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

Exact match. Not showing close matches.
PICList Thread
'[EE]: PCB making once again. Eagle Specific.'
2003\04\25@152406 by Byron A Jeff

face picon face
I realize that this is a Pandora's box topic. But I've finally reached the
realization that I'm going to have to come up with something sturdier than
wire wrap. One of my permanent projects (a wall mounted thermostat)
is falling apart after a couple of years of use. So I'm I wandering into the
realm of PCB making and I'm soliciting advise.

Of course The PicList has several extended threads on the subject.
And yes I've
read them all.

Now not to come in empty handed I come with a few of the resources I've been
doing research from/with. Then the questions.

RESOURCES
---------
One of the best groups I've seen on the subject is the Yahoo group Homebrew
PCBs: http://groups.yahoo.com/group/Homebrew_PCBs
They talk about every method under the sun and have a vast amount of resources.

One of the best overall "how to do it" posts can be found here:

http://groups.yahoo.com/group/Homebrew_PCBs/message/839

Eagle (http://www.cadsoft.de) does represent an opportunity for schematic and
board layout of small boards. However both the free and hobbyist versions of
the products are quite limited. The cost for reasonable sized (4" x 6") boards
is $125! (And only for strictly non commercial use) Ouch!!!
I've been playing with it and will probably use it for my first couple of
tests. Questions are Eagle related.


Some interesting suppliers:

  Circuit Specialists: http://www.web-tronics.com
     Really cheap presensistized copper boards

  Dyna-Art: http://www.dynaart.com
     Silver plating among other items.

  Austin Electronics: http://www.austinelex.com/ae_118.htm
     PCB PhotoFab kit

After slogging through all the posts and all the different techniques I
finally concluded that presensitied positive photoresist boards etched in
plain old Ferric Cloride optimizes the costs and process repeatability.
This is especially true because I only have inkjet printers at home, so
printing to transparancy then exposing, developing, and etching is very
cost effective.

QUESTIONS
---------------------------------------------------

Now on to the questions.

1)
  I'm looking for one small eagle tip. How in the heck do you create a power
  bus? I've used a few of the numerous tutorials
  out there to layout my first board (a 16F628, 3 resistors, and an
  LED). But I'm clueless as to how to create a physical representation
  of the power supply buses. Just draw a thick line?

2) More Eagle. Is there any way to force the autorouter to generate a single
  sided board only? Even after forcing the cost of the top side to 99,
  sometimes it will still generate a top side trace or two.

3) Any standards as to line thickness and pad size for novice boardmakers.

4) Final Eagle. Has anyone tried any tricks for creating larger boards by
  segmenting and cut/pasting the smaller boards into a larger board?

5) Specifically for Olin. Your PIC library is great. Would you object if I
  posted a copy of it (with proper attribution of course) on my PIC page?

Thanks,

BAJ

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

2003\04\25@153452 by Jai Dhar

flavicon
face
>
> 3) Any standards as to line thickness and pad size for novice boardmakers.
>

What type of transfer method will you be using? UV, etch-resistant marker? Just
out of personal experience, I have been using 15 mil tracks with 13 mil spacing
no problem using UV transfer. Haven't tried going down to 12 mil, but I don't
see any problem....

----------------------------------------
This mail sent through http://www.mywaterloo.ca

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

2003\04\25@153957 by Mike Hord

picon face
Take a look at LabCenter's ARES Lite program.  At ~$30 US (site is British
and I'm not sure what the exact L->$ conversion rate is now), it is a
surprisingly tidy little program.  They also offer a program which allows
for simulation of the PIC16Fxxx series (only up to 1k programs) with some
very nice plug-in modules (Virtual Scope, Logic Analyzer, keypad, LCD, etc).
 I have used it quite a bit and always been happy with the results.  You
can silk screen, make quite sizable boards, and yes, turn off auto-routing
on one layer.

Worth a look...I don't know why I never hear about it.

