Author Topic: Panelising Gerber files  (Read 9848 times)

0 Members and 1 Guest are viewing this topic.

Offline LukeWTopic starter

  • Frequent Contributor
  • **
  • Posts: 684
Panelising Gerber files
« on: April 10, 2014, 01:56:47 am »
Is there any tool or process you would recommend that can take a standard stack of Gerber files (usually 2-layer, although the potential capability to support 4-layer would be nice) and bring them all together into one set of Gerber files on a combined single panel for fabrication, for fab houses where this is required or economically attractive.

I want to do this in a way that isn't labor intensive, doesn't corrupt or change the existing Gerber files, and takes Gerber files as its input, meaning it is independent of whatever EDA/CAD software is used by different people - Altium, Eagle, KiCad, whatever - as long as they're just able to generate and provide standard Gerbers from their software.
 

Offline free_electron

  • Super Contributor
  • ***
  • Posts: 8503
  • Country: us
    • SiliconValleyGarage
Re: Panelising Gerber files
« Reply #1 on: April 10, 2014, 02:41:13 am »
Frontline's Genesis , ucamco's ucam or lavenir.
But not free and very expensive.
That is what the industry uses to panelise
Professional Electron Wrangler.
Any comments, or points of view expressed, are my own and not endorsed , induced or compensated by my employer(s).
 

Offline kizzap

  • Supporter
  • ****
  • Posts: 477
  • Country: au
Re: Panelising Gerber files
« Reply #2 on: April 10, 2014, 02:45:20 am »
The only software I have used that I was able to do what you are after is some software called CAM350. It imports all the gerbers from whatever software you produced your PCBs in, and allows you to do whatever you need to do with panelizing, including your borders, copper theifing, panel fiducials, dril checks, etc. It will also do an automatic step and repeat of your PCB design for you.

cons: not cheap at $500 for the basic version of the software.
<MatCat> The thing with aircraft is murphy loves to hang out with them
<Baljem> hey, you're the one who apparently pronounces FPGA 'fuhpugger'
 

Offline DerekG

  • Frequent Contributor
  • **
  • Posts: 882
  • Country: nf
Re: Panelising Gerber files
« Reply #3 on: April 10, 2014, 02:47:38 am »
Frontline's Genesis , ucamco's ucam or lavenir.
But not free and very expensive.
That is what the industry uses to panelise

Yep. You just plug in the dimensions of the panel you wish to use & Genesis will pretty much do the rest for you to minimise any wasted panel space.
I also sat between Elvis & Bigfoot on the UFO.
 

Offline Hideki

  • Frequent Contributor
  • **
  • Posts: 256
  • Country: no
Re: Panelising Gerber files
« Reply #4 on: April 10, 2014, 07:49:39 pm »
One free solution is GerbMerge, written in Python and a royal pain in the ass to use... but hey... that's the price you have to pay for something that's free :)
 

Offline gregariz

  • Frequent Contributor
  • **
  • Posts: 545
  • Country: us
Re: Panelising Gerber files
« Reply #5 on: April 24, 2014, 09:49:06 am »
 

Offline oboemasesetokoe

  • Newbie
  • Posts: 1
Re: Panelising Gerber files
« Reply #6 on: August 21, 2014, 08:55:57 pm »
Hi,

I also used CAM350 but the workflow i donĀ“t like. I found Macaos . I just tried their demo and found it works great.



It includes a stencil generator too, very powerful program.
 

Offline DerekG

  • Frequent Contributor
  • **
  • Posts: 882
  • Country: nf
Re: Panelising Gerber files
« Reply #7 on: August 21, 2014, 09:18:29 pm »
Is there any tool or process .... and bring them all together into one set of Gerber files on a combined single panel for fabrication, for fab houses where this is required or economically attractive.

Actually, unless you run a fab plant yourself, you are generally just creating more work for yourself.

Just advise the fab shop of the maximum panel size you can handle, the positioning & diameter of any locating holes and/or fiducial marks.

You can simply provide them with a PDF showing all this information. As your maximum panel size & locating holes are unlikely to change, you can simply generate one PDF & attach it to your outgoing gerbers each time you send them to the fab shop.

Advise them if you want your pcbs V-grooved or routed & you're done.

This leaves the fab shop to do what they do best.

I always use a fab shop that will also supply the solder paste screen. Then, if there are any problems they have to fix if for free :)
I also sat between Elvis & Bigfoot on the UFO.
 

Offline nctnico

  • Super Contributor
  • ***
  • Posts: 26219
  • Country: nl
    • NCT Developments
Re: Panelising Gerber files
« Reply #8 on: August 21, 2014, 10:40:38 pm »
One free solution is GerbMerge, written in Python and a royal pain in the ass to use... but hey... that's the price you have to pay for something that's free :)
True but once you get the configuration file and job file done a next project is easy to do. I use it every now and then.
There are small lies, big lies and then there is what is on the screen of your oscilloscope.
 

Offline Legit-Design

  • Frequent Contributor
  • **
  • Posts: 562
Re: Panelising Gerber files
« Reply #9 on: August 21, 2014, 10:58:01 pm »
What about pick and place data after panelising? Should there be fiducials on every pcb and pick and place machine will then do each pcb separately? Or does someone has to sit there and manually all the pick and place data to every pcb?

One free solution is GerbMerge, written in Python and a royal pain in the ass to use... but hey... that's the price you have to pay for something that's free :)
http://africa.princeton.edu:8090/pages/viewpage.action?pageId=8487148 How to use gerbmerge.
http://174.136.57.11/~ruggedci/gerbmerge/
« Last Edit: August 21, 2014, 11:00:11 pm by Legit-Design »
 

Offline DerekG

  • Frequent Contributor
  • **
  • Posts: 882
  • Country: nf
Re: Panelising Gerber files
« Reply #10 on: August 22, 2014, 12:45:25 am »
What about pick and place data after panelising? Should there be fiducials on every pcb and pick and place machine will then do each pcb separately?

