Searching \ for '[EE] PCB critique' 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: 'PCB critique'.

Exact match. Not showing close matches.
PICList Thread
'[EE] PCB critique'
2010\10\28@190421 by David

flavicon
face
(Reposting with tag)

Thanks to all for the comments in the "routing SMD boards" thread, which were really helpful in finishing this off.  Opening this to critique on here will be fun I'm sure :)

The circuit is a FT232R breakout, for use with breadboards.  It exposes all of the serial pins and includes the LEDs, selectable VCCIO and switched USB power with soft-start.

Never having used this chip (and being a complete electronics amateur) I am unsure how well these different features will interact.

The board is designed to meet BatchPCB 2-layer rules.  That does mean fairly large vias.

Schematic: http://tinyurl.com/2uhbr68
     Route: http://tinyurl.com/33kxen6
      Silk: http://tinyurl.com/3575prt

Constructive feedback welcome.

Davi

2010\10\28@231442 by Mark Rages

face picon face
On Thu, Oct 28, 2010 at 6:04 PM, David <spam_OUTlistsTakeThisOuTspamedeca.net> wrote:
{Quote hidden}

I suggest you remove all those islands of unconnected copper.

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

2010\10\28@233542 by Brent Brown

picon face
On 29 Oct 2010 at 0:04, David wrote:

{Quote hidden}

In the schematic T1 is a P channel MOSFET and it appears Drain/Source may be the wrong way around from what is intended. The symbol for the body diode gives it away... with the orientation shown the diode will conduct and USB5V_SWITCHED will be on all the time regardless of the state of the Gate.

I'm not sure what C1 is there for. At power on, assuming C1 is discharged, it will try to turn the MOSFET on - probably creating a a power on glitch in USB5V_SWITCHED which may not be desireable.

Otherwise it looks good~!

-- Brent Brown, Electronic Design Solutions
16 English Street, St Andrews,
Hamilton 3200, New Zealand
Ph: +64 7 849 0069
Fax: +64 7 849 0071
Cell: +64 27 433 4069
eMail:  brent.brownspamKILLspamclear.net.nz

2010\10\29@070419 by David

flavicon
face
Quoting Brent Brown <.....brent.brownKILLspamspam.....clear.net.nz>:
> On 29 Oct 2010 at 0:04, David wrote:
>> Schematic: http://tinyurl.com/2uhbr68
>
> In the schematic T1 is a P channel MOSFET and it appears Drain/Source may be
> the wrong way around from what is intended. The symbol for the body  
> diode gives it
> away... with the orientation shown the diode will conduct and USB5V_SWITCHED
> will be on all the time regardless of the state of the Gate.

Brent, thanks!  Yes, this is backwards.  What a stupid mistake on my part.

> I'm not sure what C1 is there for. At power on, assuming C1 is  
> discharged, it will try
> to turn the MOSFET on - probably creating a a power on glitch in
> USB5V_SWITCHED which may not be desireable.

The datasheet appears to suggest that it forms part of the "soft  start" for the USB controlled power.  Section 6.3 (page 25) of  http://tinyurl.com/32mwfp2 if you are interested.

I'll fix that mistake.

Davi

2010\10\29@081239 by Olin Lathrop

face picon face
part 1 2148 bytes content-type:text/plain; charset="iso-8859-1" (decoded quoted-printable)

David wrote:
> Schematic: http://tinyurl.com/2uhbr68

Some of the writing is so small that I can't read it even though I'm viewing
it in a browser maximized on a 1920x1200 screen.  It's also a vertical
format which is unusual at best and uses my screen inefficiently.

Raster images (yours was a PNG file) are not appropriate for schematics.
PDF is much better.  For maximum ease of others viewing your schematics,
design them up front with sheets in landscape format the size of normal
paper.  Here in the US that would be 8 1/2 x 11 inches.  Use more sheets as
you need to, then print all sheets to a single PDF document.

If you're using Eagle, you can start each sheet with the FRAME-8X10-XY-H
device in my SYMBOLS library.  That puts a nice frame on the page of the
right size, leaves a space for the title, last modified time, etc, and puts
coordinates around the edges.  These coordinates come in handy later when
you use my INDEX ULP to make a parts locator index.

Before Russell or anyone else jumps on me for saying this, they should look
at the attached screen shot.  That's what a piece of the schematic looked
like in my maximized browser window.

> Route: http://tinyurl.com/33kxen6

I see some things, possibly unconnected islands, but it's hard to tell on
this small image.  If this is done in Eagle, post the Eagle .brd file.
Those that don't have Eagle won't be able to comment, but those that do can
examine the board the way they are used to.  I fell like both hands are tied
behind my back when looking at that tiny image.

>        Silk: http://tinyurl.com/3575prt

There appears to be some mirrored writing in the top right corner.  What's
the point of the elaborate graphic under the USB connector?  It won't help
the manufacture install it correctly and it can't be seen once installed.
This is also apparently more than just the silkscreen since SMD pads are
shown.

Again, it would be better to post the Eagle .brd file instead of or in
addition to these files.  Without being able to poke around and really see
what's on what layer, I don't feel I can say much.


part 2 2355 bytes content-type:image/gif; name="b.gif" (decode)


part 3 181 bytes content-type:text/plain; name="ATT00001.txt"
(decoded base64)

--
http://www.piclist.com PIC/SX FAQ & list archive
View/change your membership options at
mailman.mit.edu/mailman/listinfo/piclist

2010\10\29@083052 by David

flavicon
face
Quoting Olin Lathrop <EraseMEolin_piclistspam_OUTspamTakeThisOuTembedinc.com>:
> David wrote:
>> Route: http://tinyurl.com/33kxen6
>
> I see some things, possibly unconnected islands, but it's hard to tell on
> this small image.

There are indeed.  You are the second person to comment on this, so I  will turn that off on the pour.

>>        Silk: http://tinyurl.com/3575prt
>
> There appears to be some mirrored writing in the top right corner.

That's on the underside.  I simply use it for my own future reference  to pull up the right project.  Two sided silkscreen at my current  board maker is standard.

> What's
> the point of the elaborate graphic under the USB connector?  It won't help
> the manufacture install it correctly and it can't be seen once installed.
> This is also apparently more than just the silkscreen since SMD pads are
> shown.

No idea!  I didn't design the USB connector, it is from one of the  standard libraries.

> Again, it would be better to post the Eagle .brd file instead of or in
> addition to these files.  Without being able to poke around and really see
> what's on what layer, I don't feel I can say much.

OK, that advice and your information about PDF and orientation are all  taken.  Once I have fixed other errors tonight I will upload them.

Thanks.

Davi

2010\10\29@190525 by David

flavicon
face
On 29/10/2010 13:13, Olin Lathrop wrote:
> Again, it would be better to post the Eagle .brd file instead of or in
> addition to these files.  Without being able to poke around and really see
> what's on what layer, I don't feel I can say much.

Taken on board most comments.  Also fixed a bunch of stuff that was wrong in v1 (from comments on PIClist and a forum).

The board is now more compact and space is used more wisely I think. The PDF is even in landscape format (A4).

  PDF: http://tinyurl.com/36xp3u2
Eagle: http://tinyurl.com/2vrj2e6 (ZIP)

Comments on attempt two are very welcome.

Davi

2010\10\30@101240 by Olin Lathrop

face picon face
David wrote:
> PDF: http://tinyurl.com/36xp3u2

That's a lot better although still sloppy in various places.  Many of the
labels are rotated making them difficult to read.  A good example is T1, the
IRLML6402.  Neatness counts.  The level of care you take in your schematic
(and most everything else for that matter) says a lot about you.

For most common parts I have two or more versions of them in the library,
one for each of the common rotations.  For example, I have both vertical and
horizontal resistors premade.  That way you don't end up with a mess like
your R5, R4, etc.  If you don't have a pre-rotated part, then you have to
"smash" the part and rotate and position the text manually.  That's part of
the job, especially when you ask others to look at your schematic.

Inductors are drawn as coils, not as solid filled rectangle.  Pay attention
to details.

> Eagle: http://tinyurl.com/2vrj2e6 (ZIP)

Yikes, you've got silkscreen overlapping pads all over the place!  Most
board houses will clip the silkscreen off of pad areas, but they may hold up
the job while they ask you.  Either way they'll think you're a moron, which
may matter depending on how automated or not their process is.  Production
techs are people too, and can develop attitudes.  You don't want to invite
them to make you their victim.

This is a two layer board with the bottom layer only sparsely used.  You'd
be better off making it as much of a ground plane as you can instead of
trying to fill in the top layer as you did.  All the islands in the top
layer will prevent it being a effective ground plane anyway.

You apparently didn't use net classes at all, since everything is in the
default class and its width and other values were never set.

I looked around the board a bit more and found that some of your 0805
resistors like R1 have a border around them in the copper layer!  WTF?
Since you're obviously very new to Eagle, you should at least look around a
bit at how those that know what they're doing make library parts.  You also
clearly didn't run a DRC check, which would have found a number of clearance
violations.  You do need to get used to making your own parts and definitely
not rely on the Cadsoft libraries, but you have to learn how to do it right
first.  Several of my libraries are available in my Eagle Tools release at
http://www.embedinc.com/pic/dload.htm.

The pins at the top right side of IC1 have lines coming out from them, but
aren't labeled.  There is no indication in the schematic that they are
connected to anything.  Some of the names start with "^" apparently in a
errant attempt to show inverted logic.  Didn't you read the manual at all?
This is done in Eagle by preceeding a signal name with "!".  I fixed one of
them to illustrate.

The bypass cap for IC1 is poorly placed.

As a challenge and to demonstrate some of the things I am talking about, I
edited your board and schematic.  The route was a mess, so I ripped it all
up.  Somewhere in this process I did something wrong or Eagle got confused
about the GND net connections.  Even though I deleted the GND polygon from
the top layer, it still thought everything on the GND net was connected and
showed no airwires.  I got around it by deleting all your GND connections
and recreating them using my own GND1 ground symbols.  After that Eagle
understood the connections again and showed the proper airwires.  As far as
I can tell, your GND connections were done correctly and I don't know why
Eagle had this problem.

I created a ground polygon on the *bottom* layer, and then rerouted the
board.  I also replaced your 0805 resistor with my own package since yours
had that bizarre copper ring around them.  Note the more readable
orientation of the text.  I didn't have to do anything special as I have
separate parts for vertical and horizontal resistors.  I also fixed the text
of T1 as a example.

The oblong holes for the connector pads were just silly.  They added nothing
electrically but used up valuable space by the edge of the board that
prevented routing there.  I replaced them with smaller pads.  I may not have
put them all back in the right place.  Unless these need to be in those
specific places due to external constraints, some of them could be moved
around to make routing easier.

I then manually routed all the GND1 SMD pads each with their own via to the
bottom (ground) polygon.  That leaves as much routing flexibility for the
remaining signals as possible.  I routed a few obvious connection and places
where I thought the auto router might paint itself into a corner, then auto
routed the rest.  You can see the result at
http://www.embedinc.com/temp/david.zip.  The auto route isn't all that bad,
but there are some obvious cleanups to minimize the impact on the ground
polygon.  I didn't do any of that, so you can see how the auto router left
things.

