Searching \ for '[PIC] My First PIC Development Board PCB Design' in subject line. ()
Make payments with PayPal - it's fast, free and secure! Help us get a faster server
FAQ page: massmind.org/techref/pcbs.htm?key=pcb
Search entire site for: 'My First PIC Development Board PCB Design'.

Exact match. Not showing close matches.
PICList Thread
'[PIC] My First PIC Development Board PCB Design'
2009\01\31@214041 by solarwind

picon face
omploader.org/vMTcyaA

Here it is. Created with FreePCB. I did not pirate anything -.-

In the socket will fit a 28 pin DIP holder for my PIC 16F886 or 18F2620

Is it an OK design? Can anyone spot anything wrong? Are the traces too thin?

This will be for homebrew PCB making by the way (using toner transfer
and FeCl etching).

--
solarwind

2009\01\31@221231 by solarwind

picon face
On Sat, Jan 31, 2009 at 9:40 PM, solarwind <spam_OUTx.solarwind.xTakeThisOuTspamgmail.com> wrote:
> http://omploader.org/vMTcyaA
>
> Here it is. Created with FreePCB. I did not pirate anything -.-
>
> In the socket will fit a 28 pin DIP holder for my PIC 16F886 or 18F2620
>
> Is it an OK design? Can anyone spot anything wrong? Are the traces too thin?
>
> This will be for homebrew PCB making by the way (using toner transfer
> and FeCl etching).
>
> --
> solarwind

Update, routing done by autorouter

http://omploader.org/vMTcybA

Left: my hand routing           Right: autorouter



--
solarwind

2009\01\31@223148 by gardenyu

picon face
part 1 722 bytes content-type:text/plain; charset="gb2312" (decoded quoted-printable)


Don't make 90 degree turn path for signals.
Always use 45 degree whereever possible.

{Quote hidden}

> --!

2009\01\31@223913 by solarwind

picon face
On Sat, Jan 31, 2009 at 10:31 PM, gardenyu <.....gardenyu2004KILLspamspam.....hotmail.com> wrote:
>
> Don't make 90 degree turn path for signals.
>
> Always use 45 degree whereever possible.

Yep :)

In my updated post: http://omploader.org/vMTcybA the freerouter did all that.

--
solarwind

2009\01\31@230938 by Ray Newman

picon
part 1 730 bytes content-type:text/plain; charset="us-ascii" (decoded quoted-printable)

Try to use only 45 degree trace.
Try to place only one trace between dip pins. (use zero ohm jumper to free up space)
Center trace between pins.
Don't crowd lines. If you have space, spread them out.
Ray



On Sat, 31 Jan 2009 21:40:40 -0500, solarwind wrote:
{Quote hidden}


part 2 35 bytes content-type:text/plain; charset="us-ascii"
(decoded 7bit)


'[PIC] My First PIC Development Board PCB Design'
2009\02\01@000949 by William \Chops\ Westfield
face picon face

On Jan 31, 2009, at 6:40 PM, solarwind wrote:

> Is it an OK design? Can anyone spot anything wrong? Are the traces  
> too thin?

You will have trouble trying to get two traces between 0.1inch pins  
using toner transfer and hand drilling...  The fact that it looks ok  
in the drawing probably means your tracks ARE too thin.

BillW

2009\02\01@002723 by solarwind

picon face
On Sun, Feb 1, 2009 at 12:09 AM, William Chops Westfield <EraseMEwestfwspam_OUTspamTakeThisOuTmac.com> wrote:
>
> On Jan 31, 2009, at 6:40 PM, solarwind wrote:
>
>> Is it an OK design? Can anyone spot anything wrong? Are the traces
>> too thin?
>
> You will have trouble trying to get two traces between 0.1inch pins
> using toner transfer and hand drilling...  The fact that it looks ok
> in the drawing probably means your tracks ARE too thin.
>
> BillW

Unfortunately, this is the ONLY way to get my design on a single layer
PCB with the layout that I want. The autorouter verified this. But
people have had success doing 0.5 mm pitch TQFP so the two traces
between the two dip holes shouldn't be THAT bad... And I could always
flood that part with a marker and use a knife to cut the spaces if i
absolutely have to. And I can get this trace drawing pen at my local
electronics hobby shop that lets you draw very thin traces with
conducive ink I think it was...

