Plateau's Parallel Port Breakout Board Project

Hello, dear friends, how are you all?

Lately I have studied something about parallel breakout boards because I'm creating a CNC Unipolar Driver based on Mr Laurent's project (CNC3AX SGS L297) and thus I need a board to join all drivers and isolate the PC parallel port.

Well, here is my project (Schematic and Board) made on Eagle CAD and I would like to know opinions about it (suggestions, corrections, etc.).

Some features:

1. Totally optically isolated;
2. HC family buffers to insure compatibility with any parallel port;
3. It can control until 4 axis;
4. High speed optocouplers (6N135) to drive STEP pulses;
5. Two modules: Axis & Peripheral;
6. Contains 2 relays, 4 limit switches, 1 e-stop switch and Aux output;
7. 10 x 10 cm;
8. Centronic 36 connector;
9. Power supply isolated and protected against voltage inversion.

Many thanks and regards,

Pedro Rosa.

---

Plateau's Breakout Board

**broken link removed**



X axis CNCAX-M by Plateau

---

References

Mr Laurent's Project CNC3AX - http://cnc25.free.fr/electronique/eleclfouga.htm

Bunch of Breakout Board Projects -

http://www.embeddedtronics.com/opto.html
http://cnc4pc.com/Tech_Docs/C31R1_USER_MANUAL_REV1.pdf
**broken link removed**
http://www.guiacnc.com.br/eletronica/interface-paralela-opto-isolada/30/
http://www.guiacnc.com.br/projeto-c...adores-reles-e-sensores-para-placa-cnc3ax/60/
http://www.guiacnc.com.br/projeto-cnc3ax/cnc-ax-m-releitura-da-placa-cnc3ax/450/
http://www.thebackshed.com/cnc/images/RouterVer1.gif
http://www.imsolidstate.com/archives/636
http://forum.allaboutcircuits.com/archive/index.php/t-67725.html
http://members.shaw.ca/swstuff/bob.html
http://books.google.com.br/books?id...=onepage&q=74LS244 pull-down resistor&f=false

Run the signal from pin 18 of the HYC244N on the red layer, you can then get route all the signals from that side of the device on the top layer getting rid of 12 vias.
I do not see decoupling capacitors?
I would try and make the bottom (RED) layer as near a contiguous ground plane as possible minimising the breaks due to tracks on this layer. Doing the above will help, as would routing the 5V on the top layer only.
What voltage isolation are you after?

It looks like its a single sided board.
The red lines being wire links I assume?

So not able to do as Marc wisely suggests.

Run the signal from pin 18 of the HYC244N on the red layer, you can then get route all the signals from that side of the device on the BOTTOM layer getting rid of 12 vias.[\quote] (Corrected for you )
Blue is bottom, red is top links.

Thus if pin 18 of the 244n comes out, vias and a link is used then all the other tracks that currently have links in can travel on the blue side without several (6) links.
Many of the resistors are stood up korean style when they do not need to be.

Please review the path of the VSS on the RH side, it appears to come in, go up and around in a big loop before getting to the cap side of IC3.
Some moving of tracks/components around that psu will enable the copper to flood better and link up.
rotate c4 180.

The schematic looks like a jigsaw, can't it be drawn better with the connections included?

The whole project is about 10 years too late, parallel ports are quickly disappearing from pc's lol

BTW, Marc - take strong coffee and heavy drugs in on Monday - your going to need it

Click to expand...

First of all, many thanks Marce and Mattylad for having answered me too fast.

I've accepted a challenge to make this board and it must be single side (as Mattylad told) and can't be larger than 10 x 10 cm.

The project is a "little bit" old, but my current CNC runs through EMC2, Turbo CNC and Mach2 and all these programs don't have USB support. Furthermore, to use USB breakout board, I probably would need to program an PIC (PIC18F2550 or PIC18F4550) and buy a Mach3 license. Create the USB breakout board and program the PIC wouldn't be a problem but a Mach3 license in Brazil can be a "little" expensive.

Mattylad,

About the schematic and board layouts, I considered part of your advices and now I'm going to show some changes:

1) The Korean resistor style is to reduce the space wasted on the board;
2) I got rid of the 6 top links and they became only 1;
3) I rotated the C4 and changed the C3 from the original place (This is correct now, isn't it?);
4) I thought the "jigsaw way" of drawing was a good approach (I'm sorry).

Well, the changes below...

1) The new schematic

**broken link removed**

2) The new board

**broken link removed**

---

One more time, thank you all so much for everything.

Regards,

Pedro Rosa.

Looking OK.

The schematic looks more sensible now, identified sections etc.

If you look at the pcb, you have little segments of groundplane that, by simply moving a track a little would reach the segment at the other end.
Like stalagmites and stalagtites trying to reach each other

i.e. by r17 to under d5, from r4 to between pins 4/5, r10 to pins 7/8 and so on throughout the rest of the board.

If your going to flood it, you might as well make it connected as best it can be.

BTW, bottom RH mounting hole is not the same distance from the edges as the others?
(too close to the edge for the screw head etc).

If this is going to be hand etched then you may want to also check your spacings, the gap under the PL1 refname text looks mighty narrow as do many others.
I always found boards with lots of copper but thin spacings were hard to hand etch. leaving lots of shorts to fix.