Creating Printed Circuit Boards using EAGLE and the Roland EGX-300 Engraver

Overview

There are four stages to the PCB design and manufacturing process:

1. Design stage. Here the board is designed using EAGLE's schematic draw and board layout programs. There are special considerations based on the fact that the board will be produced on the Roland Engraver.

2. File Prep stage. Here CAD files are produced from EAGLE and other external conversion tools. The ultimate goal is HPGL (Hewlett-Packard Graphics Language) .plt files which can be sent directly to the engraver.

3. File Preview stage. At this stage, we load the HPGL CAD files into GraphicCode's free “GCPREVUE,”. This venerable PCB CAD file viewer program lets us verify that the files were outputted properly.

4. Manufacturing Stage. In this stage, the board is actually manufactured. Steps include: anchoring the blank PCB to the workspace; XY calibration of the machine to your board files and the location of the blank PCB; installation of engraving tools and drills, and Z axis calibration before each tool is used.

Let's begin!

Design Stage

We will be designing single sided PCBs with copper layer on the solder side (bottom).

Here are some considerations for board layout in EAGLE.

• Make sure all parts are on a 50 mil grid. Before you do parts placement, type GRID .05 into the command line at the top of the Board program, or, from the View menu, bring up the Grid dialog, and enter 0.05 inches.

  

  If you've accidentally placed some parts with finer grid, you can run a ULP (user language program) to reposition everything on the grid. First make sure you've set the 50 mil grid per above. Then choose File:Run, and select cmd-snap-board.ulp from the file dialog. Run the program, accepting its defaults.

• Use thick traces. 32 mils thick is a good value. You can tell the autorouter to use 32 mil traces with the "Net Classes" feature. This is available from either the Schematic or Board program; choose "Net Classes" from the Edit menu and change the default net class to 32 mils. (In the diagram below, I've also created a "power" class for traces carrying power and ground, but this isn't necessary.)

  

• Make pads larger. It's hard to solder to pads that are too small, especially since solder won't flow down into the holes (since they are not plated-through).

  EAGLE's default libraries have pads that are too small. I recommend pads 70 mils across.

  In the Engaging Computing Lab, you won't have write permissions to EAGLE's libraries. So you should copy needed library files into your own directories, modify them, and then use those libraries. Please make sure to give the copied library a different name to distinguish it from the stock factory libraries!

  From EAGLE's Control Panel, open your copy of the library. Click on the Package tool:

  

  This will bring up an Edit dialog. In the example below, I have chosen the "LED3MM" from the led.lbr library.

  

  Next, use the change tool (the little wrench). Select Diameter -> 0.07. Then click on the LED's pads to change them. (You can also specify change parameters at the command line, e.g., CHANGE DIAMETER .07 or simply CH DIA .07.)

  

  Click on the pads to change their diameter. I have also changed the pad shape to mark the cathode with a square pad. This is a standard convention for diodes (cathodes marked with a square pad). It helps you when you go to stuff your board, especially since there will not be a printed silkscreen component guide.

  Here is how the LED looks after the changes:

  

  Save the library. Now you will have to go back to the schematic program and tell it to use the new library (Library:Use ... menu choice). Finally, you may have to delete parts you are using from the factory library and replace them with the same part from your newly modified library.

• Turn off the top layer when running the Autorouter, so all traces are laid out on the bottom side of the board. Do this by choosing "n/a" as the Preferred Direction for the Top layer in the Autorouter Setup dialog. Also, set the Routing Grid to 25 mils so the autorouter has more flexibility with placement of traces:

  

• Run the Autorouter to route your board! If your board doesn't route well, make more space between the parts for the wires, and play with the position and orientation of your parts.

• Manually create pads and traces for jumpers for wires that won't route.

  Here's how my sample board looks after routing. Notice the two unrouted air-wires. One of these, from the pin labeled “Wh” of the jack in the lower left, to pin 17 of the IC, will actually be implemented with a jumper. Each of those connections has a trace leading to via hole. When stuffing the board, I'll use a jumper wire to make the connection. (For the other air-wire, the signals are connected but EAGLE doesn't realize it.).

  

When your board design is done, we move on to the File Preparation Stage!

File Preparation Stage

1. Create Solder Side Artwork. From the EAGLE PCB program, choose File:Cam Processor. From the CAM Processor window, choose File:Open:Job. Select the gerb274x job. Click the tab to the Solder side and then click the "Process Section" button at the bottom. You don't have to process the whole job. This creates a file with a .sol (solder side) suffix.

2. Create Drill Configuration File. From the EAGLE PCB program, select File:Run... and then select drillcfg.ulp. Choose inches as the units. When done, it will create a file with a .DRL suffix, which contains tooling information (your drill diameters), e.g.:

   T01 0.024in
   T02 0.032in
   T03 0.040in
   T04 0.047in
   T05 0.066in
   

   You won't need this file directly, but it's used in the very next stage.