--
solarwind

2009\02\01@003910 by Tony Vandiver

flavicon
face
If you're going to etch this, the bigger the traces, and wider the
spaces, the better.  Wherever possible, I'd go with at least a 25mil
trace/space, and where not, just neck down in the particular trouble
area.  Take U10 and rotate it 90deg CC and move it under the dip so that
you could move the headers in toward the chip and make extra room on the
outside of the headers for better spacing, or if you have to have the
headers where they are to match something, make the board bigger.  The
auto-router has made traces arbitrarily close, and you might be able to
fix that just by changing the design rules to force a larger spacing.  
Wouldn't hurt to have decoupling capacitors close to all power/ground
combinations on the chip.  I'm also guessing that you'ld mirror this
design to put the traces on the back side of the board so that you don't
have to try and solder a dip or headers to pads that are hidden by the
components?  You can also save a little headache by filling dead areas
with copper so that you don't have to etch away most of the board area.  
When you're starting, the autorouter can give you ideas that you might
not come up with just looking at the board, but in general most are crap
that will lead you in the wrong direction so given what the autorouter
has produced, you might try again by hand.  Also, there are probably
remappable pins that could give you an edge that the autorouter doesn't
have.  When you get to a point in the layout where it just seems like it
would be alot easier if this pin went here instead of there, don't
hesitate to rewrite the code to support a better layout.  That's one of
the great advantages of designing a board that you also write the
firmware for : you aren't stuck with the schematic as handed to you by
some other design engineer.

Thanks,

Tony




solarwind wrote:
{Quote hidden}

2009\02\01@004948 by Forrest W. Christian

flavicon
face
William "Chops" Westfield wrote:
> You will have trouble trying to get two traces between 0.1inch pins  
> using toner transfer and hand drilling...  The fact that it looks ok  
> in the drawing probably means your tracks ARE too thin.
>  
I agree the tracks are way too thin..   Especially if two will fit
between dip pins.   Heck, fitting *one* beween dip pins can be a
challenge when doing it by hand.

-forrest

2009\02\01@013531 by Bob Blick

face
flavicon
face
solarwind wrote:

> Unfortunately, this is the ONLY way to get my design on a single layer
> PCB with the layout that I want. The autorouter verified this. But
> people have had success doing 0.5 mm pitch TQFP so the two traces
> between the two dip holes shouldn't be THAT bad... And I could always
> flood that part with a marker and use a knife to cut the spaces if i
> absolutely have to. And I can get this trace drawing pen at my local
> electronics hobby shop that lets you draw very thin traces with
> conducive ink I think it was...

OK, let's look at what this would take. Say your IC pads are 60 mils on
100 mil centers. That leaves 40 mils space between them. If you put two
tracks between them with equal spacing that's 8 mil tracks with 8 mil
space (called 8/8 in the business). That's about the best you can get at
budget board houses before you have to pay a premium. But when I do a
toner transfer board in my kitchen, I consider the minimum to be 12/12.
So I can get one track between IC pins.

I'm not saying you can't do two tracks, but you will have to be very
very good about your ironing. You need just the right temperature and
extremely even pressure or you will get some fat areas and thin areas.
For your first few boards I suggest 12/12 at very minimum.

Jumper wires are OK to use, they are not like GOTO's in C :)

Also, if you can flood fill the blank areas of the board you will use
less etchant. But don't do it unless you can set the clearance from the
flooded copper to traces and pins. For toner transfer boards I usually
set that clearance at 20 mils. Try to associate it with the ground net
if you can, then you'll have a ground plane.

Cheerful regards,

Bob

2009\02\01@021026 by Sean Breheny

face picon face
Why are you recommending avoiding 90 degree bends? Yes, for very high
frequency signals it will affect the transmission line properties of
the trace, but for what most of us do on a regular basis, it should
have no effect.

Sean


On Sat, Jan 31, 2009 at 10:31 PM, gardenyu <@spam@gardenyu2004KILLspamspamhotmail.com> wrote:
>
> Don't make 90 degree turn path for signals.
>
> Always use 45 degree whereever possible.
>

2009\02\01@030637 by solarwind

picon face
On Sun, Feb 1, 2009 at 12:38 AM, Tony Vandiver
<KILLspamtonyKILLspamspamtraceelectronics.com> wrote:
> Wouldn't hurt to have decoupling capacitors close to all power/ground
> combinations on the chip.

