Searching \ for '[PIC] Need critique of my SMD PIC18F4550 PCB' in subject line. ()
Make payments with PayPal - it's fast, free and secure! Help us get a faster server
FAQ page: www.piclist.com/techref/pcbs.htm?key=pcb
Search entire site for: 'Need critique of my SMD PIC18F4550 PCB'.

Exact match. Not showing close matches.
PICList Thread
'[PIC] Need critique of my SMD PIC18F4550 PCB'
2010\12\19@173955 by Nathan House

picon face
I've made a PCB for the DIP version of the PIC18F4550, but now I'm trying to
make a board for the TQFN package of the 4550. I was wondering if you guys
would mind checking out my schematic and layout below and let me know if it
looks alright?

Schematic:
www.roboticsguy.com/images/misc/pic18f4550_tqfn_schematic.png
Layout: http://www.roboticsguy.com/images/misc/pic18f4550_tqfn_pcb.png

Appreciate your help

2010\12\19@180134 by Mark Rages

face picon face
On Sun, Dec 19, 2010 at 4:39 PM, Nathan House <spam_OUTnathanpiclistTakeThisOuTspamgmail.com> wrote:
> I've made a PCB for the DIP version of the PIC18F4550, but now I'm trying to
> make a board for the TQFN package of the 4550. I was wondering if you guys
> would mind checking out my schematic and layout below and let me know if it
> looks alright?
>
> Schematic:
> www.roboticsguy.com/images/misc/pic18f4550_tqfn_schematic.png
> Layout: http://www.roboticsguy.com/images/misc/pic18f4550_tqfn_pcb.png

If the DIP version of the circuit works, I'll assume your schematic is OK.

I think that running ground and power in a circle around the board
might invite inductive noise pickup.  Think "star," not "circle."

Regards,
Mark
markrages@gmail
-- Mark Rages, Engineer
Midwest Telecine LLC
.....markragesKILLspamspam@spam@midwesttelecine.co

2010\12\19@183626 by Philippe Paternotte

flavicon
face



Nathan House-5 wrote:
>
> Schematic:
> www.roboticsguy.com/images/misc/pic18f4550_tqfn_schematic.png
> The D1 LED is upside-down...

-----
Best regards,

Philippe.

http://www.pmpcomp.fr Pic Micro Pascal for all! -- View this message in context: old.nabble.com/Need-critique-of-my-SMD-PIC18F4550-PCB-tp30495074p30495259.html
Sent from the PIC - [PIC] mailing list archive at Nabble.com.

2010\12\19@183833 by Oli Glaser

flavicon
face
On 19/12/2010 23:01, Mark Rages wrote:
> On Sun, Dec 19, 2010 at 4:39 PM, Nathan House<nathanpiclistspamKILLspamgmail.com>  wrote:
>> I've made a PCB for the DIP version of the PIC18F4550, but now I'm trying to
>> make a board for the TQFN package of the 4550. I was wondering if you guys
>> would mind checking out my schematic and layout below and let me know if it
>> looks alright?
>>
>> Schematic:
>> www.roboticsguy.com/images/misc/pic18f4550_tqfn_schematic.png
>> Layout: www.roboticsguy.com/images/misc/pic18f4550_tqfn_pcb.png
> If the DIP version of the circuit works, I'll assume your schematic is OK..
>
> I think that running ground and power in a circle around the board
> might invite inductive noise pickup.  Think "star," not "circle."

Yes, better to try and run them together or use a plane.
In general it looks fine, only thing I could see is on the power jack input the LED seems to be the wrong way round. Also the part no (SFH482) looks to be for an IR part?



2010\12\19@191141 by Olin Lathrop

face picon face
Nathan House wrote:
> Schematic:
> http://www.roboticsguy.com/images/misc/pic18f4550_tqfn_schematic.png

You've got to be kidding!  You are always judged by the examples of your
work you let others see.  The fact that you're not sufficiently embarassed
by this says a lot about what kind of engineer you are (or aren't in this
case), even more than the mess itself.

Schematics are not only to define what's connected to what inside the ECAD
software, but also to explain the circuit to humans.

1 - The pins of IC1 are in pin number order!  That may save you a few
minutes making the symbol once, but wastes many times that over the life of
the schematic as people have to figure out what's where.

2 - Do you really need all those big fat circles with Xs thru them to show
no connections (if that's what they indeed are)?  Just don't connect
anything to a pin and it will be obvious nothing is connected to it.

3 - It's nice to have logical flow of signals from left to right.  That's
not always possible, especially with complicated ICs, but at least you can
put power on top and ground on bottom.  You've got Vdd going every which way
except the one logical direction, which is up.  If you'd bothered arranging
power going from top to bottom, you might have noticed that D1 is backwards..
See how taking a little care actually makes a concrete difference?

4 - Neatness counts, since it effects readability.  It's even more important
when you expect others to see your work.  Since this is of course obvious,
it logically follows that not taking some care is either stupid or
deliberately rude.  So which is it?

The vertical text and even text overlapping other parts is really sloppy and
annoying to read.  What's with the long label for J1?  I don't wee what it's
trying to tell us beyond that it's a RJ11 connector.  Meanwhile the label
collides with R1.  Now how come you couldn't see this for yourself!?

5 - What's with all the polarized capacitors?  Clearly C4 and C5 at 22pF are
going to be ceramic, which is not polarized.  None of the other values are
large enough at high enough voltage to require polarized capacitor
technologies.  These should all be the much cheaper and more effective
ceramics.

6 - If I remember right, 20MHz crystal doesn't work with USB.  Did you read
the datasheet before designing the circuit?  I didn't think so.  Go read it..

7 - 330nF may be in spec for the Vusb cap, but it's definitely on the low
end.  Here's a case where the datasheet is misleading and actually
contradicts itself.  I've had private communication with Microchip about
this, and you can use considerably more, like 1uF or even higher.

8 - Where is the power coming from?  It says "Power Jack" in the bottom
right corner, but there is no jack there nor anywhere else on the schematic
I can find.

9 - What's the point of this PIC if it's not connected to anything other
than the USB?  As far as I can see, the only connections to other pins are
to the infrastructure around the PIC.  Shouldn't there be sensors,
transducers, a serial port, analog inputs, digital outputs, *something*?

> Layout: http://www.roboticsguy.com/images/misc/pic18f4550_tqfn_pcb.png

10 - Do I see this right?  You are using a QFN package for the PIC but the
other parts around it are all thru hole!!?  If that's true, it's really
funny!

11 - It makes sense for external connectors to be thru hole for mechanical
strength, but it looks like the pads on the USB connector short to each
other.  This looks to be done with Eagle.  Didn't you run a DRC check?

12 - It looks like there is silkscreen writing over pads in a number of
places.  Board houses will generally clip silkscreen to the solder mask
layer, but its very sloppy to rely on this.  It might hold up the board too..

13 - Daisy chained ground is a really bad idea.  At least the local ground
around the PIC should be locally connected.  The PIC ground over by the
crystal loops halfway around the board before connecting to the other side
of the PIC.  Making a single ground plane and blindly connecting all grounds
to it isn't the best, but it would be better than what you did.  It appears
everything is on one layer.  Why not use the bottom at least for ground?


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

2010\12\19@191306 by Olin Lathrop

face picon face
Mark Rages wrote:
> I think that running ground and power in a circle around the board
> might invite inductive noise pickup.  Think "star," not "circle."

I agree with half of that.  You definitely don't want circuitous ground.
However, circuitous power is OK as long as it's locally bypassed to the
solid ground close to where it's used.


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

2010\12\19@191913 by Xiaofan Chen

face picon face
On Mon, Dec 20, 2010 at 8:12 AM, Olin Lathrop <.....olin_piclistKILLspamspam.....embedinc.com> wrote:
> 6 - If I remember right, 20MHz crystal doesn't work with USB.  Did you read
> the datasheet before designing the circuit?  I didn't think so.  Go read it.
>

Now it is your turn to read the datasheet ...

-- Xiaofan

2010\12\19@192855 by peter green

flavicon
face
Nathan House wrote:
> I've made a PCB for the DIP version of the PIC18F4550, but now I'm trying to
> make a board for the TQFN package of the 4550. Afaict there is no package of that name. Do you mean TQFP or QFN?

2010\12\19@200041 by peter green

flavicon
face
Olin Lathrop wrote:
{Quote hidden}

Do watch the dielectrics though. Y5V ceramics in particular are nasty with capacitance dropping off heavilly with voltage and temperature, I would avoid them. IIRC X5R, X7R and NPO are the good ceramics.
{Quote hidden}

But even then there isn't anything obstructing him from just taking all the grounds together to one big pour under the pic

2010\12\19@203942 by Nathan House

picon face
>>In general it looks fine, only thing I could see is on the power jack
>>input the LED seems to be the wrong way round. Also the part no (SFH482)
>>looks to be for an IR part?

Thanks for catching that, I didn't notice the LED was backwards. I have no
idea if it's IR or not, I just found that it had the footprint I needed so I
used it..

>>You've got to be kidding!  You are always judged by the examples of your
>>work you let others see.  The fact that you're not sufficiently
embarrassed
>>by this says a lot about what kind of engineer you are (or aren't in this
>>case), even more than the mess itself.

I'm not embarrassed, and you're right, I'm not an engineer. I'm a student
who has only had one "real" electronics course (basic DC circuit analysis).

I appreciate your bluntness, though. I know my work isn't professional at
all, which is because I haven't had much experience. But the only way for me
to improve is to ask the advice of experienced engineers like yourself and
to learn from my mistakes. So, thank you!

>>>1 - The pins of IC1 are in pin number order!  That may save you a few
>>minutes making the symbol once, but wastes many times that over the life
of
>>the schematic as people have to figure out what's where.

I grabbed the symbol from the Microchip Eagle library I found online. Are
you suggesting I put the pins into "groups"? (like all the power pins next
to one another, separating the different ports, etc..?).

>>2 - Do you really need all those big fat circles with Xs thru them to show
>>no connections (if that's what they indeed are)?  Just don't connect
>>anything to a pin and it will be obvious nothing is connected to it.

Those are actually solder pads that I found in the SOLPAD library in Eagle.
Is there a better way to show a solder pad connection?

>>4 - Neatness counts, since it effects readability.  It's even more
important
>>when you expect others to see your work.  Since this is of course obvious,
>>it logically follows that not taking some care is either stupid or
>>deliberately rude.  So which is it?

I'll go with ignorance, since I'm definitely not trying to be rude. What it
really boils down to is that I don't know what I'm doing. I hope you
recognize that I am making an effort to learn, however.

>>5 - What's with all the polarized capacitors?

I'm sorry, that was really stupid of me. Your right that almost all of the
capacitors are ceramic; only one is polarized. I was lazy and just copied
the symbol since all the caps have the same footprint. It was sloppy work
and I'll change it.

>> 6 - If I remember right, 20MHz crystal doesn't work with USB.

I think it does actually. Page 28 of the datasheet lists it as one of the
crystal frequencies.
http://ww1.microchip.com/downloads/en/devicedoc/39632e.pdf

>> 7 - 330nF may be in spec for the Vusb cap, but it's definitely on the low
end.

Wow, I had no idea! I believe the datasheet actually shows a 220nF capacitor
being used, but I put 330nF because I didn't have any of the other. I'll try
using a 1uF like you suggested.

>>8 - Where is the power coming from?

Again, I suppose this was laziness on my part. The power connector I'm using
is not in any of the Eagle libraries (that I could find), so I threw down
three pads at the right spacing and labeled it as the power connector. I
know how to make a part in Eagle, so I should have created the part in the
library myself.

>>9 - What's the point of this PIC if it's not connected to anything other
>>than the USB?

That's what all of the solder pads are for. I'm still a total novice when it
comes to PICs, so I wanted to make a kind of "general purpose" board that I
could use for different projects.

>>10 - Do I see this right?  You are using a QFN package for the PIC but the
>>other parts around it are all thru hole!!?  If that's true, it's really
>>funny!

Correct. I've never made a PCB with a SMD before and considering that I'm
making this myself, reflowing the TQFP on a skillet no less, I decided to
use through-hole parts - which I'm used to soldering - for the rest of the
board.

>>11 - It makes sense for external connectors to be thru hole for mechanical
>>strength, but it looks like the pads on the USB connector short to each
other.

I don't know why the picture I exported from Eagle looks like that, I didn't
notice when I uploaded it. In Eagle there is space between the pads.
However, now that you mention it, there really isn't much space between the
pads. I should change that.

>>12 It looks like there is silkscreen writing over pads in a number of
places
I can't do a silkscreen at home. The gray text is just for my reference.
Sorry for the confusion!

>>13 - Daisy chained ground is a really bad idea.  At least the local ground
>>around the PIC should be locally connected.  The PIC ground over by the
>>crystal loops halfway around the board before connecting to the other side
>>of the PIC.  Making a single ground plane and blindly connecting all
grounds
>>to it isn't the best, but it would be better than what you did.  It
appears
>>everything is on one layer.  Why not use the bottom at least for ground?

