Searching \ for '[PIC]: EAGLE Question' 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=eagle
Search entire site for: 'EAGLE Question'.

Exact match. Not showing close matches.
PICList Thread
'[PIC]: Eagle Question'
2002\05\31@135255 by tundra

flavicon
face
I've been using the freeware version of Eagle for various PIC projects.
In so doing, I had to add something to the transistor-fet libraray (the
2n7000 is oddly missing).  Now that I have upgraded to the latest version
of Eagle, is there a simple way to extract my definition from the old library
and add it to the new one.  More to the point, is there a way to extract
my FET defintion and creat a new library where I can just put my own stuff?

TIA,
--
------------------------------------------------------------------------------
Tim Daneliuk
spam_OUTtundraTakeThisOuTspamtundraware.com

--
http://www.piclist.com hint: To leave the PICList
.....piclist-unsubscribe-requestKILLspamspam@spam@mitvma.mit.edu


2002\05\31@141208 by Lawrence Lile

flavicon
face
Eagle's library management is not it's strongest point.  They have promised
to improve it in the next version, but so far we are stuck with this:

I could not find a way to copy a "Device".  There IS a way to copy a
package, and copy a symbol, then create a new device in a new library.

To copy a package or symbol:
Open the appropriate library, and load the device using LIBRARY:PACKAGE or
LIBRARY:SYMBOL
Select the GROUP icon and pick everything
Select EDIT:CUT (not COPY) and press the GO button which looks light a
stoplight.   This is important. COPY doesn't work, and the GO button seems
to be key to the whole thing.  Your Mileage May Vary.

Create a new library with FILE:NEW
Choose LIBRARY:PACKAGE:NEW and name it
Choose EDIT:PASTE and place your new package

Likewise with the symbol

Create a new device, add the symbol and package, and wire up the terminals.

Like I said, not the smoothest user interface, and admittedly Eagle's
biggest weak point.  There are some ULP (user language programs) that
purport to make library management easier but I haven't looked into them.

--Lawrence



{Original Message removed}

2002\05\31@163745 by David P. Harris

picon face
Hi-
Group everthing, then select Cut (scissors), then RIGHT click on the screen to
select the group.  Change to the new library, select Paste (paste bottle), and
right clck again.  You don't need to use the Go button.
David

Lawrence Lile wrote:

{Quote hidden}

> {Original Message removed}

2002\05\31@172725 by Lawrence Lile

flavicon
face
Yup, that is another way to do it.  There is probably a third way as well.
I just find that the COPY command does not work like I expect it to.

--Lawrence
{Original Message removed}

2002\05\31@173336 by Jim

flavicon
face
1. EXPORT the particular library you are interested in as an
  ASCII text/script file.

2. Edit said ASCII text file - editting as many parameters for
  device symbol or device outline and pads as needed **en masse**.

3. Import/'run' the ASCII text file as a 'script' file -

4. Then SAVE it under a different name (leaves the old library
  intact!).


This reduces the repetitive work-load within the GUI editor
in Eagle when changing *hoards* of, say, pad sizes ....

Jim


{Original Message removed}

2002\05\31@174024 by Jim

flavicon
face
   "I could not find a way to copy a "Device". "

Export library

Edit file

Import the text/script file.

Save new library


Jim


{Original Message removed}

2002\05\31@181102 by tundra

flavicon
face
Jim wrote:
>
>     "I could not find a way to copy a "Device". "
>
> Export library
>
> Edit file
>
> Import the text/script file.
>
> Save new library
>
> Jim
>


Many thanks to all who provided their insight ...
------------------------------------------------------------------------------
Tim Daneliuk
tundraspamKILLspamtundraware.com

--
http://www.piclist.com hint: To leave the PICList
.....piclist-unsubscribe-requestKILLspamspam.....mitvma.mit.edu


2002\05\31@182013 by Lawrence Lile

flavicon
face
I guess I have tried that.  Another method of managing libraries in Eagle is
this, copied from the Eagle manual page 215:

At midnight on June 22, wave a dead fish over the library.  As soon as the
full moon rises over your left shoulder, tie a string to a rabbit's tail,
and have the string go through a set of pulleys and knock a water vase off a
shelf to wake a midget captain.  The midget captain then pulls a lever which
presses the "GO" button which looks like a stop button. Select the "Grep"
button, then press the middle left mouse button while holding the Control,
ALT, left shift, big orange switch and F13 buttons down with your other hand
and pressing the CD open button on your computer with your big toe.  Hold
your mouth so your left lip is curled up and your right lip is curled down,
chanting "all your base are belong to us" and simple! that's all there is to
it!

