Generating Gerbers
When you’ve finalized your design, the last step before sending it off to the fab house is to generate gerber files. Gerber files are kind of a “universal language” for PCB designs. EAGLE is far from the only PCB CAD software out there, and its design files are nothing like those of Orcad or Altium. Fab houses can’t possibly support every piece of software out there, so we send them the gerber files instead.
Gerber files – note the plurality – each describe single layers of the PCB. One gerber might describe the silkscreen, while another defines where the top copper is. In all, we’ll generate seven gerber files to send to the fab house.
CAM Processor
Before we get too much further, you’ll need to download another definition file: SparkFun’s CAM file.
Then, load up the CAM processor by clicking the CAM icon –
From here, go to the File menu, then go Open > Job…. In the file browser that opens, select the sfe-gerb274x.camfile that you just downloaded. Now the CAM processor window should have a series of tabs: “Top Copper”, “Bottom Copper”, “Top Silkscreen”, etc. Each of these tabs define how to create one of the gerber files. Now all you have to do is click Process Job. If you haven’t saved recently, it’ll prompt you to.
The gerber generation process should be pretty quick. Once it’s run its course, have a look in your project directory, which should have loads of new files in it. In addition to the board (BRD) and schematic (SCH) files, there should now be a .dri, .GBL, .GBO, .GBS, .GML, .gpi, .GTO, .GTP, .GTS, and a .TXT. Meet the Gerbers!
Gerber File
Extension
Bottom Copper =GBL
Bottom Silkscreen =GBO
Bottom Soldermask =GBS
Top Copper =GTL
Top Silkscreen =GTO
Top Soldermask =GTS
Drill File =TXT
Drill Station Info File =dri
Photoplotter Info File =gpi
Mill Layer =GML
Top Paste =GTP
Delivering the Gerbers
The process of sending gerber files varies by fab house. Most will ask you to send them a zipped folder of select files. Which gerber files? Check with your fab house again (e.g. Advanced Circuits and OSH Park’s guidelines), but usually you want to send them GTL, GBL, GTS, GBS, GTO, GBO and the TXT files. The GTP file isn’t necessary for the PCB fabrication, but (if your design had SMD parts) it can be used to create a stencil.
So zip those gerbers up. Play the waiting game. And get ready to assemble your very own PCB!
When you’ve finalized your design, the last step before sending it off to the fab house is to generate gerber files. Gerber files are kind of a “universal language” for PCB designs. EAGLE is far from the only PCB CAD software out there, and its design files are nothing like those of Orcad or Altium. Fab houses can’t possibly support every piece of software out there, so we send them the gerber files instead.
Gerber files – note the plurality – each describe single layers of the PCB. One gerber might describe the silkscreen, while another defines where the top copper is. In all, we’ll generate seven gerber files to send to the fab house.
CAM Processor
Before we get too much further, you’ll need to download another definition file: SparkFun’s CAM file.
Then, load up the CAM processor by clicking the CAM icon –
From here, go to the File menu, then go Open > Job…. In the file browser that opens, select the sfe-gerb274x.camfile that you just downloaded. Now the CAM processor window should have a series of tabs: “Top Copper”, “Bottom Copper”, “Top Silkscreen”, etc. Each of these tabs define how to create one of the gerber files. Now all you have to do is click Process Job. If you haven’t saved recently, it’ll prompt you to.
The gerber generation process should be pretty quick. Once it’s run its course, have a look in your project directory, which should have loads of new files in it. In addition to the board (BRD) and schematic (SCH) files, there should now be a .dri, .GBL, .GBO, .GBS, .GML, .gpi, .GTO, .GTP, .GTS, and a .TXT. Meet the Gerbers!
Gerber File
Extension
Bottom Copper =GBL
Bottom Silkscreen =GBO
Bottom Soldermask =GBS
Top Copper =GTL
Top Silkscreen =GTO
Top Soldermask =GTS
Drill File =TXT
Drill Station Info File =dri
Photoplotter Info File =gpi
Mill Layer =GML
Top Paste =GTP
Delivering the Gerbers
The process of sending gerber files varies by fab house. Most will ask you to send them a zipped folder of select files. Which gerber files? Check with your fab house again (e.g. Advanced Circuits and OSH Park’s guidelines), but usually you want to send them GTL, GBL, GTS, GBS, GTO, GBO and the TXT files. The GTP file isn’t necessary for the PCB fabrication, but (if your design had SMD parts) it can be used to create a stencil.
So zip those gerbers up. Play the waiting game. And get ready to assemble your very own PCB!
Make sure you understand how the PCB fab house prefers to have the information presented in the Gerber files. Even though there has been a slow convergence toward an industry "standard practice" over the last decade or two, there are still a few holdouts. I have observed differences of opinion among fab houses on these points:
- Board outlines (sometimes called "router layer" or "milling layer"). Usually this is ONLY shown in a separate file containing ONLY the outline, and the board will be machined to the center of the line (plus or minus the vendor's stated tolerance).