It's a single layer board, so unfortunately I can't make a bottom ground
plane.. Here's another picture of the board, this time with the ground
traces highlighted.

http://www.roboticsguy.com/images/misc/pic18f4550_tqfp_pcb2.png

I only see two other ways to route the ground trace. One, go under the VDD
trace under the ICD connector and up the right hand side of the board, or
two, have a jumper wire cut across the center of the board (which would not
look pretty). How do you think I should route it? Do you see a better
option?


>> Afaict there is no package of that name. Do you mean TQFP or QFN?

I'm sorry, I meant TQFP. I've never used a SMD before so I find all the
different acronyms confusing :-)


>>Maybe he wants to make/have it made single sided (btw to the OP: if you
>>are going to get the board made single sided remember SMT parts need to
>>be on the same side as the tracks and through hole parts on the opposite
>>side from the tracks!)

I found that out the hard way! The few PCBs I've made had only through hole
parts, so when designing them it was like I was "looking through" the board..
When making this board, though, I forgot to mirror the PIC which created a
mess later on.


>>Do you really need to take such an accusatory tone when pointing such
things out?
>>As ususal you are being unessacerally accusatory.

He probably didn't know that I'm a student, and if I were an engineer right
now, I'd agree I'd be a pretty crappy one with my lack of knowledge and
experience.

I REALLY appreciate all of the advice everyone has given me, thank you!

2010\12\19@210319 by Oli Glaser

flavicon
face
On 20/12/2010 00:12, Olin Lathrop wrote:
> Nathan House wrote:
>> Schematic:
>> www.roboticsguy.com/images/misc/pic18f4550_tqfn_schematic.png
> You've got to be kidding!  You are always judged by the examples of your
> work you let others see.  The fact that you're not sufficiently embarassed
> by this says a lot about what kind of engineer you are (or aren't in this
> case), even more than the mess itself.
>

Olin, this really is unnecessary..
I find the point about one's posts saying a lot about them a little ironic... :-)


> 6 - If I remember right, 20MHz crystal doesn't work with USB.  Did you read
> the datasheet before designing the circuit?  I didn't think so.  Go read it.

You don't remember right.

2010\12\19@211900 by Oli Glaser

flavicon
face
On 20/12/2010 01:39, Nathan House wrote:
> I've never made a PCB with a SMD before and considering that I'm
> making this myself, reflowing the TQFP on a skillet no less, I decided to
> use through-hole parts - which I'm used to soldering - for the rest of the
> board.

Although I understand being cautious with SMD initially,  there is no need to be afraid of 95% of SMD stuff.
With a decent iron and a sharp pair of tweezers you can solder TQFP packages and 0805 resistors/caps no problem. No real need to use reflow for this, but no harm in getting familiar with that either for future, more complex projects (such as ones involving BGA packages)
There are many tutorial videos on hand soldering SMD packages, give Google/You tube a go (check out "drag soldering" technique)

2010\12\19@213634 by William \Chops\ Westfield

face picon face

On Dec 19, 2010, at 5:39 PM, Nathan House wrote:

>> 1 - The pins of IC1 are in pin number order!  That may save you a  
>> few minutes making the symbol once, but wastes many times that over  
>> the life of
>> the schematic as people have to figure out what's where.

> I grabbed the symbol from the Microchip Eagle library I found  
> online. Are you suggesting I put the pins into "groups"? (like all  
> the power pins next to one another, separating the different ports,  
> etc..?).

I think it's a matter of style/opinion, and will somewhat depend on  the complexity of the application.  I've used symbols with logical  groupings, and wished they had at least some clue about actual pin  positions, so that I could make arbitrary connections from io ports to  external devices in a way that would make sense from a pcb routing  perspective.  And I've used symbols with pin-number ordering and  cursed the lack of logic.  And I've used symbols that someone had laid  out using SOME logic that I guess made sense to them, but I didn't like!

BillW

2010\12\19@220916 by RussellMc

face picon face
> I've made a PCB for the DIP version of the PIC18F4550, but now I'm trying to
> make a board for the TQFN package of the 4550. I was wondering if you guys
> would mind checking out my schematic and layout below and let me know if it
> looks alright?

The price of freedom is eternal vigilance.
And similar :-).
Alas I had to go to the airport and this post was 4 hours old when I
read it, so I thought "Oh no."
Actually, probably more like "OH! NO!!!"
Where is (I thought) the

            <FlameShieldsOn> instruction ? !!!!!!!!!!!!!!

Usually an utterly necessary prerequisite to such material in this context.

And I expected to find blood all over the ranks.

I read on with trepidation and some surprise.
I did find a modest amount of blood, almost a trivial amount, but it
seemed as far as I could tell, to come from Middlesex County, so its
loss  will almost certainly not be noticed, and it will almost
certainly have no effect whatsoever (more's, perhaps, the shame) so
all is weller (nothing to do with Copper group [tm]) than may have
been.

So, congratulations. Well ridden. Looked like a Class IV verging on V
on entry but, as is often the case, with suitable handling and
adequate disdain of bluster abs appearance, proved to be only a Class
I (Waves small; passages clear; no serious obstacles).

No that there was some good & useful Class III technical stuff in
there amongst the spray and eddies. Also some good Class II
contributed by lookers on and well wishers. Note for reference that
the V/I may be followed by a III tail in an attempt at redress - so
success in the V/I should be taken as modestly as it appears to have
been and the following III approached with due diligence. If note is
taken of " ... requiring expertise in maneuvering ... " you'll
probably do OK - you seem pretty competent at this so far.



        Russell

____________


V: Exceedingly difficult, long and violent rapids, following each
other almost without interruption; riverbed extremely obstructed; big
drops; violent current; very steep gradient; close study essential but
often difficult. Requires best person, boat, and outfit suited to the
situation. All possible precautions must be taken

III Waves numerous, high, irregular; rocks; eddies; rapids with
passages clear though narrow, requiring expertise in maneuvering;
scouting usually needed. Requires good operator and boat.

More:

                          http://bit.ly/RiverRatings

2010\12\19@231435 by Bob Blick

face
flavicon
face

On Sun, 19 Dec 2010 19:12:34 -0500, "Olin Lathrop" said:
> 1 - The pins of IC1 are in pin number order!  That may save you a few
> minutes making the symbol once, but wastes many times that over the life
> of
> the schematic as people have to figure out what's where.

In this case I agree with you, since the schematic symbol puts the pins
on two sides and the chip has them on four. But quite often when doing a
design from scratch I like to have the pins on the schematic symbol echo
the physical layout of the part. If I have a choice about pin
assignment, I can pre-optimize my board layout just by making the
schematic look tidy. I don't know about other CAD packages, but the one
I use lets me have unlimited schematic symbols for each part, and I take
advantage of that. So I have no hard and fast rules, I do what works
best for each job.

Best regards,

Bob


-- http://www.fastmail.fm - Access all of your messages and folders
                         wherever you are

2010\12\20@025111 by Ruben Jönsson

flavicon
face
> I've made a PCB for the DIP version of the PIC18F4550, but now I'm trying to
> make a board for the TQFN package of the 4550. I was wondering if you guys
> would mind checking out my schematic and layout below and let me know if it
> looks alright?
>
> Schematic:
> www.roboticsguy.com/images/misc/pic18f4550_tqfn_schematic.png
> Layout: www.roboticsguy.com/images/misc/pic18f4550_tqfn_pcb.png
>
My suggestion is to use SMD parts for everything except the connectors and the LEDs (since they are going to be placed on the top side). It really is not very hard to mount the SMD components if you have a decent solder iron and some good tweezers. In fact it might even be easier than to use TH parts since you don't need to drill holes for them.

Use a through hole connector instead of just pads for the external connections. If that messes up your layout, use two or more. This way the board can be easily switched between projects without desoldering/soldering. Bare wires also have a tendency to get broken off at the board surface. Don't forget power and ground in the connectors. Flat ribbon ICD type connectors usually works good for this. If you don't go with the connector idea, you still will need some pads for ground and power.

The groundplane - Use a two sided board instead and use all the top layer as the ground. Just make clearances for the TH component pads on the top side. If this is a hobby project with a few home made boards, then make solderpads (vias) besides the ground pads for pins that should be grounded but not directly under the component and connect the top and bottom side with a bare wire through the via pads. This way you can remove the ground traces on the bottom side and make better room for connectors for the external signals. If you really, really want to stick to a single sided board you can use jumper wires on the top side to connect all ground islands on the bottom side so it more closely will resemble a ground plane - the more jumper wires, the better.

Make room/pads for test points and ground connection for a oscilloscope. Sometimes it may be hard to find a good connection for the probe ground. (Using a ground plane will make it easy - just solder a short piece of bare wire or a cut of resistor leg to the ground plane.)

Good luck with your project / Ruben

==============================
Ruben Jönsson
AB Liros Electronic
Box 9124, 200 39 Malmö, Sweden
TEL INT +46 40142078
FAX INT +46 40947388
EraseMErubenspam_OUTspamTakeThisOuTpp.sbbs.se
==============================

2010\12\20@060306 by Michael Watterson

face picon face
On 20/12/2010 00:12, Olin Lathrop wrote:
> 6 - If I remember right, 20MHz crystal doesn't work with USB.  Did you read
> the datasheet before designing the circuit?  I didn't think so.  Go read it.
>
It does.
Internal 96MHz  oscillator and PLL locked to the 20MHz.

2.3Oscillator Settings for USB
When these devices are used for USB connectivity,
they must have either a 6MHz or 48MHz clock for
USB operation, depending on whether Low-Speed or
Full-Speed mode is being used. This may require some
forethought in selecting an oscillator frequency and
programming the device.
The full range of possible oscillator configurations
compatible with USB operation is shown in Table2-3.

Table 2.3 OSCILLATOR CONFIGURATION OPTIONS FOR USB OPERATION

Possible Crystals for  24MHz  CPU (6MHz USB low speed) or 48MHz CPU (48MHz USB high speed) are
4, 8, 12, 16, 20, 24 and 48MHz

Consult also
FIGURE 2-1:PIC18F2455/2550/4455/4550 CLOCK DIAGRAM

(page 26)

Crystal is divided by 1, 2, 3, 4, 5, 6,  10 or 12 to get 4MHz
96Mhz osc PLL to the 4MHz
For High Speed you divide by 2 for USB clock
CPU clock is 96 MHz divide by 2, 3, 4 or 6  -OR- Crystal  divided by 1, 2 ,3 or 4

For Low speed USB you can use either CPU Primary clock divider (the via 96MHz or direct external), but must be 24MHz as it's divided by 4

CPU clock can also be secondary external  or Internal Osc (not the 96MHz).

It's very flexible

2010\12\20@063924 by RussellMc

face picon face
On 21 December 2010 00:02, Michael Watterson <mikespamspam_OUTradioway.org> wrote:
> On 20/12/2010 00:12, Olin Lathrop wrote:
> > 6 - If I remember right, 20MHz crystal doesn't work with USB.  Did you read
> > the datasheet before designing the circuit?  I didn't think so.  Go read it.

> It does.
> Internal 96MHz  oscillator and PLL locked to the 20MHz.

OL has special dispensation to not read the data sheet himself while
misremembering it and to "I didn't think so" people, apparently.

Note that this is a different dispensation from remembering the
datasheet incorrectly and politely incorrectly correcting people, or
even from the dispensation for remembering the datasheeet correctly
and politely informing somebody about it, which we are several el, or
leagues, away from here. I'm not sure where the special dispensation
to NRTDSHWMIAT"IDTS"P came from and as soon as I find who dispensed it
I'll see if it can be revoked (rendered indispensable?), if only
because it makes him look silly when he uses it. Can't have people
looking silly on this list now, can we? (Except, perhaps, me
occasionally).

Thanks for the chapter and verse showing that 20 MHz clock is indeed
OK for USB operation.

I was interested to note that even our Singaporean X-man rose to the
challenge on this occasion* :-).



       Russell

* Apologies if there are more than one Singaporean X-men here - you
know who you are :-).

2010\12\20@072958 by Olin Lathrop

face picon face
Xiaofan Chen wrote:
>> 6 - If I remember right, 20MHz crystal doesn't work with USB. Did
>> you read the datasheet before designing the circuit? I didn't think
>> so. Go read it.
>
> Now it is your turn to read the datasheet ...

Ah yes, you're right.  For some reason I thought the crystal had to be a
multiple of 8MHz, but I see that is incorrect.  Sorry for the confusion.

To use the full speed USB peripheral, you need a oscillator that can be
divided by 1, 2, 3, 4, 5, 6, 10, or 12 to get 4MHz.  That means the allowed
oscillator frequencies are 4, 8, 12, 16, 20, 24, 40, and 48 MHz.  Note that
the last two at least can't be achieved by just connecting a crystal to the
PIC.  They have to be clock signals derived elsewhere and fed directly into
the PIC.


