Let's Make Robots!

Maxhirez' PICAXE board

9-29-2014: This update just adds the zip file containing the board in its current layout. Send the zip file to your favorite board house and get your own stack of boards. :) I still have a few that I am dispersing.

A week or so ago Max was trying to find a layout for a PICAXE 18 or 20 board with an L293/754410 motor driver. He was hoping for something similar to what sanc04 assembled.

After spending some time with my layout software of choice, I had to walk away for a bit because the group that works on the schematic software and the group that works on the pcb software do not communicate very well. :P What I am saying is not all of the symbols and footprints jive with respect to their pin labels. It causes connections in the pcb software to be misrouted.

Before I got hip deep in laying out the board, I hit up some of the more intelligent minds in the SB to get an opinion on my schematic. First, I am sorry I don't recall everyone that was offering advice on the board. I remember bdk6 specifically because I know he is on top of the layout/schematic/design game. :) bdk6 suggested 3 extra capacitors and jumpers to allow for use of external power for the 3 pin headers attached to Port B. He also suggested that the option be split between the 8 connections half and half.

PICAXE 20m2 L293 schematic
The above image can be clicked for a full size image.

What you see above is what I came up with. I did make a few adjustments after I started laying it out in the pcb software, but, nothing too terribly important.

A week or so after games in Windows I jumped back on Max's board. I managed to get my symbols and footprints straightened out and moved on to actually laying out the board.

Knowing that the board might be sent off to be produced, I was hoping I could get it to fit in the 2" x 2" area that the board houses charge the least for. Success! (i think)

PICAXE20m2 L293 pcb artwork
The above image can be clicked for a full size image.

I am showing this off here to hopefully get some input as to whether or not this is a viable layout. I see no reason in wasting a board house's time to have someone tell me this board just ain't gonna cut it. (In case anyone is curious. The circles in the corners are meant to be 3mm mounting holes.)

If the above board is viable, I may consider trying to make one myself first just to see if I can.

Side note: I use gEDA and PCB for my schematics and pcb layout.

6-28-2013 Updates

sanc04 pointed out a DOH! error on my part. The board above would work, but, the motordriver would need to be inserted backwards in to the board. Not a good plan :P

Updated schematic (Click to view full sized)

Basically just moved a few traces and C3.

Updated board (Click to open full size)

Added inexpensive heatsink, screw terminals, changed the stereo jack to one from Jameco, added more spacing due to outline of screw heads. All of the resistors were changed from laying down to standing up, hence the .1" spacing. The screw terminals for the motors are optional. If they aren't installed, the labels will be visible. After a bit of finagling, I believe it will pass OSHPark DRC. There are a few bits that are pushing the limits. Namely the 4 3 pin headers at the top and the stereo jack at the edge of the board.

I didn't manage to save myself any area (poor knowledge of layout?). I did, however, get by with less copper being etched.

Any more suggestions before I actually try to have this made?

Max says there are a number of people that would want these, if they are producable. I will throw up a parts list with an attempt to source everything from Jameco for no better reason than that is where I located a couple of the components I drew up to include (heatsink, stereo jack). The holes are 3mm w/ silkscreen for 6mm heads.