2010\10\30@111235 by David

flavicon
face
On 30/10/2010 15:13, Olin Lathrop wrote:
> Pay attention to details.

OK, all of these points are very valid.  However, I do this as a hobby and relying on Eagle for some parts saves a lot of time!  I will take more care to smash the parts and fix labels in future, I tend to spend a lot less time than I should on the schematic.

> Yikes, you've got silkscreen overlapping pads all over the place!

Yes, the silkscreen has issues.  Turns out I exported the tDocu layer along with tPlace.  I will make sure I am more careful when exporting the gerbers for the board house.

(Note that the Eagle USB connector still has silkscreen all over the pads on tPlace, I'll fix that up)

> You apparently didn't use net classes at all, since everything is in the
> default class and its width and other values were never set.

I had not heard of these, so some research is needed for future.  Thanks for the pointer.

> You also clearly didn't run a DRC check, which would have found a number
> of clearance violations.

Actually the board I uploaded passes the Sparkfun/BatchPCB DRC just fine.

> You do need to get used to making your own parts and definitely
> not rely on the Cadsoft libraries, but you have to learn how to do it right
> first.  Several of my libraries are available in my Eagle Tools release at
> http://www.embedinc.com/pic/dload.htm.

I have made a few parts so far but have a lot to learn, clearly.  I have grabbed your tools and will look through the libraries for inspiration.

I am hoping that the new release of Eagle with XML libraries will make a big difference to how easy these things are to share/modify (even just importing a good footprint from one library to another is a pain).

> The bypass cap for IC1 is poorly placed.

Noted.

> As a challenge and to demonstrate some of the things I am talking about, I
> edited your board and schematic.  The route was a mess, so I ripped it all
> up.  Somewhere in this process I did something wrong or Eagle got confused
> about the GND net connections.  Even though I deleted the GND polygon from
> the top layer, it still thought everything on the GND net was connected and
> showed no airwires.

That's because GND airwires were hidden (Eagle does show this in the status bar when you run ratsnest).  Didn't you read the manual at all? ;)

> I created a ground polygon on the *bottom* layer, and then rerouted the
> board.  I also replaced your 0805 resistor with my own package since yours
> had that bizarre copper ring around them.

The "bizarre copper ring" is not copper, it's on the keepout layer.  It doesn't get used except for a visual guide of where not to place components..

The poly on the bottom layer is much better.

> Note the more readable
> orientation of the text.  I didn't have to do anything special as I have
> separate parts for vertical and horizontal resistors.  I also fixed the text
> of T1 as a example.

Yes, that is much more readable.

> The oblong holes for the connector pads were just silly.

Very sensible.  I generally use a pin header for insertion into a breadboard, hence the 0.1" spacing.  I'll make some PINHDR variations with round pads.

> I then manually routed all the GND1 SMD pads each with their own via to the
> bottom (ground) polygon.  That leaves as much routing flexibility for the
> remaining signals as possible.  I routed a few obvious connection and places
> where I thought the auto router might paint itself into a corner, then auto
> routed the rest.

That's a really neat example, thanks.  I have learned a lot creating this and reading through the feedback.

Unfortunately BatchPCB don't allow buried vias and the clearance between some of them is also too small.  A few of the vias could be moved away from pads, I will attempt to do that later.  I might just send off my board and learn from what I get back.  The few I have made before I am slowly documenting on my website.

Thanks so much for taking the time to look at it.

Davi

2010\10\30@120410 by Olin Lathrop

face picon face
David wrote:
> That's because GND airwires were hidden (Eagle does show this in the
> status bar when you run ratsnest).  Didn't you read the manual at
> all? ;)

I have not heard of this before and routinely see GND airwires in my
layouts, so I'm not sure what you're referring to.

> The "bizarre copper ring" is not copper, it's on the keepout layer.

Ah, the keepout and top copper layers look nearly the same, especially for
thin lines.  Apparently I didn't look closely enough.  However, I'm not sure
what the point of such a keepout ring is.  Take a look at my 0805 resistors..
They have no such ring.  Any spacing to other nets should be handled by the
net classes and DRC rules.

> It doesn't get used except for a visual guide of where not to place
> components.

Since 0805 is big enough, I use a silkscreen ring around the part for that.

> Unfortunately BatchPCB don't allow buried vias and the clearance
> between some of them is also too small.

This is a two layer board, so there are no buried vias and my normal setup I
used doesn't create any anyway.  I set the minimum width and space both to 8
mils in this example.  That's my default because just about any board house
on the planet can handle that without extra charges.  Most allow a little
tighter, but I stick to 8/8 unless I have a special situation that requires
less precisely because it's so universal.  Are you really sure BatchPCB
can't handle that?

> A few of the vias could be moved away
> from pads, I will attempt to do that later.

They could be, but why would you want to?  I assume you are talking about
the vias that are on the same net as the pad.  Why add inductance and
resistance between the pad and via, especially since most of the ones where
I deliberately had the via touch the pad are ground connections to the
bottom layer.


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

2010\10\30@152347 by Gerhard Fiedler

picon face
Olin Lathrop wrote:

> Inductors are drawn as coils, not as solid filled rectangle.  Pay
> attention to details.

Says who (besides you, of course)? :)

Note that I have nothing against the coil version, but the other version
is pretty common, too. I think any EE should be familiar with it,
something like being familiar with "km" even though it's not frequently
used everywhere.

Gerhar

2010\10\30@154310 by Michael Watterson

face picon face
 On 30/10/2010 20:23, Gerhard Fiedler wrote:
> Olin Lathrop wrote:
>
>> Inductors are drawn as coils, not as solid filled rectangle.  Pay
>> attention to details.
> Says who (besides you, of course)? :)
>
> Note that I have nothing against the coil version, but the other version
> is pretty common, too. I think any EE should be familiar with it,
> something like being familiar with "km" even though it's not frequently
> used everywhere.
>
> Gerhard
I'm familiar with the thick bar at one side rectangle. It's been standard over 40 years...
Also boxes instead of ___/\/\/\/\___  for resistors.

There is quite a big difference in style between US and Europe.
We also use A4, A3, A2 etc, which scale nicely... I can do A3 and print without distortion as A4
US letter size is a bit awkward, but fine if that's your standard and only use Letter Size printing.

2010\10\30@155646 by Olin Lathrop

face picon face
Gerhard Fiedler wrote:
>> Inductors are drawn as coils, not as solid filled rectangle.  Pay
>> attention to details.
>
> Says who (besides you, of course)? :)
>
> Note that I have nothing against the coil version, but the other
> version is pretty common, too.

Not where I've looked.  Sometimes inductors are drawn with a bunch of top
half of circles stuck together.  I think that's good enough, but I like to
take a little extra care and show the loops.  Put it this way, which is more
likely to be confused, a loopy inductor or a filled box?  I would find it
hard to believe that the loopy version would be ambiguous to anyone around
the world who has at least a cursory knowledge of schematics, whereas I
wouldn't say the same for the filled box.  Where's the upside?

The point of many electrical symbols is that they are intended to be quick
visual reminders of what the part does.  In that context resistors as
zigzags, capacitors are two parallel lines, and inductors as loops make a
lot of sense.  The symbols for vacuum tubes, diodes, and even transistors
were clearly designed with this concept in mind too.  It gets more
complicated for intgrated circuits, so you usually give up and draw a box
and label the lines.

Unfortunately we see more and more shortcuts.  I don't know if it's
laziness, sloppiness, or what.  The old way makes sense.  This is the first
I've seen a inductor look not loopy though.  Let's not get sloppy with those
too.  It's bad enough that it's become acceptable in some places to draw
resistors as rectangular boxes.  I don't know where that came from, but I
don't understand why someone had to go invent a new and less descriptive
symbol when there was a nice one already standard.  All "old" schematics
I've ever seen show resistors as zigzags, so I think the box came later.

> I think any EE should be familiar with
> it, something like being familiar with "km" even though it's not
> frequently used everywhere.

I don't know what "km" is either.  Do you mean "Km" perhaps?


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

2010\10\30@155912 by Olin Lathrop

face picon face
Michael Watterson wrote:
> I'm familiar with the thick bar at one side rectangle.

What is that?  I don't understand "thick bar at one side rectangle".


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

2010\10\30@163635 by KPL

picon face
> Not where I've looked.  Sometimes inductors are drawn with a bunch of top
> half of circles stuck together. I think that's good enough, but I like to
> take a little extra care and show the loops.  Put it this way, which is more
> likely to be confused, a loopy inductor or a filled box?  I would find it
> hard to believe that the loopy version would be ambiguous to anyone around
> the world who has at least a cursory knowledge of schematics, whereas I
> wouldn't say the same for the filled box.  Where's the upside?

That was standard coil symbol in eastern block, at least in USSR. It
could even have a single thick solid line along those half-circles if
that coil had iron-based core, and dashed thick line if it had
ferrite-based core. Most probably there were other options too.
That symbol was very easy to draw using hand drawing tools.

Resistors were drawn as empty rectangles, and even there it was
possible to give more information - empty rectangle usually was
meaning 0.125W, one diagonal line was 0.25W, one line perpendiculat to
length meant 0.5w, and so on.

So there are lots of engineers all over the world now, coming from
there, who have to think twice when reading circuits that contain
rectangles :)

{Quote hidden}

As a side note, ex-USSR standard for drawing digital circuits was
quite good either, it was much easier to understand from the first
look, not like many of the versions we see now.


-- KPL
P.S. Just do not think I liked USSR itself:)

2010\10\30@172358 by Michael Watterson

face picon face
 On 30/10/2010 21:36, KPL wrote:
>
> That was standard coil symbol in eastern block, at least in USSR. It
> could even have a single thick solid line along those half-circles if
> that coil had iron-based core, and dashed thick line if it had
> ferrite-based core. Most probably there were other options too.
> That symbol was very easy to draw using hand drawing tools.
>
> Resistors were drawn as empty rectangles, and even there it was
> possible to give more information - empty rectangle usually was
> meaning 0.125W, one diagonal line was 0.25W, one line perpendiculat to
> length meant 0.5w, and so on.
>
> So there are lots of engineers all over the world now, coming from
> there, who have to think twice when reading circuits that contain
> rectangles :)
>
>
I never knew the Russians copied it too :)

I live in Europe. From the 1960s I remember US stuff used Olin's style and Philips, Grundig etc used the cleaner easier to drawn neat with templates style.