 ;-)

One of the biggest complaints on the Eagle suggestion board is an
improvement in library management, and a return to Windows default behavior
in the copy/cut/paste functions.  Hopefully they will get it right soon.
Other than that it is a good program.

--Lawrence

{Original Message removed}

2002\05\31@202958 by Tal (Zapta)

flavicon
face
How do one exports a library ?

I tried

1. Right click on the library name in the tree

2. Select open from the popup menu

3. File -> Export ->

4. Eagle shows a popup menu with Script, Directory and Image ?????????

Thanks,

Tal

> {Original Message removed}

2002\05\31@213458 by Jim

flavicon
face
Choose 'script'.

It will actually be a text file that one can use
any common text editor to use and edit the file.

Jim


----- Original Message -----
From: "Tal (Zapta)" <EraseMEtalspam_OUTspamTakeThisOuTZAPTA.COM>
To: <PICLISTspamspam_OUTMITVMA.MIT.EDU>
Sent: Friday, May 31, 2002 7:27 PM
Subject: Re: [PIC]: Eagle Question


{Quote hidden}

> > {Original Message removed}

2002\05\31@233237 by gaston gagnon

face
flavicon
face
Hi Tim,

Tim Daneliuk a icrit :

> <...>  I had to add something to the transistor-fet libraray (the
> 2n7000 is oddly missing).  Now that I have upgraded to the latest version
> of Eagle, is there a simple way to extract my definition from the old library
> and add it to the new one.  More to the point, is there a way to extract
> my FET defintion and creat a new library where I can just put my own stuff?

One other way to do this is :
1) create a new schematic ;
2) Add only the part(s) that you wish to export to your new library;
3) clic on the board icon to make a board as well ;
4) clic ont ULP icon ;
5) select "exp-project-lbr.ulp"  ;
6) "Collect data" and Create library.

There you have a new library with only the parts you want.

Hope this works for you.
Gaston

--
http://www.piclist.com hint: To leave the PICList
@spam@piclist-unsubscribe-requestKILLspamspammitvma.mit.edu



'[PIC]: EAGLE Question'
2003\02\14@045405 by Sean Alcorn - PIC Stuff
flavicon
face
Hi all,

Has anybody tried to make a dual diode SOT-23 package in EAGLE?

The ideal way to do it would be to have two "Gates" that are diode
symbols in order to be able to place the two diodes anywhere on a
schematic - however this is four connections to be made to 3 pads and
EAGLE does not seem to allow this.

The only other way is to draw the entire "double diode" as one symbol
with 3 pins - however this seems restrictive when trying to place the
component on a sheet. :-(

Any ideas greatly appreciated.

Regards,

Sean

--
http://www.piclist.com#nomail Going offline? Don't AutoReply us!
email KILLspamlistservKILLspamspammitvma.mit.edu with SET PICList DIGEST in the body

2003\02\14@081730 by Olin Lathrop

face picon face
> Has anybody tried to make a dual diode SOT-23 package in EAGLE?
>
> The ideal way to do it would be to have two "Gates" that are diode
> symbols in order to be able to place the two diodes anywhere on a
> schematic - however this is four connections to be made to 3 pads and
> EAGLE does not seem to allow this.
>
> The only other way is to draw the entire "double diode" as one symbol
> with 3 pins - however this seems restrictive when trying to place the
> component on a sheet. :-(

Since the two diodes are physically connected, it doesn't make sense in
most cases to separate them in the schematic.  You can define the two
separate pins as swappable.