U1 L293DNE $2.95 Jameco PN 1341966


$3.20 RobotShop PN RB-Pic-31
U3 7805 $0.29 Jameco PN 51262

(optional) 2940 $1.55 Jameco PN 897381

$0.29 Jameco PN 326596

R1, R5 2.2k 1/4W (minimum purchase 10) $0.99 Jameco PN 690945

R2 22k 1/4W (minimum purchase 10) $0.99 Jameco PN 691180

R3, R4, R6 10k 1/4W (minimum purchase 10) $0.99 Jameco PN 691104

C1 .33 uF $0.32 Jameco PN 33523

C2 – C4 .1 uF $1.17 Jameco PN 33488

C5 1000 uF $0.25 Jameco PN 30015

Q1, Q2 2N2222 (minimum purchase 10) $0.70 Jameco PN 178512

CONN 1 Screw terminal $0.39 Jameco PN 2094506

CONN 2, 3 2 x 2 pin headers

(optional) Screw terminals $0.78 Jameco PN 2094506

CONN 4 Stereo Jack $1.49 Jameco PN 2095437

DIP 16 socket (minimum purchase 10) $2.00 Jameco PN 112222

$0.75 Jameco PN 37402

DIP 20 socket (minimum purchase 10) $1.70 Jameco PN 112248

$0.85 Jameco PN 38623

Headers 2 x 40 position header strips $1.50 Jameco PN 160882

Base total No options No PICAXE $16.02

All Options No PICAXE $15.96

No shipping costs are included in the above Parts list. I would imagine most of the parts are already in ones parts bins. The transistors could be swapped for 2n3904s, I believe. I am sure the smart people around here can suggest capacitor ranges. I am sure you can mix and match parts to come in under $16 + PICAXE, board, and shipping. I just checked Jameco shipping. I managed to get the price to $14.73 + $7.90 shipping.

One thing I am extremely concerned about is whether or not I read the drawing correctly for the stereo jack. I don't imagine the jack can be plugged in to the other side of the board. :P Either that or I just got the dimensions all kinds of wrong, and, it will be more like a square peg in a round hole.


07-03-2013 UPDATE

After deciding to go to a double sided board and talking to Dan M, I spun some mods into the original plan.

MaxBoard rev2 
Click image for full size version

 I added jumpers on the 4 lines that were originally hardwired to the motor driver. A jumper was installed between the stereo jack and the Serial Out pin. I increased the thickness of the line that goes to the motor driver. Also, obviously, I made the top layer a power plane to cut down on some of the power runs. 

I welcome any comments. I would like critiques on anything anyone thinks should be changed or modified.

It seems the top layer being 5V is a phenominally bad idea. :) There was mention of the makings of a plate capacitor. Worse yet MarkusB offered that a small scratch in the solder mask under the heatsink could be really bad too.

There were more calls for a shield like setup. Either way I will have to do a bit of rerouting. I will update this in a few days.

Ok, I lied. After a nap I converted the top layer to a second ground plane, and, increased the thickness of the traces that feed the motors.

Click for larger image

Update 9-25-2013

I made a mess of things not once, but, twice. The artwork above has two major issues and a minor one.

  1. The footprints for all of the headers are SIP footprints. SIP pins are the size of IC pins and not the nearly 1mm required to allow the headers to fit.
  2. The footprint for the stereo jack has holes that are about 1/3 the size they need to be.
  3. The footprint I used for the "big" electrolytic at the Vreg was too small when compared to the actual capacitor I have.

Click image for larger version

All of that means that the beautiful, purple OSHPark boards I have, won't work. At all.

Skip ahead a month, or, back a few days ago based on the date of this update. I received my next set of boards from SeeedStudio after first forgetting to add an outline, then not making a completely closed outline. Doh!

Click image for larger version

Mail comes and a box with a stack of pretty green boards from Seeed. I start looking them over. Test fitting a few parts. Then I look at the bottom side. It is solid green. Where are the traces, I think to myself. Maybe they are hidden under the soldermask. Out comes the DVM. No conectivity between pins. WTH?!?

I go back and look at the artwork I sent them. The gerber layer labeled bottom by gEDA is not the same type of layer as the one labeled top. The top layer is what you would expect with all the connections that one has made on the top layer of their board. The one labeled bottom is only the annular rings. There are no traces. Looking at a different form of export I found that the layer labeled group1 is the layer I needed to include and label as the bottom layer.

So, I have updated some things. I increased the size of most all of the annular rings. I was not happy with their size on my second set of unusable boards. Increasing their size required me to shrink the size of the motor leads where it passes between the motor driver pins. The new boards were ordered( re-ordered :P ) today. I will see if I can get Max' board to him before he dies of old age. :P

Only bonus to all this messing is that I am learning what mistakes to not make again. :)

Dropbox link to the ps file for anyone that wants to try printing one of these at home. I am not sure how easy it would be. there are some 10 mil traces. The only reason it is double sided is to let me run power from the input to the motors.