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

2010\12\20@080818 by Olin Lathrop

face picon face
peter green wrote:
> meh the pic mostly has logically grouped stuff next to each other
> anyway
> so IMO the troubleshooting advantages of keeping the physical layout
> outweigh any gains that would come from using another layout in the
> case of pics.

So you think a schematic should be optimized for the short term hardly-used
case of troubleshooting and pessimized for understanding the circuit.
That's backwards.  It's also not so clear that pin order symbols make
troubleshooting any easier.  It more quickly answers the question of "what's
on this pin", but that's not what you usually want to know.  Usually you
want to look at a particular signal, so you want to translate logical signal
to pin number quickly, not the other way around.

> From looking at his layout it seems like those represent loose pads
> connected to the unused IO (not a bad idea if you are trying to make a
> board flexible, much easier to solder to a pad than straight to the
> pin of a tiny SMT chip).

Test points on unused pins are a good idea if the layout and routing can
support them.  If that's what he meant, then what are the Xs thru the
circles supposed to be telling us?

>> The vertical text and even text overlapping other parts is really
>> sloppy and annoying to read.  What's with the long label for J1?  I
>> don't wee what it's trying to tell us beyond that it's a RJ11
>> connector.  Meanwhile the label collides with R1.  Now how come you
>> couldn't see this for yourself!?
>>
> Do you really need to take such an accusatory tone when pointing such
> things out?

Yes.  This is not a electronics knowledge or newbie issue.  There is no
excuse for sloppiness.  Not only is it rude to ask 2000 people to review
something you haven't bothered to clean up a bit, but it also points to
messy thinking.  He should be ashamed of himself.  Since that obviously
isn't working, we'll have to do it for him.

> Agreed, provided you are buying from a supplier that stocks them

Huh?  It would be hard to find a electronics supplier that doesn't stock a
large variety of ceramic capacitors.  They are a very common item.  You also
make it sound like you're stuck with whatever supplier you are buying from.
Mouser, DigiKey, Newark, and many others are easily accessible via the
internet.

> and you are prepared to deal with SMT

This makes no sense.  I don't know what you think you have to "prepare" to
use surface mount capacitors.  If you can solder thru hole you can solder
surface mount, more easily in fact.  Thru hole capacitors of these sizes are
orphan products at best.  All the development is happening in surface mount,
and has for some years.  The OP is laying out a new board, so he has the
flexibility to design it for surface mount.

> Never had a problem with 220nf on there myself but I have seen reports
> that bigger is better.

I've had this discussion with Microchip since the datasheet actually
contradicts itself (at least the early versions, perhaps this is fixed now)..
I typically use 1uF and have been specifically told by Microchip that this
is fine.  Even in the early datasheet, 220nF was the minimum, so there is no
margin for error.  Where do you get your stock of 0% capacitors?

> Looks like there are two pads LSP1 an LSP2 in that part of the
> schematic which i'd assume are the power input

Exactly, you have to assume.  Those are also not that close where it says
"Power Jack", so it's really not that clear.

> I've done similar before. I find SMT passives a PITA to deal with
> compared to through hole ones

That is a statement about you, not surface mount.  The only people I hear
complain about surface mount are hobbiest that just want to keep doing what
they've always done and want to pretend the new way is worse somehow.
That's just silly.  Everyone I know that's gotten reasonable experience with
surface mount parts doesn't want to go back.  Keep in mind we're talking
about the large surface mount parts, like 0805 capacitors.  Those are easier
to solder on and much easier to unsolder than any thru hole part.

Some surface mount parts are tricky and require some skill, like small QFN
packages.  However, that's what the OP is already using for the PIC.  If he
can handle a 44 pin QFN, then 0805 resistors and capacitors are certainly no
obstacle to him.

> If you are going to stencil and oven the
> whole board this doesn't apply but I doubt this is the case here.

You don't need stencil and oven for surface mount to be easier.  0805
resistors and capacitors are easier to solder on a board than their thru
hole counterparts, even if all you have is a soldering iron and a roll of
solder.  Unsoldering 0805 is much easier than a 1/4 watt radial lead
resistor.

> Maybe he wants to make/have it made single sided

Why?  In very high volume single sided punched boards can save a little
money, but this is clearly a hobby project.  The board house will use a 2
layer process even if you just use copper on one layer.  It's not cheaper to
make a 1 layer board than a 2 layer board, so you might as well get the
benefit of a ground plane or easier routing.


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

2010\12\20@082916 by Olin Lathrop

face picon face
Nathan House wrote:
> I'm not embarrassed, and you're right, I'm not an engineer.

Neatness trancends disciplines.  Would you seriously hand in a homework
assignment looking like that?

> I grabbed the symbol from the Microchip Eagle library I found online.

Symbols you find with Eagle were optimized to take as little time to make as
possible.  They are there so that CadSoft can say they have the part in
their library.

I make some of my Eagle libraries available for free in the Eagle Tools
release at http://www.embedinc.com/pic/dload.htm.  I know the 18F4550 is in
there in at least one footprint, maybe even the one you are using.

> Are you suggesting I put the pins into "groups"? (like all the power
> pins next to one another, separating the different ports, etc..?).

Yes.  Take a look at my 18F4550 symbol, for example.

> Those are actually solder pads that I found in the SOLPAD library in
> Eagle. Is there a better way to show a solder pad connection?

Again, Eagle libraries are wildly inconsistant.  I've never seen a pad
symbol with a X thru it like that before, so wasn't sure what it was
supposed to be.  I use open circles myself for such things.  I've seen
others use small squares.  Usually when I've seen Xs, it means something is
specifically shown to not be connected.  One of the expensive packages
(Orcad?) seems to do that.  Mostly I see the X symbol in schematics made
with that package.

> Your right that almost all
> of the capacitors are ceramic; only one is polarized.

I don't think you need any polarized capacitors for this design.  Pretty
much up to 10uF at 10V is a no-brainer for ceramic.  10uF 10V capacitors in
0805 footprint are widely available and cheap, probably cheaper than
electrolytic or tantalum of the same value, if you can find those at all.
Higher values are available too, but you should dig around a bit before
specifying them.

Someone mentioned about the Y ceramics.  That's a good point to keep in
mind.  These are often specified with very wide tolerance.  They are
slightly cheaper so can make sense in high volume designs in places where
the value isn't critical, like bypass caps.  For small volumes, it's easier
just to stay away from them.

> I think it does actually. Page 28 of the datasheet lists it as one of
> the crystal frequencies.
> http://ww1.microchip.com/downloads/en/devicedoc/39632e.pdf

Yes, my mistake.

> I've never made a PCB with a SMD before and considering that
> I'm making this myself, reflowing the TQFP on a skillet no less, I
> decided to use through-hole parts - which I'm used to soldering - for
> the rest of the board.

You'll find SMD parts easier once you get used to them.  However a tight
pitch QFN is not easy to get right.  I suggest you use the 44 pin TQFP
package at least.  That will be a lot more forgiving.  I see that some of
the pins aren't connected, so maybe you can use the 18F2550 in the 28 pin
SOIC package instead.  That's fairly easy to solder by hand.

> I don't know why the picture I exported from Eagle looks like that, I
> didn't notice when I uploaded it. In Eagle there is space between the
> pads. However, now that you mention it, there really isn't much space
> between the pads. I should change that.

Set your DRC to 8mil/8mil width/space and run the DRC check.  If the pads
are too close it will tell you.

> It's a single layer board,

Why?  You don't get a price break for using only a single layer because the
board house will use a 2 layer process anyway.


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

2010\12\20@083854 by Gordon

flavicon
face
> Why?  You don't get a price break for using only a single layer because the
> board house will use a 2 layer process anyway.

Depends where but you do get a little break.

http://www.olimex.com/pcb/pcb-price.html

But, I would agree, for a hobby project cost (within reason) isn't the
biggest factor, and from my example of a 100x160mm board the
difference was only 6euro, which for the PCB layout and easy of
routing, makes the 2 layer far more appealing.

Regards,
Gordon

2010\12\20@084430 by Isaac Marino Bavaresco

flavicon
face
Em 20/12/2010 11:09, Olin Lathrop escreveu:
>> Do you really need to take such an accusatory tone when pointing such
>> things out?
> Yes.  This is not a electronics knowledge or newbie issue.  There is no
> excuse for sloppiness.  Not only is it rude to ask 2000 people to review
> something you haven't bothered to clean up a bit, but it also points to
> messy thinking.  He should be ashamed of himself.  Since that obviously
> isn't working, we'll have to do it for him.


Two nights ago, The movie "Only the Lonely" was aired here in Brazil by
open TV.

Olin's behavior reminds me of the main character's mother, Mrs. Rose
Muldoon (Maureen O'Hara).

In the movie she keeps "enumerating the facts" (I don't know what was
the original expression, the movie was dubbed in Portuguese), that is,
pointing other people's defects.


Isaac
__________________________________________________
Fale com seus amigos  de graça com o novo Yahoo! Messenger http://br.messenger.yahoo.com

2010\12\20@085241 by Isaac Marino Bavaresco

flavicon
face
Em 20/12/2010 11:30, Olin Lathrop escreveu:
>> It's a single layer board,
> Why?  You don't get a price break for using only a single layer because the
> board house will use a 2 layer process anyway.


Perhaps he wants to etch the board himself, with a home process.


Isaac

__________________________________________________
Fale com seus amigos  de graça com o novo Yahoo! Messenger http://br.messenger.yahoo.com

2010\12\20@090314 by RussellMc

face picon face
>> ... we'll have to do it for him.

The Royal "we" I think.
Maybe some Kennedy blood?


2010\12\20@092132 by jimf

flavicon
face



       Good luck with that one..  I suck at making SMT capable homebrew
boards and where possible i hash things up using PTH and have the
real ones made by a people with more skill than I, (at a cost of
course).
On Mon 20/12/10 1:52 PM , Isaac Marino Bavaresco
@spam@isaacbavarescoKILLspamspamyahoo.com.br sent:
 Em 20/12/2010 11:30, Olin Lathrop escreveu:
>> It's a single layer board,
> Why? You don't get a price break for using only a single layer
because the
> board house will use a 2 layer process anyway.
Perhaps he wants to etch the board himself, with a home process.
Isaac
__________________________________________________
Fale com seus amigos de graça com o novo Yahoo! Messenger
http://br.messenger.yahoo.com/ [1]
--
http://www.piclist.com [2] PIC/SX FAQ & list archive
View/change your membership options at
http://mailman.mit.edu/mailman/listinfo/piclist [3]


Links:
------
[1] http://br.messenger.yahoo.com/
[2] http://www.piclist.com
[3] http://mailman.mit.edu/mailman/listinfo/piclist

2010\12\20@093238 by alan.b.pearce

face picon face
> One of the expensive packages
> (Orcad?) seems to do that

Yes, you can put an X on a pin to show it is not connected, and that then also stops it generating a connection error message in the log for an unconnected pin, so it has a definite purpose other than showing a non-connect.
-- Scanned by iCritical.

2010\12\20@093321 by Olin Lathrop

face picon face
Isaac Marino Bavaresco wrote:
> Perhaps he wants to etch the board himself, with a home process.

That's at odds with using a 44 pin QFN package.

I know some hobbyiest etch their own boards.  A long time ago I did that
too.  You can get usable results somewhat more cheaply with much much more
hassle and lower quality.

Etch your own boards if you want to for the experience, the satisfaction, or
whatever, but don't kid yourself that its easy or that you'll save all that
much money.  And then you don't get plated thru holes and vias, soldermask,
silkscreen, and need to be more generous with the width/space parameters.


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

2010\12\20@093944 by Kerry Wentworth

flavicon
face

It really isn't that hard.  Print the artwork on to magazine paper with
a laser printer, transfer to copper clad using a laminator, and etch.  I
can reliably do .5mm spacing, which is as small as I can comfortably do
hand soldering.

There is a group:

http://groups.yahoo.com/group/Homebrew_PCBsYahoo


Kerry




KILLspamjimfKILLspamspamwebstudios.co.uk wrote:
{Quote hidden}

--
Internal Virus Database is out-of-date.
Checked by AVG Anti-Virus.
Version: 7.0.289 / Virus Database: 267.11.13 - Release Date: 10/6/05

2010\12\20@100611 by Olin Lathrop

face picon face
Kerry Wentworth wrote:
> It really isn't that hard.  Print the artwork on to magazine paper
> with a laser printer, transfer to copper clad using a laminator, and
> etch.  I can reliably do .5mm spacing, which is as small as I can
> comfortably do hand soldering.

Note that's a whopping bit 20 mils.  Your not going to do a .65mm (26 mil)
pitch QFN package with that as the OP is trying to do.  He either needs to
use a larger package or have the board professionally made.