> As a side note, ex-USSR standard for drawing digital circuits was
> quite good either, it was much easier to understand from the first
> look, not like many of the versions we see now.
>
>

2010\10\30@173137 by Oli Glaser

flavicon
face
On 30/10/2010 00:05, David wrote:
> On 29/10/2010 13:13, Olin Lathrop wrote:
>> Again, it would be better to post the Eagle .brd file instead of or in
>> addition to these files.  Without being able to poke around and really see
>> what's on what layer, I don't feel I can say much.
> Taken on board most comments.  Also fixed a bunch of stuff that was
> wrong in v1 (from comments on PIClist and a forum).
>
> The board is now more compact and space is used more wisely I think.
> The PDF is even in landscape format (A4).
>
>     PDF: http://tinyurl.com/36xp3u2
> Eagle: http://tinyurl.com/2vrj2e6 (ZIP)
>
> Comments on attempt two are very welcome.
>
> David

I think most stuff has been covered. I was going to say that C1 and C4 were not given values, but you have sorted that with this version. L1 has no value though - I appreciate it's value is probably not critical, but I usually at least put a range of acceptable values in when there is a choice. The more info, notes etc, the better, makes coming back to a design later much easier (amongst other things)
Also, I assume you have checked the datasheet for the FT232RL and confirmed that leaving the pins RESET, TEST, OSCI, OSCO, CBUSx etc unconnected and floating is okay? I'm assuming the RESET has a weak internal pullup or something. If they *are* actually conected (I don't use Eagle so I don't know if there is some invisible net link option) to something then it should be made clear.
All looks pretty good though in general - let us know how it performs when assembled (pretty sure it will be fine from what I can see of the routing - I've had full speed USB running on more "risky" setups, not used an FT232 yet however, though I do have some here somewhere along with some FT245s)


2010\10\30@173640 by Oli Glaser

flavicon
face
Doh! Ignore the bit about the RESET - I noticed at the bottom of your schematic it says "reset can be left floating according to datasheet".
TIme to get some sleep here I think... :-)

2010\10\30@174940 by jim

flavicon
face
For a polarized component.  Typically an electrolytic capacitor or a diode.


-----Original Message-----
From: piclist-bouncesspamspam_OUTmit.edu [@spam@piclist-bouncesKILLspamspammit.edu] On Behalf Of
Olin Lathrop
Sent: Saturday, October 30, 2010 3:00 PM
To: Microcontroller discussion list - Public.
Subject: Re: [EE] PCB critique

Michael Watterson wrote:
> I'm familiar with the thick bar at one side rectangle.

What is that?  I don't understand "thick bar at one side rectangle".


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

2010\10\30@181625 by William \Chops\ Westfield

face picon face

>> Taken on board most comments.

Are you sure about the size of your polyfuse?  It looks significantly  smaller than the 500mA fuse on most Arduinos, for example...   (I  guess 500mA 1206-sized polyfuses do exist...)

I would move some of your traces to provide more clearance, and make  traces thicker when its easily possible...

The actual paths taken by GND to reach the supply pins of the FTDI  chip are pretty twisted.  Having a ground plane doesn't guarantee that  the plane doesn't narrow inappropriately before it reaches where it  needs to go.  I'd stick another ground plane on the bottom layer, with  a bunch of gratuitous vias.

220 ohms is a really low value for a modern SMT indicator LED.  Unless  you really want them to be as bright as possible and consume more  current than the entire rest of the circuit...  Current arduino boards  are using 1k, and even that is uncomfortably bright in some cases (The  blue "pin 13" LED on the solarbotics Freeduino, for example.)

Hiding the GND airwires makes me nervous.

Are you sure you don't want to break out the CBUS signals to pads as  well?  There's a hack out there that lets you use them to bit-bang  program an AVR, for example.

BillW

2010\10\30@185809 by Harold Hallikainen

face
flavicon
face
The board comments I've seen so far look good. One thing I like to see in
schematics is for the netnames to be identified as active low or active
high. For example, the nets driving your LEDs are active low. Depending on
your cad system, you can either put a bar over the netname or maybe end
the netname with "n" (for not). Similarly, chip pins should, in my
opinion, be marked as active high or low. If there is a pin whose name
(the name inside the chip) is RESET, I expect the pin to be active high
UNLESS there is a bubble outside the chip, which would make it active low.
This way, I can quickly look at the schematic and know whether I need to
drive the pin low or high to reset the chip. I don't have to go digging
through the datasheet on the chip. This sort of stuff really helps me in
understanding a circuit and writing code for it.

Harold



-- FCC Rules Updated Daily at http://www.hallikainen.com - Advertising
opportunities available

2010\10\31@015359 by Gerhard Fiedler

picon face
Olin Lathrop wrote:

> Gerhard Fiedler wrote:
>>> Inductors are drawn as coils, not as solid filled rectangle.  Pay
>>> attention to details.
>>
>> Says who (besides you, of course)? :)
>>
>> Note that I have nothing against the coil version, but the other
>> version is pretty common, too.
>
> Not where I've looked.  
Then you just looked in the wrong places. IEC would be a good place to
start; it seems to list both versions. (I don't have the actual
standard, but I've seen several publications refer to it -- with both
versions. Same for the resistor symbols that you mention later.)

This is not a question which one is better -- it's a question whether
the solid rectangle is wrong or sloppy. It isn't, even though your
phrase above strongly suggests so. This coming from a recognized
authority requires this to be corrected :)

> Sometimes inductors are drawn with a bunch of top half of circles
> stuck together.  I think that's good enough, but I like to take a
> little extra care and show the loops.  
See, when I use this style, I prefer the half circles. Looks cleaner to
me -- and if I'm not mistaken, even the US standard bodies side with me.
I like to take a little extra care and use actual standard symbols
instead of making up my own.

> Put it this way, which is more likely to be confused, a loopy inductor
> or a filled box?  I would find it hard to believe that the loopy
> version would be ambiguous to anyone around the world who has at
> least a cursory knowledge of schematics, whereas I wouldn't say the
> same for the filled box.  Where's the upside?

This isn't a question of upsides and downsides. This is about standard
symbols. And like it or not, there are standards for these standard
symbols, and all standard symbols are (or should be?) acceptable. IMO.
Independently of their artistic value or how expressive someone thinks a
symbol is or is not.

> The point of many electrical symbols is that they are intended to be
> quick visual reminders of what the part does.  
That's one point. Another is to be a standardized symbol that, once
learned, is easy to recognize. You just failed to learn about this one,
and now wrote a long email talking around this simple fact. Something
like "ah, thanks, I didn't know this one" would have been enough :)

> Unfortunately we see more and more shortcuts.  I don't know if it's
> laziness, sloppiness, or what.  The old way makes sense.  This is the
> first I've seen a inductor look not loopy though.  
This just shows your lack of (international) experience. Many schematics
in Europe, for example, use this style. It's not sloppiness, it's just a
standard symbol you didn't know. That's sloppiness on your part -- you
could have looked it up before talking about it.

> It's bad enough that it's become acceptable in some places to draw
> resistors as rectangular boxes.  I don't know where that came from,
> but I don't understand why someone had to go invent a new and less
> descriptive symbol when there was a nice one already standard.  
Geez... NIH at its best. I bet you don't have a clue which symbol was
there first -- you just know which one /you/ saw first. Do you really
/know/ anything about this?
> All "old" schematics I've ever seen show resistors as zigzags, so I
> think the box came later.

It may be new to you, but there were electronic symbols around before
you were around, and I saw schematics from before your time that used
the rectangle, so this symbol definitely predates you and you have to
find more objective sources than your limited experience if you want to
say something substantial about the relative ages of these symbols. The
box may have come later /to you/, but that doesn't really mean much in
the grand scheme of things.


>> I think any EE should be familiar with it, something like being
>> familiar with "km" even though it's not frequently used everywhere.
>
> I don't know what "km" is either.  Do you mean "Km" perhaps?

No, I meant "km" -- and you definitely should make yourself familiar
with it. Being something so basic, you could actually look pretty dumb
having to admit you don't know what "km" is when it counts... So look it
up; any introductory text about SI should suffice. (And if you don't
trust non-US publications, the NIST site has enough to get you started.)
Gerhar

2010\10\31@041952 by Oli Glaser

flavicon
face
On 30/10/2010 15:13, Olin Lathrop wrote:
>
> Inductors are drawn as coils, not as solid filled rectangle.  Pay attention
> to details.
>

This is not true, inductors can be drawn this way sometimes. At risk of doing the OP a disservice, it is probably better to label *your* particular preferences as such, to avoid them sounding like facts as the above does. Even if something is true 99% of the time, I think it is good practice to mention the other 1%.

>>  I think any EE should be familiar with
>>  it, something like being familiar with "km" even though it's not
>>  frequently used everywhere.

>I don't know what "km" is either.  Do you mean "Km" perhaps?

I think you have this mixed up - a small k is the standard notation for kilo for SI units.
This link may help:
http://en.wikipedia.org/wiki/SI_prefix

If you check under the "Similar systems in abbreviations" header it mentions that a large K is the official symbol of the Kelvin, and describes situations where it is sometimes used unofficially, when attention to detail is lacking thus confusing matters.

2010\10\31@050823 by Justin Richards

face picon face
> This isn't a question of upsides and downsides. This is about standard
> symbols. And like it or not, there are standards for these standard
> symbols, and all standard symbols are (or should be?) acceptable. IMO.
> Independently of their artistic value or how expressive someone thinks a
> symbol is or is not.
>

But they are symbols and should be symbolic and I think that the
standards people get it wrong from time to time.

So if Olin pushes his acceptable symbols and it takes, then perhaps
they can change the standards.  I personally prefer loopy and zigzag
for inductors and resistors respectively.

I often wonder if I was exposed to both types of logic gate symbols at
the same time which one I would prefer.  But I was exposed to the
roundy ones first and they seem more intuitive.

I tried looking for a standard house light switch when doing some
house plans.  I could not find a standard and I looked in a bunch of
electrical symbols books and the web.

Justi

2010\10\31@052616 by KPL

picon face
>>
> I never knew the Russians copied it too :)

Most probably yes, as mostly everything. Just that's not bad in case
of standards.

> I live in Europe. From the 1960s I remember US stuff used Olin's style
> and Philips, Grundig etc used the cleaner easier to drawn neat with
> templates style.

So is there a real standard for them in EU now? Seems like everybody
is drawing his own way.

I'm working in completely different field so do not know what is used now.

-- KP

2010\10\31@053229 by Philip Pemberton

face
flavicon
face
On 29/10/10 13:30, David wrote:
>> What's
>> the point of the elaborate graphic under the USB connector?  It won't help
>> the manufacture install it correctly and it can't be seen once installed..
>> This is also apparently more than just the silkscreen since SMD pads are
>> shown.
>
> No idea!  I didn't design the USB connector, it is from one of the
> standard libraries.

Turn the tDocu and bDocu layers off and it should disappear. You'll probably end up with a square outline instead, and it'll get rid of most if not all of the silkscreen lines which are straddling pads.

-- Phil.
KILLspampiclistKILLspamspamphilpem.me.uk
http://www.philpem.me.uk

2010\10\31@053931 by Philip Pemberton

face
flavicon
face
On 30/10/10 17:04, Olin Lathrop wrote:
>> The "bizarre copper ring" is not copper, it's on the keepout layer.
>
> Ah, the keepout and top copper layers look nearly the same, especially for
> thin lines.  Apparently I didn't look closely enough.  However, I'm not sure
> what the point of such a keepout ring is.  Take a look at my 0805 resistors.
> They have no such ring.  Any spacing to other nets should be handled by the
> net classes and DRC rules.

