Altium Gerber Export

[x18]

hi,

did anyone ordered pcbs here? http://iteadstudio.com/store/index.php?main_page=product_info&cPath=19_20&products_id=174
i want to order some and i am not sure what to export...

i choose the standard RS-274x format for the gerber export and exportet all the needed layers. do i have to change anything in the preferences of the export?
how do i export the drillfile?

some explanation with screenshots would be nice. perhaps anyone who ordered at iteadstudio can screenshot his preferences in the gerber export dialogs!?

thanks.

[joelby]

I follow this helpful guide: http://www.olimex.com/pcb/How%20to%20export%20Gerber%20files%20from%20Altium%20Designer%202009.pdf

I've never had any trouble sending the resulting files to ITead or PCBCart.

[x18]

hi thanks for the reply.

i followed the instructions in the pdf file. there were some things that i didn't do at the first try.

itead studio replied to my first try that there are no D-Codes. why shouldnt those codes not be exported to my gerber files? are D-codes exported if i follow the insctructions of your pdf?

greetings.

[mikeselectricstuff]

I suggest getting a gerber viewer like GC-Prevue - if the files load in that, a PCB manufacturer will be able to use it.

I think Altium comes with camtastic - you could use that to check the gerbers

[x18]

in altium everything is loading. also those files which the manufacture critized. but i used another viewer which couldn't open the old files but he could open the new ones.

[x18]

another problem apeared:

why are there areas in my gerber files which arent filled like in the altium pcb editor viewer?

[joelby]

I can't see your file, possibly due to the server move, but in the past I've noticed that BatchPCB's online gerber preview didn't show up polygon fills but apparently this is a known issue with Altium and I've never had trouble with manufacturers actually filling in fills. The problem could extend to other viewers. If you're worried, you could ask your PCB manufacturer to confirm that fills are present.

[x18]

perhaps you can see this image:
http://img87.imageshack.us/img87/3853/indexwg.jpg

the problem is the same in every gerber viewer i watches the output files vom altium designer with. so i suppose those fields aren't filled. they are only filles in the pcb editor.

[jahonen]

Most likely a bug with gerber generation in Altium Designer. I have stumbled upon similar bug with PADS in the past, some 2007.x-version, gerber generation failed to generate proper outline for fill polygon. I caught it with CAM350, I always check gerbers and do a netlist comparison against IPC-D356A netlist. For this reason, I often generate gerbers with drawn fills, even if it produces hugely larger files but no errors with fills.

Can you post the actual gerber file in question, I can check it with CAM350 (often used by PCB manufacturers)?

Regards,
Janne

[x18]

I deleted the dead copper regions in Altium so there are only a few not filles polygons left.

[jahonen]

Indeed, the problem shows up also in CAM350 (version 10.5). It looks strange, outermost fill is properly done but inner missing areas have no proper polygon border.

I did some attempts to fill them using CAM350 but did not easily manage that (not a very good idea to use CAM software to edit the data anyway!).

Regards,
Janne

[jahonen]

After some fiddling, managed to fill the voids.

Regards,
Janne

[joelby]

Ugh, I've confirmed that this is still a bug in the very latest AD10. Fills aren't filled when they are completely enclosed by other tracks.

It turns out that the Olimex document has an unnecessary step, and there's a bug in Camtastic when you export the gerbers in step 8 (File, Export, Gerber). The gerbers are actually generated and saved after you do (File, Fabrication Outputs, Gerber Files) - look in the Projects pane under Generated/CAMtastic! Documents.

So just generate the Gerber Files and NC Drill Files, find the newly created files (right click and Explore). If you look at these files in Camtastic, they won't have the same problem.

Answers were found at http://forum.live.altium.com/#posts/188130 , where the OP also used this Olimex document! I'm very sorry about the bum steer

[vl400]

So just generate the Gerber Files and NC Drill Files, find the newly created files (right click and Explore). If you look at these files in Camtastic, they won't have the same problem.

Another unhappy gerber export user All good up to this point, where do you find the newly created files - I can view the layers (and gerber names) in camtastic but cant seem to find where they are saved to individual files? Can only find the cam file.

[joelby]

Hi vl400,

After doing File, Fabrication Outputs, Gerber Files, have a look in the Projects panel:

[vl400]

Thanks