But a few fabricators may still ask for the outline on EVERY layer (presumably to assist with registration), or for the outline to be shown on another specified layer (top solder mask, if I recall correctly). And I vaguely recall one vendor who said the boards would be machined to the INSIDE edge of the outline line. - Filename extensions. Pay attention to these. Your fab house may ask you to identify the layers using filename extensions that are different from the default nomenclature built into Eagle or ORCAD. Some vendors will accept ANY filename extensions, provided that you clearly identify the layer for each extension in a "Readme.txt" file.
- Outline shapes. In the past, ANY departure from a strictly rectangular outline - even rounding the corners - was an extra-cost option, and may have been unavailable on quick-turn or low-volume boards. Now many vendors allow more complex shapes with no additional charge - but ask before submitting your order.
- Depicting through-hole pads. The Gerber-generating routines in your layout software probably let you specify whether the Gerber files will show the hole in a through-hole pad, or show the pad as a solid shape. Some vendors prefer to have the holes shown in pads that have them, some want the solid pads without any indication of where the hole goes, and some will accept either format.
- Hole sizes. You should specify the size of the FINISHED hole - after plating. If a PCB fab house asks you to specify the drill size BEFORE plating and finishing (and lets you guess how much the hole size will be reduced by his plating process), get a different vendor.
Each fab house has a "standard tool rack" containing an assortment of drills to produce particular finished hole sizes. I don't think any two of them have exactly the same list of sizes in their racks. Of course, they can produce ANY hole size you ask for (within their range of capabilities) - for a price. For quick-turn and low-volume boards you are going to get the standard rack. Know what standard hole sizes are available and specify them in your pad-stacks. If you ask for a hole size that isn't in the standard list it's hard to tell what will be delivered. Some vendors will select the nearest standard size, others will use the next-larger size, and some may supply the next-smaller size. I once had a vendor put my job on "hold" until my drawing callouts matched his available standard sizes.
(As a practical matter, hole size variations by one or two standard sizes are tolerable for hand-insertion and manual soldering. That's not the case in automated production environments.) - Board-edge setbacks. The fab house will not produce a board if any copper feature (pad, trace, filled- or poured-region) touches the edge of the board. The minimum setback from the board edge varies among suppliers; recently I've seen constraints as close as 0.010" (0.25 mm) and as much as 0.025" (0.6 mm). Silk screen (or "legend") features are often permitted right up to the board edge, or even outside the outline.
Use ODB++ if possible, much better.
Silly Gerber file extensions were there because of DOS 8 character file name limitation, use a std. GBR or similar extension and differentiate in the file name.
No mention of Excellon drill format, this must be created and sent with the Gerbers, preferably one file for plated and non-plated holes.
IPC-D-356 output, again best practice for checking data and boards.
Board outline is a basic dimension, it should be drawn in the smallest line width possible, the centre of the line is the datum, nothing else, board manufacturers who don't work this way are cr**, the general tolerance on this outline is +/-0.2mm.
Annulus pads.... only ever did theses for simple boards that were going to be drilled by hand, if you do your own boards it is recommended so you have a drilling target, for professional manufactured boards never used them.
Use RS-274X format
Use Excellon 2 format
PTH holes are generally drilled 0.1mm larger than the finished hole size, this allows for approx. 0.025mm plating in the barrel.
Each job should have at least a basic master drawing showing main board dimensions and at least some references to board finish, copper weight, resist type and colour, ident type and colour, general tolerances and references to any special requirements.
Most manufacturers will work to IPC specs and guidelines, knowing the basics of these will help you get what you want at the cost you want from a manufacturer and an assembly house if you use one....
IPC-2221 and 2222 are a good start, from there it escalates with specs covering every aspect of PCB design, manufacture and assembly.
Silly Gerber file extensions were there because of DOS 8 character file name limitation, use a std. GBR or similar extension and differentiate in the file name.
No mention of Excellon drill format, this must be created and sent with the Gerbers, preferably one file for plated and non-plated holes.
IPC-D-356 output, again best practice for checking data and boards.
Board outline is a basic dimension, it should be drawn in the smallest line width possible, the centre of the line is the datum, nothing else, board manufacturers who don't work this way are cr**, the general tolerance on this outline is +/-0.2mm.
Annulus pads.... only ever did theses for simple boards that were going to be drilled by hand, if you do your own boards it is recommended so you have a drilling target, for professional manufactured boards never used them.
Use RS-274X format
Use Excellon 2 format
PTH holes are generally drilled 0.1mm larger than the finished hole size, this allows for approx. 0.025mm plating in the barrel.
Each job should have at least a basic master drawing showing main board dimensions and at least some references to board finish, copper weight, resist type and colour, ident type and colour, general tolerances and references to any special requirements.
Most manufacturers will work to IPC specs and guidelines, knowing the basics of these will help you get what you want at the cost you want from a manufacturer and an assembly house if you use one....
IPC-2221 and 2222 are a good start, from there it escalates with specs covering every aspect of PCB design, manufacture and assembly.
- Status
- This old topic is closed. If you want to reopen this topic, contact a moderator using the "Report Post" button.