Will do.

> I'm also guessing that you'ld mirror this
> design to put the traces on the back side of the board so that you don't
> have to try and solder a dip or headers to pads that are hidden by the
> components?

What do you mean?

> You can also save a little headache by filling dead areas
> with copper so that you don't have to etch away most of the board area.

Gotcha.

--
solarwind

2009\02\01@030816 by solarwind

picon face
On Sun, Feb 1, 2009 at 1:35 AM, Bob Blick <RemoveMEbobblickTakeThisOuTspamftml.net> wrote:
> I'm not saying you can't do two tracks, but you will have to be very
> very good about your ironing. You need just the right temperature and
> extremely even pressure or you will get some fat areas and thin areas.
> For your first few boards I suggest 12/12 at very minimum.

Thanks. I'll try my best :)

> Jumper wires are OK to use, they are not like GOTO's in C :)

LOL!

> Also, if you can flood fill the blank areas of the board you will use
> less etchant. But don't do it unless you can set the clearance from the
> flooded copper to traces and pins. For toner transfer boards I usually
> set that clearance at 20 mils. Try to associate it with the ground net
> if you can, then you'll have a ground plane.

What's the advantage of a ground plane? I see that filling in dead
areas saves FeCl though.

--
solarwind

2009\02\01@070045 by Alan B. Pearce

face picon face
>Jumper wires are OK to use,

Especially if you need only one to remove the two tracks between pins
problem.

As to the autorouted version, it does several things that I would regard as
'unsightly layout' rather than wrong or erroneous., for example the top pin
on U9 has the two tracks join the go to the pin, where a hand laid board
would bring them into the pin separately, on each side of the connector,
more like your original layout. similar things occur in a number of places,
and while the autorouted version is not bad, I would use it as a stating
place to then manually move the traces around to remove these sorts of
artifacts.



2009\02\01@070840 by Alan B. Pearce

face picon face
>Why are you recommending avoiding 90 degree bends?
>Yes, for very high frequency signals it will affect
>the transmission line properties of the trace, but
>for what most of us do on a regular basis, it should
>have no effect.

It is generally considered bad practice for a couple of reasons.

1. The inside of the corner can be a trap point for the etchant which
doesn't get washed out properly after etching, resulting in possible
problems later. This is a point of discussion in reviews of high reliability
equipment, such as the space instruments I work on.

2. there have been problems in the past with copper peeling from the outside
of the corner. Different adhesives may have largely mitigated this problem
now, but if it is needed to solder to the track at that point, peelback is
highly likely to happen. Doesn't seem to be such a problem on a large fill
area, although it is generally still considered good practice to not leave a
square corner, rather to angle it.

2009\02\01@101201 by olin piclist

face picon face
solarwind wrote:
> http://omploader.org/vMTcyaA
>
> Here it is. Created with FreePCB. I did not pirate anything -.-
>
> In the socket will fit a 28 pin DIP holder for my PIC 16F886 or
> 18F2620
>
> Is it an OK design? Can anyone spot anything wrong? Are the traces
> too thin?

It's rather pointless to look at this without a schematic.  I don't see
obvious pads for a bypass cap and crystal load caps though.  Also, you've
got pleny of room.  I don't see why the traces need to be as thin as you
made them.


********************************************************************
Embed Inc, Littleton Massachusetts, http://www.embedinc.com/products
(978) 742-9014.  Gold level PIC consultants since 2000.

2009\02\01@102125 by olin piclist

face picon face
solarwind wrote:
> Unfortunately, this is the ONLY way to get my design on a single layer
> PCB with the layout that I want.

So use a jumper or two.

> But
> people have had success doing 0.5 mm pitch TQFP so the two traces
> between the two dip holes shouldn't be THAT bad.

You don't have a solder mask, so no, it does sound pretty bad.

********************************************************************
Embed Inc, Littleton Massachusetts, http://www.embedinc.com/products
(978) 742-9014.  Gold level PIC consultants since 2000.