Maybe someone that's really really good with homemade PC boards can do this,
but that's going to take some experience and experimenting at best.


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

2010\12\20@101924 by Kerry Wentworth

flavicon
face
I should have said ".5mm pitch", not spacing.  Sorry. 10 mil traces and spacing are no problem.

Kerry


Olin Lathrop wrote:
{Quote hidden}

-- Internal Virus Database is out-of-date.
Checked by AVG Anti-Virus.
Version: 7.0.289 / Virus Database: 267.11.13 - Release Date: 10/6/05

2010\12\20@103158 by Oli Glaser

flavicon
face
On 20/12/2010 14:34, Olin Lathrop wrote:
> Isaac Marino Bavaresco wrote:
>> Perhaps he wants to etch the board himself, with a home process.
> That's at odds with using a 44 pin QFN package.
>
> I know some hobbyiest etch their own boards.  A long time ago I did that
> too.  You can get usable results somewhat more cheaply with much much more
> hassle and lower quality.

It is possible with some practice - I have done down to 0.4mm pitch QFN and TQFP footprints with 0.2mm tracks, double sided with (rivet type) plated through holes. I agree it can be messy and time consuming with trays, *but* with a heated bubble or spray tank you can just keep the solution in there, and I find it can (in certain cases) speed some prototyping up quite a bit - print/expose/chuck in tank/drill and have board ready in 15 mins or so with minimal mess/hassle, great when trying a few different ideas out quickly.
Depends on what you are doing I suppose, and having a decent setup and largish work area is helpful. I don't do it that often, but I do like having the option of trying something quickly (while the idea is fresh) I might otherwise have to wait a few days for - it's the time factor, not the price (although <48hr turnaround boards are very expensive)
I like to keep an open mind and use whatever tools get the job done, whether the end result is commercial or for personal use.


2010\12\20@103809 by Isaac Marino Bavaresco

flavicon
face
Em 20/12/2010 13:07, Olin Lathrop escreveu:
> Kerry Wentworth wrote:
>> It really isn't that hard.  Print the artwork on to magazine paper
>> with a laser printer, transfer to copper clad using a laminator, and
>> etch.  I can reliably do .5mm spacing, which is as small as I can
>> comfortably do hand soldering.
> Note that's a whopping bit 20 mils.  Your not going to do a .65mm (26 mil)
> pitch QFN package with that as the OP is trying to do.  He either needs to
> use a larger package or have the board professionally made.
>
> Maybe someone that's really really good with homemade PC boards can do this,
> but that's going to take some experience and experimenting at best.
>
>
> ********************************************************************
> Embed Inc, Littleton Massachusetts, http://www.embedinc.com/products
> (978) 742-9014.  Gold level PIC consultants since 2000.


The nearest PCB manufacturer is 500mi away from where I live. When I
order boards from them, I have to spend at least $200 plus 10 business
days to have the boards.

It happens that in my city there is a small company that makes metal
stamps for the graphic industries, and their process is also adequate
for PCB making.
When I need urgent prototypes, I just e-mail them a post-script file in
the morning and I receive the boards in the afternoon, for around $10 each.

They just etch the board, no holes or plated holes, I simply ask an
assistant to drill the holes. Double-sided possible, but the alignment
may be tricky. 0.5mm pitch perfectly usable.

Their service is the only possible way to have a working prototype in
one day around here.


Isaac

__________________________________________________
Fale com seus amigos  de graça com o novo Yahoo! Messenger http://br.messenger.yahoo.com

2010\12\20@104631 by Oli Glaser

flavicon
face
On 20/12/2010 13:09, Olin Lathrop wrote:
>> Do you really need to take such an accusatory tone when pointing such
>> >  things out?
> Yes.  This is not a electronics knowledge or newbie issue.  There is no
> excuse for sloppiness.  Not only is it rude to ask 2000 people to review
> something you haven't bothered to clean up a bit, but it also points to
> messy thinking.  He should be ashamed of himself.  Since that obviously
> isn't working, we'll have to do it for him.
>

Rude?...  Messy thinking?...  Ashamed?...      Irony?
We are not amused...

2010\12\20@110655 by Nathan

picon face
>If that's what he meant, then what are the Xs thru the
>circles supposed to be telling us?

I have no idea what the x's are for. As I said in my previous email, I
found the part in the solpad library in Eagle and assumed it was
standard.

>> Do you really need to take such an accusatory tone when pointing such
>> things out?

>Yes.  This is not a electronics knowledge or newbie issue.

Actually, it is. I believe I said several times before that I'm a
know-nothing student. Things like the vdd symbol not pointing up,
that's because I didn't know any better, not because of sloppiness or
rudeness. The same thing goes for most of my other mistakes.

>Not only is it rude to ask 2000 people to review
>something you haven't bothered to clean up a bit, but it also points to
>messy thinking.

This is the fourth PCB I have designed. Is it really reasonable for
you to expect it to be perfect?

>He should be ashamed of himself.  Since that obviously
>isn't working, we'll have to do it for him.

I don't understand why you believe I should be ashamed of myself. From
the things you have said, you might not understand why, but I'm
actually proud of my work. No, it's not professional. But considering
that 95% of my peers don't even really know what a PCB is, let alone
how to make one, I think I'm doing pretty well.

Maybe you forget what it's like to be a student, but learning is a
process that takes time. I doubt you just "woke up" one day knowing
everything you now know. Furthermore, most people learn best by trying
something, making mistakes, and then being shown the correct way to do
it. I welcome your constructive criticism, but there's no need to be
rude.

I know that I'm not a professional engineer like you, Olin, but the
only way for me to become one is to continue learning by working on
projects like this. You say I should be ashamed of myself, but I'm
not. I'm proud of the fact that I've taught myself all of this stuff
and that I'm actually making an effort to learn.

If this list is for professional engineers only then I'll stop posting
on it; I didn't know.

>Neatness trancends disciplines.  Would you seriously hand in a homework
>assignment looking like that?

You may not have read my previous email, but I said that I've really
only had one electronics course. I think my professors would be
thrilled if I handed this in as a homework assignment. Most of my
peers have close to zero practical experience when it comes to
electronics.

>You'll find SMD parts easier once you get used to them.  However a tight
>pitch QFN is not easy to get right.  I suggest you use the 44 pin TQFP
>package at least.

I'm sorry, when I said TQFN in my original email I meant TQFP. I am
using the 44 pin TQFP package.

>I see that some of
>the pins aren't connected, so maybe you can use the 18F2550 in the 28 pin
>SOIC package instead.  That's fairly easy to solder by hand.

All but three pins are connected, aside from the NC pins (which I
assumed were not supposed to be connected to anything).

>> It's a single layer board,
>Why?  You don't get a price break for using only a single layer because the
>board house will use a 2 layer process anyway.

As a few people deduced, I'm making this at home. As of now I've only
made single layer boards and would like to stick to that.

>But, I would agree, for a hobby project cost (within reason) isn't the
>biggest factor

It is for me! I'm your typical broke college student..

>Etch your own boards if you want to for the experience, the satisfaction, or
>whatever, but don't kid yourself that its easy or that you'll save all that
>much money.

It costs about one dollar for me to make a 3x4" PCB. I couldn't afford
to get a PCB professionally made.

>It really isn't that hard.  Print the artwork on to magazine paper with
>a laser printer, transfer to copper clad using a laminator, and etch.  I
>can reliably do .5mm spacing, which is as small as I can comfortably do
>hand soldering.

That's pretty much how I do it.


I apologize to everyone if my lack of experience has made me seem
rude; I really am not trying to be. Almost every engineer I've talked
to over the past few years has been extremely supportive of my hobbies
and excited for me that I'm trying so hard to learn, but if a student
like me is not welcome on the piclist, then as I said before, I'll
stop posting

2010\12\20@111438 by Kerry Wentworth

flavicon
face
I wouldn't worry about it too much.  I estimate that 1,999 people here don't think you are the one being rude.

Kerry


Nathan wrote:
{Quote hidden}

-- Internal Virus Database is out-of-date.
Checked by AVG Anti-Virus.
Version: 7.0.289 / Virus Database: 267.11.13 - Release Date: 10/6/05

2010\12\20@112438 by Olin Lathrop

face picon face
Isaac Marino Bavaresco wrote:
> The nearest PCB manufacturer is 500mi away from where I live. When I
> order boards from them, I have to spend at least $200 plus 10 business
> days to have the boards.

I usually get prototype boards done well over 5000 miles away, but they only
cost $120 for however many fit in 100 square inches, two sided.  Usually
that means more boards than we really need.  The PCB house is Gold Phoenix,
http://www.goldphoenixpcb.biz.

> Their service is the only possible way to have a working prototype in
> one day around here.

Other than instant gratification, I very rarely need boards done that fast.
After sending out the board, you still have to do the BOM, buy the parts,
and put the kit together before you need boards to put the parts on.  Use
cheap shipping on whatever parts you have to buy and work on a different
project in the mean time.


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

2010\12\20@113437 by Olin Lathrop

face picon face
Nathan wrote:
> I believe I said several times before that I'm a
> know-nothing student.

After these comments were made.  Students do get a certain kind of slack,
but you have to let people know you're a student.  If you'd have pointed
that out with your request for critique, the tone of some of the replies
would have been different.  Maybe you mentioned it in some earlier thread.
There are a lot of people on this list, and unless you are a active poster
many are not going to remember your occupation, age, etc, if they ever knew
in the first place.

That said, it doesn't take electronics knowledge to understand why anything
you present should show a little care.  Nobody is faulting you for some
electronics mistakes.  We all had to learn it at some time.  You seem to be
doing quite reasonably with the design of the circuit.


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

2010\12\20@115147 by alan.b.pearce

face picon face
> Isaac Marino Bavaresco wrote:
> > The nearest PCB manufacturer is 500mi away from where I live. When I
> > order boards from them, I have to spend at least $200 plus 10 business
> > days to have the boards.
>
> I usually get prototype boards done well over 5000 miles away, but they only
> cost $120 for however many fit in 100 square inches, two sided.  Usually
> that means more boards than we really need.  The PCB house is Gold Phoenix,
> http://www.goldphoenixpcb.biz.
>
> > Their service is the only possible way to have a working prototype in
> > one day around here.
>
> Other than instant gratification, I very rarely need boards done that fast.
> After sending out the board, you still have to do the BOM, buy the parts,
> and put the kit together before you need boards to put the parts on.  Use
> cheap shipping on whatever parts you have to buy and work on a different
> project in the mean time.

Yeah, but Isaac uses a Brazilian email address, so he presumably lives and works there (as a first guess anyway), and from things people have said on this list in the past about supply problems there, if he did things in the order you are suggesting he would have the PCB about 6 months before the components ...
-- Scanned by iCritical.

2010\12\20@115211 by Isaac Marino Bavaresco

flavicon
face
Em 20/12/2010 14:25, Olin Lathrop escreveu:
> Isaac Marino Bavaresco wrote:
>> The nearest PCB manufacturer is 500mi away from where I live. When I
>> order boards from them, I have to spend at least $200 plus 10 business
>> days to have the boards.
> I usually get prototype boards done well over 5000 miles away, but they only
> cost $120 for however many fit in 100 square inches, two sided.  Usually
> that means more boards than we really need.  The PCB house is Gold Phoenix,
> http://www.goldphoenixpcb.biz.


Here in Brazil our government doesn't help us. The importing taxes are
too high.
They charge us 60% over the total price of the merchandise, including
the freight, plus 17% ICMS (VAT) and 5% IPI (tax over manufactured goods).



>> Their service is the only possible way to have a working prototype in
>> one day around here.
> Other than instant gratification, I very rarely need boards done that fast.
> After sending out the board, you still have to do the BOM, buy the parts,
> and put the kit together before you need boards to put the parts on.  Use
> cheap shipping on whatever parts you have to buy and work on a different
> project in the mean time.


I don't use their services too much, but it saved may day more than once.


Isaac

__________________________________________________
Fale com seus amigos  de graça com o novo Yahoo! Messenger http://br.messenger.yahoo.com

2010\12\20@115524 by Oli Glaser

flavicon
face
On 20/12/2010 16:06, Nathan wrote:
> I apologize to everyone if my lack of experience has made me seem
> rude; I really am not trying to be. Almost every engineer I've talked
> to over the past few years has been extremely supportive of my hobbies
> and excited for me that I'm trying so hard to learn, but if a student
> like me is not welcome on the piclist, then as I said before, I'll
> stop posting.

If anyone needs to apologise, it is certainly not you. You are most welcome here.
I think most people here will also be extremely supportive, and there is certainly a wealth of knowledge to be gained.
Don't let anything shake your passion for learning, it's a wonderful process.

2010\12\20@115558 by Dwayne Reid

flavicon
face
At 06:09 AM 12/20/2010, Olin Lathrop wrote:

> > Maybe he wants to make/have it made single sided
>
>Why?  In very high volume single sided punched boards can save a little
>money, but this is clearly a hobby project.  The board house will use a 2
>layer process even if you just use copper on one layer.  It's not cheaper to
>make a 1 layer board than a 2 layer board, so you might as well get the
>benefit of a ground plane or easier routing.