If you really want two separate schematic symbols for the two (not really
independent) diodes, you could create a "gate" for each separate end.  The
symbol for each gate would have one pin coming out with the other end
inside a box or something connected to a common rail.  Unfortunately this
would have to be part of the symbol itself, so there is no way to document
in that symbol automatically what rail the common pin is connected to.
The common pin would also be a separate "must" or "always" gate (I
remember which is which and have to look it up every time), similar to the
way you deal with power and ground connection of multi-gate logic ICs.


*****************************************************************
Embed Inc, embedded system specialists in Littleton Massachusetts
(978) 742-9014, http://www.embedinc.com

--
http://www.piclist.com#nomail Going offline? Don't AutoReply us!
email RemoveMElistservTakeThisOuTspammitvma.mit.edu with SET PICList DIGEST in the body

2003\02\14@112838 by Ned Konz

flavicon
face
On Friday 14 February 2003 01:52 am, Sean Alcorn - PIC Stuff wrote:
> Hi all,
>
> Has anybody tried to make a dual diode SOT-23 package in EAGLE?

There are already dual diode SOT-23 packages in Eagle.
Look in diode.lbr and zetex.lbr.

> The ideal way to do it would be to have two "Gates" that are diode
> symbols in order to be able to place the two diodes anywhere on a
> schematic - however this is four connections to be made to 3 pads
> and EAGLE does not seem to allow this.

You can add a 4th connection/pad.

> The only other way is to draw the entire "double diode" as one
> symbol with 3 pins - however this seems restrictive when trying to
> place the component on a sheet. :-(

I've never had any problem with it, especially as the diodes have a
common pin.

--
Ned Konz
http://bike-nomad.com
GPG key ID: BEEA7EFE

--
http://www.piclist.com#nomail Going offline? Don't AutoReply us!
email spamBeGonelistservspamBeGonespammitvma.mit.edu with SET PICList DIGEST in the body

2003\02\14@123349 by Peter L. Peres

picon face
On Fri, 14 Feb 2003, Sean Alcorn - PIC Stuff wrote:

*>The only other way is to draw the entire "double diode" as one symbol
*>with 3 pins - however this seems restrictive when trying to place the
*>component on a sheet. :-(

How can you 'separate' the two diodes ?!

Peter

--
http://www.piclist.com#nomail Going offline? Don't AutoReply us!
email TakeThisOuTlistservEraseMEspamspam_OUTmitvma.mit.edu with SET PICList DIGEST in the body

2003\02\14@203805 by Sean Alcorn - PIC Stuff

flavicon
face
Peter,

> How can you 'separate' the two diodes ?!

Just because they are physically connected in the same package does not
mean you always want them in the same spot on the schematic -
particularly with say a BAV99 - a A-K-A-K arrangement. You want the
common (A-K junction) pin to go to a PIC input (for example) and one
diode (gate) to be placed above that input line (to Vcc normally) and
another below it (to Ground usually)

Regards,

Sean

--
http://www.piclist.com#nomail Going offline? Don't AutoReply us!
email RemoveMElistservspamTakeThisOuTmitvma.mit.edu with SET PICList DIGEST in the body

2003\02\15@052232 by Peter L. Peres

picon face
On Sat, 15 Feb 2003, Sean Alcorn - PIC Stuff wrote:

*>Peter,
*>
*>> How can you 'separate' the two diodes ?!
*>
*>Just because they are physically connected in the same package does not
*>mean you always want them in the same spot on the schematic -
*>particularly with say a BAV99 - a A-K-A-K arrangement. You want the
*>common (A-K junction) pin to go to a PIC input (for example) and one
*>diode (gate) to be placed above that input line (to Vcc normally) and
*>another below it (to Ground usually)

But you clearly said 3 pins ? I am clear about 4 pin devices. Maybe I
misunderstood.