It's a useful placement guide IMO. If you overlap the lines just on the edges (so the two lines look like one) you'll usually be fine, but if they merge further back (so you effectively turn the two keepout boxes into three) then the parts are getting too close together.

And by that I mean they're going to be an absolute pig to place and solder.

-- Phil.
RemoveMEpiclistTakeThisOuTspamphilpem.me.uk
http://www.philpem.me.uk

2010\10\31@054541 by Philip Pemberton

face
flavicon
face
On 30/10/10 20:57, Olin Lathrop wrote:
> Not where I've looked.  Sometimes inductors are drawn with a bunch of top
> half of circles stuck together.  I think that's good enough, but I like to
> take a little extra care and show the loops.  Put it this way, which is more
> likely to be confused, a loopy inductor or a filled box?  I would find it
> hard to believe that the loopy version would be ambiguous to anyone around
> the world who has at least a cursory knowledge of schematics, whereas I
> wouldn't say the same for the filled box.  Where's the upside?

The EU / BSI / DIN standards prohibit the use of the "loopy wire" inductor symbol. There is, however, a reason for the "white box and filled block" capacitor symbol: it's MUCH harder to confuse a polarised capacitor with a non-polarised capacitor (where the white box is filled too).

Bear in mind, these standards originated in the bad old days when designs could be photocopied through 5 or 6 generations. Readability counts..

In most cases, component designators (L1, L2, etc.) and values (1uH, 5uH, 2mH, 600R@100MHz ...) will give away what the component is.

>> I think any EE should be familiar with
>> it, something like being familiar with "km" even though it's not
>> frequently used everywhere.
>
> I don't know what "km" is either.  Do you mean "Km" perhaps?

"Kilometres". Lowercase-k being the 'kilo' multiplier, and 'metre' being the unit of distance.

-- Phil.
spamBeGonepiclistspamBeGonespamphilpem.me.uk
http://www.philpem.me.uk

2010\10\31@090911 by Olin Lathrop

face picon face
Gerhard Fiedler wrote:
> This is not a question which one is better --

Of course it is.  A schematic is documentation of a circuit for human
understanding.  Clarity and chance of reducing errors is therefore
important.  From what you are saying, there are apparently various
"standards" out there.  Unfortunately that happens the more something gets
into common use, especially as it gets around the world.  The fact that the
US and the Soviet Union were largely disconnected during the formative years
of schematic symbols probably made this worse.

As someone once said, the nice thing about standards is there are so many to
chose from ;-)

Now we have to make intelligent choices.  Perhaps the filled box for a
inductor is not "wrong" in the strict sense in some parts of the world (it
would be if you were working here), but that doesn't make it a good idea.
There is simply no upside to using that over the more descriptive loopy
symbol.

To check a sortof neutral source, I looked at Wikipedia
(http://en.wikipedia.org/wiki/Electronic_symbol).  At the top they show a
inductor with full loops, and lower on the page with the half circles.  As I
said before, I'm OK with either since I think both are unlikely to be
confused.  I think the full loops look cleaner and like a little extra care
was taken, but that's just opinion.  However, nowhere on that page does it
mention inductors as filled boxes.

> This isn't a question of upsides and downsides. This is about standard
> symbols. And like it or not, there are standards for these standard
> symbols, and all standard symbols are (or should be?) acceptable. IMO.
> Independently of their artistic value or how expressive someone
> thinks a symbol is or is not.

Anyone can make up a standard.  It *is* about descriptiveness and conveying
information in a way least likely to be confused.  Since there is no single
standard, you should think a little about which standard makes the most
sense to follow.  Unfortunately the "standard" becomes like human languages
which are sortof defined by a standard which then evolves as common usage
drifts, which causes the standard to be rewritten, etc.

I looked around some more searching in Google for inductor and other
electrical symbols:

www.rapidtables.com/electric/electrical_symbols.htm
library.thinkquest.org/10784/circuit_symbols.html
http://www.tutorvista.com/physics/electrical-symbols-and-meanings

These are just the first few relevant hits from a Google search.  I didn't
leave out any up to as far as I got going thru the search results.  Every
one of them shows loopy inductors without a single mention of a filled box.
There is mention of unfilled boxes for resistors, although the more
descriptive zigzag is also shown in all cases.

The result seems clear.  If you want your schematic to be understood by the
widest possible audience, use a loopy symbol for inductors.  The filled box
may be acceptable in some cases, but certainly not all.  It is therefore a
bad idea.

> I bet you don't have a clue which symbol was
> there first -- you just know which one /you/ saw first. Do you really
> /know/ anything about this?

As I was careful to point out:

>> All "old" schematics I've ever seen show resistors as zigzags, so I
>> think the box came later.

The use of "think" should make it clear that I don't really know and that I
readily admit this.  I tried to look around on the web for scans of old
schematics, but didn't turn up anything useful.  Do you know which one came
first?  If so, please provide a reference.

> No, I meant "km" -- and you definitely should make yourself familiar
> with it. Being something so basic, you could actually look pretty dumb
> having to admit you don't know what "km" is when it counts... So look
> it up;

You're the one that mentioned it.  Since you think you know what it means,
why don't you tell us, or provide a reference?


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

2010\10\31@091103 by Olin Lathrop

face picon face
jim wrote:
>> I'm familiar with the thick bar at one side rectangle.
>
> What is that?  I don't understand "thick bar at one side rectangle".
> For a polarized component.
>
> Typically an electrolytic capacitor or a diode.

So he meant "thick bar at one side [of a] rectangle"?  The original was too
garbled to have any clear meaning.


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

2010\10\31@095723 by Gerhard Fiedler

picon face
Justin Richards wrote:

>> This isn't a question of upsides and downsides. This is about
>> standard symbols. And like it or not, there are standards for these
>> standard symbols, and all standard symbols are (or should be?)
>> acceptable. IMO. Independently of their artistic value or how
>> expressive someone thinks a symbol is or is not.
>
> But they are symbols and should be symbolic and I think that the
> standards people get it wrong from time to time.

If you take Olin's argument for the loopy inductor symbol and apply it
to the resistor, you end up either with a symbol that looks pretty much
like the inductor symbol (peel a typical through-hole resistor some time
or a wire-wound resistor (common in the old days) and you know what I
mean) or with one that looks like the European resistor symbol (if you
don't peel it :). While there are resistors that have some similarity to
the zigzag, somewhere, they are rare in typical electronic circuits --
and if you find them, they look more rectangled than actually zigzag. So
the semblance argument doesn't really hold in general.
I suspect it's really more about what you get used to at an early stage.
Which would explain the persistent preferences.  
> So if Olin pushes his acceptable symbols and it takes, then perhaps
> they can change the standards.  
Nothing wrong with pushing his preferences or changing standards, but
calling other's preferences "wrong" and "sloppy" and that to somebody
who might not know that they are not wrong and there's nothing sloppy
about using a standard symbol is just... you pick your adjective.
> I personally prefer loopy and zigzag for inductors and resistors
> respectively.

It seems that most US-Americans prefer the US-American symbols. I happen
to prefer the European-style resistor symbol; for me, the drawing looks
"cleaner" and makes it easier (for me) to quickly "see" a circuit. For
me that's important.

I definitely prefer the half-circle (not loopy) inductor symbol for hand
drawings (quicker to draw with a pen or pencil than to fill out a
rectangle); for printed stuff, I don't care much either way.


> I tried looking for a standard house light switch when doing some
> house plans.  I could not find a standard and I looked in a bunch of
> electrical symbols books and the web.

Electrical building plans have much to do with building codes, and those
are AIUI highly nationalized, because they typically are affected by
(usually national) legislation. So I wouldn't bet on an international
standard in this area.

This shows what is common (that is, standard) in Germany
http://de.wikipedia.org/wiki/Liste_der_Schaltzeichen_%28Elektrik/Elektronik%29

Differently from most Wikipedia pages, this doesn't seem to have a
version in other languages. You may find some hints in CAD for
architecture, texts about industrial electrics and ECAD programs for
that purpose.

Gerhar

2010\10\31@102512 by Wouter van Ooijen

face picon face
> www.rapidtables.com/electric/electrical_symbols.htm
> library.thinkquest.org/10784/circuit_symbols.html
> http://www.tutorvista.com/physics/electrical-symbols-and-meanings

Note that two of these three are the same list, and that they all show the USA logic symbols. Check Gerhard's German page (next email on the list) for the symbols that are more common in Europe.

I associate a diagram with the coiled inductor (full loops, not half circles) with Ham radio's, hand-wound coils, tesla-coil hobbyists and other home-brew activities. I know the zigzag resistor is in common use in some parts of the world, but for me it is as arcane as pounds and inches. I grew up with shape-defined logic symbols and still find them easier to draw, but I find the IEC symbols much easier to read.

Note that google "nand gate symbol" shows only the old-fashioned symbols, and the first match http://www.kpsec.freeuk.com/gates.htm expresses a clear preference for the old-fashioned symbools :(

--
Wouter van Ooijen

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

2010\10\31@104301 by Olin Lathrop

face picon face
Wouter van Ooijen wrote:
> Note that google "nand gate symbol" shows only the old-fashioned
> symbols, and the first match http://www.kpsec.freeuk.com/gates.htm
> expresses a clear preference for the old-fashioned symbools :(

Yeah, I like how it says "They are rarely used despite their official
status, but you may need to know them for an examination.".  This was a
clear case of a previously existing and widely used standard, and a bunch of
people deliberately trying to invent a new standard later, apparently
because they got left out of creating the original standard.

Anyone can write up something and claim it to be a standard.  That doesn't
really make it one until it gets commonly adopted.  I don't think I'm the
only one that really dislikes the new logic symbols and refuses to use them..
Maybe it's because I grew up with them, but I always have to decipher the
new ones whereas the old ones just click.


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

2010\10\31@114723 by Olin Lathrop

face picon face
Gerhard Fiedler wrote:
> If you take Olin's argument for the loopy inductor symbol and apply it
> to the resistor, you end up either with a symbol that looks pretty
> much
> like the inductor symbol (peel a typical through-hole resistor some
> time
> or a wire-wound resistor (common in the old days) and you know what I
> mean) or with one that looks like the European resistor symbol (if you
> don't peel it :). While there are resistors that have some similarity
> to
> the zigzag, somewhere, they are rare in typical electronic circuits --
> and if you find them, they look more rectangled than actually zigzag.
> So
> the semblance argument doesn't really hold in general.

You are missing the point.  It's not what the part physically looks like,
but a reminder icon of what it does electrically.  Most capacitors don't
look like two plates, and vacuum tubes aren't physically built at all like
the schematic symbol.

I remember reading somewhere long ago that the zigzag resistor symbol was
designed to give a hint of resistance to current.  Think of something
flowing thru a straight pipe versus a all bent up one.  Of course these
icons aren't perfect because symplicity of drawing is also important, but I
think the resistor symbol does quite well on both counts.