My main board supplier definitely charges significantly less for single-sided boards.  These are boards that we order in 500pc or 1000pc lots and we do a total of 6000 to 10,000 single-sided boards per year.

Actual price difference to me is about 35% less expensive for single vs double-sided boards but that figure includes shipping charges from China.  Actual PCB cost savings is considerably more when you take the shipping charges out of the equation.

My best guess is that the cost is less because they don't have to do the process for plated-through-holes - but that's just a guess.

dwayne

-- Dwayne Reid   <spamBeGonedwaynerspamBeGonespamplanet.eon.net>
Trinity Electronics Systems Ltd    Edmonton, AB, CANADA
(780) 489-3199 voice          (780) 487-6397 fax
http://www.trinity-electronics.com
Custom Electronics Design and Manufacturing

2010\12\20@121211 by Bob Blick

face
flavicon
face

On Mon, 20 Dec 2010 10:07:05 -0500, "Olin Lathrop" said:
> Kerry Wentworth wrote:
> > It really isn't that hard.  Print the artwork on to magazine paper
> > with a laser printer, transfer to copper clad using a laminator, and
> > etch.  I can reliably do .5mm spacing, which is as small as I can
> > comfortably do hand soldering.
>
> Note that's a whopping bit 20 mils.  Your not going to do a .65mm (26
> mil)
> pitch QFN package with that as the OP is trying to do.  He either needs
> to
> use a larger package or have the board professionally made.
>
> Maybe someone that's really really good with homemade PC boards can do
> this,
> but that's going to take some experience and experimenting at best.

It is doable, but painful. QFN is a horrible package to deal with at
home, especially if it's more than 20 pins and tight pitch. Getting heat
to flow under the chip with such thin traces is really hard.

Bob

-- http://www.fastmail.fm - Access your email from home and the web

2010\12\20@123007 by Dwayne Reid

flavicon
face
At 08:07 AM 12/20/2010, Olin Lathrop wrote:
>Kerry Wentworth wrote:
> > It really isn't that hard.  Print the artwork on to magazine paper
> > with a laser printer, transfer to copper clad using a laminator, and
> > etch.  I can reliably do .5mm spacing, which is as small as I can
> > comfortably do hand soldering.
>
>Maybe someone that's really really good with homemade PC boards can do this,
>but that's going to take some experience and experimenting at best.

We don't make many PCB's in-house anymore but we used to.

Our process changed: we started out by using a negative photo process using DuPont Riston laminate - easy to do, extremely good resolution, relatively non-hazardous chemistry.  We made thousands of boards using that process over a 15 year period.

Eventually our production volumes increased to the point where using dedicated PCB fab houses made sense.  We kept the photo process going for several years so that we could do extremely quick prototypes (it was often possible to run 2 or 3 different spins on the same design in a single day) but one day, our extremely geeky hardware guy got his little CNC mill working well enough that milling PCB's became easier.

We still mill simple prototype boards but AP Circuits out of Calgary, Canada does most of the rest.  I generally have 1 or 2 designs into APC each month for their 2-day quick-turn proto service.

I've also got an inexpensive Chinese supplier who will supply a 200 square inch panel in 3 weeks for $90 (includes shipping).  I've mentioned them previously on this list - the company is Univelop and the website is <http://www.pcbgeek.com> .

But I can understand why hobbyists want to etch the boards themselves - it ** IS ** quick and the results can be extremely rewarding.

dwayne

-- Dwayne Reid   <TakeThisOuTdwaynerEraseMEspamspam_OUTplanet.eon.net>
Trinity Electronics Systems Ltd    Edmonton, AB, CANADA
(780) 489-3199 voice          (780) 487-6397 fax
http://www.trinity-electronics.com
Custom Electronics Design and Manufacturing

2010\12\20@123205 by Mark Rages

face picon face
On Mon, Dec 20, 2010 at 11:12 AM, Bob Blick <RemoveMEbobblickspamTakeThisOuTftml.net> wrote:
{Quote hidden}

QFN is not bad with a toaster oven / hot plate process.  I wouldn't
try it with an iron.

Regards,
Mark
markrages@gmail
-- Mark Rages, Engineer
Midwest Telecine LLC
markragesEraseMEspam.....midwesttelecine.com

2010\12\20@124526 by fred jones

picon face


> > It is doable, but painful. QFN is a horrible package to deal with at
> > home, especially if it's more than 20 pins and tight pitch. Getting heat
> > to flow under the chip with such thin traces is really hard.
> >
> > Bob
>
> QFN is not bad with a toaster oven / hot plate process. I wouldn't
> try it with an iron.
>
> Regards,
> Mark
> markrages@gmail

I do it.  I tin a couple of side by side pads.  Then I place the chip so that the pins line up with the pads (the hardest part of it).  Then I touch the pins over the tinned pads to tack the chip down.  Then I go to another row of pins and blob solder down the row of pins.  I do this for all sides.  Then I get de-soldering braid and suck up the excess.  This sounds terrible but works great.  I very rarely end up with a pin not soldered or a short..  I have to admit I was nervous the first time I tried it but it's standard practice for me now.
BTW, keep up the good work Nathan.
Good luck,
FJ                                          

2010\12\20@124554 by Spehro Pefhany

picon face
At 11:55 AM 20/12/2010, you wrote:
{Quote hidden}

IME, different factories or at least production lines are used for
single and double-sided boards when supplied in quantity. If you get
quotes for single-side boards from domestic companies that are set up
primarily to do double-sided, the price won't be much different. If your
niche is small lots of expensive stuff, that's fine. If you have to make
stuff as cost-effectively as possible in quantities in excess of (say) 5K,
then it would be irresponsible not to look carefully at single-sided boards,
despite the obvious(?) disadvantages. Punched boards can be even cheaper
because they avoid the NC drilling step AND routing (or shearing) step
(not generally compatible with conventional plated-through holes,
though you'll see exceptions like the boards in TV remote controls).

Double-sided and multilayer boards are typicaly quoted by the square
inch or cm^2, and single-sided by the square _meter_, which should tell
you something!


>Best regards,

Spehro Pefhany --"it's the network..."            "The Journey is the reward"
EraseMEspeffspaminterlog.com             Info for manufacturers: http://www.trexon.com
Embedded software/hardware/analog  Info for designers:  http://www.speff.com

2010\12\20@163511 by IVP

face picon face
> My main board supplier definitely charges significantly less for
> single-sided boards

Same here. I always get SS if I really don't need DS

Jo

2010\12\20@163512 by IVP

face picon face
>> Maybe someone that's really really good with homemade PC
>> boards can do this, but that's going to take some experience
>> and experimenting at best

Making the PCB is the easy bit. I can go as small as you like
with a Sharpie. SSOP (0.65mm), TQFP (0.8mm) are reasonably
routine for me as a lot of ICs are not desirable or available in DIP

> It is doable, but painful. QFN is a horrible package to deal with at
> home, especially if it's more than 20 pins and tight pitch. Getting
> heat to flow under the chip with such thin traces is really hard.

Agree. The experimental failure rate is 'off-putting'. I don't even
consider QFN at home any more

SSOP is about as small as I'm comfortable with for hand-soldering.
I've found the best way is to very thinly tin the copper and reflow
with the iron. Extra solder can be added, carefully, at a distance
and letting it run to the pin, which avoids bridging

Jo

2010\12\23@195318 by Nathan House

picon face
I think I've corrected the mistakes that were noted. Here's the new
schematic and layout:

Schematic: www.roboticsguy.com/images/misc/pic18f4550_tqfp_schematic2.png
Layout #1: www.roboticsguy.com/images/misc/pcb1.png
Layout #2: http://www.roboticsguy.com/images/misc/pcb2.png

Do the new schematic and layout look any better? Any more suggestions
how I can improve them?

I think the biggest problem that people noticed with the board was the
ground loop. I posted two different ways of routing the ground traces
above; is one better than the other?

Thanks again for all of your help, everyone

2010\12\23@225021 by Oli Glaser

flavicon
face
On 24/12/2010 00:53, Nathan House wrote:
> I think I've corrected the mistakes that were noted. Here's the new
> schematic and layout:
>
> Schematic: www.roboticsguy.com/images/misc/pic18f4550_tqfp_schematic2.png
> Layout #1: www.roboticsguy.com/images/misc/pcb1.png
> Layout #2: http://www.roboticsguy.com/images/misc/pcb2.png
>
> Do the new schematic and layout look any better? Any more suggestions
> how I can improve them?
>
> I think the biggest problem that people noticed with the board was the
> ground loop. I posted two different ways of routing the ground traces
> above; is one better than the other?
>
> Thanks again for all of your help, everyone!

Both look reasonable to me, not much to choose between them - probably as good as you will get for a single layer layout without lots of jumpers.
If pushed I might pick the second one as it has a better approximation of a star ground (the first looks to have a larger loop area)
This is at a glance though, others may disagree. Both should work okay though (assuming no plans to use the analogue peripherals for sensitive tasks)
I have had a 4550 running 20MHz crystal and USB fine on a breadboard with a fairly dodgy layout.
I would go ahead and try it out now - good luck..

2010\12\24@073803 by Olin Lathrop

face picon face
Nathan House wrote:
> Schematic:
> http://www.roboticsguy.com/images/misc/pic18f4550_tqfp_schematic2.png

That is much more readable.  The PIC is more undestandable, but it took me a
while to catch that MCLR is now placed in the middle of port B.

I didn't check whether you had PGC/PGD the right way around.  Since this
chip has the dedicated programming port, you can use that and free up the
port B programming pins.  What you have will work fine though.

It would be a good idea to note what the expected Vdd voltage range is.

C7 still doesn't need to be polarized.  10uF 10V ceramic caps are plentiful,
and cheaper and better than their electrolytic or tantalum counterparts.
With C7 being ceramic, you can get rid of C6 altogether.

If you just want a indicator LED, I would connect it to something other than
the only UART receive pin.  In fact, I would bring the RX and TX pins out to
pads in preference to most of the others.


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

2010\12\24@095954 by Matt Bennett

flavicon
face
On Thu, December 23, 2010 6:53 pm, Nathan House wrote:
> I think I've corrected the mistakes that were noted. Here's the new
> schematic and layout:
>
> Schematic:
> www.roboticsguy.com/images/misc/pic18f4550_tqfp_schematic2.png
> Layout #1: www.roboticsguy.com/images/misc/pcb1.png
> Layout #2: http://www.roboticsguy.com/images/misc/pcb2.png
>
> Do the new schematic and layout look any better? Any more suggestions
> how I can improve them?
>
> I think the biggest problem that people noticed with the board was the
> ground loop. I posted two different ways of routing the ground traces
> above; is one better than the other?

I didn't see all of the original thread- too lazy to look back at the 3000
unread piclist emails to find the all the previous comments :) But in the
spirit of the Internet, I'll boldy go on without full knowledge.

With respect to the ground trace- if possible with your layout program
(Eagle?), do a flood of the ground plane- with a bit of extra space around
the differential pair of the USB. The important part to remember is that
every current has a return current- with a flood there is more opportunity
for the current to get back to the source.  In addition, it uses up less
etchant.  Also, since you are doing this yourself, watch out for the acute
angles (such as you have with the differential pair going to the USB
connector- it can have a tendency to overetch- this is known by some
people as an "acid trap"

You should also connect the power pin of the USB to an I/O (as in figure
17-11 of the part's datasheet).  Not an absolute requirement for
operation, but a really good idea.

Since you're going SMT on the PIC, why not do SMT on other components? The
components are cheap and you don't have to drill.  I definitely recommend
a decoupling capacitor at every power pin pair- SMT allows you to put it
really close to the PIC, where it does the most good.

Instead of the RJ11, consider using a 0.1" spacing single-row header. Microchip has an adapter to the RJ11 (AC164110) that is pretty cheap, and
Olimex also has one that is half the price (you can get it via sparkfun). It uses the same basic pinout, (you can find the pinout in the PICKIT2 or
3 manuals).  Most of the newer Microchip demo boards support this, and it
takes up far less room on your PCB.

One other thing that is cheap insurance- consider putting a diode across
the power input- just in case you accidentally reverse the power leads,
you'll short out the power supply (and if you're using a typical
wall-wart, it won't blow up, it will just go into current limit, while
making the diode very hot, but it gives you a few seconds to realize your
error and remove power before you destroy the PIC).

Matt Bennett
Austin, TX

The views I express are my own, not that of my employer, a large
multinational corporation that you are familiar with

2010\12\24@113123 by Nathan House

picon face
>Both look reasonable to me, not much to choose between them - probably
>as good as you will get for a single layer layout without lots of jumpers.

So really the only alternative is to make a second layer a ground
plane? Is that what most people do?