Peter

--
http://www.piclist.com hint: To leave the PICList
piclist-unsubscribe-requestEraseMEspam.....mitvma.mit.edu>

2003\02\15@104459 by David Harris

picon face
Sean-
I'm confused.  The layout of the BAV199 (I couln't find a BAV99) appears
to be laid out for exactly this application.  Granted you might have to
draw a net throught the device to continue you inout line, but I do not
find that terrible.
David

Sean Alcorn - PIC Stuff wrote:

{Quote hidden}

--
http://www.piclist.com hint: To leave the PICList
RemoveMEpiclist-unsubscribe-requestEraseMEspamEraseMEmitvma.mit.edu>

2003\02\16@002613 by Sean Alcorn - PIC Stuff

flavicon
face
--Apple-Mail-6-493900152
Content-Transfer-Encoding: 7bit
Content-Type: text/plain;
       charset=US-ASCII;
       format=flowed

Peter,

> But you clearly said 3 pins ? I am clear about 4 pin devices. Maybe I
> misunderstood.

Yes. I did. Still does not mean I don't want them in different places
on my schematic.

Regards,

Sean

--
http://www.piclist.com hint: PICList Posts must start with ONE topic:
[PIC]:,[SX]:,[AVR]: ->uP ONLY! [EE]:,[OT]: ->Other [BUY]:,[AD]: ->Ads



--Apple-Mail-6-493900152
Content-Transfer-Encoding: 7bit
Content-Type: text/enriched;
       charset=US-ASCII

Peter,


<excerpt><fixed>But you clearly said 3 pins ? I am clear about 4 pin
devices. Maybe I

misunderstood.

</fixed></excerpt>

Yes. I did. Still does not mean I don't want them in different places
on my schematic.


Regards,


Sean


--Apple-Mail-6-493900152--

2003\02\18@001700 by Roman Black

flavicon
face
Sean Alcorn - PIC Stuff wrote:

> > How can you 'separate' the two diodes ?!
>
> Just because they are physically connected in the same package does not
> mean you always want them in the same spot on the schematic -


Sure, Sean, check the library parts for the SIL
resistor networks. I noticed some do what you
need. ie separate resistors on SCH and the part
has one common wire. One SCH one is shown with
both legs, the other Rs in the package are only
shown with one leg. :o)
-Roman

--
http://www.piclist.com hint: The PICList is archived three different
ways.  See http://www.piclist.com/#archives for details.

2003\02\18@002312 by Sean Alcorn - PIC Stuff

flavicon
face
--Apple-Mail-12-666530272
Content-Transfer-Encoding: 7bit
Content-Type: text/plain;
       charset=US-ASCII;
       format=flowed


On Tuesday, Feb 18, 2003, at 15:58 Australia/Sydney, Roman Black wrote:

> Sure, Sean, check the library parts for the SIL
> resistor networks. I noticed some do what you
> need. ie separate resistors on SCH and the part
> has one common wire. One SCH one is shown with
> both legs, the other Rs in the package are only
> shown with one leg. :o)

Good thinkin' 99 :-)

Thanks,

Sean

--
http://www.piclist.com hint: The PICList is archived three different
ways.  See http://www.piclist.com/#archives for details.



--Apple-Mail-12-666530272
Content-Transfer-Encoding: 7bit
Content-Type: text/enriched;
       charset=US-ASCII



On Tuesday, Feb 18, 2003, at 15:58 Australia/Sydney, Roman Black wrote:


<excerpt><fixed>Sure, Sean, check the library parts for the SIL

resistor networks. I noticed some do what you

need. ie separate resistors on SCH and the part

has one common wire. One SCH one is shown with

both legs, the other Rs in the package are only

shown with one leg. :o)

</fixed></excerpt>

Good thinkin' 99 :-)


Thanks,


Sean


--Apple-Mail-12-666530272--

2003\02\18@134312 by Wagner Lipnharski

flavicon
face
Roman Black wrote:
> Sean Alcorn - PIC Stuff wrote:
>
>>> How can you 'separate' the two diodes ?!
>>
>> Just because they are physically connected in the same package does
>> not mean you always want them in the same spot on the schematic -
>
>
> Sure, Sean, check the library parts for the SIL
> resistor networks. I noticed some do what you
> need. ie separate resistors on SCH and the part
> has one common wire. One SCH one is shown with
> both legs, the other Rs in the package are only
> shown with one leg. :o)
> -Roman


Hi Roman, I was to comment that, but I personally hate that solution.
It is so "out of sense" to have an electronic part on the schematic that
has only one lead connected to something.  If it was made by you, perhaps
in 2 years you still remembering what is it, but not somebody else - this
unawared person can take a while until he can understand what a heck means
that one leg component, antenna?  :)

At this point, I would choose to just run wires to the packed 3 leads twin
component, at least it still more "professional" and readable.  Perhaps it
still influence from IBM heavy mainframe schematic books I used to work for
many years, where sometimes it takes you flipping pages up and down for 5
minutes until you can put a whole small circuit together, or concept, into
your brain.

