Author Topic: Gerber to footprint  (Read 3178 times)

0 Members and 1 Guest are viewing this topic.

exapod

  • Guest
Gerber to footprint
« on: July 16, 2015, 07:59:14 am »
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
 

Offline free_electron

  • Super Contributor
  • ***
  • Posts: 6848
  • Country: us
    • SiliconValleyGarage
Re: Gerber to footprint
« Reply #1 on: July 16, 2015, 08:02:20 am »
load in camtastic. assign layers , pull netlist - export to pcb. done
Professional Electron Wrangler.
Any comments, or points of view expressed, are my own and not endorsed , induced or compensated by my employer(s).
 

Online T3sl4co1l

  • Super Contributor
  • ***
  • Posts: 10605
  • Country: us
  • Expert, Analog Electronics, PCB Layout, EMC
    • Seven Transistor Labs
Re: Gerber to footprint
« Reply #2 on: July 16, 2015, 01:42:21 pm »
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
Seven Transistor Labs, LLC
Electronic Design, from Concept to Layout.
Need engineering assistance? Drop me a message!
 

Offline free_electron

  • Super Contributor
  • ***
  • Posts: 6848
  • Country: us
    • SiliconValleyGarage
Re: Gerber to footprint
« Reply #3 on: July 16, 2015, 01:47:18 pm »
what ?
i do that frequently
load gerber
load ncdrill
tables -> layers:   set that up correctly
tools -> netlist -> extract
Professional Electron Wrangler.
Any comments, or points of view expressed, are my own and not endorsed , induced or compensated by my employer(s).
 

exapod

  • Guest
Re: Gerber to footprint
« Reply #4 on: July 16, 2015, 09:26:18 pm »
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.
 

Offline zeke

  • Contributor
  • Posts: 13
Re: Gerber to footprint
« Reply #5 on: July 21, 2015, 09:38:35 am »
@free_electron,

You should have your own fan club. I learn something new every time I read one of your posts.

Thanks!

 :-+
 

Offline Gribo

  • Frequent Contributor
  • **
  • Posts: 262
  • Country: ca
Re: Gerber to footprint
« Reply #6 on: July 23, 2015, 11:32:38 pm »
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.
 

Offline mariaadnan

  • Newbie
  • Posts: 2
  • Country: pk
Gerber to footprint- whole component
« Reply #7 on: January 12, 2018, 04:43:31 pm »
load in camtastic. assign layers , pull netlist - export to pcb. done


thanks 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. |O
 

Online T3sl4co1l

  • Super Contributor
  • ***
  • Posts: 10605
  • Country: us
  • Expert, Analog Electronics, PCB Layout, EMC
    • Seven Transistor Labs
Re: Gerber to footprint
« Reply #8 on: January 12, 2018, 07:50:24 pm »
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
Seven Transistor Labs, LLC
Electronic Design, from Concept to Layout.
Need engineering assistance? Drop me a message!
 
The following users thanked this post: mariaadnan

Offline mariaadnan

  • Newbie
  • Posts: 2
  • Country: pk
Re: Gerber to footprint
« Reply #9 on: January 15, 2018, 03:33:52 pm »
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?


 

Online T3sl4co1l

  • Super Contributor
  • ***
  • Posts: 10605
  • Country: us
  • Expert, Analog Electronics, PCB Layout, EMC
    • Seven Transistor Labs
Re: Gerber to footprint
« Reply #10 on: January 15, 2018, 05:52:57 pm »
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
Seven Transistor Labs, LLC
Electronic Design, from Concept to Layout.
Need engineering assistance? Drop me a message!
 

Offline free_electron

  • Super Contributor
  • ***
  • Posts: 6848
  • Country: us
    • SiliconValleyGarage
Re: Gerber to footprint
« Reply #11 on: January 16, 2018, 07:06:56 am »
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 away

You 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.
Professional Electron Wrangler.
Any comments, or points of view expressed, are my own and not endorsed , induced or compensated by my employer(s).
 

Online julianhigginson

  • Frequent Contributor
  • **
  • Posts: 524
  • Country: au
Re: Gerber to footprint
« Reply #12 on: February 23, 2018, 12:28:50 am »
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.
 

Online T3sl4co1l

  • Super Contributor
  • ***
  • Posts: 10605
  • Country: us
  • Expert, Analog Electronics, PCB Layout, EMC
    • Seven Transistor Labs
Re: Gerber to footprint
« Reply #13 on: February 23, 2018, 06:14:00 am »
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
Seven Transistor Labs, LLC
Electronic Design, from Concept to Layout.
Need engineering assistance? Drop me a message!
 

Online julianhigginson

  • Frequent Contributor
  • **
  • Posts: 524
  • Country: au
Re: Gerber to footprint
« Reply #14 on: February 23, 2018, 04:02:34 pm »
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.
 


Share me

Digg  Facebook  SlashDot  Delicious  Technorati  Twitter  Google  Yahoo
Smf