2009\02\01@124737 by Bob Blick

face
flavicon
face
solarwind wrote:

>> Also, if you can flood fill the blank areas of the board you will use
>> less etchant. But don't do it unless you can set the clearance from the
>> flooded copper to traces and pins. For toner transfer boards I usually
>> set that clearance at 20 mils. Try to associate it with the ground net
>> if you can, then you'll have a ground plane.
>
> What's the advantage of a ground plane? I see that filling in dead
> areas saves FeCl though.

Anything that's not ground is an antenna, so if you have unconnected
copper it can increase crosstalk and radiated emissions.

If it is ground it can improve the routing since you no longer need
ground tracks or work your copper around them.

Generally anything that lowers the resistance of ground is a good thing.

If you walk up all charged with static and touch your board, you're more
likely to discharge to ground rather than to a sensitive part of your
circuit.

And another reason why you want copper in the empty areas:

Large empty areas tax the etchant locally so those areas will etch
slower than the rest of the board.

Cheers,

Bob

2009\02\01@131348 by Derward Myrick

picon face

----- Original Message -----
From: "Olin Lathrop" <spamBeGoneolin_piclistspamBeGonespamembedinc.com>

I don't see why the traces need to be as thin as you
made them.

Olin,  I agree with you on this.

I look at the making of PCBs different than most on the list.
I leave large traces  every where I can.  I have a Design
package that makes it easy to use any size trace you want.
Most of my design is for consumer use so the board is not
as critical as the commercial boards.  Of course when I do RF
design that changes every thing.

Derward  KD5WWI


2009\02\01@142341 by Jinx

face picon face
> Large empty areas tax the etchant locally so those areas will etch
> slower than the rest of the board.

That's very true. The first copper to be etched right through is next
to the resist, ie along the track edges. Always wondered why and I
did ask here years ago if anyone had suggestions. Might Google
later

2009\02\01@151704 by Ian Smith

flavicon
face
On Mon, 2 Feb 2009, Jinx wrote:
> That's very true. The first copper to be etched right through is next
> to the resist, ie along the track edges. Always wondered why and I
> did ask here years ago if anyone had suggestions. Might Google
> later

It makes sense to me.  If you think about a spot above a large area of
copper, once the etchant directly touching the copper is used up, more has
to come from above.  But a spot next to a trace can draw from fresh
etchant both from the top and from the side.

--
Ian Smith
http://www.ian.org

2009\02\01@155158 by solarwind

picon face
Thank you for the advice guys!

I'll increase trace width whenever I can. I'll also try out diptrace
and see if it does a better job at autorouting. And for the ground
plane, how should I fill it in? Should I print, transfer and use a
marker to colour over the blank areas? Or is there a better way?

2009\02\01@175152 by Jinx

face picon face
> The first copper to be etched right through is next to the resist

> a spot next to a trace can draw from fresh etchant both from the
> top and from the side

I guess that does make some sense. It would be on a very tiny scale
of course. Of all the configuations I've etched boards in - upsidedown,
right way up, stirred, not stirred - etching always progresses the same
way. I've got a few small identical boards to do shortly. Might experiment
with deep scratching and cross-hatching to see if it would make a large
area etch faster. Not that I'm a hurry. Taking the time to modify an area
would probably take longer than just leaving the etchant to do its work
removing all the copper from a plain area

2009\02\01@180412 by Bob Blick

face
flavicon
face
solarwind wrote:
> I'll increase trace width whenever I can. I'll also try out diptrace
> and see if it does a better job at autorouting. And for the ground
> plane, how should I fill it in? Should I print, transfer and use a
> marker to colour over the blank areas? Or is there a better way?

Most pc board layout packages will do it for you. In PADS you create a
pour outline on the correct layer, associate it with a net, and pour. It
fills according to the ruleset for copper, such as clearance from
various things like traces, pads, vias, drills, text, etc and thermal
reliefs for connections to the pour. You also get the choice of a flood
or hatch fill(with its own rules as well). These things are all in menus
or you can import text files with rules in them.

-Bob

2009\02\01@185455 by Vitaliy

flavicon
face
"solarwind" wrote:
> http://omploader.org/vMTcyaA
>
> Here it is. Created with FreePCB. I did not pirate anything -.-

Congratulations! :-) (no sarcasm)


> In the socket will fit a 28 pin DIP holder for my PIC 16F886 or 18F2620
>
> Is it an OK design? Can anyone spot anything wrong? Are the traces too
> thin?