Trying to make the symbol look like the package is just silly.  There are so
many different packages, and different parts come in similar packages.  I
have some capacitors here that are in a round radial package just like a
common 1/4 Watt thru hole resistor.  Should the European symbol for a
capacitor then look like their resistor but with a different bar or fatter
line someplace to distinguish it?  Imagine what a transistor symbol would
look like if you followed this logic.  It would probably be something more
like a sandwich.

> Nothing wrong with pushing his preferences or changing standards, but
> calling other's preferences "wrong" and "sloppy" and that to somebody
> who might not know that they are not wrong and there's nothing sloppy
> about using a standard symbol is just... you pick your adjective.

While the box resistor isn't wrong, it's unfortunate.  At best though, the
filled box inductor is a bad idea, and certainly wrong in many contexts.

> It seems that most US-Americans prefer the US-American symbols.

That's supposed to be surprising?  It's what we grew up with, but it's also
because the symbols were designed with some thought and serve their purpose
well.  What we find hard to understand is why alternate and less descriptive
symbols ever evolved in the first place.  Sometimes it seems others make up
their own standard only because they didn't get to make up the original, not
because there is anything wrong with it.

> I happen
> to prefer the European-style resistor symbol; for me, the drawing
> looks "cleaner" and makes it easier (for me) to quickly "see" a
> circuit. For
> me that's important.
>
> I definitely prefer the half-circle (not loopy) inductor symbol for
> hand drawings (quicker to draw with a pen or pencil than to fill out a
> rectangle); for printed stuff, I don't care much either way.

Preference is all about what you got used to when you learned it.  I
actually think the half-circle inductors are harder to draw freehand.  It's
hard not to accidentally make a little loop or not make a sharp point when
drawing.  Look at old schematics like from the early days of radio, and you
will see full loop inductor symbols.  If I remember right, the half circles
came along later as a shortcut when drawing templates became popular.  Now
that things are computer drawn, we can go back to the original "real" symbol
easily.  Unfortunately some people have forgotten the the half-circles were
a shortcut expediant for a particular situation.

Out of curiosity I dug around on the net a bit looking for old schematics,
like from the first days of vacuum tubes.  It would be interesting to see if
any of them used other than the zigzag resistor symbol.  I'd be rather
surprised if inductors and transformer windings weren't all the full loop
kind.  Unfortunately a quick search didn't yield anything that wasn't
recently redrawn.


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

2010\10\31@130117 by Gary Crowell

picon face
Interesting discussion, and like someone said, there are so many standards
to choose from.

I'm surprised it didn't turn to the straight line/curved line type capacitor
symbol (often but not always indicating polarized capacitors), and, horrors,
the 1K and 5K (Kelvin?) values on the resistors.

Oh, and the brief comments about 'buried vias', I think the poster was
concerned about 'via-in-pad'; but of course they're not that either.  They
are simply close to the pad.  Depending on your assembly method and
soldermasking they might be too close, but for hand assembly it would
probably make no difference.

Just curious, on designs like these, does anybody bother to use teardrops?

Finally, with respect to the OP's OT, on the schematic, the VCCIO connect on
pin 4 of IC1 is missing a connection dot.  I suspect it's not the case in
Eagle, but in some CAD systems, that net would not be connected to VCCIO.

Gary


----------------------------------------------
Gary A. Crowell Sr., P.E., CID+
Linkedin <http://www.linkedin.com/in/garyacrowellsr>
Elance<www.linkedin.com/redirect?url=http%3A%2F%2Fgaryacrowellsr%2Eelance%2Ecom&urlhash=kJm9>
 KE7FIZ <http://www.arrl.org

2010\10\31@140612 by Wouter van Ooijen

face picon face
> Anyone can write up something and claim it to be a standard.  That doesn't
> really make it one until it gets commonly adopted.  I don't think I'm the
> only one that really dislikes the new logic symbols and refuses to use them.
> Maybe it's because I grew up with them, but I always have to decipher the
> new ones whereas the old ones just click.

I grew up with the old ones too, but find the new ones much easier to read. They also scale much better to more complex functions. And in Europe they are definitely *the* standard.

If you seriously say "anyone can write up a standard" then a new standard (by definition not in wide use yet) is not to be taken seriously?

--
Wouter van Ooijen

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

2010\10\31@140908 by Michael Watterson

face picon face
 On 31/10/2010 15:48, Olin Lathrop wrote:
>
> Out of curiosity I dug around on the net a bit looking for old schematics,
> like from the first days of vacuum tubes.  It would be interesting to see if
> any of them used other than the zigzag resistor symbol.  I'd be rather
> surprised if inductors and transformer windings weren't all the full loop
> kind.  Unfortunately a quick search didn't yield anything that wasn't
> recently redrawn.
>

The Web is still highly American Biased, though it's changing.

Hence the fruitless nature of your search.

BTW OT I looked at  Web site log for a site I maintain. IE6 was about 1.75% and most of those actually spambots.

Here is old Grundig Valve (Tube for US speakers) radio
www.radiomuseum.org/r/grundig_drucktastensuper_298wukw.html
Uses rectangles for resistors and solid rectangles for transformer windings but loop symbol for RF coils

But English versions for UK market often redrawn in same style as US
http://www.radio-workshop.co.uk/service/grundig-marlborough-3028.pdf

The UK schematics unlike mainland Europe very similar to US.
OLD Schematics. But almost no Native mainland Europe
*http://www.radio-workshop.co.uk/
http://www2.faculty.sbc.edu/kgrimm/boatanchor/

2010\10\31@141308 by Geo

picon face
Apologies if this appears twice - getting old

Olin Lathrop wrote:
>
> Out of curiosity I dug around on the net a bit looking for old schematics,
> like from the first days of vacuum tubes.  It would be interesting to see if
> any of them used other than the zigzag resistor symbol.  I'd be rather
> surprised if inductors and transformer windings weren't all the full loop
> kind.  Unfortunately a quick search didn't yield anything that wasn't
> recently redrawn.

My oldest  magazine from the bookshelf is 1948 - I have photographed the cover and a circuit diagram of a receiver:-
http://www.8zero.co.uk/circuit.jpg
http://www.8zero.co.uk/cover.jpg

In the drawing office of a radio factory in 1961 all circuit diagrams were hand drawn for production, test and service manuals.
There were no rectangles.

Ge

2010\10\31@143233 by Gerhard Fiedler

picon face
Olin Lathrop wrote:

> Gerhard Fiedler wrote:
>> This is not a question which one is better --
>
> Of course it is.  
??

You called the use of a symbol that's part of an IEC standard "sloppy",
I argued that this is not sloppy. This is the only real point I made.
Everything else are attempts of yours to talk your way around this one,
basic issue.

I know both versions of the symbol in question, and I know that everyone
who knows both has their preference -- and of course everybody thinks
their preference is "better".

I have my reasons for my preference, you have yours for your preference.
I never challenged your preference, only your odd judgment to call
someone else's preference for a perfectly fine standard symbol "sloppy".
It's not sloppy, and no straw man set up by you will change that.


> Clarity and chance of reducing errors is therefore important.  
That's why we have international standards.

> From what you are saying, there are apparently various "standards" out
> there.  
I know that in the US there is a certain
counter-international-standard-culture, but it doesn't make achieving
clarity and reducing errors easier. (See the confusion around "ma",
"MA", "mA" -- all seen in US documents to mean "milliampere" -- and
"km", "Km" and "KM" -- all seen in US documents to mean "kilometer". If
anybody doesn't know which one is correct and unambiguous, I recommend
reading the references I cite at the end of this message.)

There aren't that many standards (no need to use quotes around
standard), and the two (only two!) standardized symbols for an inductor
are the sequence of half-circles and the filled rectangle, and the two
standardized symbols for the resistor are the zigzag and the unfilled
rectangle. Anybody with any time in professional electronics who looked
a bit past his own backyard should have seen both versions of each and
be enough familiar with them to know what they mean and that they are
standard -- and that all are frequently used in certain parts of the
globe.

> Now we have to make intelligent choices.  Perhaps the filled box for a
> inductor is not "wrong" in the strict sense in some parts of the
> world (it would be if you were working here), but that doesn't make
> it a good idea. There is simply no upside to using that over the more
> descriptive loopy symbol.

There is. In the parts of the world where this symbol is common, it
would be a bad idea to use a different one, even though that different
one has Olin's approval stamp and is more common elsewhere. There is
nothing sloppy about this; it's simply the right thing to do. Just like
using inches and letter format in the USA and cm and A4 elsewhere, or
like spelling "meter" in the USA and "metre" in the UK. None of these is
an indication of sloppiness, just of cultural differences associated
with geographical locations).

> To check a sortof neutral source, I looked at Wikipedia
> (http://en.wikipedia.org/wiki/Electronic_symbol).  
How is this neutral WRT geographical location? Most of the (English)
Wikipedia is US-centric. Nothing wrong about this (it's mostly written
by US-Americans), but you just have to know this and consider this when
you research things that may depend on geographical differences.
> Anyone can make up a standard.  
You showed already a few times that it doesn't work that way -- at least
you don't get to make up standards, no matter how hard you try :)
(Nothing personal, though... we others don't get to make up standards,
either. But most of us don't try so hard.)

Apparently you haven't been exposed to many schematics of European
origin. Nothing wrong with this, but your lack of knowledge (about the
frequency of use of this symbol) is not an indication of sloppiness on
someone else's part.


> The use of "think" should make it clear that I don't really know and
> that I readily admit this.  I tried to look around on the web for
> scans of old schematics, but didn't turn up anything useful.  Do you
> know which one came first?  If so, please provide a reference.

No, I don't know, and I don't have a reference for what I don't know and
don't claim. But you claimed that the US symbols came first... so why
don't you provide one? Or you can just let this whole "my symbol is
better than yours" be good... and stop calling someone sloppy just
because they use a perfectly normal standard symbol that you don't like.

I suppose both predate both of us. What I know is that I grew up with
schematics with rectangles for resistors and filled rectangles for
inductors, and only when I entered the field professionally and became
exposed to US-American schematics in the seventies I learned about the
zigzag resistor and the fact that some people use the half-circle (or
even the loopy) inductor symbol in actual schematics that are more than
introductory "pictures".

Here you see a few old schematics. Obviously none of them is anywhere
near the time where the symbols weren't already (more or less, at least)
standardized, but in any case you can see that the use of the filled
rectangle for an inductor and a transformer goes way back in some parts
of the world and is not something recent.
http://www.radiotechnik-web.de/page1.php?view=thumbnailList&category=15

I don't have a beef with the symbols you prefer nor with your
preference. But I do think it is wrong to call the use of the other
common standard symbols "sloppy".


>> No, I meant "km" -- and you definitely should make yourself familiar
>> with it. Being something so basic, you could actually look pretty
>> dumb having to admit you don't know what "km" is when it counts...
>> So look it up;
>
> You're the one that mentioned it.  Since you think you know what it
> means, why don't you tell us, or provide a reference?

