The following is presented for the drill file format enhancements included from V8.1.2.
V8.1.3 patch Is recommend. If you are using an earlier version please update to the latest version.
V8.1.2 had a bug that transposed the LZ and TZ commands.
The Excellon file format originally published in 1985 has evolved to meet CAD/CNC requirements, but it also has limitations for manufacturers and users alike in attempting to achieve the correct drill hole positions for data exchange. Many manufacturers specify their expected file format for example 2,3 and you must match their requirements when producing the drill file.Similarly Gerber viewers will often require you to generate a specific file format or select what you have used when importing the drill file.
What format do you require?
As mentioned the format will be n,m and typically 2,3 usually when inches are specified or 3,3 when millimeters are used, so what are the meanings of these numbers?
The first number "n" is the number of digits before the decimal point referred to as the"Integer", the second digit "m" is referred to as the "Decimal" which is the the precision i.e. the number of digits after the decimal point.
In the example 2,3 this allows 0 to 99 inches with a precision on 1 thousandths of an inch so actually a maximum position coordinate of 99.999 inches.
There is another format requirement that requires to be selected, this relates to leading or trailing zeros. DesignSpark PCB from V8.1 allows complete control of these, but what are they?
First they are set up in the Manufacturing Outputs dialog.
Select the "Drill Data" plot and then the "Device Setup". In this Window where you set the "integer" and "Decimal" digits you also select "None", "Leading" or "Trailing" in the "Omit Zeros" option. Manufacturers will refer to these as Leading or Trailing Zero Suppression.
The table below is for the same PCB which has had the Manufacturing Outputs run three time to illustrate each option.
The table shows the 3 options as set at the top of the column. All are using the format 3,3 for this illustration, so the coordinates for each drill hole will have 3 digits before the decimal point and 3 after.
X000873Y001680 is position X0.873 and Y 1.680 as we have specified "None" for "Omit Zeros" you will observe they are packed out with zeros to keep the 3,3 format.
We have selected to omit the "Leading Zeros". In this instance the trailing zeros will remain to identify the position of the decimal point, using the same example entry it is represented by X873Y1680 and as we have defined the "Decimal" to be "3" we know there are three digits after the decimal point so this represents X0.873 and Y 1.680
We have selected to omit "Trailing Zeros". In this instance the leading zeros will remain and for the same entry is X000873Y00168, as we know the "Integer" is defined as "3" we again have X0.873 and Y 1.680
All options result in having the same actual coordinates presented in three different formats, you must select as required by your manufacturer and in your Gerber viewer.
Command format options.
This is all tied up in the history of the Excellon drill file format, and there is yet another option you need to be aware of. This is "Format" which determines FMAT,1 or FMAT,2 options in the output file.
Format 1 is the typical format used by manufacturers (but again check their requirements).
Historically Excellon developed their format for their own CNC machines, their first generation were drilling machines only and "Format 1" produces drilling data only.
Their second generation machines performed drilling and routing and extra commands are built in for routing processes, this became known as Format 2.
You will only require "Format 2" if your own drilling and routing machine supports this.
Why do we have this old and potentially unsatisfactory situation and why has it not been improved?
It has! ODB++ which is available in DesignSpark PCB overcomes these concerns with a defined format for ease of use. It now requires the manufacturers to catch up and start using this new standard, until then the above will allow you to submit the correct format drill file and import your files into a Gerber viewer correctly.
Please also be aware of the requirement not to have board outlines enabled in the drill file for normal manufacturing requirements. This feature is for personal CNC use where the drill and milling has an advanced drilling mode.
Ensure the check boxes identified below for "Boards" on the Drill Data "Settings" tab are NOT checked.
PCB manufacturers use the Gerber board outline as defined here.