3. Create NC Drill File. From the EAGLE PCB program, choose File:Cam Processor. From the CAM Processor window, choose File:Open:Job. Select the excellon job. Make sure to select the Mirror checkbox. You'll be drilling from the bottom just as you're engraving from the bottom, so you need to mirror. Click on either Process Job or Process Section (there is only one section, so “process job” will do the right thing). This creates a file with a .ncd (NC Drill) suffix.

4. Create Engraver File from .sol File Use MIT web tool to create engraver path from solder side file, http://sinfor.lcs.mit.edu:8180/pcbmill/g2h. Give it your .sol file. It will return a file with a .plt suffix.

5. Create Drill Hit Files from the NCD File. Use Fred's Java program to create drill hit file(s) from NC Drill file, NCDrill.java. Download this file to your working directory and then compile it with javac NCDrill.java. Then run it with java NCDrill . This will create files with a _t01.plt, _t02.plt etc. suffix (one for each tool from your drill configuration file).

File Preview Stage

1. Load Engraver PLT File. Use GC-PREVUE's File:Import (not File Open). Choose HPGL as the file type in the pop-up window; the software will otherwise mis-recognize the file type.

2. Load the Drill Hit PLT File(s) with the same method. These files should be recognized properly by GC-PREVUE.

3. Make sure the drill files and the engraving file are superimposed properly.

4. See directions below for determining offset of your design from the XY = 0,0 origin.

Manufacturing Stage

• Anchor board to workspace. use linoleum tile spacer. use little chunks of linoleum underneath flat brackets to keep them parallel to PCB. indentations of brackets should face down on the little linoleum pieces. medium tightening with wrench.

  

• Find the engraver tool and the narrow Roland collet. The engraver should be in its case.

  

• Slide the collet over the tool. Check that you have the right collet. It should be snug. If it is loose, you have the wrong collet.

  

• Now mount the collet in the engraver. GENTLY tighten it with two wrenches, one from the top and one on collet.

• Now insert the engraver and rotate it down. Note that the brass knob turns the opposite way you'd expect. HAND-TIGHTEN the brass knob, using a wrench to hold the top of the tool (not the collet).

  

  The engraver is now installed.

• Set XY origin. Bring up the main engraving file in GC-PREVUE and note its offset from the lower left X=0, Y=0 origin. (Lower left on the screen equals front left of the machine.)

  

  From GCPREVUE, look at the "Absolute mm" coordinates. The design is at an offset of X = ~50mm, Y = 2.5mm from the real 0, 0 origin.

  So what we are going to do is:

  1. position the tool head over where we want the design to start,
  2. zero the Roland's coordinate system,
  3. back off the tool head to the offset to the design's true 0,0 origin, and
  4. re-zero the Roland's coordinate system.

  In other words, we must set the Roland's XY origin so that when the tool moves 50 mm to the right, it will hit the PCB mounted on the table.

  Move the tool to the front left corner of the PCB, and set this as the XY zero. (From the XYZ position display, hit Enter, then Enter again over Position Set XY-Axis, then Enter again over the absolute XY position display, then hit Left-Arrow and Enter to make it happen.)

  Calculate the offset required. We are looking for 50 mm in the X coordinate. Each Roland step is 0.025 mm. So 50 / 0.025 = 2000. Move the X coordinate to -2000 ticks. Similarly for the Y axis, we are looking for -2.5 mm, which is 100 ticks, so set the Y for -100.

  Now repeat the process for setting the XY origin.

  You may wish to write down the coordinates in case the tool head gets jarred and you have to re-zero. For the job I'm photographing, the absolute Roland coordinates are X=406, Y=2694.

• Set the Z origin for a trial run. Before we engrave the job, it is worth setting the engraver tool up in the air and making sure that the tool path (1) really is over the blank PCB, and (2) is not going to drive into the clamping brackets! Please note that there are actually three Z origins. These are: Z0, the surface of the part, Z2, the "UP" position, and Z1, the "DOWN" position:

  IF THERE IS ONE DIAGRAM YOU REMEMBER FROM THIS WHOLE DOCUMENT, PLEASE LET IT BE THIS ONE.
   
  <—

  
  

  It is critical to set all three of these Z origins before any tool run!

  For now, we'll set all three to a position where no harm can be done. Using the Z+ and Z- keys, move the Z axis so it is higher than the top of the jigging apparatus:

  

  Now use the keys to set the Z0 origin there. Hit Enter, choose Position Set Z-Axis, etc. First set the Z0 workpiece origin. Then set the Z1 DOWN and Z2 UP positions. When you are done, still in this menu area, Z1 and Z2 should both show zero!.

  For the photograph, I have a Z0 setting of -1207.

  When you are done, hit Menu to go back to the XYZ display. Z should now show 0, with the tool high up above the jigging.

• Set the XY speed. Hit Menu till you see the XY Speed display. Use the arrow keys to get 15 mm/s as the XY speed.

• Set the rotational tool speed, to about 2/3 of full speed (clockwise is faster).

• Do the trial run. Close the protective lid on the engraver. Bring the tool home by hitting Menu till you see Home, then hitting Enter.