A number of other people already told you explicitly, and I already told
you a reference (NIST). "k" (and not "K") is the SI multiplier for
"kilo", meaning 1000, and "m" is the SI symbol for the unit "meter",
therefore "km" is the "kilometer" (or "kilometre"; that is, thousand
meter or metre). Definitely a common unit, and one that one should be
familiar with when working in any technical field.

I don't know what you meant with "Km", though -- in any case it's not a
widely used unit. It's not "km" (as "kilo" is always a lower case "k"),
and it's probably not really "Kelvin meter" either... (the symbol for
Kelvin is the upper case "K", but if you really meant "Kelvin meter",
you probably should have written K·m to avoid confusion with the
kilometer). If you actually meant "Km" to mean "kilometer", then /this/
was really sloppy.

References galore on the net... Here just a few: - NIST SI Units http://physics.nist.gov/cuu/Units/units.html
- NIST SI Prefixes physics.nist.gov/cuu/Units/prefixes.html
- Wikipedia Kilometer article http://en.wikipedia.org/wiki/Km

Since you seem to value clarity and precision, the NIST style guide is
good reading. IMO it should be part of any college course in any
technical or scientific field.
http://physics.nist.gov/cuu/Units/checklist.html
Gerhard

2010\10\31@143729 by Olin Lathrop

face picon face
Wouter van Ooijen wrote:
> If you seriously say "anyone can write up a standard" then a new
> standard (by definition not in wide use yet) is not to be taken
> seriously?

Of course every standard has to start somehow.  What I mean is that a
standard is one in name only until people actually use it.  Whether it is
taken seriously during its startup period has a lot to do with how good it
is, whether it meets a need, who is behind it, perception, marketing etc.

In this case though we were talking about standards old enough so that it's
fair to judge how real they are based on how widely they are adopted.


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

2010\10\31@144407 by Olin Lathrop

face picon face
Michael Watterson wrote:
>> Out of curiosity I dug around on the net a bit looking for old
>> schematics, like from the first days of vacuum tubes.  It would be
>> interesting to see if any of them used other than the zigzag
>> resistor symbol.  I'd be rather surprised if inductors and
>> transformer windings weren't all the full loop kind.  Unfortunately
>> a quick search didn't yield anything that wasn't recently redrawn.
>
> The Web is still highly American Biased, though it's changing.
>
> Hence the fruitless nature of your search.

So you're saying americans haven't scanned old schematics and put them on
the web?  I don't see why that should be the case more so than for other
regions.

> BTW OT I looked at  Web site log for a site I maintain. IE6 was about
> 1.75% and most of those actually spambots.

And this is somehow relevant to schematics because ...?

> But English versions for UK market often redrawn in same style as US
> http://www.radio-workshop.co.uk/service/grundig-marlborough-3028.pdf

Is there a date on that somewhere?  I didn't see one.


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

2010\10\31@144629 by Olin Lathrop

face picon face
Geo wrote:
> My oldest  magazine from the bookshelf is 1948 - I have photographed
> the cover and a circuit diagram of a receiver:-
> http://www.8zero.co.uk/circuit.jpg
> http://www.8zero.co.uk/cover.jpg

This implies that loopy inductor and zigzag resistor symbols were at least
accepted usage in the UK in 1948.


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

2010\10\31@150651 by Olin Lathrop

face picon face
Gerhard Fiedler wrote:
> No, I don't know, and I don't have a reference for what I don't know
> and don't claim. But you claimed that the US symbols came first...

You really should read what I write before arguing about it.  This is now
the third time I'm saying I don't know for sure which came first.  I even
mentioned I tried to look around for really old schematics but didn't find
any.

> Here you see a few old schematics. Obviously none of them is anywhere
> near the time where the symbols weren't already (more or less, at
> least) standardized, but in any case you can see that the use of the
> filled rectangle for an inductor and a transformer goes way back in
> some parts of the world and is not something recent.
> http://www.radiotechnik-web.de/page1.php?view=thumbnailList&category=15

The second picture there of the Dominante W2 schematic is interesting.
Unfortunately the scan is so low res it's hard to tell for sure, but it
looks like they are using something wiggly for inductors, and blocks for
resistors.  It looks like the lower right corner is a key to the power
rating of different resistors.  Different stuff in the box apparently
describes the power rating.

So far all the tube-era schematics, including at least the first two from
your link above, seem to use wiggly or loopy symbols for inductors.  I
suspect those came first, which makes me wonder who decided to invent a new
symbol and why?


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

2010\10\31@154937 by cdb

flavicon
face


::I 'm surprised it didn't turn to the straight line/curved line type
:: capacitor
:: symbol (often but not always indicating polarized capacitors),

I'll just add in the annoying (to me) electrolytic capacitor symbol used in China, the plunger in a washing bucket symbol, with the bucket being gnd and the plunger positive.

Colin
--
cdb, TakeThisOuTcolinEraseMEspamspam_OUTbtech-online.co.uk on 1/11/2010
Web presence: http://www.btech-online.co.uk   Hosted by:  http://www.1and1.co.uk/?k_id=7988359
 

2010\10\31@161839 by cdb

flavicon
face
I wonder if the two types of inductor symbols might not be down to the bleed over of electrical symbols into electronics.

Having said that I have seen many especially European (not including UK generally speaking) inductor (note the term inductor) symbols as rectangular boxes and coils as loops. The symbols sometimes seem to be used whereby a 'resistor' style inductor is being used rather than a wirewound coil. I think Maplin used use the rectangular type for chokes and the loopies for coils and transformers.

Colin
--
cdb, RemoveMEcolinspamTakeThisOuTbtech-online.co.uk on 1/11/2010
Web presence: http://www.btech-online.co.uk   Hosted by:  http://www.1and1.co.uk/?k_id=7988359
 

2010\10\31@162516 by David

flavicon
face
 On 30/10/2010 23:16, William "Chops" Westfield wrote:
> Are you sure about the size of your polyfuse?  It looks significantly
> smaller than the 500mA fuse on most Arduinos, for example...   (I
> guess 500mA 1206-sized polyfuses do exist...)

Yes, I base my footprint choice on what I can get from Farnell for a sensible price in small quantities!  In many cases I could use smaller parts, but I don't have the confidence to try soldering them yet.

> I would move some of your traces to provide more clearance, and make
> traces thicker when its easily possible...

OK, I have started to do this.  In some cases bumping to 10 or 16mil is fairly easy.

> The actual paths taken by GND to reach the supply pins of the FTDI
> chip are pretty twisted.  Having a ground plane doesn't guarantee that
> the plane doesn't narrow inappropriately before it reaches where it
> needs to go.  I'd stick another ground plane on the bottom layer, with
> a bunch of gratuitous vias.

Based on multiple sets of feedback I have now done this too.  GND plane on the bottom, lots of vias from individual pins.  I will see if I can reroute some of the top now to tidy it up.  For serial at 19200 baud, I'm pretty sure it isn't essential!  However, very important points to learn for the future.

> 220 ohms is a really low value for a modern SMT indicator LED.  Unless
> you really want them to be as bright as possible and consume more
> current than the entire rest of the circuit...  Current arduino boards
> are using 1k, and even that is uncomfortably bright in some cases (The
> blue "pin 13" LED on the solarbotics Freeduino, for example.)

Good point, now bumped to 1K.  I will investigate a few of my other boards to see what I used, the LEDs on those are not unacceptably bright.

> Are you sure you don't want to break out the CBUS signals to pads as
> well?  There's a hack out there that lets you use them to bit-bang
> program an AVR, for example.

I should have thought of this, it is possibly more useful than the other serial pins in many cases.  However, I don't forsee it being something I will need just yet.  Perhaps on a v2 of this board, if I ever make one.  I'm more eager to stop fiddling and send this off for manufacture!

Thanks very much.

Davi

2010\10\31@165851 by Michael Watterson

face picon face
 On 31/10/2010 18:38, Olin Lathrop wrote:
> Wouter van Ooijen wrote:
>> If you seriously say "anyone can write up a standard" then a new
>> standard (by definition not in wide use yet) is not to be taken
>> seriously?
> Of course every standard has to start somehow.  What I mean is that a
> standard is one in name only until people actually use it.  Whether it is
> taken seriously during its startup period has a lot to do with how good it
> is, whether it meets a need, who is behind it, perception, marketing etc.
>
> In this case though we were talking about standards old enough so that it's
> fair to judge how real they are based on how widely they are adopted.
>
There are basically only two standards for schematics. I can't believe you are not familiar with Continental European usage. It's at least as widely used and predates CAD and MSI.
Maybe Elecktor Magazine, isn't sold in USA. Radcom house style (RSGB) seems a mix of the US and European, they don't consistently use rectangle or /\/\/\/\ symbol for resistor. . But that is UK, who are never quite sure about Europe :)

Again here you have solid rectangle for non-RF coils on mains and audio and loops only for RF inductors
http://www.radiotechnik-web.de/data/storage/attachments/12818847083955.jpg

http://www.radiotechnik-web.de/page1.php?view=preview&category=15&image=5956

It's not very relevant who was 1st or the process. It's very well known and a standard to use rectangles for coils

2010\10\31@183034 by Bob Blick

face
flavicon
face
On Sat, 30 Oct 2010 15:57:26 -0400, "Olin Lathrop" said:

> Unfortunately we see more and more shortcuts.  I don't know if it's
> laziness, sloppiness, or what.  The old way makes sense.  This is the
> first
> I've seen a inductor look not loopy though.  Let's not get sloppy with
> those
> too.  It's bad enough that it's become acceptable in some places to draw
> resistors as rectangular boxes.  I don't know where that came from, but I
> don't understand why someone had to go invent a new and less descriptive
> symbol when there was a nice one already standard.  All "old" schematics
> I've ever seen show resistors as zigzags, so I think the box came later.

As an engineer I figure there is a certain minimum level of knowledge
and competence one is expected to have.
You use Eagle, so I would expect you to know about "other" symbols that
are standard.

If a client came to me asking me to do a drawing and handed me a
schematic with symbols from the other standard, I might ask them if they
wanted the same style.

If I didn't understand one or more of the symbols, there are two things
I would not do:

1) Let them know of my ignorance. I'd find out what that symbol was
later.
2) Tell them they were wrong to use symbols that I didn't like.

I also would not tell them I used Internet Explorer 6, because added up,
all those things might make them think I was an old crank (but certainly
not a moron, or lazy, or sloppy, because those are bad). Either way, not
someone easy to do business with.

Especially when you are clearly wrong about which symbols are "correct".
There is often more than one choice in symbol to use, and if you are an
engineer, I would expect you to be familiar with the international style
and be able to use it, just as I would expect you to be able to lay out
a board using metric units. So if someone posts a schematic to the
Piclist, you should be able understand it even if it's not in your
preferred style. Because your preferred style is just that. It's not
universally preferred.

> > I think any EE should be familiar with
> > it, something like being familiar with "km" even though it's not
> > frequently used everywhere.
>
> I don't know what "km" is either.  Do you mean "Km" perhaps?