The gerbers don't contain the pick & place information. This is generated by your pcb design software & supplied directly to the SMD shop (or to yourself if running your own SMD robot). Part of this pick & place information contains the exact centre point of each component along with the rotation angle of each component.

Normally you would place at least one fiducial mark on your circuit. Some robots look for a crosshair (each part of the "hair" say being 35mils long & of a thickness of 15mils) & others a small circle (say 15mils in diameter). Open up the top solder mask so that the copper reflects nicely from the fiducial marks. Remember your particular SMD shop may have a preference for what type & size fiducials they prefer, so ask first. They will also have a preference for the position, number & diameter of the panels outside locating holes, so again ask first.

If you forget any of the above, the SMD shop will work with something existing on the circuit (like a small component pad as a fiducial mark), but they normally prefer you to generate one that will not have solder paste placed over it.

The SMD shop will measure the X & Y distance from the first circuit's fiducial mark to the fiducial mark on the most distant circuit. They will then divide this measure by the number of circuits on the panel and then end up with the exact X & Y separations of each circuit.

They enter the X & Y offset into their software & away they go.

Even if you were to generate the panelised gerbers & supply the pick & place file for the entire panel, the SMD shop would do the above manual check everytime, just to be absolutely sure that the offset you supplied them was identical to the panels they have actually received.

So, generally if your not a fab shop, your wasting your time generating gerbers for entire panels yourself. They are the experts & will minimise any unused substrate. They know how much space they require around the edges of each panel to manage them through their baths etc. You just need to give them the maximum size of the panels that your SMD fab shop can handle. This maximum size would normally be dictated by the size of their infrared reflow oven, their SMD robot, their wave solderer or your board holding frames if you have to complete any finishing work manually.

I hope this helps :)
I also sat between Elvis & Bigfoot on the UFO.
 

Offline Legit-Design

  • Frequent Contributor
  • **
  • Posts: 562
Re: Panelising Gerber files
« Reply #11 on: August 22, 2014, 01:33:14 am »
I hope this helps :)
It does  :-+

Dave has shown panelization on altium, but no all pcb packages are the same. So Altium will automatically include all the pick and place data for the whole panel since it has also fiducials which are made for the panel?
What put me off was that they specify the fiducials on the panel material itself, outside the actual pcbs on the panel. At least three in the corners of the panel. And assembly house want's these fiducial coordinates in the pick and place data. However not every pcb package can do the panelization as it is done usually in some actual CAM software, and therefore no panel and no fiducials in the pick and place data. So what I was thinking it wouldn't be nearly as elegant way to just put the the three fiducials on every board that goes on the panel.
 

Offline DerekG

  • Frequent Contributor
  • **
  • Posts: 882
  • Country: nf
Re: Panelising Gerber files
« Reply #12 on: August 22, 2014, 03:12:08 am »
Dave has shown panelization on Altium, but not all pcb packages are the same.
Ahh ........... it is important to differentiate between "panelisation" & generating a gerber of an entire panel for production. I have suggested that you leave the generation of gerbers of the entire panel to the board production shop.

It is usual however to generate the gerbers for your (individual) circuit & to then send this to the board shop.

Altium can be used to layout all the circuits on the panel. This is called panelisation.

An example would be when I layed out an entire panel of round circuits which were going to be routed out in a circular fashion. These boards contained hard gold contacts that were going to be electrically plated & so copper tracks led to the edges of the panel to enable this to be done. After electrically plating the hard gold onto the contacts, the circuits were then routed, leaving some tags to hold them in the panel so that the SMD work could be completed. After this, the circuits were snapped out & placed into specially designed plastic boxes.

This was rather special & so I completed the work myself. Of course the way to do this is to design a single circuit & then step & repeat to end up with as many circuits as the panel will hold. I added a mechanical layer showing the circular routing required & the tags to hold the circuits in the panel. The routing also disconnected the various hard gold segments from each other as was required by the schematic.

I then generated the gerbers for the entire panel from within Altium in exactly the same way as I would have for a single circuit.
Quote
Altium will automatically include all the pick and place data for the whole panel since it has also fiducials which are made for the panel?
When you produce all the manufacturing files within Altium, you will see separate files for pick & place & the drill sizes. The drill size file will be sent with the gerbers to the board shop & the pick & place file will be sent to the SMD shop.
Quote
What put me off was that they specify the fiducials on the panel material itself, outside the actual pcbs on the panel. At least three in the corners of the panel.
Normally any fiducials can be placed within the bounds of the circuits itself. I suggest you find a spot (near one corner is always good but not locked in stone) & place a "+" (or circle) as detailed in my previous post.

As you don't know what magin the panel shop wants around the outside of their panels, I suggest you just send them your single circuit gerber & tell them to sort it out for themselves. Most fab shops want to do this anyway. If they complain, they have little idea about what they are doing & so you are best to find another fab shop anyway.
Quote
So what I was thinking it wouldn't be nearly as elegant way to just put the the three fiducials on every board that goes on the panel.
Absolutely the right way to go. If you don't have enough room, one per circuit will be enough as the SMD shop will maximise the accuracy by taking two or three fiducials from the furthest apart circuits as mentioned in my post above.
I also sat between Elvis & Bigfoot on the UFO.
 


Share me

Digg  Facebook  SlashDot  Delicious  Technorati  Twitter  Google  Yahoo
Smf