Yes, the traces are too thin. As others have suggested, make the traces as
wide as possible. It's perfectly OK to have jumpers in a one-off design.


> This will be for homebrew PCB making by the way (using toner transfer
> and FeCl etching).

You can look at how things are done on production PCBs (done by
professionals), and try to emulate their style. My first boards also had
right angle bends, and to me the main reason for switching at the time, was
aesthetics. Right angles look ugly.

Another suggestion I have, is doing the routing by hand, especially for a
simple circuit like yours. I've done it for circuits with hundreds of
components, and we still do our PCB layouts by hand. Autorouter technology
just isn't there yet, at least not at a price that most people can afford.

Vitaliy

2009\02\01@200840 by Jinx

face picon face
> http://omploader.org/vMTcyaA

If possible, re-arrange connections to U3 to avoid going around
the outside and the through-pin @ 24/25 (it could go over the top
of 28 for example). Tracking from that position to U7 (instead of
from pin 8) would open up a little more room for traces going to U7

Move U9 and U7 down to get rid of the kinks in traces and especially
to avoid the double through-pin @ 8/9. There's unused room under
U10 for traces, and you can put jumper links under the IC. For example
a link for the pin 18 track to jump over the 0V line at pin 8. The track
from pin 18 can come out between 6/7 (if pin 8 track is re-routed to
come from the through-pin @ 25/26)

The more direct the traces, ie fewest turns, the easier it will be to make
them fatter. And for example redrawing the trace from the upper pad
of U10 to the left in an L shape would help uncramp the traces above it.
Or if U9 went down 0.2" that would be a direct horizontal connection

2009\02\01@204251 by peter green

flavicon
face

> In the socket will fit a 28 pin DIP holder for my PIC 16F886 or 18F2620
>
> Is it an OK design? Can anyone spot anything wrong? Are the traces too thin?
>  
A few comments.

(note: in this post as is conventional in the PCB industry mil reffers
to a thousanth of an inch)

You have two traces between a pair of pins, this is best avoided due to
the very small tracks and gaps required. You can fix this by moving the
trace from pin 15 of the pic to come out one pair of holes lower. Then
taking that trace through the connector and joining to the connector
round the back.

When taking a trace through between a pair of pins make sure it is
centered and try to roughly match the track size and gap size.

Also while a trace will have to be relatively small (12mil or so) to get
between dip pins that doesn't mean it should spend it's entire length at
that size. a 24mil track is much easier to wiremod and likely to etch
much more reliablly than a 12mil one so widen up to 24mil as soon as the
trace gets out of the cramed area.

As others have said here right angle corners are more prone to etch
problems than 45 degree ones so try and mitre your corners whereever
possible.

> This will be for homebrew PCB making by the way (using toner transfer
> and FeCl etching).


2009\02\02@043447 by Alan B. Pearce

face picon face
>It's perfectly OK to have jumpers in a one-off design.

It can be perfectly OK in a production design too - a video recorder that I
own failed a while back, and I dismantled it. All the PCBs are single sided,
with surface mount resistors, ceramic capacitors and ICs, and through hole
electrolytic caps, large transistors and inductors.

But what amazed me was the number of jumper wires. It is quite clear these
are standard lengths, machine cut, bent and inserted, but it still surprised
me that it was more economic to do this than use a double sided PCB with
PTH.

2009\02\02@044330 by Peter Restall

flavicon
face

Just my 2p, but those traces look very thin for homebrew PCB - I can get
about 6-8thou at a push (ie. not necessarily consistently) using a 1200dpi
laser printer, lightbox and bubble etcher (FeCl) - the hardest part is the
coating of the boards (I don't use pre-sensitised ones, but I think I should !)
I don't know what it would be like with the toner transfer method though - I'm
presuming the same sort of resolution.

I try to stick with 25thou traces for signals and neck down to 15thou between
pins to give a generous clearance - I wouldn't try sticking more than one
trace between a pin either.  I use 45 degree angles for my traces - I think
they look a little nicer than right-angles and are less likely to peel away
from the board.  And you might want to snap to grid too.  These parameters work
alright for me for the boards I do anyway - I dare say everybody has their
own slant on it.