  From the PC controlling the Roland, bring up an MS-DOS shell. Send your engraving file to the machine by copying it to lpt1, e.g.:

  copy yourfile.plt lpt1:

  Watch the trial run! Make sure the tool head doesn't move over anything bad.

• set the Z axes for the real engraving run.

  First, move the tool head over a portion of the board that won't be used (e.g., near the right edge). next, move the z axis down until the tool tip just touches the board. Establish this as the Z0 SURFACE origin.

  Use piece of paper to tell if the tool is down. Or use ohm meter.

  Move the tool head up about 200 ticks. Establish this as the Z2 UP position.

  Hit Menu to go to the XYZ position display, and move the tool head over beyond the edge of the PCB. Move Z down until it's just below the surface origin, at position -10.

  Now determine if this is going to be a good depth for engraving. Close the safety shield and press the button to turn on the spindle. Turn the speed knob about 2/3 of the way up.

  Now manually move the cutter into the board, engraving about a 1/4" long groove. Move the cutter up, then turn off the spindle and move the tool head out of the way.

  Examine the groove! It should be just under the depth of the copper. The copper should be fully removed, but you don't want to be digging too far down into the phenolic substrate, or the cut will be too wide and too much of the pads or lines will be removed.

  If the cut is too shallow, move the Z axis down (say to -15) and try again.

  If the cut is too deep, move the Z axis up and try again. If you need to go "above 0" to get a good cut, then the Z0 point is set too low, so you'll have to re-establish that. If you change the Z0, make sure to re-establish the Z2 UP position also.

  When you have a good depth for cutting, establish it for the Z1 DOWN position.

• do the run! Move the tool head home, close the shield, and copy the engraving file to the machine!

  Make sure to watch. If anything goes wrong, please be ready to hit the red EMERGENCY STOP button.

  If it all works out, you should be rewarded with a nicely engraved board, all of the traces isolated but not cut too deep:

  

• Drilling, and a tool change! Now we're going to remove the engraving tool and collet, and replace it with the collet and adapter for 1/8" shank drills.

  First unscrew the engraver. The knob turns clockwise and the wrench goes counter-clockwise, backward to how you'd expect. use the wrench to hold the top of the tool hand, and your fingers on the brass knob:

  

  Please put the engraver back into its plastic tube.

• Next remove the collet. Use a wrench at the top and a wrench at the bottom. Turn as you'd expect.

• Now, get the 1/4" collet with 1/8" adapter:

  

• Insert the 1/8" adapter flush into the collet:

  

• Now screw this up into the tool head. Just hand-tighten; you'll be wrench-tightening when the drills are installed.

• Install the drill. The standard size drill is the 1/32" drill, which is 0.031" or 31 mils. We'll use this for EAGLE's standard 32 mil component holes.

  Get the drill. Be gentle—they break easily! It looks like this:

  

  The red plastic shield protects the cutting end.

  Now at the engraving machine, position the tool head over some unused area of your PC board. Move the Z axis up so that you can get the drill into position. Now, still holding the drill, lower the Z axis so that most of the drill shank is up into the collet. You have not tightened anything down yet! It should look like this:

  

  Now, tighten down. This is the only time you have to really apply elbow grease.

  Next, before moving the tool head, establish the Z0 SURFACE as here.

• Move the Z axis up about 200 ticks and establish that at the Z2 UP position.

• Now go back to the XYZ display and move the tool head over beyond the edge of the PCB and the linoleum mat. We have to establish the Z DOWN position fully through the PCB and a little into the linoleum mat. With the drill just to the side of the linoleum, move the tool down until the tip of the bit is just below the linoleum:

  

  I get a Z DOWN value of -300. Establish this via the menu keys.

  Next, move the tool up and tighten the drill some more. You have to really crank it.

• Do the drilling! Copy the plt file corresponding to the 32 mil drill to the engraver and watch it go!

  Note: if the drill is not sufficiently tightened, it will get pushed up into the collet!!! If this happens, stop the job as soon as you notice it. Follow the procedure below (for drill changes without recalibrating). Then re-run the drill job.

• Repeat with additional drills. If you follow the below procedure, you won't have to re-establish the Z origins.

  First, move the tool head over an unused portion of your PCB, and move the head up. Loosen the collet. Remove the old drill and put it away.

  With the collet still loose, insert the new drill. Move the tool head down to exactly the Z = 0 position. The drill tip should be touching the PCB surface as the tool head slides down onto it.

  With the tool head at Z = 0 and the drill tip resting on the PCB surface, tighten down. Now the Z0 tool surface position is re-established, and Z1 and Z2 don't need to change.

  Move the tool head up and tighten some more. Then send the plt file for your new drill!

• Cut out the board. For now, reinstall the engraver and manually engrave some guidelines, across the whole extent of the PCB if possible. Then remove the board from the machine, hold it on a tabletop with the engraved edge just at the end of the table, and use the palm of your hand to strike the board, snapping it at the engraved line.