill import parameters. An additional offset can be applied later.

 

[cyberrat]

What your PCB guy is probably doing is outputting his gerbers using gerber.usr and ncdrill.usr.

Get him to use rs274-x.usr and excellon2.usr, also to modify them using Notepad.

Point him to https://cadstar.blogspot.com/2015/09/my-gerber-files-do-not-line-up-with-my.html as information on which files to use.

Also tell him that he needs to edit them both and set the units in both to MM, also to ensure that both have the same bed size (about 500mm).
Having different bed sizes causes the offset, using MM for the Gerbers and thou for the drill causes the size difference.

If he insists on using thou for it all tell him that he's a dinosaur as we have only had MM for over 30 years.
Now if only someone had told Zuken that they ought to change the default files that they ship Cadstar with then this would not happen.

On the GC-Prevue end - there is a long term bug when you try to auto import, you must always check and set the settings manually, this is on one of the import screens.

 

[marce]

Set the default to bottom left of the design for both gerber and excellon, then it will also line up with the IPC-D-356 data if you use it.
It is not a bug, Excellon2 data only contains the drill table, it does not contain a line giving the data format (RS-274-X does) so the front end system has to guess the data format, leading trailing 3.4, 4.5 etc.