No, not an old crank. Not at all :)

Friendly regards,

Bob


-- http://www.fastmail.fm - The professional email service

2010\10\31@184441 by Jon Chandler

picon face
Some examples of schematics from the mid 40's can be found in the Weston Engineering Notes I've posted here:

http://www.clever4hire.com/throwawaypic/home/weston-engineering-notes

Resistors and capacitors are according to Olin's "standard."  I'm not sure about inductors.  Transformer windings are shown as coils but in a quick scan I didn't see any clear inductor examples.  In one place it looks like an inductor may be shown more like a resistor.....


Jon

2010\10\31@185923 by ivp

face picon face
> As an engineer I figure there is a certain minimum level of knowledge
> and competence one is expected to have

Agreed. There are 'two' of lots of things. Upper and lower case,
miles and kilometers (I'm actually very surprised Olin didn't know
km), Arabic and Roman numerals etc etc

I prefer resistors to be represented by zigzags because zigzags are
clearer when glancing. Schematics drawn using boxes with the value
inside the box look a little tidier but could lead to mistakes if not
well drawn. Silicon Chip's Vintage Radio section reprints original
circuits from as long ago as 100 years. A mix of US, Australian and
British designs. And they all look pretty much the same. Zigzags for
resistors, loops for coils and a pair of solid bars for capacitors

Joe

*
*
**********
Quality PIC programmers
http://www.embedinc.com/products/index.ht

2010\10\31@193043 by Gerhard Fiedler

picon face
Olin Lathrop wrote:

> Gerhard Fiedler wrote:
>> Here you see a few old schematics. Obviously none of them is anywhere
>> near the time where the symbols weren't already (more or less, at
>> least) standardized, but in any case you can see that the use of the
>> filled rectangle for an inductor and a transformer goes way back in
>> some parts of the world and is not something recent.
>> www.radiotechnik-web.de/page1.php?view=thumbnailList&category=15
>
> The second picture there of the Dominante W2 schematic is
> interesting. Unfortunately the scan is so low res it's hard to tell
> for sure, but it looks like they are using something wiggly for
> inductors, and blocks for resistors.  It looks like the lower right
> corner is a key to the power rating of different resistors.
> Different stuff in the box apparently describes the power rating.
>
> So far all the tube-era schematics, including at least the first two
> from your link above, seem to use wiggly or loopy symbols for
> inductors.  I suspect those came first, which makes me wonder who
> decided to invent a new symbol and why?

You apparently didn't have a close look. The second schematic (the one
you're talking about) uses three quite prominent filled-rectangle
transformers (mains transformer, lower left, and two loudspeaker
transformers, far right). The RF inductors in this schematic are
half-circle style. The first schematic uses the filled rectangle for the
loudspeaker transformer, far right.

I didn't check all of the schematics at that link, but the eight or so I
checked did have at least one inductor or transformer in
filled-rectangle style. This is pretty easy to spot (just look for the
fat black areas), but you have to /want/ to see them -- no graphic can
convince the brain of something it doesn't want to be convinced of :)

I even told you that they were there... the fact that even this didn't
make you "see" them speaks quite loudly. Among other things, it tells me
that it's time to quit this exchange.


Just get over it... for reasons we probably can't find out with
certainty, the solid rectangle style became common in certain parts of
the world.

Maybe the beginning was trying to squash many windings together... if
you do that with the loopy symbol, you get the black rectangle. This
would match the style that uses the black rectangles for transformers
with many windings and the semi-circle style for RF inductors (with
probably fewer windings).
Gerhar

2010\10\31@193459 by Gerhard Fiedler

picon face
Jon Chandler wrote:

> Some examples of schematics from the mid 40's can be found in the
> Weston Engineering Notes I've posted here:
>
> www.clever4hire.com/throwawaypic/home/weston-engineering-notes
>
> Resistors and capacitors are according to Olin's "standard."  I'm not
> sure about inductors.  Transformer windings are shown as coils but in
> a quick scan I didn't see any clear inductor examples.  
I think it's a pretty safe bet to assume that a reasonably consistent
schematic that uses zigzag resistors also uses half-circle or loop
coils. I have never seen a schematic with solid rectangle inductors that
didn't also use rectangle resistors.

> In one place it looks like an inductor may be shown more like a
> resistor.....

Where's that?

Gerhar


'[EE] PCB critique'
2010\11\01@113923 by Herbert Graf
picon face
On Sun, 2010-10-31 at 15:24 +0100, Wouter van Ooijen wrote:
> Note that google "nand gate symbol" shows only the old-fashioned
> symbols, and the first match http://www.kpsec.freeuk.com/gates.htm
> expresses a clear preference for the old-fashioned symbools :(

I've never even seen those "new" symbols, they are truly horrible,
hopefully they'll never catch on.

TTYL

2010\11\01@114343 by Herbert Graf

picon face
On Sun, 2010-10-31 at 18:12 +0000, Geo wrote:
> My oldest  magazine from the bookshelf is 1948 - I have photographed the
> cover and a circuit diagram of a receiver:-
> http://www.8zero.co.uk/circuit.jpg
> http://www.8zero.co.uk/cover.jpg
>
> In the drawing office of a radio factory in 1961 all circuit diagrams
> were hand drawn for production, test and service manuals.
> There were no rectangles.

Cool, thanks!

It's amazing that a design over 60 years old still still pretty
recognizable in function to me. Some things at a fundamental level just
don't change that much.

TTYL

2010\11\01@120337 by alan.b.pearce

face picon face
> > Note that google "nand gate symbol" shows only the old-fashioned
> > symbols, and the first match http://www.kpsec.freeuk.com/gates.htm
> > expresses a clear preference for the old-fashioned symbools :(
>
> I've never even seen those "new" symbols, they are truly horrible,
> hopefully they'll never catch on.

The IEC symbols have been around for several decades, and are common on
schematics that originate in Europe.
But I agree with your comment about the symbols for gates. More complex
devices like counters and so on do have symbols that can be better than
the 'American' ones.
-- Scanned by iCritical.

2010\11\01@120722 by alan.b.pearce

face picon face
> In the drawing office of a radio factory in 1961 all circuit diagrams
> were hand drawn for production, test and service manuals.
> There were no rectangles.

Same when I started my apprenticeship in new Zealand, in 1969. They were
still hand drawn 10 years later and PCBs laid out with real tape,
although I suspect by then any large company in the USA would have had
CAD systems for both functions.
-- Scanned by iCritical.

2010\11\01@121739 by Jon Chandler

picon face
Gerhard Fiedler wrote:
{Quote hidden}

>    On page 6 of the 5th issue from 1946, a current transformer is shown where the windings seem to be represented more like a zig-zag resistor

2010\11\01@122138 by Herbert Graf

picon face
On Mon, 2010-11-01 at 16:04 +0000, alan.b.pearceEraseMEspam.....stfc.ac.uk wrote:
> The IEC symbols have been around for several decades, and are common on
> schematics that originate in Europe.
Wow, didn't know that.

> But I agree with your comment about the symbols for gates. More complex
> devices like counters and so on do have symbols that can be better than
> the 'American' ones.

FWIW and IMHO, beyond "simple" gates I don't want any schematic symbol,
at that point HDL is FAR more efficient then a mess of boxes with
writing in it.
TTYL

2010\11\01@123430 by Harold Hallikainen

face
flavicon
face

> On Sun, 2010-10-31 at 15:24 +0100, Wouter van Ooijen wrote:
>> Note that google "nand gate symbol" shows only the old-fashioned
>> symbols, and the first match http://www.kpsec.freeuk.com/gates.htm
>> expresses a clear preference for the old-fashioned symbools :(
>
> I've never even seen those "new" symbols, they are truly horrible,
> hopefully they'll never catch on.
>
> TTYL
>

I think I first saw these "new" symbols in a TI catalog in the 1980s. I'm
not used to them, so I do find them hard to read. Most stuff I'm using now
tends to be represented as boxes since there's so much stuff in them. I
note that the above referenced web page uses bubbles to indicate an active
low output. TI uses a triangle or slanted line. See
http://focus.ti.com/lit/ds/symlink/74ac11000.pdf . Also, from that
datasheet, "This symbol is in accordance with ANSI/IEEE Std 91-1984 and
IEC Publication 617-12."

Harold




-- FCC Rules Updated Daily at http://www.hallikainen.com - Advertising
opportunities available

2010\11\01@123913 by alan.b.pearce

face picon face
> > But I agree with your comment about the symbols for gates. More
complex
> > devices like counters and so on do have symbols that can be better
than
> > the 'American' ones.
>
> FWIW and IMHO, beyond "simple" gates I don't want any schematic
symbol,
> at that point HDL is FAR more efficient then a mess of boxes with
> writing in it.

But somewhere along the line, that device containing the HDL needs a
symbol that gets put on a schematic to generate a net list to lay out a
PCB ...
-- Scanned by iCritical.

2010\11\01@124506 by Olin Lathrop

face picon face
alan.b.pearce@stfc.ac.uk wrote:
> Same when I started my apprenticeship in new Zealand, in 1969. They
> were still hand drawn 10 years later and PCBs laid out with real tape,
> although I suspect by then any large company in the USA would have had
> CAD systems for both functions.

Hewlett Packard in New Jersey didn't when I started there in 1980.  I drew
schematics on D size vellum using pencil and eraser.  These were eventually
given to a board guy who would lay it out at 2.5x or 4x scale with
calibrated tape.  That would get photographed in transparency mode to make
the 1:1 mask films.

They were getting in and testing a CAD system when I left there in 1982.

2010\11\01@131017 by Michael Watterson

face picon face
 On 01/11/2010 16:45, Olin Lathrop wrote:
> EraseMEalan.b.pearcespamstfc.ac.uk wrote:
>> Same when I started my apprenticeship in new Zealand, in 1969. They
>> were still hand drawn 10 years later and PCBs laid out with real tape,
>> although I suspect by then any large company in the USA would have had
>> CAD systems for both functions.
> Hewlett Packard in New Jersey didn't when I started there in 1980.  I drew
> schematics on D size vellum using pencil and eraser.  These were eventually
> given to a board guy who would lay it out at 2.5x or 4x scale with
> calibrated tape.  That would get photographed in transparency mode to make
> the 1:1 mask films.
>
> They were getting in and testing a CAD system when I left there in 1982.
>
My last tape design was in 1981. I still have one prototype model of it, a single Eurocard Z80 controller.
From 1982 it was CAD
For schematic capture stage "Futurenet" was really good, used it up to about 1988
I use Eagle now. Used orcad, Autotrax, No1 systems and some other in the past. I had a quicl look at kicad as it is "free" and they imported all the Eagle libraries they could find..
But Eagle is kind of a standard, I have a paid version and anyone can view/print/plot anysize board with the free download

2010\11\01@151901 by Philip Pemberton

face
flavicon
face
On 01/11/10 16:04, RemoveMEalan.b.pearceEraseMEspamEraseMEstfc.ac.uk wrote:
> The IEC symbols have been around for several decades, and are common on
> schematics that originate in Europe.

Elektor love those symbols. I think they're pure, distilled evil...

