first attempt at pcb for picaxe circuit

B

barneydog

Member
Hi,

Hopefully one day i might actually be able to help people and answer questions rather than always asking them and taking up your time :eek:

I built a indicator circuit for one of my model trucks. I have it working on strip board, and now i want to attempt getting it onto pcb.

I have designed the pcb layout, and just wondered if one of you would mind checking it for me, and seeing if it looks ok....more component placement and routing.....



ch1 - RC reciever channel 1 - one push up makes all 4 leds flash (hazard lights)
ch2 - RC reciever channel 2 - steer left/left leds - steer right/right leds
Servo - To the steering servo...

resistor near picaxe is a 10K serial one (i remembered :) )
other 2 are for the leds and are 56k

I decided to connect off the board as i have a load of extension cables i can cut in half rather than use Y cables.

hope this makes sense... and i really appreciate any comments good or bad

thanks :cool:
 
Last edited:
hippy

hippy

Technical Support
Staff member
The things I'd suggest are -

Rotating the 08M so you can more easily lever it out to program. Possibly easiest to do with notch to the bottom.

Add a decoupling capacitor.

Possibly add a power-on LED+R so you know when the board is 'live'.
 
J

John O

Senior Member
What method are you using to make the PCB? Tracks between IC pins can be a bit hairy to do.

John.
 
J

JoeFromOzarks

Senior Member
I normally use DipTrace. MS Paint is way above my paygrade and way above my artistic abilities. (grin)

Looks like to me, the PicAxe 08m (?) isn’t getting any power unless CH1 is on. If CH2 is on, you’re feeding Leg-6 with a signal without V+ to the PicAxe if CH1 is off.

I’d add a bypass cap across the PicAxe power pins and a healthy electrolytic too.

Is the servo transmitter (CH1) putting out 5VDC constant for the PicAxe? (My back is screaming today – my brain isn’t cookin’ on all cylinders, sorry if I’m missing something obvious!)

I think you’ll be much happier with successful traces if you round the corners. A 90 degree turn can etch away in the inside corner where a 45 degree has a better shot of etching away intact. In other words, off PicAxe leg 4 you have three 90’s (not good) – on PicAxe leg 3 you have a three 45’s (better!) I’d also fill in the corners on the “T” below Legs 5 and 6 and the other “T” above Leg 8.

I’d also make the traces as thick (wide) as possible everywhere you can, leaving the traces that pass between pins (legs) narrow(er). Depending on your PCB making methods, running traces between IC Pins/Legs might make you insane.

:) joe
 

Attachments

J

John West

Senior Member
Not essentially a part of the bd layout, but I'd suggest you mount the PICAXE on a machined pin socket for reliability. They are more expensive than other types of sockets, but are more reliable.

Another concern is how you intend to mount the bd. I see no mounting screw holes.

P.S. We're all still learning about all this. Some of us are just learning faster as we try to catch up with the more experienced.
 
Last edited:
J

John O

Senior Member
As joe said, make tracks as thick as possible. The bottom (-) track is essentially Ground so you may as well extend that right round the board perimeter. If nothing else, etching away as little copper as possible will make your etching solution last much longer.

John.
 
B

barneydog

Member
hi thanks for the advice and tips...

the RX power is always on running through a bec at 5v... its only the signal that ever changes...i should have mentioned that and been more thoughtful lol..


the board will be covered in heatshrink, except for the led plugs which may need to be accessed so leaving them open... other end for channels and servo will be leads coming out so a case of just plug into any truck i choose.

im using a picaxe 08 for now.

what would the bypass caps and electrolyte do? and what values would be required... would this be classed as decoupling also as hippy stated ? (still none the wiser what it is...)

rotating the picaxe i have had it every which way, and with the routes that was the only way nothing crossed over...I used pcb wizard to design it and its auto routing facility... I did think of placing a ground plane on there going around the whole edge of board to save having to many tracks running and crossing about..

method to make pcb... will print out image onto blue sheets i got from ebay designed to make pcb boards (i hope), iron onto copper board, places in etching solution, clean off, cover tracks in a pcb lacquer once all components are placed (i think i do that after soldering)

hope i got and responded to everyones points and bits
 
hippy

hippy

Technical Support
Staff member
barneydog said:
rotating the picaxe i have had it every which way, and with the routes that was the only way nothing crossed over
Click to expand...
Don't forget that the beauty of PICAXE is that you can move I/O to different pins ...