MaxBoard-rev2.zip76.51 KB

Comment viewing options

Select your preferred way to display the comments and click "Save settings" to activate your changes.

How can i add L293 IC TO TO PICAXE 28X1 BORAD?

Please correct me if i am wrong.....

Firstly, the output from the 7805 ie. the +5 volt trace is going  through junctions J1, J, J3, J4 fine till now but between J4 and R it is splitting into two one to picaxe's first pin and the other trace is going to the junction above the J5 where it is marked VBAT V+ but it is 5v? same below J12 and the same trace is then going to L923d's 8th pin which is motor power input pin. so are you going to run the motors with the same 5v supply used to power the picaxe?

Secondly, the battery + voltage trace near the top left corner of the board below the 7805 is going straight to the 16th pin of the L293d whch is the power input for the logic circuitry and the datasheet recommends it to be less than 7 volts but usually it is given the same +5 volts on which microcontroller is running. So what i think is you have placed L293d 180 degrees rotated cause then the VBAT will go to the 8th pin and the +5 volt will go to the 16th pin. 

I misunderstood/misread the L293 pinout. I will work on getting the power connections straightened out.

Re: your first comment. The silkscreen is wrong. :)

I'm with Markus and his sentiments with the > 0.1" cap pitches. I don't like the BJT inverters cuz howz u gunna break??? j/k nifty idea. I also like terminal blocks for motor connections; just easier. I found these guys are smaller than the usual beast and will handle most AWGs used...


Shrink it to 50x50mm and it will be ready for cheap-o Chinese bulk fab as well!

Some recommandations, bird:

No footprint for capacitors? Pin spacing of the cap's too large. Normally 100 mil for such small ceramic and electrolytic. They are standing not stable if you use so long leads. Add polarity symbols for the electrolytic capacitors as well. Move the voltage regulator a bit down and to the right so a heat sink can be added and do not interference with the mounting hole. Screw terminal instead of male pin header for battery connection. Instead of "-" use "GND", instead of "+" use the recommanded positive operating voltage. The right top mounting hole is too close to the audio jack. Keep in mind that the screw heads are bigger than the screw threads :)


The footprints that I called out and can be seen are just kind of generic footprints for 300mil components. I used them because I really have not looked at what parts I would suggest using. I didn't even think about C5 being an electrolytic until I looked it up the other day. The electrolytic footprints do have polarization marks on the silkscreen.

I was hoping that having the vreg up top would allow for space to let the heatsink to hang off the back of the board.

Battery connection: I labeled them with + and - to begin with because I wasn't thinking about how much space I had for actual text there. Screw terminals? I will look for the footprint for those. They do make more sense considering the power before the vreg is being channeled to the motor driver.

Excellent point on the audio jack. The 3mm holes are the inner points. That still probably only gives me room for a 4mm head at best. :P There is nothing that says the screw holes need to be in each corner, right?

There is plenty of space between U1 and U3, even more if you use 100 mil for the cap's. Don't let the heatsink hang off on the back of the board. One careless movement, and you'll pull out the voltage regulator like a dentist a teeth: ) The complete button surface of the heatsink should be on the PCB, so it's well supported.


Nice board, Bird. No blinkies? It looks like input 3 (pin 10) of the L293 is held high through R3? I might not know what I'm talking about. :P

pin 10 and pin 7 are treated the same way. 10/15 and 7/2 are on opposite sides of a NOT gate made up by the two resistors and the transistor.

When the IN is LOW, the transistor will be off and the OUT will be held HIGH. When the IN is HIGH, the transistor will be on and OUT will be pulled low due to the higher resistance between it and V+.

Also, blinkies and bouncies were not requested. :D

Call it Bird Board Blue and add a little bird :D