Gerber to footprint - Page 1
Forum section: electronics / general

author: Unknown
author_rank: Unknown
timestamp: July 15, 2015, 09:59:14 pm
content: I have to gerbers files (.grb) of a small pcb antenna, one for the top layer and one for the bottom. I would like to copy the gerber to the library footprint editor so i can make a part.Thanks for the help

author: free_electron
author_rank: Super Contributor
timestamp: July 15, 2015, 10:02:20 pm
content: load in camtastic. assign layers , pull netlist - export to pcb. done

author: T3sl4co1l
author_rank: Super Contributor
timestamp: July 16, 2015, 03:42:21 am
content: Speaking of, I've never been able to generate a netlist in CAMTastic. It wants a tool file (.mta or something?) that's never present, and doesn't seem to have any way to generate it from a drill drawing (duh?).Tim

author: free_electron
author_rank: Super Contributor
timestamp: July 16, 2015, 03:47:18 am
content: what ?i do that frequentlyload gerberload ncdrilltables -> layers: set that up correctlytools -> netlist -> extract

author: Unknown
author_rank: Unknown
timestamp: July 16, 2015, 11:26:18 am
content: I imported the two gerber files, assigned the layers but i don't have an ncdrill and when i try to export the netlist i get this error : Netlist extraction error: Missing drill layer.

author: zeke
author_rank: Contributor
timestamp: July 20, 2015, 11:38:35 pm
content: @free_electron,You should have your own fan club. I learn something new every time I read one of your posts.Thanks!

author: Gribo
author_rank: Frequent Contributor
timestamp: July 23, 2015, 01:32:38 pm
content: If the gerber does not contain any drills, you can create an empty drill layer with the same size as the other layers and import that one.

author: mariaadnan
author_rank: Newbie
timestamp: January 12, 2018, 05:43:31 am
content: Quote from: free_electron on July 15, 2015, 10:02:20 pmthanks for sharing the tip,have done that successfully!but i want access to the components but altium or camtastic exports them as single pin connections. i cant access them like move, place or get info about single whole component?is there any way i can export gerber parts to actual footprints?in desparate need of help please.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: January 12, 2018, 08:50:24 am
content: Gerbers are flattened vector graphics. They do not contain structural design information like footprints, or polygons sometimes for that matter (e.g., PADS exports polys as trace fill patterns, and I think Altium does as well for certain poly types). You have to reconstruct that yourself.Tim

author: mariaadnan
author_rank: Newbie
timestamp: January 15, 2018, 04:33:52 am
content: thankyou very much for the reply.is there anyway i can convert DXF file to a footrpint... any tool or package designer for that purpose?

author: T3sl4co1l
author_rank: Super Contributor
timestamp: January 15, 2018, 06:52:57 am
content: DXF is a structured format, AFAIK, but you may not be able to use that structure without AutoCAD or equivalent tools. Also, whatever produced the file, may've flattened it, removing that structure.For example, Altium's DXF import only produces flat objects (no components or unions).Tim

author: free_electron
author_rank: Super Contributor
timestamp: January 15, 2018, 08:06:56 pm
content: import in camtastic. - pull netlist - assign layers and export to PCB.then delete anything that is a track or polygon on the electrical layers ( selectsimilar and filter on electrical layers and tracks / polygons ) or write a rule : (IsTrack or InPolygon or isvia) and InLayerClass('electrical layers') and blow those awayYou will now be left with pads and lines on mechanical layers.clean up the layers you do not want by killing them off.select all pads and apply a mask setting for solder and paste. ( global edit )now simply select the items you want : copy and paste them in a library.i steal parts from boards all the time ( TI and many other provide gerbers for their demoboards . rip em up and grab their approved footprints.

author: julianhigginson
author_rank: Frequent Contributor
timestamp: February 22, 2018, 01:28:50 pm
content: I pulled an inverted F PCB antenna from a TI reference design board today.. was interesting - the antenna was made up with tracks right around the outline, and the inside filled in with polygons. (and 3 pads, all designated pad 1)the feedline was particularly interesting being made of 2 polygons and two sets of very close parallel tracks, when it could just as easily have been a single track.I'm wondering if that's a feature of being pulled out of a gerber file and turned into altium primitives, or if that's how cadstar actually designs things like that?Interestingly enough it exported one side of the top layer groundplane as a poly pour outlined with tracks, in the same way the antenna was. But the other side of the groundplane it just make up of a whole pile of parallel tracks.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: February 22, 2018, 07:14:00 pm
content: You mean by importing Gerbers?Some convert polys to track fill, some don't. Though it's odd that both would be done in the same file.Outlined polys are fairly normal, where the poly perimeter is a "soft" trace shape (rounded corners, actual outer perimeter beyond where the vertices are placed). Ultiboard does that, but it uses polys to fill. It would be weird for something to (arbitrarily?) use both fill methods. Eagle (I think?) and PADS only fill with lines.Tim

author: julianhigginson
author_rank: Frequent Contributor
timestamp: February 23, 2018, 05:02:34 am
content: yep. importing gerbers (and then making a footprint out of some data on a gerber layer) - just like what this thread is about.It was interesting to see the way that the PCB features in the gerber come in to Altium as a pcb file.Especially the different treatment of two halves of what I'd expect would have been the same ground plane pour in the original design file.