PCB Libraries Forum : 7 Common Mistakes With Gerber Files

7 Common Mistakes With Gerber Files : Chenonn, if you have CAM350 then...

Mon, 05 Oct 2015 02:30:07 +0000

Author: Matthew Lamkin
Subject: 1375
Posted: 05 Oct 2015 at 2:30am

Chenonn, if you have CAM350 then there is a forum on the downstream site where you may obtain assistance.

Confirming that they are actually Gerber files is essential, opening them in Notepad can show this.
Checking that you have the correct format also helps load it in - is it 2.3 or 4.5 etc?
Often loading in a Gerber file when the resolution is not set correctly can result in a mess on screen or everything in a corner etc.

7 Common Mistakes With Gerber Files : The first thing to check is to...

Fri, 02 Oct 2015 02:45:28 +0000

Author: jameshead
Subject: 1375
Posted: 02 Oct 2015 at 2:45am

The first thing to check is to see if it is actually a Gerber file at all by opening it in a text editor.

Users often send all sorts of files together with Gerber and excellon data such as GenCAD and original Binary CAD data so if you have a modern Gerber viewer like GC-Prevue or CAM350 and it's not recognising it as a Gerber file, odd on, it isn't.

7 Common Mistakes With Gerber Files : I have a question,sometimes I...

Thu, 01 Oct 2015 20:04:02 +0000

Author: CHENONN
Subject: 1375
Posted: 01 Oct 2015 at 8:04pm

I have a question,sometimes I can not open the gerber file which my customer send to me,I try to open it,but there is nothing on the desk,I usually use the CAM350 10.1/9.5 software.

7 Common Mistakes With Gerber Files : This looks like a list copied...

Tue, 04 Nov 2014 09:16:35 +0000

Author: jameshead
Subject: 1375
Posted: 04 Nov 2014 at 9:16am

This looks like a list copied and pasted from the early nineties. Look at point 1, who uses aperture tables and RS-274D these days? I guess it covers old designs.

It's totally out of date with regard to units. I was a CAM Engineer for a high technology PCB Fabricator for two years after leaving university and we didn't care if customers provided data in imperial or metric. The CAM software would handle both easily.

At this PCB fabricator the CNC drill machines used metric sized drill bits but photo tools were worked on in the CAM system in imperial.

A large number of customers provided gerber data in imperial (2.3 or 2.4 inch format) and excellon drill data in metric ( 3.3 mm format) together with a drawing from a mechanical cad system that used metric. Sure the drill hits didn't always tie up with the pad centres, and the PCB profile from the gerber didn't tie up with the mechanical drawing, but we dealt with this. We had built in tools in the CAM software to snap drill hits into pad centres and we always created the rout program from the metric drawing.

Nowadays things are different, particulary as Mechanical Design has progressed and the improved integration between the PCB Design and Mechanical design.

My guidence would be to pick one system and stick with that throughout the design for both PCB Design and Mechanical design, and make sure your outputs are in the same system used for design.

My preference is for metric everywhere and I agree with bac_a_sable's comments to a point, although converting thou (MIL for American readers) to metric mm will produce rounding errors if you don't take account of the resolution.

For example 1 thou equates to 0.0254 mm, and 2 thou equates to 0.0508 mm, but if you are using an 3.3 format metric output then you've lost the 0.0004 or 0.0008 at the end of these values so you could still end up with (small) rounding errors in your design.

7 Common Mistakes With Gerber Files : I desagree with one point: the...

Tue, 04 Nov 2014 01:31:10 +0000

Author: bac_a_sable
Subject: 1375
Posted: 04 Nov 2014 at 1:31am

I desagree with one point: the use of english unit.
You cans always convert inch to millimeters; convert milimmeters to ich will produce roundoff accuracie problems.

Read IPC-2221B paragraph 1.3.1 about this

7 Common Mistakes With Gerber Files : Creating Gerber files that accurately reflect...

Wed, 02 Jul 2014 19:56:29 +0000

Author: frankicic
Subject: 1375
Posted: 02 Jul 2014 at 7:56pm

Creating Gerber files that accuratelyreflect what you want manufactured is a challenge no matter how long you havebeen a pcb designer. However, by learning from others and avoiding the mostcommon mistakes, you can speed up the turnaround time, reduce the chance oforders placed on hold, and complete your projects faster. The following listreviews the top seven most common mistakes made with Gerber files and how youcan avoid them.