There's a good reason I keep the Texas Instruments Logic Pocket Databook around: it has both sets of symbols, and full pinouts for almost the entire 74LS and 4000 series. Well worth pestering your local TI rep for a copy, if it's still available :)

-- Phil.
RemoveMEpiclistspam_OUTspamKILLspamphilpem.me.uk
http://www.philpem.me.uk

2010\11\01@162840 by Herbert Graf

picon face
On Mon, 2010-11-01 at 16:39 +0000, RemoveMEalan.b.pearceTakeThisOuTspamspamstfc.ac.uk wrote:
> > > But I agree with your comment about the symbols for gates. More
> complex
> > > devices like counters and so on do have symbols that can be better
> than
> > > the 'American' ones.
> >
> > FWIW and IMHO, beyond "simple" gates I don't want any schematic
> symbol,
> > at that point HDL is FAR more efficient then a mess of boxes with
> > writing in it.
>
> But somewhere along the line, that device containing the HDL needs a
> symbol that gets put on a schematic to generate a net list to lay out a
> PCB ...

Actually for many here, the HDL is usually uploaded to a piece of
programmable logic (be it PAL, CPLD, FPGA, etc.), so the schematic
symbol is of that device (an "IC" symbol).

Otherwise the HDL is being made into an ASIC, in which case it will of
course have a schematic symbol, but it'll just be an "IC" symbol as
well.

Function specific symbols are actually kinda rare in the digital domain,
other then basic gates, the only ones I sometimes use are DAC/ADC
symbols, even there the physical device often is multifunction negating
the possibility of just plunking down a fixed function symbol (i.e. a
DAC with HDMI and analog outputs).

TTYL

2010\11\02@144007 by Charles Rogers

flavicon
face


From: "Olin Lathrop"
> For most common parts I have two or more versions of them in the library,
> one for each of the common rotations.  For example, I have both vertical
> and
> horizontal resistors premade.  That way you don't end up with a mess like
> your R5, R4, etc.  If you don't have a pre-rotated part, then you have to
> "smash" the part and rotate and position the text manually.  That's part
> of


This is why a lot of people don't use Eagle.  It is a third rate program that
is used because its free to start with.  I used it five years before I finally
found a good cad program.

CR

2010\11\02@165500 by M.L.

flavicon
face

On Tue, Nov 2, 2010 at 2:40 PM, Charles Rogers <EraseMEcrogersspamspamspamBeGonetotelcsi.com> wrote:

>
> This is why a lot of people don't use Eagle.  It is a third rate program
> that
> is used because its free to start with.  I used it five years before I
> finally
> found a good cad program.
>
> CR

How much did your good CAD program cost? I'm going to go ahead and
guess that it was more than 3 times as much as the pro version of
Eagle.

--
Martin K.

2010\11\02@170916 by Wouter van Ooijen

face picon face
>> This is why a lot of people don't use Eagle.  It is a third rate program
>> that
>> is used because its free to start with.  I used it five years before I
>> finally
>> found a good cad program.

> How much did your good CAD program cost? I'm going to go ahead and
> guess that it was more than 3 times as much as the pro version of
> Eagle.

and <numeric-overflow> times more than the free version ....

--
Wouter van Ooijen

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

2010\11\02@185329 by David

flavicon
face
On 02/11/2010 18:40, Charles Rogers wrote:
> From: "Olin Lathrop"
>> For most common parts I have two or more versions of them in the library,
>> one for each of the common rotations.  For example, I have both vertical
>> and
>> horizontal resistors premade.  That way you don't end up with a mess like
>> your R5, R4, etc.  If you don't have a pre-rotated part, then you have to
>> "smash" the part and rotate and position the text manually.  That's part
>> of
>
> This is why a lot of people don't use Eagle.  It is a third rate program
> that
> is used because its free to start with.  I used it five years before I
> finally
> found a good cad program.

Which is that good it deserves naming! :)

Honestly, I'm open to suggestions but I can't mind read..

Davi

2010\11\02@192142 by Joseph Bento

face
flavicon
face

On Nov 2, 2010, at 12:40 PM, Charles Rogers wrote:

>
> This is why a lot of people don't use Eagle.  It is a third rate program
> that
> is used because its free to start with.  I used it five years before I
> finally
> found a good cad program.
>
> CR
>
I can't say I know too many hobbyists that can afford the US$5,000 or more that Altium costs, not to mention their annual maintenance subscription.

I think Eagle does very well for the market it's intended to serve.

Joe

2010\11\03@042906 by Michael Watterson

face picon face
 On 02/11/2010 23:21, Joseph Bento wrote:
> On Nov 2, 2010, at 12:40 PM, Charles Rogers wrote:
>
>> This is why a lot of people don't use Eagle.  It is a third rate program
>> that
>> is used because its free to start with.  I used it five years before I
>> finally
>> found a good cad program.
>>
>> CR
>>
> I can't say I know too many hobbyists that can afford the US$5,000 or more that Altium costs, not to mention their annual maintenance subscription.
>
> I think Eagle does very well for the market it's intended to serve.
>
> Joe
>
>
If you want multipage schematics and bigger than 100mm x 160mm board and all the features, then Eagle is not a budget package.

1 user $1494
5 user $2988

The free version is only one page schematic, and 100mm x 80mm board

100mm x 160mm board $747

It would not be the nicest schematic capture GUI I have ever used, but other aspects are OK.
I've used 3rd rate programs. Eagle might be in 2nd tier, not 3rd rate

2010\11\03@055850 by Isaac Marino Bavaresco

flavicon
face
Em 3/11/2010 06:28, Michael Watterson escreveu:
> If you want multipage schematics and bigger than 100mm x 160mm board and
> all the features, then Eagle is not a budget package.
>
> 1 user $1494
> 5 user $2988
>
> The free version is only one page schematic, and 100mm x 80mm board
>
> 100mm x 160mm board $747
>
> It would not be the nicest schematic capture GUI I have ever used, but
> other aspects are OK.
> I've used 3rd rate programs. Eagle might be in 2nd tier, not 3rd rate.

KiCAD and gEDA are free and open-source.

I tried gEDA once but it was ugly, as a text-mode application converted
to run inside a graphical window (what it probably was). I found it very
awkward also. It seemed a little derelicted. Perhaps by now they had
updated it.

KiCAD is modern and works well, apart from a little odd user interface.
If I were in need for a free EDA package, I would give KiCAD a try.
It comes with some very sophisticated example designs. Besides, it is
built around wxWidgets and is truly multi-platform.


Best regards,

Isaac

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

2010\11\03@072953 by Michael Watterson

face picon face
 On 03/11/2010 09:58, Isaac Marino Bavaresco wrote:
{Quote hidden}

KiCAD is worth a look, as I mentioned earlier. It's the best "actually" free package I've seen. If I need bigger than 160x100 I may invest the time.

2010\11\03@075337 by Olin Lathrop

face picon face
Charles Rogers wrote:
> This is why a lot of people don't use Eagle.  It is a third rate
> program that
> is used because its free to start with.  I used it five years before I
> finally
> found a good cad program.

Wow, that's quite the attitude to the point it sounds religious and
therefore a bit hard to take seriously.  The fact that you didn't say what
your alternative program was further undermines the credibility of your
comment.

We have 3 full licenses of Eagle here and have done dozens of designs with
it.  It has it quirks and things you have to get used to, but so does every
other large piece of software I've ever seen.  One really great feature of
Eagle is that you can write ULPs, which are programs that run internally to
Eagle and can access all the internal data.  The UI is also done right, in
that the clickety-click interface is layered on the same command engine you
can type commands to directly or from scripts or from the result of ULPs.

If I remember right, we paid $1200 for the first full license and $400 for
each of the two additional ones probably ten years ago.  There has been one
paid upgrade during that time, which came out to something like $600 total
if I remember right.

So please tell us, what is this "good" program you found and how much did it
cost?


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

2010\11\03@081028 by Olin Lathrop

face picon face
Michael Watterson wrote:
> If you want multipage schematics and bigger than 100mm x 160mm board
> and all the features, then Eagle is not a budget package.
>
> 1 user $1494
> 5 user $2988

Sounds pretty good actually.  For 5 users, that's $600/seat for integrated
schematic capture, layout, routing, and auto-routing.  That's a fraction of
a billable day you have to spend once, with smaller amounts every few years..
Think of it in terms of time, and you can see it's way less than the cost of
learning any complex package.  Or put another way, the price of the software
is a small fraction of the overall cost, so there is really nothing to
complain about with Eagle in that regard.


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

2010\11\03@091123 by Sean Breheny

face picon face
I wholeheartedly second these recommendations. I have now done two
moderately complex designs with KiCAD with good results.


>  On 03/11/2010 09:58, Isaac Marino Bavaresco wrote:
>> KiCAD is modern and works well, apart from a little odd user interface.
>> If I were in need for a free EDA package, I would give KiCAD a try.
>> It comes with some very sophisticated example designs. Besides, it is
>> built around wxWidgets and is truly multi-platform.
>>


On Wed, Nov 3, 2010 at 7:29 AM, Michael Watterson <RemoveMEmikeKILLspamspamradioway.org> wrote:
> KiCAD is worth a look, as I mentioned earlier. It's the best "actually"
> free package I've seen. If I need bigger than 160x100 I may invest the time.
>

2010\11\03@123146 by William \Chops\ Westfield

face picon face

> If you want multipage schematics and bigger than 100mm x 160mm board  
> and
> all the features, then Eagle is not a budget package.
>
> 1 user $1494

What are you comparing it to?  As far as I have been able to tell, the  packages that (almost) everyone agrees are better than Eagle run  several times that price, and STILL make EAGLE look like a "budget"  option.


> The free version is only one page schematic, and 100mm x 80mm board

The free version is also only for non-commercial use.  You're supposed  to pony up a whopping $49 if you want to put up with those  restrictions in a for-profit business.  For non-profit use there is  also a special license that does 100x160mm and 6 layers for $125 (http://www.cadsoftusa.com/nonprofit.htm )


>> It is a third rate program that is used because its free to start  
>> with.

Trollish behavior.  EAGLE is at least 2nd-rate!  Compared to other  programs in the same price range (0-$2k), EAGLE is starting to achieve  the enviable position of being popular because lots of people use it,  and support (community and company) is ... pretty good.

BillW

2010\11\03@234430 by Harold Hallikainen

face
flavicon
face
Another system I used at a previous job (from the first DOS version as a
replacement of my Dasoft CP/M system) was
http://www.advancedmsinc.com/creator/index.htm . It worked pretty well for
me for many years.

Harold

-- FCC Rules Updated Daily at http://www.hallikainen.com - Advertising
opportunities available

2010\11\04@173821 by Gerhard Fiedler

picon face
Jon Chandler wrote:

{Quote hidden}

Ah, yes... I'm glad we're (mostly) past that stage with standardization.
If they hadn't written what it was meant to be in text... :)

Gerhar

More... (looser matching)
- Last day of these posts
- In 2010 , 2011 only
- Today
- New search...