Produce a schematic is always an art.  It is not only the job to put
components down and connect wires.  Some schematics are clean, even being
complex, they are easy to understand in seconds.  Others even being simple,
are hard to visualize and understand.  I am not even talking about those
schematics with hundreds of components, requiring several pages and
interconnecting symbols, wires and buses with names and codes.

We should not generalize, but in most cases, you can recognize a good
technician by the way he draws his schematics. Not talking about using
special software, I am talking about the way the schematic is transfered
from his brain to the restaurant napkin.

--
http://www.piclist.com hint: The PICList is archived three different
ways.  See http://www.piclist.com/#archives for details.

2003\02\18@141001 by Ned Konz

flavicon
face
On Friday 14 February 2003 01:52 am, Sean Alcorn - PIC Stuff wrote:
> Hi all,
>
> Has anybody tried to make a dual diode SOT-23 package in EAGLE?
>
> The ideal way to do it would be to have two "Gates" that are diode
> symbols in order to be able to place the two diodes anywhere on a
> schematic - however this is four connections to be made to 3 pads
> and EAGLE does not seem to allow this.
>
> The only other way is to draw the entire "double diode" as one
> symbol with 3 pins - however this seems restrictive when trying to
> place the component on a sheet. :-(

I drew one with two diode symbols and a single package that had 2 SMD
pads on top of each other.

However, the DRC flagged these pads as having clearance problems.

On the other hand, you could change the DRC rules to allow SMD pads
with the same signal to overlap (I think).

--
Ned Konz
http://bike-nomad.com
GPG key ID: BEEA7EFE

--
http://www.piclist.com hint: The PICList is archived three different
ways.  See http://www.piclist.com/#archives for details.

2003\02\18@172311 by William Chops Westfield

face picon face
   The ideal way to do it would be to have two "Gates" that are diode
   symbols in order to be able to place the two diodes anywhere on a
   schematic

Well, you CAN'T, really, since two of pins are common.  If you're using
them in a common situation (relay coil bypass?), you might define the
common pin as a hidden GND type connection, with two symbols each having
only a single pin...

I've been wanting to ask the opposite question - does anyone have some eagle
libraries (especially for micros and micro-related logic) where the symbol
definition has a more direct corrosponance with the physical part?  When
I'm arbitrarilly assigning functions to IO pins, it might be nice to have
at least some idea where on the chips those pins actually are...

BillW

--
http://www.piclist.com hint: The PICList is archived three different
ways.  See http://www.piclist.com/#archives for details.

2003\02\19@043141 by Roman Black

flavicon
face
Wagner Lipnharski wrote:
> It is so "out of sense" to have an electronic part on the schematic that
> has only one lead connected to something.

I agree totally.

> We should not generalize, but in most cases, you can recognize a good
> technician by the way he draws his schematics. Not talking about using
> special software, I am talking about the way the schematic is transfered
> from his brain to the restaurant napkin.

Yep, volts from top to bottom, pref drawn as rails,
and signal flow from left to right. No spastic sideways
Amercian transistors (grin) or little isolated blips
marked as Vdd or Gnd all over the place.
<asbestic> ;o)
-Roman

--
http://www.piclist.com#nomail Going offline? Don't AutoReply us!
email RemoveMElistservspam_OUTspamKILLspammitvma.mit.edu with SET PICList DIGEST in the body

2003\02\19@053444 by hael Rigby-Jones

picon face
{Quote hidden}

I agree this is desirable, but not always practical.  In a circuit where you
have multiple 100+ pin IC's and the schematic spans 7 or 8 pages it's pretty
much impossible not to use labels to show connections rather than actually
drawing the lines from chip to chip.