Mike Hord

_________________________________________________________________
Tired of spam? Get advanced junk mail protection with MSN 8.
http://join.msn.com/?page=features/junkmail

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

2003\04\25@154225 by Ned Konz

flavicon
face
On Friday 25 April 2003 12:23 pm, Byron A Jeff wrote:

>
> 1)
>    I'm looking for one small eagle tip. How in the heck do you
> create a power bus? I've used a few of the numerous tutorials
>    out there to layout my first board (a 16F628, 3 resistors, and
> an LED). But I'm clueless as to how to create a physical
> representation of the power supply buses. Just draw a thick line?

Change the net class if you want so when you route it it'll make a
thicker wire. Don't draw lines, instead route segments from airwires.

> 2) More Eagle. Is there any way to force the autorouter to generate
> a single sided board only? Even after forcing the cost of the top
> side to 99, sometimes it will still generate a top side trace or
> two.

Yes, there's some sample design rules, and one is for a single-sided
board with jumpers.

> 3) Any standards as to line thickness and pad size for novice
> boardmakers.

As big as possible. If you're doing photoboards, 12 mils should be OK
for traces, though if you could go to 16 mils it would be easier.


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

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

2003\04\25@154827 by Dave King

flavicon
face
>1)
>    I'm looking for one small eagle tip. How in the heck do you create a power
>    bus? I've used a few of the numerous tutorials
>    out there to layout my first board (a 16F628, 3 resistors, and an
>    LED). But I'm clueless as to how to create a physical representation
>    of the power supply buses. Just draw a thick line?

You did RTFM the manual ?? ;-]]]  Actually I never could get that to
behave as I expected it. As long as your power connections have the same
name they are treated as a bus. Use the top eyeball icon to click on and
see what the names are it also highlights the line so you can see if its not
all named the same. If its not use the Name icon under the X (delete) click
on the line and simply type the same name in. Then check to see if it picks
it up properly. I found I had about 5 little sections initially on my power bus
all with different names.  When you route you just need to change the width.

>2) More Eagle. Is there any way to force the autorouter to generate a single
>    sided board only? Even after forcing the cost of the top side to 99,
>    sometimes it will still generate a top side trace or two.

Tools-Auto- set layer 1 to N/A

>3) Any standards as to line thickness and pad size for novice boardmakers.

There are a few charts on-line that show traces widths to use for the current
through a trace on a FR4/1oz board.

>4) Final Eagle. Has anyone tried any tricks for creating larger boards by
>    segmenting and cut/pasting the smaller boards into a larger board?

The free proggy is limited to size so if you go over it won't let you route
or place
parts outside the limit.


Dave

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

2003\04\25@154833 by Ben Jackson

flavicon
face
On Fri, Apr 25, 2003 at 03:23:51PM -0400, Byron A Jeff wrote:
> 2) More Eagle. Is there any way to force the autorouter to generate a single
>    sided board only? Even after forcing the cost of the top side to 99,
>    sometimes it will still generate a top side trace or two.

Why not just live with it and put a few jumper wires there?  Graph theory
can tell you whether what you want is even possible (all traces on a single
side) for a given component layout, but it's probably easier to just put in
a few jumpers.

> 5) Specifically for Olin. Your PIC library is great. Would you object if I
>    posted a copy of it (with proper attribution of course) on my PIC page?

There's an Eagle PIC library?  I'd really like to see that.

--
Ben Jackson
<benspamspam_OUTben.com>
http://www.ben.com/

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

2003\04\25@155241 by Picdude

flavicon
face
On Friday 25 April 2003 14:23, Byron A Jeff wrote:
> I realize that this is a Pandora's box topic. But I've finally reached the
> realization that I'm going to have to come up with something sturdier than
> wire wrap.
There's a term I haven't heard in a long time.  :-)


{Quote hidden}

In the autorouting options, select "N/A" for preferred direction for the top layer.


> 3) Any standards as to line thickness and pad size for novice boardmakers.

Check expresspcb.com  -- this have a tips section that gives ballpark trace widths based on current carrying capacity.
For outsourced boards, I choose pad ODs by selecting the ID based on the component-lead diameter, then let it auto-select the OD.  If space permits, I'll manually raise that a bit.  For boards I do myself, I raise that quite a bit in case my holes are drilled perfectly center, and since drilling my eat up a small pad.


>
> 4) Final Eagle. Has anyone tried any tricks for creating larger boards by
>    segmenting and cut/pasting the smaller boards into a larger board?