>That is much more readable.  The PIC is more undestandable, but it took me a
>while to catch that MCLR is now placed in the middle of port B.

I think on your eagle part the MCLR pin is located at the lower left
hand corner. I moved mine up with the PGM, PGC, and PGD pins so that I
didn't have to run a wire down, across, and back up the PIC symbol in
the schematic (for the ICD connector). Is that what you would have
done?


>Since this chip has the dedicated programming port, you can use that and
>free up the port B programming pins.

I'm a little confused about the dedicated programming port. The datasheet says:

"The ICPRT Configuration bit can only be programmed through the
default ICSP port MCLR/RB6/RB7)."

So from what I've read it looks like I have to do the initial
programming of the chip through the default ICSP port, which is a
problem if I wire the RJ-11 connector to the dedicated programming
port, right?

This does raise another question I had, though. I read on some forum
that ICPORTS should be tied to VDD instead of being left floating.
Should I do the same for the other NC pins?


>You should also connect the power pin of the USB to an I/O (as in figure
>17-11 of the part's datasheet).  Not an absolute requirement for
>operation, but a really good idea.

Is this for sensing when the USB is plugged in?


>Instead of the RJ11, consider using a 0.1" spacing single-row header

I used to, but it seemed like my ICSP cable was always really loose
and sometimes didn't have a good connection. The RJ-11 jack is really
sturdy and guarantees a good connection. But your right that it would
save a lot of space.


>Since you're going SMT on the PIC, why not do SMT on other components?

Everybody seems to be suggesting this, maybe I should..

If I did get SMT parts for the capacitors and resistors, should I go
for 0805, 1206, or 1210 packages? From what I've read it doesn't seem
like the package size affects capacitors, but for resistors the
package size represents the power rating, being 1/10W, 1/8W and 1/4W
respectively. It seems like 1/10W (or 20mA at 5V) is a little low, so
I'm leaning towards getting the 1210 packages, but I want to see what
you guys think

2010\12\24@120453 by Olin Lathrop

face picon face
Nathan House wrote:
> So really the only alternative is to make a second layer a ground
> plane? Is that what most people do?

Yes, or at least mostly a ground plane.  Single layer boards are for
hobbyists who make their own boards, or for commercial products when the
volume is very high and the engineer knows exactly what he's doing.

Often I will make a two layer board and use the bottom as a pseudo ground
plane.  I make it a ground polygon and set the cost of routing in that layer
high.  That way it gets used only for "jumpers" when routing on the top
layer only is impossible.  You do have to clean up these jumpers, especially
since Eagle likes to clump them together despite the hugging parameter set
to 0.  In this case, distributed multiple small jumpers are better than a
single large clump.

> I think on your eagle part the MCLR pin is located at the lower left
> hand corner. I moved mine up with the PGM, PGC, and PGD pins so that I
> didn't have to run a wire down, across, and back up the PIC symbol in
> the schematic (for the ICD connector). Is that what you would have
> done?

Obviously not, since I put MCLR in a corner, which you even noted (actually
it's usually the upper left corner, but it certainly doesn't appear in the
middle of a contiguous port).

> I'm a little confused about the dedicated programming port. The
> datasheet says:

The datasheet is a bit confusing in this area.  The dedicated port can be
used by itself, but you're fine leaving things the way you have them.

>> You should also connect the power pin of the USB to an I/O (as in
>> figure 17-11 of the part's datasheet).  Not an absolute requirement
>> for
>> operation, but a really good idea.
>
> Is this for sensing when the USB is plugged in?

That's probably what he had in mind.  However, that can cause another
problem too.  You have to make sure USB is only plugged in after the other
power is already applied, and unplugged before the other power is removed.
You could get around this with a diode or just leave it how you had it.

On the other hand, why not power the whole thing just off the USB?  Do you
really need a separate power supply?

> Everybody seems to be suggesting this, maybe I should..
>
> If I did get SMT parts for the capacitors and resistors, should I go
> for 0805, 1206, or 1210 packages?

0805.  That is a mainstream package, but big enough to be easy to handle.
Lots of parts are available in 1206 and 1210, but consider those for only
when you need higher power resistors or extra capacitance at a particular
voltage not available in 0805.  If I remember right, the largest capacitor
in your design is 10uF 10V (or even 6.3V).  That will be readily available
in 0805.  Remember to stay away from ceramics that start with Y though.
Those are for high volume designs when the engineer knows exactly what he's
doing.


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

2010\12\24@123135 by Matt Bennett

flavicon
face
On Fri, December 24, 2010 10:31 am, Nathan House wrote:
>>Both look reasonable to me, not much to choose between them - probably
>>as good as you will get for a single layer layout without lots of
>> jumpers.
>
> So really the only alternative is to make a second layer a ground
> plane? Is that what most people do?

For learning- doing things on one layer with jumpers is usually good
enough.  You might run into issues if you went to production.  A ground
plane tends to make the board radiate less and be less susceptible to
external interference.  It can be a pain to etch your own 2 sided board.


{Quote hidden}

That's how I read it, too. Makes it kinda difficult to prototype with.

> This does raise another question I had, though. I read on some forum
> that ICPORTS should be tied to VDD instead of being left floating.
> Should I do the same for the other NC pins?

Datasheet explicitly says to leave them NC.

>>You should also connect the power pin of the USB to an I/O (as in figure
>>17-11 of the part's datasheet).  Not an absolute requirement for
>>operation, but a really good idea.
>
> Is this for sensing when the USB is plugged in?

Yes.  The USB spec says that there shouldn't be anything on the USB pins
unless the device detects voltage on the USB power pin.  It may also
confuse the USB code and/or host.


{Quote hidden}

Cost is the biggest issue on capacitors (small high value parts get pretty
expensive).  If you're thinking about decoupling capacitors, ideally you
want to use the smallest package, but for the frequencies that these parts
are concerned with, it won't matter.  You'll probably find 0603 caps way
too much of a pain to solder as a beginner, particularly without an
assembly microscope. 0805 is a good compromise.

SMT parts are so commonplace that you should get used to working with
them. Also, if you avoid SMT, a huge variety of parts will be inaccessible
to you (as many parts are just not available in through hole packages). Get a good pair of very sharp tweezers (not terribly expensive- I've
gotten a couple from dealextreme.com). Keep the tips in good shape- I try
to store my tweezers in some packaging foam.  Dropping them onto a hard
surface will destroy them... or they may miss the floor and pierce your
foot.

Matt Bennett
Austin, TX



The views I express are my own, not that of my employer, a large
multinational corporation that you are familiar with

2010\12\24@171123 by Christopher Head

picon face
-----BEGIN PGP SIGNED MESSAGE-----
Hash: SHA1

On Fri, 24 Dec 2010 12:05:47 -0500
"Olin Lathrop" <RemoveMEolin_piclistEraseMEspamEraseMEembedinc.com> wrote:

[snip]
> > I'm a little confused about the dedicated programming port. The
> > datasheet says:
>
> The datasheet is a bit confusing in this area.  The dedicated port
> can be used by itself, but you're fine leaving things the way you
> have them.
>
Can it really? Register 25-6 (CONFIG4L) shows that the ICPRT fuse is 0
in its unprogrammed state, which disables the dedicated port. How could
one possibly make use of the dedicated port without first changing the
value of at least this fuse, which can itself only be done through ICSP
on the RB6/7 port? I myself considered using the dedicated port but
discarded the idea for exactly this reason. If anyone actually knows
how the port is intended to be used, I'm genuinely curious!

All I can think of is bringing both ports out to headers, using the
RB6/7 port to enable ICPRT, then using the dedicated port for all
subsequent work, reusing RB6/7 in the application and just leaving the
header open. But allocating all the board space for the second header
seems pretty excessive... Maybe you could use a single header with
jumpers which you later cut, or something...

Chris
-----BEGIN PGP SIGNATURE-----
Version: GnuPG v2.0.16 (GNU/Linux)
Comment: GnuPT 2.7.2

iEYEARECAAYFAk0VGocACgkQXUF6hOTGP7eRNwCfc1AMqKw9VfniOD6Ukl+odMaq
9/YAnR8Fm5J5LS2r31T/xFBtOd18ERPn
=8928
-----END PGP SIGNATURE-----

2010\12\25@023650 by RussellMc

face picon face
> This does raise another question I had, though. I read on some forum
> that ICPORTS should be tied to VDD instead of being left floating.
> Should I do the same for the other NC pins?

I'll "answer" that generally. Others are welcome to disagree with my answer..

Doing other than what is recommended or allowed by the manufacturer
with any pin immediately puts you outside safe territory. It may be
the right or best thing to do for some reason but you are immediately
"fighting city hall". City Hall isn't always right - but if you
insiste on fighting them you MUST know why you are doing it,
understand what the implications may be, be prepared to take the
consequences and be aware that you leave yourself with no comeback if
almost any result occurs as a consequence.

NC pins are specified  as NC for a range of reasons. Some are obvious
enough in intent that you might safely connect them to "something"
with a fair chance of success. But eg grounding some internal circuit
node that exists perhaps as a test point for the manufacturer may have
unknowable consequences which can be as subtle as you could wish. As a
guide (more below), if a change is trivially simple and apparently
beneficial(eg ground NC pin xxx) then odds are somebody hasn't
understood something that the manufacturer had in mind.

As you will be well aware, the quality of internet sourced information
and the capability, competence and degree of understanding of people
who are prepared to provide a confidently assertive opinion or
statement of fact is very very very variable. It is usually easier to
find a technically poor option than a high quality one.
You know this :-). Even in a forum with many members and with some of
high competence, opinions which contradict manufacturers' advice or
instructions are at the least "risky" and need to be understood at
least aswell as possible and/or vouchsafed for by people who are
apparently more competent than yourself and whose abilities you trust.
They may be wrong. You know all that too.

When it comes to connecting NC pins to eg ground: Who says so, why do
they think there is a need, why do they think it is not harmful, why
do they think it is useful or necessary, what does it appear to do,
why should it do what it is claimed to do, what are the apparent
possible undesired consequences, hazard a guess at unanticipated
consequences. THEN if this is such a fantastic idea why didn't the
manufacturer specify it this way, what may they know that others have
missed, why do we think that these others know so much more than the
manufacturer that they can decide better than them.
Then - has anyone taken this up with the manufacturer as a design
error or necessary revision, ... ???? !!!!
And more.

All that said, they MAY be right. BUT, know who you are believing  and
why and the probable consequence-probability locus.
:-)

After applying all this to NC pins, consider applying it to the rest
of life :-).


           Russell

2010\12\26@083620 by Olin Lathrop

face picon face
Matt Bennett wrote:
> A ground plane tends to make the board radiate less and be less
> susceptible to external interference.

It does, but that is not much of a issue for one-off or hobby boards.  For
such boards, the main point of a ground plane is to provide a very low
impedence common reference voltage for the other signals.


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

2010\12\26@180512 by William \Chops\ Westfield

face picon face

>> A ground plane

Is the loop in the GND/Power signals in this design really so much of  a problem?  With many modern chips having power on each side, I've  done (or rather, thought about doing) similar things in order to keep  a PCB single-sided.

1) The chips involved are small, so it's not a BIG loop.
2) As an antenna, you'd be looking at relevant frequencies of ~1GHz or  more; well above the operating frequency of the circuits.
3) Bypassing at each end (or at multiple points?) ought to mostly  negate inductance issues of the "long" traces.
4) I like having a loop of GND around the edge of my board even if  it's not specifically required by power wiring.  It feels like cheap  protection against ESD (contact with 'stuff' quickly shorts to GND  rather than entering a chip signal pin.)  Does this become a bad  idea?  (This includes a loop of GND on the PCB side opposite the  Ground plane, when doing a double-sided PCB.)

Trying to keep the PCB single-sided, is star-shaped gnd/power made of  jumper wires any better?  In the interests of short straight jumpers,  I've shaped GND/PWR into loop-like structures around the chips and  components on a board, rather than splayed or grid-like structure.  No ?

Thanks
BillW

2010\12\26@234526 by Matt Bennett

flavicon
face
On Sun, December 26, 2010 5:05 pm, William \"Chops\" Westfield wrote:
>
>>> A ground plane
>
> Is the loop in the GND/Power signals in this design really so much of
> a problem?  With many modern chips having power on each side, I've
> done (or rather, thought about doing) similar things in order to keep
> a PCB single-sided.

Umm... if you look at most modern chips, the power pins are usually
located really close to each other (old PICs, TTL, and analog parts are
the exception) but all the newer parts have the power pins located close
together- and on the quad parts (leads on 4 sides) there is usually power
on each side.