Mike

--
http://www.piclist.com#nomail Going offline? Don't AutoReply us!
email RemoveMElistservKILLspamspammitvma.mit.edu with SET PICList DIGEST in the body

2003\02\19@104853 by Wagner Lipnharski

flavicon
face
Roman Black wrote:
> Wagner Lipnharski wrote:
>> It is so "out of sense" to have an electronic part on the schematic
>> that has only one lead connected to something.
>
> I agree totally.
>
>> We should not generalize, but in most cases, you can recognize a good
>> technician by the way he draws his schematics. Not talking about
>> using special software, I am talking about the way the schematic is
>> transfered from his brain to the restaurant napkin.
>
> Yep, volts from top to bottom, pref drawn as rails,
> and signal flow from left to right. No spastic sideways
> Amercian transistors (grin) or little isolated blips
> marked as Vdd or Gnd all over the place.
> <asbestic> ;o)
> -Roman


I am not totally against any necessary change or sometimes innovative ways
to skin a cat, but personally I feel very strange to see a logic sequence
of events going down to top or from right to left.  Of course that it is
purely based on culture.  Many other cultures write books in this way.

As when reading a book, I expect to see some vital information about power
or voltages on top left.  It has been changed in time, and most power
supply circuits, regulators and filters are being positioned on bottom
left, but I still feel more comfortable to see them otherwise.  Also, I
expect to see input signals at the left, expecting the resulting output at
the right.

Of course, digital circuits, with mixed pins, not even talking about
bi-directional circuits, messed this up completely, not even talking about
several different supply voltages.

In the old electronic schematics, it was clear that the left side of the
paper would tell you the main line voltage path, the transformer section,
then the right side would be the useful electronics, of course, at that
time, mostly electronic components identified as 6BQ5, 12AX7, 6V6, and so
on... :)

Perhaps the top to bottom may have connections with reading, or the natural
way to understand hidromechanical machines (water flow).

One thing that I feel completely annoying is when a signal path going to
right, not being a feedback suddenly returns to left, it really pesters my
good mood, even understanding that sometimes it is done by lack of space on
the paper or something like that.

But it is being fun to see what the "uncultured" mind can comes up with
different ways to do the same old things.

Wagner.

--
http://www.piclist.com#nomail Going offline? Don't AutoReply us!
email listservSTOPspamspamspam_OUTmitvma.mit.edu with SET PICList DIGEST in the body

2003\02\19@115200 by Adi Linden

flavicon
face
> Yep, volts from top to bottom, pref drawn as rails,
> and signal flow from left to right. No spastic sideways
> Amercian transistors (grin) or little isolated blips
> marked as Vdd or Gnd all over the place.

Now that I am doing schematics just for fun, I do whatever I find makes a
schematic easy to read. That does mean adhering to the signal flow from
left to right and top to bottom. But with digital circuits I have long ago
come to the conclusion that little blips of vdd or gnd or little arrows
with signal names in lieu of wires often greatly increases readability of
a schematic. I absolutely dislike many (often Japanese) schematics that
are just a mess of lines all over the place. I find it easier to hunt for
a signal name on the same sheet than following a bus of 25 parallel
lines...

Adi

--
http://www.piclist.com#nomail Going offline? Don't AutoReply us!
email spamBeGonelistservSTOPspamspamEraseMEmitvma.mit.edu with SET PICList DIGEST in the body

2003\02\19@163501 by Wagner Lipnharski

flavicon
face
Adi Linden wrote:
>> Yep, volts from top to bottom, pref drawn as rails,
>> and signal flow from left to right. No spastic sideways
>> Amercian transistors (grin) or little isolated blips
>> marked as Vdd or Gnd all over the place.
>
> Now that I am doing schematics just for fun, I do whatever I find
> makes a schematic easy to read. That does mean adhering to the signal
> flow from left to right and top to bottom. But with digital circuits
> I have long ago come to the conclusion that little blips of vdd or
> gnd or little arrows with signal names in lieu of wires often greatly
> increases readability of a schematic. I absolutely dislike many
> (often Japanese) schematics that are just a mess of lines all over
> the place. I find it easier to hunt for a signal name on the same
> sheet than following a bus of 25 parallel lines...
>
> Adi


As funny as you can think, today I was talking to some people today about
it.