And with a bit more effort could probably get what you already have :)
 

Attachments

B

barneydog

Member
yes very good post.. not only had a giggle mainly at dippy's posts... but learnt something new...

so to clarify...

+V - 0V --- Ceramic cap around 100n

then by diagram i think dippy placed, place a electrolyte around 10n.. in the same situation.

does it matter which way you place them in the circuit ?
 
B

barneydog

Member
i did forget about swapping pins !!!!!!

back to drawing board....

points going to be adding

  1. wider tracks
  2. change pins where needed
  3. decoupler/bypass filters
  4. source head ache tablets
  5. no nipping through IC legs!!!!!!
 
B

barneydog

Member
here is an updated board




i tried to follow everything advised, and i think i got it all...

making the bends thicker the software has no option, so all i can do is use pcb pen to add that once on the copper board
 
hippy

hippy

Technical Support
Staff member
That bend next to pin 7 looks mighty close. Perhaps lose that connection as it's a loop of 0V anyway.
 
B

barneydog

Member



was trying to keep lots of grounds... not for any particular reason...had the space on remaining board so popped them in
 
J

jaka

Member
What caps are you using. Most poly's are 0.2.

Disc ceramic would probably fit but a poly would possibly hit the 8 pin base.

Also the electrolytic looks a bit close to the 3 pin bases.

I would use a 10uf tant on its own.

Jim
 
techElder

techElder

Well-known member
barneydog, it's not going to hurt you in this circuit, but there are some circuits where you need to be careful with having extra ground current paths. More is not always better.

That looks like a real nice bit of work on that board. You'll be proud of it when you get it etched, populated, wired up and working!

barneydog said:
...was trying to keep lots of grounds... not for any particular reason...had the space on remaining board so popped them in
Click to expand...
 
J

John O

Senior Member
Texasclodhopper said:
barneydog, it's not going to hurt you in this circuit, but there are some circuits where you need to be careful with having extra ground current paths. More is not always better.

That looks like a real nice bit of work on that board. You'll be proud of it when you get it etched, populated, wired up and working!
Click to expand...
Yes, I agree. It's usually best to avoid circular paths. If it were me, I'd remove the track between pin 8 and the resistor. You could then centralize the loop between pin 2 and the resistor which is currently quite close to pin 3.

John.
 
J

JoeFromOzarks

Senior Member
Texasclodhopper and John O are correct, that ground thing you have going is a nice looking EMI/RFI antenna.

Also, since the .01 ceramic is a small beast, you might get away with putting it right next to the PicAxe socket Legs 1 and 8, allowing more room for say, oh, a 220uF 16V electrolytic where the two caps currently reside.

Many times, I will put a Pad just outside the V+ Leg and another just outside the 0V Leg and solder the .01 bypass on the trace side of the board, after mounting the socket for the PicAxe. Might look goofy, but gets the bypass as close as possible to the IC and might save a bit on board real estate.

:) joe
 
Last edited:
B

barneydog

Member
some more brilliant ideas....

as for capacitors the software im using they are the smallest it has on offer... have printed it out and the ones i have here are a lot smaller than the print out...

everything else fits fine...

i did see someone say about the 3 blocks at the end... they wont be blocks the servo plugs will be wired straight to the board, as thats going to be easier and save some space. i used the blocks in the file to show out whats what and understand what i was doing....

similar with the other end, they arent block connectors they will be the connectors tamiya use on their MFU modules.. i think they call them jst2 2 pin connectors.. i cant find the pack right now to be precise.
http://www.robotshop.com/Images/big/en/seeedstudio-jst-2-pin-power-connector.jpg

hope its ok to link, theres a picture of one... please remove link if its not ok to link to images like that...
 
J

JoeFromOzarks

Senior Member
I apologize, I became carried away with my keyboard, keypress happy.

