| Back to Synth DIY home |
|
Notes on using the Easytrax PCB layout CAD software
|
| The purpose of this page is to provide some information about using the Easytrax software package. It is not intended to be a complete tutorial or user's guide. Rather it contains some knowledge and information I learned that was not obvious to me when first starting out, or that did not seem to be available on the web. I will try to add to this page as time permits, I hope you find it useful. |
|
Creating Aperature files The aperature file is a holdover from the days when PCB layouts were created with photo plotters. These plotters would shine light through a movable head onto a photosensitive sheet, thus tracing the shape of the PCB layer onto the sheet. The light was shined through various preset aperature shapes and the aperature file was used to specify these shapes. It's all done by computer now of course, but the aperature files remain. The aperature file is referenced by Easyplot when creating the Gerber output files that represent the layout contained in your EasyEdit .pcb file. A correctly sized aperature will need to be specified in the aperature file for each size of track and pad that appears in the .pcb file. If your .pcb file contains an element that can't be made with an element from the aperature file, the Easyplot program will complain when you try to make your Gerber files and will request you to specify a substitute aperature. It's better to fix the aperature file instead, so that all of your aperatures are explicitly defined. I use a freeware program called Traxan to automatically create an aperature text file (.apt file) from an Easytrax .pcb file. (Note: I am not the author of Traxan and do not support it or warrant it in any way!) If a solder mask will be created for the PC board, then additional corresponding aperatures will need to be specified in the .apt file. These new aperatures can be added by hand-editing the Traxan-created .apt file with a text editor. Make a copy of the aperatures listed in the file and paste the copy at the end of the file. Then modify the copied lines to have new D numbers, and add the size of the solder mask width to the first and second columns of numbers. Here's an example with three aperatures (to begin with) and a solder mask width of 16 mils:
D10 CIRCULAR 5 5 0
D13 CIRCULAR 21 21 0 Note that when setting a solder mask enlargement in Easyplot (Options->Solder Mask Enlargement from the main menu), a radius is specified. So for the example above, an 8 would be entered for the Easyplot option (half of 16). |
| About Drill Holes: |
|
EasyEdit itself has no notion of drill hole sizes as far as I am aware.
Specifying drill holes for your board involves a somewhat arcane process
that I will attempt to describe below. In addition to making gerber files, EasyPlot (not EasyEdit) is used to make the "drill file", which is the CAD file that the PCB manufacturer uses to drill the holes in your boards. The "NC Drill" option on the main menu of EasyPlot is used to make the drill file. The drill file produced by EasyPlot ends in .txt and is an ascii file. When making the drill file, EasyPlot cross-references the pads used in your .pcb file with a list of pads contained in another file to determine what drill sizes to use. This other file is the ".etl" file, also called the tool file. The default .etl file used by EasyPlot is "standard.etl" in your easytrax directory. If you wish, you can specify a different .etl file in EasyPlot using the "Setup->NC Drill->Tool Table" option. Here's a sample of a few lines from a .etl file:
ROUND40 T01 23 The first column contains pad sizes. The entries in this column correspond to the pad sizes you can select in EasyEdit. The second column contains tool numbers. This corresponds to a drill tool located in the manufacturer's drilling machine. The third column is the drill size for each tool, in thousandths of an inch. The result of all this is that, according to the example .etl file above, anywhere you place a ROUND40 pad in your .pcb file, the drilling machine should drill a hole using Tool 1, which is a .023" diameter drill. Anywhere you place a ROUND50 pad, the drilling machine should use Tool 2 to drill the hole, which is a .028" diameter drill, etc. When EasyPlot is making your drill file, it will look at the first column in the .etl file to find the pad size, and will write out all the drill hits that correspond to that pad size by issuing the tool number and x,y coordinates of each hit to the output drill file. The actual drill size (the number in the third column) is not specified anywhere in the drill file, only the tool numbers and x,y coordinates of the drill holes are stored. For this reason you will need to tell your manufacturer what drill size corresponds to each tool number. Just sending them the .etl file is usually sufficient. Ultimately you will probably want to make your own .etl file (use a text editor). Keep the following four things in mind when doing so: 1) Once you specify T04 to be a .042 drill bit, then T04 must always be a .042 drill bit. In other words, the following is illegal:
ROUND70 T04 35 Just imagine that T04 (or T01 or whatever) is an actual drill bit sitting in a machine somewhere, and it can't be two different sizes at the same time. 2) There is a limit to how large your drill size can be in relation to the pad size. Your manufacturer will specify a minimum "annular ring", which is the amount of conductive pad material that must surround the drill hole. In other words, it's the distance between the edge of the drill hole and the outer edge of the pad itself. So, if the annular ring spec. is 10 thousandths, then the largest drill you could specify for a 70 thousandths pad is 70 - (10 * 2 ) or 50 thousandths. 3) When using EasyEdit/EasyPlot to make your PCB, you have to think about your pad size usage in advance because only one drill hole size can be specified per pad size. This means that if you design 99% of your board and then realize that you simply must have some ROUND70 pads with .035" holes and some others with .042" holes; you're in trouble. Gather all your parts in advance, figure out their lead sizes and pad size requirements, and plan your pad/hole usage accordingly. 4) When computing your hole sizes, remember that you are specifying the raw drilled hole size. The hole diameter will shrink from 3 to 5 thousandths when the holes are plated with metal, so be sure your holes are large enough to fit your component leads plus a 5 to 10 thousandths "slop factor".
|