According to my findings, most people who used to draw their own circuit
boards, lay down layouts and tracks by hand (well, using some software
aid), they use to like to see the entire schematics on the paper, all
likes, all connections, including all the wires to ground and VCC.  For
those, the circuit board visual looks like the schematic, and when they see
one, they also see another. You practically can locate any schematic
component in the board in a questions of less than 3 seconds.

For the "other" people, who build the schematic and just pour components
over the board and use auto-router heavily for the dirty job, the
schematics are not so much important, neither much the circuit board.
Those guys told me that the most important thing is the product ready and
working.  It was presented to me a circuit board for a X-Ray type machine,
motors systems controller, man, perhaps it is me, but I didn't like it.
Heavy and large heatsinks in middle of the board (it tends to be difficult
to repair and install), little and fragile components close to assembly
bolts (easy to damage during installation), not even considering the odd
way the assembly holes were positioned (for no apparent reason), low power
cables directly soldered to the board (tsk, tsk) what connectors were made
for?

Different points of view, different worries and results, still open
positions all over the world for both of this people.  I don't know, I feel
as if technology (mostly software) is surpassing technique, when technique
is what should be holding technology on the rails...

"Don't try to find an application that will use the new tool you just found
over the bench, try yes to find the right tool for the application in
hand".

Some people think that just because now exist software that "HELPS" to draw
a schematic and produce a circuit board, now everyone could be a
specialized engineer in the area.  20 years ago, before this kind of
software applications appeared in the market, it was difficult to find a
good circuit board layout professional.  Today, it is even harder.

A good doctor doesn't need a catscan to realize that you have a "cold", he
can find it out in 3 seconds just by watching your red eyes, sneezing and
running nose.  This is the marriage between knowledge and "art".

Wagner.

--
http://www.piclist.com#nomail Going offline? Don't AutoReply us!
email KILLspamlistservspamBeGonespammitvma.mit.edu with SET PICList DIGEST in the body

2003\02\20@122704 by Dwayne Reid

flavicon
face
At 10:50 AM 2/19/03 -0600, Adi Linden wrote:

>But with digital circuits I have long ago
>come to the conclusion that little blips of vdd or gnd or little arrows
>with signal names in lieu of wires often greatly increases readability of
>a schematic. I absolutely dislike many (often Japanese) schematics that
>are just a mess of lines all over the place. I find it easier to hunt for
>a signal name on the same sheet than following a bus of 25 parallel
>lines...

Just wait til the day that you spend hours trying to figure out how
something is supposed to work, then find (hours or days later) one of those
little arrows with a signal name on it that you overlooked.  Been there,
done that.

Arrows (or circles) and ground symbols for the various supplies are an easy
way to make a dense schematic more readable.  But you have to be careful
when trying to represent nets with arrows and net names instead of lines.

dwayne

--
Dwayne Reid   <EraseMEdwaynerspamEraseMEplanet.eon.net>
Trinity Electronics Systems Ltd    Edmonton, AB, CANADA
(780) 489-3199 voice          (780) 487-6397 fax

Celebrating 19 years of Engineering Innovation (1984 - 2003)
 .-.   .-.   .-.   .-.   .-.   .-.   .-.   .-.   .-.   .-
    `-'   `-'   `-'   `-'   `-'   `-'   `-'   `-'   `-'
Do NOT send unsolicited commercial email to this email address.
This message neither grants consent to receive unsolicited
commercial email nor is intended to solicit commercial email.

--
http://www.piclist.com hint: To leave the PICList
@spam@piclist-unsubscribe-request@spam@spamspam_OUTmitvma.mit.edu>

2003\02\20@180323 by William Chops Westfield

face picon face
We have schematics I've seen here that are little more than chips with
each pin going off to an arrow/labeled signal...  Annoying.

BillW

--
http://www.piclist.com hint: To leave the PICList
spamBeGonepiclist-unsubscribe-requestspamKILLspammitvma.mit.edu>

More... (looser matching)
- Last day of these posts
- In 2003 , 2004 only
- Today
- New search...