A magnetic antenna (a loop) is not as sensitive (frequency selective) to
size as a traditional dipole- it is more sensitive to cross sectional
area- why a ground plane really helps.  The number one thing to remember
is that every current has a return current.  If you can keep the path of
the current going in very close to the path of the current going out,
you're going to radiate far less, and be much less susceptible to
interference.  You'll also find that your rise-times are much faster.  I
did a circuit for my 2010 Master's class that had on the order of 800ps
differential rise time out of a PIC32.  It can be done- and at 800ps rise
time, there *is* energy in the GHz range. (This is with the first
generation of the PIC32, which did not have as much slew rate limiting)


{Quote hidden}

#4 can potentially mess with your rise-times, as you would have multiple
paths for the return current- and with all these paths, you very likely
will be inducing current in nearby traces- at high frequencies it doesn't
take much capacitance between traces to induce signals on nearby traces
that have nothing to do with the trace you are sending the signal down.
Signals will find a way to couple, and a few pF at high frequencies is a
relatively low impedance.

As Olin pointed out (and I pointed out as well, but I believe he
inadvertently left that part out :) it will probably be good enough for a
board you're learning with.  But it is good to know *why* your rise-times
are not what you expect, and why the signals on unrelated lines are not as
clean as they should be.  You may not be able to see them on a low
bandwidth scope, but don't let that fool you- they're there.

> Trying to keep the PCB single-sided, is star-shaped gnd/power made of
> jumper wires any better?  In the interests of short straight jumpers,
> I've shaped GND/PWR into loop-like structures around the chips and
> components on a board, rather than splayed or grid-like structure.  No ?

I've been under the impression that star grounds are more important with
high currents, to make sure that you have consistent references.  It is
important to understand where your high currents are- current across an
impedance means voltage- which can cause your ground reference to change-
which can lead to very weird outputs, particularly with respect to analog
parts.

Matt Bennett
Just outside of Austin, TX
30.510843,-97.919286

The views I express are my own, not that of my employer, a large
multinational corporation that you are familiar with

2010\12\27@054044 by RussellMc

face picon face
> I've been under the impression that star grounds are more important with
> high currents, to make sure that you have consistent references.  It is
> important to understand where your high currents are- current across an
> impedance means voltage- which can cause your ground reference to change-
> which can lead to very weird outputs, particularly with respect to analog
> parts.

I've found that when using star grounds, if the star is imperfect and
there are some common tracks (and it is unlikely that you want or are
realistically able to bring every earth back to a single point with a
star (reasons for ground planes carol gently in background) then being
sure that high current or noisy star limbs don't common up with analog
low level limbs really helps. (or, conversely, when I DIDN'T give that
enough attention ... :-) ) .

Beating a design to death with applied common sense usually gets you a
fair bit of the way there.

Q: "Does this track carry large currents and/or processor or other
digital signals?"
A: "Yes."
Q: "Do they share any common return path?"
A: "Yes."
Q: "Why?"
A: "Um. Er."


 R

2010\12\27@083013 by Olin Lathrop

face picon face
'William Chops" Westfield ' <RemoveMEwestfwspam_OUTspamKILLspammac.com wrote:
> Trying to keep the PCB single-sided, is star-shaped gnd/power made of
> jumper wires any better?

I would start the routing by connecting all the PIC grounds together and
keeping the connections from the power pins thru the bypass caps back to the
ground short.  The same goes for the crytal connections and crystal cap
grounds.

Then you route everything else.  That may require a jumper or two, no big
deal.  If you're already going to solder 20 parts to the board, does it
really matter much if you now have to solder 22 and two of them are wires?

Remember that jumpers don't always need to be thru hole.  Thru hole jumpers
have the advantage they can be any length and orientation and can jump over
lots of stuff.  Sometimes that's useful.  However, sometimes you can get
away with 0 Ohm surface mount jumpers if you only need to jump over a single
trace.  This is where using a large surface mount size like 1206 may help if
you're making the board yourself.


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

2010\12\28@143503 by Nathan House

picon face
>> This does raise another question I had, though. I read on some forum
>> that ICPORTS should be tied to VDD instead of being left floating.
>> Should I do the same for the other NC pins?

>Datasheet explicitly says to leave them NC.


In case anyone else is confused on the ICPORTS pin, I found out that
it's supposed to be connected to VDD when using the dedicated icsp
port, but left as NC otherwise.

I think this is the forum post I read that led me to believe it was
supposed to be connected:

http://www.microchip.com/forums/tm.aspx?high=&m=479082&mpage=1#479186

>Hello i have a problem ... PORTE is always zero, LATE is always zero, and TRISE is always zero ...

>Problem Solved.
>i am programming the PIC18LF4550 in dedicated Mode;
>so i have to connect PIN NC/ICPORTS to VDD. without connecting this pin.
>PIC18LF4550 is emulating a 28 pin device.


The datasheet, under Section "25.9.2 28-PIN EMULATION," says:

"This 28-pin Configuration mode is controlled through a
single pin, NC/ICPORTS. Connecting this pin to VSS
forces the device to function as a 28-pin device.
Features normally associated with the 40/44-pin
devices are disabled along with their corresponding
control registers and bits. This includes PORTD and
PORTE ... On the other hand, connecting the pin to VDD
forces the device to function in its default configuration."

However, it then goes on to say:

"The configuration option is only available when background
debugging and the dedicated ICD/ICSP port
are both enabled ... When disabled,
NC/ICPORTS is a No Connect pin."

So you guys were right, it's not supposed to be connected for my board.


'[PIC] Need critique of my SMD PIC18F4550 PCB'
2011\01\04@191357 by Nathan House
picon face
I went ahead and changed the through hole resistors and capacitors to
SMT parts, since several people suggested that I do so.

http://www.roboticsguy.com/images/misc/4550_SMD_pcb.png

I think I'm going to make it tomorrow, so any last minute suggestions
you might have would be appreciated!

Thanks,

Natha

2011\01\04@201951 by Dwayne Reid

flavicon
face
At 05:13 PM 1/4/2011, Nathan House wrote:
>I went ahead and changed the through hole resistors and capacitors to
>SMT parts, since several people suggested that I do so.
>
>http://www.roboticsguy.com/images/misc/4550_SMD_pcb.png
>
>I think I'm going to make it tomorrow, so any last minute suggestions
>you might have would be appreciated!

Good move going to all SMD devices.

Question: are you intentionally not connecting the Vdd pin on the USB connector?  If so, how do you get power onto the board?  I don't see a power connector anywhere.

dwayne

-- Dwayne Reid   <RemoveMEdwaynerTakeThisOuTspamspamplanet.eon.net>
Trinity Electronics Systems Ltd    Edmonton, AB, CANADA
(780) 489-3199 voice          (780) 487-6397 fax
http://www.trinity-electronics.com
Custom Electronics Design and Manufacturing

2011\01\04@212955 by Oli Glaser

flavicon
face
On 05/01/2011 01:19, Dwayne Reid wrote:
> At 05:13 PM 1/4/2011, Nathan House wrote:
>> I went ahead and changed the through hole resistors and capacitors to
>> SMT parts, since several people suggested that I do so.
>>
>> www.roboticsguy.com/images/misc/4550_SMD_pcb.png
>>
>> I think I'm going to make it tomorrow, so any last minute suggestions
>> you might have would be appreciated!
> Good move going to all SMD devices.
>
> Question: are you intentionally not connecting the Vdd pin on the USB
> connector?  If so, how do you get power onto the board?  I don't see
> a power connector anywhere.
>
> dwayne
>

I can see a "Pwr Pins" label on the silk, so I assume that's how. Powering from the USB would be (IMHO more) convenient - or providing a jumper for either option, and use external if you are going to need more than 500mA or other voltage levels (for most small PIC projects this is unlikely though, so I think it would be nice to at least have the option of not needing an external power supply)
Only (small) thing I can spot is to be careful the crystal case does not short the traces it sits over, with there being no mask on the board - you could just make sure it's raised a bit (or hand paint some mask on if you have a touch up pen/lacquer or something)
I would maybe make your pad rings a bit thicker for easier drilling with less risk of breaking traces as you look to have plenty of room (the etched holes in the copper can be very small just to use as a drill guide - like 0.5mm or so)
Looks pretty good though, let us know how it goes, if it works okay etc...

2011\01\04@213104 by Nathan House

picon face
Yes, the board is self powered, so I left the USB Vdd pin unconnected.
I originally had a power connector and rj-11 jack at the bottom of the
board (to the left of the led), but to save room and cut down the cost
a little I changed the power jack to a 2 pin female header and the
rj-11 jack to a 6 pin male header

2011\01\05@035946 by IVP

face picon face
> Only (small) thing I can spot is to be careful the crystal case does
> not short the traces it sits over, with there being no mask on the
> board - you could just make sure it's raised a bit (or hand paint
> some mask on if you have a touch up pen/lacquer or something)

SMT crystals have an insulating pad on the bottom. Maybe add
something similar. Anything would do, like a piece of mica, thin
rubber or card. Only takes a minute, won't hurt to

> I would maybe make your pad rings a bit thicker

Agreed. Pads always come out looking smaller physically than
you thought they looked on paper. Make them as big as you
have room for. Plus it helps if you need to re-work the board.
Bigger pads will take more wear-and-tear

Jo

2011\01\05@061036 by Ruben Jönsson

flavicon
face
> > Only (small) thing I can spot is to be careful the crystal case does
> > not short the traces it sits over, with there being no mask on the
> > board - you could just make sure it's raised a bit (or hand paint
> > some mask on if you have a touch up pen/lacquer or something)
>
> SMT crystals have an insulating pad on the bottom. Maybe add
> something similar. Anything would do, like a piece of mica, thin
> rubber or card. Only takes a minute, won't hurt to

The through-hole crystal is on the top side (where there is no copper) so this is not a problem, right?

>
> > I would maybe make your pad rings a bit thicker
>
> Agreed. Pads always come out looking smaller physically than
> you thought they looked on paper. Make them as big as you
> have room for. Plus it helps if you need to re-work the board.
> Bigger pads will take more wear-and-tear
>
As I said before, I would arrange the pads so that one or more (ICD) board connectors could be used instead of soldering single wires to the board - they have a tendency to break when wiggled a couple of times. And yes - make the pads as large as you can.

/Ruben

==============================
Ruben Jönsson
AB Liros Electronic
Box 9124, 200 39 Malmö, Sweden
TEL INT +46 40142078
FAX INT +46 40947388
EraseMErubenspamspamspamBeGonepp.sbbs.se
==============================

2011\01\05@061536 by Geo

picon face
Nathan House wrote:

> I originally had a power connector and rj-11 jack at the bottom of the
> board (to the left of the led), but to save room and cut down the cost
> a little I changed the power jack to a 2 pin female header and the
> rj-11 jack to a 6 pin male header.

If using a simple pin header for power, I always make it 3 pins (one end pin no-connect) so that reversal does not result in a connection.

For power, I would never use female on the pcb as this could/will leave live bare pins floating around the bench at the end of the power supply cable.

George Smith

2011\01\05@062309 by Oli Glaser

flavicon
face
On 05/01/2011 11:10, Ruben Jönsson wrote:
> The through-hole crystal is on the top side (where there is no copper) so this
> is not a problem, right?

Of course... sorry for the silly mistake... :-)

2011\01\05@071901 by Olin Lathrop

face picon face
Nathan House wrote:
> I went ahead and changed the through hole resistors and capacitors to
> SMT parts, since several people suggested that I do so.
>
> http://www.roboticsguy.com/images/misc/4550_SMD_pcb.png

While thru hole is a good idea for most parts, I don't like it for external
connectors that will take some mechanical stress.  After enough connects and
disconnects, the solder bond will break or the pads will lift from the
board.  I think your USB connector should be thru hole.  I would keep
everything else SMD as you have it though.


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

2011\01\05@073335 by Wouter van Ooijen

face picon face
> While thru hole is a good idea for most parts, I don't like it for external
> connectors that will take some mechanical stress.

s/thru hole/smd/ ?

--
Wouter van Ooijen

-- -------------------------------------------
Van Ooijen Technische Informatica: http://www.voti.nl
consultancy, development, PICmicro products
docent Hogeschool van Utrecht: http://www.voti.nl/hvu

2011\01\05@074346 by RussellMc

face picon face
> As I said before, I would arrange the pads so that one or more (ICD) board
> connectors could be used instead of soldering single wires to the board - they
> have a tendency to break when wiggled a couple of times. And yes - make the
> pads as large as you can.

Strain relief on wires is a very very good idea [tm] if soldering
directly to PCB.

Compromise:

Provide hole in PCB where wire is to be attached.
Thread wire through hole from other side to pad then solder.
This provides much better strain relief than having none at all.

Better:  Provide two holes. Thread wire from pade side through hole1,
back through hole 2 then solder. This provides good strain relief.

_

Thicker multi strand wires are less prone to falling off under duress
than thinner ones. More strands and/or thicker strands helps.
Do not use single strand / solid core wires for interconnection
(unless you are doing it for a very special reason and understand the
mechanical implications).