1. Missing Aperture List

Your Gerber files specify what to do and where. Your aperture list specifieswhat tool to use. A single comprehensive aperture list for all layers should besent with your Gerber files, rather than a separate aperture list for eachlayer. Please note: An aperture list does not need to be sent with 274X formatfiles. If you send 274D format, we use your aperture list in combination withyour Gerber files to create your artwork.

Requirements: One comprehensive aperture list for all layers, English Units.Please do not modify the aperture list your software outputs. An aperture listdoes not need to be sent with 274X format files.

Resolution: All layout packages which output 274D also output an aperture list.Common extensions include .rep, .apt, and .apr. If you have difficultyoutputting an aperture list, please send 274X format.

2. Missing Excellon Drill File

Excellon drill files are used to determine what size holes to drill and where.Plated and non-plated holes need to be included in one drill file, with platedand non-plated holes having different tool numbers.

Requirements: Excellon Format, ASCII Odd/ None, 2.4 Trailing Zero Suppression,English Units, No Step and Repeats.

Resolution: Nearly all layout packages will output an excellon drill file. If youcannot generate one, we can in most cases create one from your fabricationdrawing for an engineering fee.

3. Missing Tool List

A tool list is used in combination with your excellon drill file to create yourdrill. Your drill file specifies where to place the holes. Your tool listspecifies what tool to use. A tool list should be embedded in your excellondrill file or sent as a separate text file. Using a tool list provided on afabrication drawing is not preferable, as it eliminates many of the automaticverifications and makes data entry errors far more likely.

Requirements: Tool list embedded in excellon drill file or sent as a separatetext file.

Resolution: If your layout software will output an excellon drill file, it willalso output a tool list. Common extensions include .tol and .rep.

4. Missing Gerber Files

Believe it or not, many times people submit orders and forget to attach theirgerber files.

Requirements: Gerber 274X or 274D, English units are preferable.

Resolution: ODB++ files are acceptable; It is possible to convert many otherfile formats to gerber.

5. Insufficient Annular Ring

An annular ring is the donut (“annulus”) created when your drill pierces acopper layer. It is defined as the radius of this donut. For example, a .030”pad with an .020” hole would have a .005” annular ring. This is required toallow for complete plating on vias, as well as solder ability on componentholes. Many times people do not allow for the proper annular ring requirements.

Requirements: A minimum of .005” annular ring for vias or a minimum of .007”for component holes is required for manufacturing.

Resolution: All layout packages provide this as a DFM check. Setting sufficientannular ring in your layout software is the preferred method in order tomaintain proper copper spacing.

6. Insufficient Copper Trace Width/Spacing

Copper spacing is the minimum air gap between any two adjacent copper features.Trace width is the minimum width of a copper feature, usually traces.

Requirements: A minimum of .005” trace width/spacing is necessary. A premium ischarged for trace width/spacing less than .008”.

Resolution: All layout packages provide this as a DFM check. Setting sufficienttrace width/ spacing in your layout software is the preferred method. Tracewidth and spacing push and pull against one another, so changing a problem areamay require rerouting traces, adding vias, or moving components.

7. Insufficient Inner Clearances

Inner clearance is the minimum distance from the edge of a hole to anyadjacent, unconnected, inner layer copper. Sufficient inner clearances helpensure that your drill does not cause shorts to your inner copper layers. Thisis important for both plated and non-plated holes, as non-plated holes mayeither cut into an adjacent trace or cause shorts during assembly.

Requirements: A minimum of .012” inner clearance is required and .015” ispreferred.

Resolution: Most inner clearance issues can be resolved if negative imageinners are provided, but it is preferred to not modify these. Setting theseclearances in your layout software is the preferred method, as this willmaintain intended connectivity. While most layout packages provide this as aDFM check, not all do. Those that do not can usually be manipulated to checkfor this violation by setting spacing and annular ring higher.

General guidelines: Spacing + Annular ring = Inner clearance. Another trickthat can help resolve problem areas is to move the affected traces to outercopper layers, where this is not an issue.