I would recommend you take a look at:

http://www.alternatezone.com/electronics/files/PCBDesignTutorialRevA.pdf

It's a very good introduction to PCB design with some nice tips to get your
boards looking pretty and increase their desired properties.

Regards,

Pete Restall

--- Original Message ---
Date: Sat, 31 Jan 2009 21:40:40 -0500
From: solarwind <TakeThisOuTx.solarwind.xEraseMEspamspam_OUTgmail.com>
Subject: [PIC] My First PIC Development Board PCB Design
To: "Microcontroller discussion list - Public." <RemoveMEpiclistspamTakeThisOuTmit.edu>

http://omploader.org/vMTcyaA

Here it is. Created with FreePCB. I did not pirate anything -.-

In the socket will fit a 28 pin DIP holder for my PIC 16F886 or 18F2620

Is it an OK design? Can anyone spot anything wrong? Are the traces too th=
in?

This will be for homebrew PCB making by the way (using toner transfer
and FeCl etching).

--=20
solarwind

2009\02\02@045721 by Peter Restall

flavicon
face

There's more than one way to route a board, so what you have is not the only
way to get it onto a single side - give the same circuit to 10 different
people to route and you will get a different result back each time (and one is
not necessarily more 'right' than the other btw).

And low-end autorouters don't tend to do a very good job (apparently the
high-end ones do a better job, but I have no experience with those) - stick
to routing by hand.

Regards,

Pete Restall

--- Original Message ---
Date: Sun, 1 Feb 2009 00:27:21 -0500
From: solarwind <x.solarwind.xEraseMEspam.....gmail.com>
Subject: Re: [PIC] My First PIC Development Board PCB Design
To: "Microcontroller discussion list - Public." <EraseMEpiclistspammit.edu>
Message-ID:
       <RemoveMEa94764e0901312127p75c4276fm3c51c9b236c4512fEraseMEspamEraseMEmail.gmail.com>> Content-Type: text/plain; charset=3DISO-8859-1

On Sun, Feb 1, 2009 at 12:09 AM, William Chops Westfield <
RemoveMEwestfwspam_OUTspamKILLspammac.com>=
wrote:
{Quote hidden}

Unfortunately, this is the ONLY way to get my design on a single layer
PCB with the layout that I want. The autorouter verified this. But
people have had success doing 0.5 mm pitch TQFP so the two traces
between the two dip holes shouldn't be THAT bad... And I could always
flood that part with a marker and use a knife to cut the spaces if i
absolutely have to. And I can get this trace drawing pen at my local
electronics hobby shop that lets you draw very thin traces with
conducive ink I think it was...

--=20
solarwind

2009\02\02@051556 by Jinx

face picon face
( wandering away from [PIC] )

> But what amazed me was the number of jumper wires

I've seen that too, dozens of them, and usually on VCRs. Also
wire links to connect a daughter board (like a tuner or filter) to
the main board, then the daughter board bent up perpendicularly.
Must be cheaper than a connector

2009\02\02@060615 by Harry H. Arends

flavicon
face
Good paper for starters.

> Namens Peter Restall
>
>
> I would recommend you take a look at:
>
> www.alternatezone.com/electronics/files/PCBDesignTutori
> alRevA.pdf
>
> It's a very good introduction to PCB design with some nice
> tips to get your boards looking pretty and increase their
> desired properties.
>
> Regards,
>
> Pete Restall
>

2009\02\02@104655 by John van der Putte

picon face
Did you missed a trace between pin 5 and 6 at U3?

-----Oorspronkelijk bericht-----
Van: RemoveMEpiclist-bouncesTakeThisOuTspamspammit.edu [EraseMEpiclist-bouncesspamspamspamBeGonemit.edu] Namens
solarwind
Verzonden: zondag 1 februari 2009 3:41
Aan: Microcontroller discussion list - Public.
Onderwerp: [PIC] My First PIC Development Board PCB Design

http://omploader.org/vMTcyaA

Here it is. Created with FreePCB. I did not pirate anything -.-

In the socket will fit a 28 pin DIP holder for my PIC 16F886 or 18F2620

Is it an OK design? Can anyone spot anything wrong? Are the traces too thin?

This will be for homebrew PCB making by the way (using toner transfer
and FeCl etching).

--
solarwind

More... (looser matching)
- Last day of these posts
- In 2009 , 2010 only
- Today
- New search...