Let me flap my gums even more…

I usually place the bypass cap as physically close to the IC’s power pins as possible. Sometimes, that is soldered on the bottom of the board.

But on your PCB, moving the bypass closer to the PicAxe Legs 1 & 8 would save some board space and give you a bit more space for the electrolytic AND keep the bypass traces as short as possible. Keeping those bypass traces short was my original point to make.

Servo’s and motors and many other components we connect to PicAxe pins can generate unwanted noise. Noise in the power supply rails (PCB traces) and back into the signal pins of semiconductors may cause unexpected results. Sometimes, we can be a little sloppy with layout, but usually it’s just best to stick with the rules and allow those rules to become second nature. Forrest Gump said “one less thing to worry about…”

:) joe
 
B

barneydog

Member
sorry for not posting back and letting you know how the boards where coming along!!

lost the net for the last 4 weeks... damn internet company!

over next couple of days i will post pics and show you how well they came out :D

very very pleased with them!
 
J

John West

Senior Member
I'm sure your bd will work just fine, but as a further suggestion for future projects, set the trace width in your CAD program to a bit wider than you used on this one, especially for ground traces.

That adds to the circuit's current handling capacity and reduces voltage drop, as well as providing a significant bit of further mechanical strength to the connections themselves, an important and oft overlooked feature. I've seen many bd failures due to broken tiny traces at component connection points. Mechanical stresses due to component mass or connector pressures are important circuit design considerations, especially in circuits that are used in mobile devices.

Unless there is a need to maintain proper clearances between traces, the bigger the pads and the wider the traces, the better.

Plus, it's just that much less etchant that gets used, and that much less contamination that gets tossed out into the environment.
 
Last edited:
G

Grogster

Senior Member
It is a very good idea to put the programming circuit on every board - I do this by default, even if I think I might not need it - it makes life much easier to be able to program the chip on-board without having to remove it...

I also am a big fan of using a ground-plane on every board, as this makes etching faster, as there is not as much copper to remove.

There are cases when you don't use one, such as switching mains - you do NOT want an arc-over!!! :p

The attached board is just a simple serial message generator using the 08M and the ground plane concept - see how quick it would be to etch based on the fact there is not much copper to remove?

This particular board does not actually use the ground-plane(there is no ground connection to it) for two reasons: (1) I forgot to do it at the time!(all new boards use a ground-connected ground-plane by default) and (2) in this application, it does not really matter.
 

Attachments

Last edited:
S

srnet

Senior Member
Why the 0.2" spacing on the RC and servo connectors ?

I would be using the standard 0.1" pitch, smaller, and directly plug compatible with RC servos.
 
B

barneydog

Member
excellent advice thank you...

first set i etched are in pics





they didnt come out to bad... and ones with out the X through them all worked...

since these i have made some more....which all work fine

but now im off to update the design to match the advice you have given me.

larger tracks, pads, and put a ground plane in.

sounds really good ideas!

when i soldered a few of them i did get breaks. but easily fixed...now is the time to stop the breaks from happening again!

the boards only carry minimal mA and 5v from an RC receiver, and if higher drain is needed then its taken from a seperate supply connected by a MOSFET switched by the receiver.

Im pleased i have managed to design, etch, and make the board... and it worked!!!
 
B

barneydog

Member
forgot to add

heres the finished thing just before it went into truck. this was the 2nd set of board designs..much smaller than the first.. but i dont have any i can take a pic and show you

 
J

John O

Senior Member
Looks good :)

I'd cut the overall PCB to size before you etch though. All that unwanted copper area etched away just unnecessarily depletes your etching solution. And all those off-cuts can come in handy :)

If it takes less than 40 minutes to etch the board, the solution's too strong, risks undercutting the tracks and gives feathered edges. If it takes more than about 90 minutes, the solution is pretty-well on its way out!

John.
 
B

barneydog

Member
thanks again...

first lot took about 20 mins so i had that way to strong!

second lot about 1 hour....

i never thought about cutting them out prior to etching... i could have got many more boards lol

need to get some more boards and also some more etching balls...

and will try again using all the methods you have taught me here...
 
You must log in or register to reply here.
Top