ECE Electronics Services Shop

Special Requirements For Using EasyTrax With Our PCB Process

For a full tutorial on using EasyTrax, see the text file TutorialEasytrax.txt in the same directory as EasyTrax, or read it here.

Our PCB milling process has some special requirements when using EasyTrax:

Board Design in EasyEdit

Track Dimensions
  • Use track width &gn;= 10 mils (1 mil = 1/1000").
  • Separate tracks, pads, vias, fills, etc by spaces >= 10 mils wide.
Mid Layer 2 = Board Outline Definition

In EasyTrax, Mid Layer 2 is intended to be used to specify an internal board layer. We can't make boards with internal layers, so we instead use Mid Layer 2 to define the outline of the board, i.e. the "cutting" layer. On this layer you should draw the desired board outline with 10-mil-wide tracks. After your board has been drilled and milled, the cutting bit will follow the tracks on Mid Layer 2 to cut your board out of a larger piece of PCB material. The board does not have to be rectangular and can be almost any shape.

The circular cutting tool has a diameter of 2mm (~79 mils) and will follow the CENTER of the tracks you have used to define the board outline. So you need to keep the board outline tracks more than 1mm (~39 mils) away from your circuit so the cutting tool will not damage it.

Drill Diameters

The following table shows the diameters of the holes which will be drilled for each pad size in EasyEdit. It would be a good idea to check the size of your component leads to make sure they will fit through the holes produced by the pad you have selected.

Pad/Via(mils) Drill Diameter Tool Name AWG
inches mm
40 .024 .6 TO1 23
50 and 62 .032 .8 TO3 21
70 and 85 .045 1.1 TO5 17
100 .060 1.5 TO6 15
125 and 150 .080 2.0 TO7 13
175 and 200 .100 2.5 TO8 11
225 and 250 .120 3.0 TO9 9

If you want different drill hole diameters than these, give us a hardcopy printout of the board and indicate drills wanted.

Surface Mount Pads

Sometimes you will want a custom size pad for surface mount components (Other programs have libraries of hundreds of SMT footprints built in, but not EasyTrax!). Use "place-fill" in EasyEdit to define the size and shape of the pad area defined in the data sheet for your part. After you have created one pad, it can be copied to create multiple pads.





Generating NC Drill and Gerber files with EasyPlot

The Easyplot.exe program is used to generate the NC Drill and Gerber files I need to make the PCB.

Start EasyPlot.exe and do File-Load to load your PCB file.
Generate the NC Drill file 'filename.TXT'
  • From the main menu select 'NC Drill'.
  • 'CONFIRM PROCEED WITH NC DRILL?' Answer 'Yes'.
  • After running for a while you should get a message 'DRILL FILES GENERATED - filename.DRL - filename.TXT'.
  • Submit the 'filename.TXT' file to me along with the Gerber files when you send me the board request email. I don't need the 'filename.DRL' file.
Generate the Match File "filename.MAT", and the Top Layer Gerber File 'filename.GTL'
  • From the main menu select Options/Type of Plot/Top Layer.
  • Hit 'Esc' to go back to the Main Menu.
  • Select 'Gerber Plot'.
  • 'Confirm Proceed with Gerber Plot?'. Answer 'Yes'.
  • 'MATCHING OF SHAPES'. Answer 'Automatic'.
  • 'ALWAYS CONFIRM PAINT-MATCH FOR SHAPE?'. Answer 'No'.
  • 'FILL PERIMETER MATCH?'. Answer 'Automatic'.
  • It will say 'MATCHING DRAFT CODES' and run for a while.
  • You may encounter the following error message during this part of the process:


    This means the program doesn't know which aperture to use when generating the Gerber file, and typically occurs if your board contains "Fill" areas. If you get this message:

    • Select "Paint Match: NO MATCH FOUND" and hit Return. You should see this:


    • Now move the cursor down to select "D13 Circular (10x10)" and hit Return. You will get this screen:


    • Now hit Return to select 'Use Paint Match' and the program will continue matching draft codes.

  • Eventually you will get the message 'MATCH FILE GENERATED - (Filename) - Press any key to continue'. This means the program has generated the "filename.MAT" file. You do not need to submit this file to me with a board request, but the EasyPlot program will use it to generate the three Gerber files I need (filename.GTL, filename.GM2, filename.GBL).
  • Press a key to continue with Top Layer Gerber file generation.
  • The program will run some more. Hopefully you will get the message 'GERBER FILE GENERATED - filename.GTL'. The GTL file is the Gerber file for the top layer. I need this file to make the PC board.
Generate the Gerber File "filename.GM2" (the Board Outline Layer As Described Above)
  • From the main menu select Options/Type of Plot/Mid Layer 2.
  • Hit 'Esc' to go back to the Main Menu.
  • Select 'Gerber Plot'.
  • 'CONFIRM PROCEED WITH GERBER PLOT?'. Answer 'Yes'.
  • 'REASSIGN DRAFT CODES?'. Answer 'No'.
  • The program will run a while and hopefully you will get the message 'GERBER FILE GENERATED - filename.GM2'.
Generate the Gerber File "filename.GBL" for the Bottom Layer
  • Select menu Options/Type of Plot/Bottom Layer.
  • Hit 'Esc' to go back to the Main Menu.
  • Select 'Gerber Plot'.
  • 'CONFIRM PROCEED WITH GERBER PLOT?'. Answer 'Yes'.
  • 'REASSIGN DRAFT CODES?'. Answer 'No'.
  • If you get the 'MATCH NOT FOUND' error described above in the Top Layer section, then handle it as indicated above.
  • The program will run a while and hopefully you will get the message 'GERBER FILE GENERATED - filename.GBL'.
Submit the Files

Now send an email to me (click here) and attach these files:

  • EasyTrax board file 'filename.PCB'.
  • NC Drill file 'filename.TXT'.
  • Top Layer file 'filename.GTL'.
  • Mid Layer 2 file 'filename.GM2'.
  • Bottom Layer file 'filename.GBL'.

In the email specify how many boards you need and any other important info.




Easyplot Standard Settings
MENU ITEM SETTING
SETUP /NC Drill Output File A:\yourfile
X Offset 0.000 inches
Y Offset 0.000 inch
Tool Table A:\STANDARD.ETL
/GERBER Output File A:\yourfile
X Offset 0.000 inches
Y Offset 0.000 inches
Aperture Table A:\STANDARD.APT
Match Oversize 5 mils
Match Undersize -5 mils
G54 off
Arc Quality off
Software Arcs 5 mils
OPTIONS Type of Plot (current layer)
Board Layer On
Pads On
Vias On
Strings On
Title Blocks On
Pad Hole Guide 40 mils
Drill HoleSymbol 100 mils
Solder Mask 0 mils
PWR/GND Mask 0 mils
Grid Type Imperial

Electronics Service Shop Home