                Russell McMaho

2011\01\05@074857 by Gordon

flavicon
face
> While thru hole is a good idea for most parts, I don't like it for external
> connectors that will take some mechanical stress.

I was going to strongly disagree, but I think you meant SMD?

Gordo

2011\01\05@075705 by Olin Lathrop

face picon face
Wouter van Ooijen wrote:
>> While thru hole is a good idea for most parts, I don't like it for
>> external connectors that will take some mechanical stress.
>
> s/thru hole/smd/ ?

Oops, yes.  Surface mount (SMD, SMT, other TLAs?) is a good idea for most
parts, except those that have to take mechanical stress.  Sorry for the
confusion.


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

2011\01\05@080108 by Olin Lathrop

face picon face
RussellMc wrote:
> Strain relief on wires is a very very good idea [tm] if soldering
> directly to PCB.
>
> Compromise:
>
> Provide hole in PCB where wire is to be attached.
> Thread wire through hole from other side to pad then solder.
> This provides much better strain relief than having none at all.
>
> Better:  Provide two holes. Thread wire from pade side through hole1,
> back through hole 2 then solder. This provides good strain relief.

Also good: Solder wires into single holes, then gob hot glue over them.


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

2011\01\05@081553 by Dave Tweed

face
flavicon
face
Nathan House wrote:
> Yes, the board is self powered, so I left the USB Vdd pin unconnected.

I might be mistaken, but I was always under the impression that the USB
power pin is not just about power -- it's also important for initializing
a connection. Isn't that one reason that the power/ground pins are longer
than the data pins in the connector? Every chip that supports USB that I've
worked with so far has a pin dedicated to USB power sensing. Isn't that true
of PICs? Also, I always connect the data-line pullup resistor(s) (for initial
speed sensing) to USB power.

-- Dave Twee

2011\01\05@081700 by alan.b.pearce

face picon face
> Yes, the board is self powered, so I left the USB Vdd pin unconnected.

Even so you will probably need to run a track from the USB Vdd pin to a capacitor with a discharge resistor so that the host will detect when you plug in the USB, and also to a pin on the chip so your program knows when the USB is plugged in to enable the USB module.
-- Scanned by iCritical.

2011\01\05@084704 by Olin Lathrop

face picon face
Dave Tweed wrote:
> Also, I always connect the
> data-line pullup resistor(s) (for initial speed sensing) to USB power.

The PIC has the speed sensing resistors built in.  They are switched in/out
depending on how the USB module is set up.  For this PIC, it is legitimate
to connect the USB D+ and D- lines directly to the PIC without anything else
on those nets.


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

2011\01\05@085128 by Oli Glaser

flavicon
face
On 05/01/2011 12:58, Olin Lathrop wrote:
> Surface mount (SMD, SMT, other TLAs?) is a good idea for most
> parts, except those that have to take mechanical stress.

I agree here, USB connectors have to take a considerable amount of stress, and home etched boards are generally more delicate/prone to pads and tracks lifting ( depending how well the copper is bonded to the FR4 - though I have found the make/quality of board can make a large difference here)

2011\01\05@135751 by Nathan House

picon face
A lot of great suggestions, thank you!

>The through-hole crystal is on the top side (where there is no copper) so this
>is not a problem, right?

Ordering SMD crystals didn't even cross my mind when I was getting the
capacitors and resistors. I guess just I thought of a crystal as being
a "through hole part", but really, there's probably an SMD equivalent
for every through hole part, isn't there..


>I would maybe make your pad rings a bit thicker

Are you talking about the pads for the crystal, or *all* of the pads
on the board? I just changed the crystal's pads (which were pretty
thin..) to be like most of the others. I'm not sure if I can make the
..1" spaced pads larger, though, because then there won't be much room
in between them.


>If using a simple pin header for power, I always make it 3 pins (one end
>pin no-connect) so that reversal does not result in a connection.

That's a really good idea!


>As I said before, I would arrange the pads so that one or more (ICD) board
>connectors could be used instead of soldering single wires to the board - they
>have a tendency to break when wiggled a couple of times.

There aren't going to be any wires soldered directly to the board. I'm
planning on using female break away headers for all of the I/O pins,
like these: http://www.sparkfun.com/products/115 . And then Male
headers for the ICSP connector, and I guess for the power pins, like
this: http://www.sparkfun.com/products/116 .


Somebody (or maybe a couple of people) mentioned that it would be a
good idea to have the option of powering the board from USB, and also
that having the USB voltage pin tied to a sense pin could be useful. I
tried adding two jumpers to accommodate this:

http://www.roboticsguy.com/images/misc/4550_SMD_pcb2.png

I highlighted the VDD traces. Is it alright to weave the VDD trace
between C3's (1206 package) pads? It looks like there's enough room,
both on the computer and on a paper printout, but I don't know if it's
generally an acceptable practice? Also, I made the VDD and GND traces
0.03" for much of the board, but will 0.02" be wide enough for the VDD
trace coming off the USB connector?


I tried following this image for the sense pin:
http://www.roboticsguy.com/images/misc/figure_17_11.png . The routing
looks a little odd, but I think it's the way the image shows it.


So, if this is works, I would be able to use jumper #1 to choose
whether or not I want to use an I/O pin on the PIC as a sense pin, and
#2 to power the board off of USB

2011\01\05@152627 by Oli Glaser

flavicon
face
On 05/01/2011 18:57, Nathan House wrote:
> A lot of great suggestions, thank you!
>
>> The through-hole crystal is on the top side (where there is no copper) so this
>> is not a problem, right?
> Ordering SMD crystals didn't even cross my mind when I was getting the
> capacitors and resistors. I guess just I thought of a crystal as being
> a "through hole part", but really, there's probably an SMD equivalent
> for every through hole part, isn't there..
>
>

Yes, for 99% there are SMD equivalents, but not the other way round (i.e many parts nowadays have no through hole version, so avoiding SMD will limit you greatly)
As mentioned though, through hole is useful for parts that will experience mechanical stress (and also still used commercially for things like all discrete "vintage" designs, i.e audio/tube amps etc, or maybe to breadboard/stripboard an idea to confirm operation before converting design to SMD - I have a stock of generic "common" through hole parts for this purpose - passives/transistors/opamps/sensors/LEDS/timers etc)

>> I would maybe make your pad rings a bit thicker
> Are you talking about the pads for the crystal, or *all* of the pads
> on the board? I just changed the crystal's pads (which were pretty
> thin..) to be like most of the others. I'm not sure if I can make the
> .1" spaced pads larger, though, because then there won't be much room
> in between them.
>
>

All the pads, where there is room - looks to be plenty on quite a few of the pads (remember you don't have to keep the pads circular, you can extend them just in one direction - main idea is to provide a bit of extra copper make drilling easier and avoid the risk of breaking contact between pad and track)  You can go down to 0.8mm gap or so between the 2.54mm (0.1") spaced pads comfortably. As mentioned, a nice thick annular ring is good for drilling also, I use a ~0.5mm hole usually regardless of what the final hole size will be.


>> If using a simple pin header for power, I always make it 3 pins (one end
>> pin no-connect) so that reversal does not result in a connection.
> That's a really good idea!
>
>

I agree, nice idea, and easy to implement. Anything that lessens the impact of (inevitable) human error is a good thing.

{Quote hidden}

Yes that's fine, done all the time on production boards - have to be a bit more careful with no solder mask though on home etched boards, this is where a (mask) touch up pen or a bit of lacquer brushed in between the cap pads would come in handy. I have done this on quite a few (self etched) boards with no problems, just be careful soldering and check for shorts with a multimeter afterwards.

> Also, I made the VDD and GND traces
> 0.03" for much of the board, but will 0.02" be wide enough for the VDD
> trace coming off the USB connector?
>

Yes, should be fine.

> I tried following this image for the sense pin:
> http://www.roboticsguy.com/images/misc/figure_17_11.png . The routing
> looks a little odd, but I think it's the way the image shows it.
>
>
> So, if this is works, I would be able to use jumper #1 to choose
> whether or not I want to use an I/O pin on the PIC as a sense pin, and
> #2 to power the board off of USB.

Looks okay I think, the resistor to ground to pull the pin down on disconnect. Best to go from the datasheet for the various configurations anyway as it varies (some parts have an internal regulator for the USB module, dedicated sense pin etc)
By the way, I take it you are using a 5V part? (can't recall which it was)

One last thing, (pretty obvious but I have made the mistake before) - make sure the through hole parts on the other side of the board are actually placed that way in your design software, so the pads are the right way round (for asymmetrical parts like the USB connector/programming header - I think it would be the wrong way round for the Pickit2 if it is a right angle header)



2011\01\05@154734 by Christopher Head

picon face

On 5 January 2011 05:16,  <RemoveMEalan.b.pearceKILLspamspamstfc.ac.uk> wrote:
>
> > Yes, the board is self powered, so I left the USB Vdd pin unconnected.
>
>  Even so you will probably need to run a track from the USB Vdd pin to a capacitor with a discharge resistor so that the host will detect when you plug in the USB, and also to a pin on the chip so your program knows when the USB is plugged in to enable the USB module.

That's not how the host detects an attachment, it detects it when a
pullup resistor appears on one of the data lines (D- in the case of a
low-speed device or D+ in the case of a full-speed device). There is
no requirement to load Vusb. However, there *IS* the requirement that
you must never source current upstream into D+ or D- if Vusb is low,
so a self-powered device needs to sense Vusb and disable the USB
module (hence disconnecting the pullup resistor) when that happens
(e.g. when a complete cable connection exists from device to host, but
the host itself is powered down while the device is powered up). A
bus-powered device doesn't need to do this because when Vusb goes low,
the device no longer has any current to source into a data line.

Chris

2011\01\05@165430 by Bob Ammerman

flavicon
face
>>If using a simple pin header for power, I always make it 3 pins (one end
>>pin no-connect) so that reversal does not result in a connection.
>
> That's a really good idea!

Or even better: on the board connect Pins 1 & 3 to power and Pin 2 to ground. Now no matter which way you connect the three pin header it will work.

-- Bob Ammerman
RAm Systems

2011\01\05@175102 by Jon Chandler

picon face
Bob Ammerman wrote:
>>> If using a simple pin header for power, I always make it 3 pins (one end
>>> pin no-connect) so that reversal does not result in a connection.
>>>        
>> That's a really good idea!
>>      
> Or even better: on the board connect Pins 1&  3 to power and Pin 2 to
> ground. Now no matter which way you connect the three pin header it will
> work.
>
> -- Bob Ammerman
> RAm Systems
>
>
>    On one hand, I think it's a good idea to provide a blocking diode or even a bridge rectifier on products using a coaxial power connector to prevent disaster.  The down side is the products that do use a bridge rectifier but then decide not to mark any polarity for the jack.  If I don't know what power supply goes with the device and it's not marked, I worry about hooking up a supply of the wrong polarity.  I've pulled things apart before to determine the needed polarity.  It's nice but frustrating to find a bridge rectifier - a bunch of wasted effort just to determine that it doesn't matter!

Jon

2011\01\05@180256 by Dwayne Reid

flavicon
face
At 02:54 PM 1/5/2011, Bob Ammerman wrote:
> >>If using a simple pin header for power, I always make it 3 pins (one end
> >>pin no-connect) so that reversal does not result in a connection.
> >
> > That's a really good idea!
>
>Or even better: on the board connect Pins 1 & 3 to power and Pin 2 to
>ground. Now no matter which way you connect the three pin header it will
>work.

I usually do it the other way around: outside pins are Gnd, middle pin is power.

Lots of reasons but the main one is that you can NEVER have too many ground pins <grin>.  The extra ground pin is useful for clipping your scope to, for example.

dwayne

-- Dwayne Reid   <dwaynerSTOPspamspamspam_OUTplanet.eon.net>
Trinity Electronics Systems Ltd    Edmonton, AB, CANADA
(780) 489-3199 voice          (780) 487-6397 fax
http://www.trinity-electronics.com
Custom Electronics Design and Manufacturing

2011\01\05@182154 by MCH

flavicon
face
And it helps to 'guard' the power line from stray wires.

Joe M.

Dwayne Reid wrote:
{Quote hidden}

2011\01\09@200311 by IVP

face picon face
> Surface mount (SMD, SMT, other TLAs?) is a good idea for
> most parts, except those that have to take mechanical stress

I just repaired my niece's brand new mp3 player. The first time
she plugged the earphones in, the jack socket came completely
off the board

An SMT 3.5mm stereo socket with the flimsiest of soldering,
didn't even cover the pins. 2 seconds with an iron made it stronger
than the factory did. There was room to make it through-hole

But even through-hole connectors often fail. Many times the
solderable body anchors aren't used and all the strain is taken
by the pads, which are usually at the other end of the body to
the entry, meaning they have to take the added leverage of the
plug. So simple to double-side solder body lugs

Jo

More... (looser matching)
- Last day of these posts
- In 2011 , 2012 only
- Today
- New search...