Once.  Added a 2 header components to a board (single row each) and used it almost like a connector from one half of the circuit to the other half in the schematic view.  Laid out one half with the header on the extreme RHS, and the other half on its own with the header on the extreme left.  Manually adjusted the traces so that the corresponding lines were on the same layer and aligned with each other properly, then deleted the headers.  Then merged the transparencies together.  Busy work, but did the trick.  I use Eagle enough to cough up the bucks now I think.  :-(


>
> 5) Specifically for Olin. Your PIC library is great. Would you object if I
>    posted a copy of it (with proper attribution of course) on my PIC page?
>
> Thanks,
>
> BAJ

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

2003\04\25@155903 by Byron A Jeff

face picon face
On Fri, Apr 25, 2003 at 03:34:18PM -0400, Jai Dhar wrote:
> >
> > 3) Any standards as to line thickness and pad size for novice boardmakers.
> >
>
> What type of transfer method will you be using? UV,
> etch-resistant marker?

UV. No doubt about that.

> Just
> out of personal experience, I have been using 15 mil tracks with 13 mil
> spacing
> no problem using UV transfer. Haven't tried going down to 12 mil, but I don't
> see any problem....

Good to know.

BAJ

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

2003\04\25@161224 by Olin Lathrop

face picon face
>> 2) More Eagle. Is there any way to force the autorouter to generate a
>>    single sided board only? Even after forcing the cost of the top
>>    side to 99, sometimes it will still generate a top side trace or
>> two.
>
> Tools-Auto- set layer 1 to N/A

That disables the bottom layer.  He probably want layer 16 set to N/A.


*****************************************************************
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 spamBeGonelistservspamBeGonespammitvma.mit.edu with SET PICList DIGEST in the body

2003\04\25@161625 by Byron A Jeff

face picon face
On Fri, Apr 25, 2003 at 12:40:31PM -0700, Ned Konz wrote:
> On Friday 25 April 2003 12:23 pm, Byron A Jeff wrote:
>
> >
> > 1)
> >    I'm looking for one small eagle tip. How in the heck do you
> > create a power bus? I've used a few of the numerous tutorials
> >    out there to layout my first board (a 16F628, 3 resistors, and
> > an LED). But I'm clueless as to how to create a physical
> > representation of the power supply buses. Just draw a thick line?
>
> Change the net class if you want so when you route it it'll make a
> thicker wire. Don't draw lines, instead route segments from airwires.

Ned, unfortunately I'm a real novice here. Please forgive me for being dense.
I understand what you're saying above and will test that. However I'm asking
a more fundamental question. I figured out how to create a power net. I see
that it's possible to change that net class. What I can't figure out is how
to create a physical point on the board to attach the power wire. See what I
mistakenly thought was that putting a Vcc/Vdd/+5V and Vss/GND/0V power element
on the schematic would create an actual attachment element on the board.

So I guess I need to go look for a banana jack donut or somesuch to attach
to the power nets.

>
> > 2) More Eagle. Is there any way to force the autorouter to generate
> > a single sided board only? Even after forcing the cost of the top
> > side to 99, sometimes it will still generate a top side trace or
> > two.
>
> Yes, there's some sample design rules, and one is for a single-sided
> board with jumpers.

Actually I got that there is a N/A option for the top layer when you
autoroute from another post. Thanks.

>
> > 3) Any standards as to line thickness and pad size for novice
> > boardmakers.
>
> As big as possible. If you're doing photoboards, 12 mils should be OK
> for traces, though if you could go to 16 mils it would be easier.

Will check.

Thanks for the quick response.

BAJ

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

2003\04\25@162108 by Byron A Jeff

face picon face
On Fri, Apr 25, 2003 at 12:48:06PM -0700, Ben Jackson wrote:

Olin. I have a question for you. Read to the bottom.

> On Fri, Apr 25, 2003 at 03:23:51PM -0400, Byron A Jeff wrote:
> > 2) More Eagle. Is there any way to force the autorouter to generate a single
> >    sided board only? Even after forcing the cost of the top side to 99,
> >    sometimes it will still generate a top side trace or two.
>
> Why not just live with it and put a few jumper wires there?  Graph theory
> can tell you whether what you want is even possible (all traces on a single
> side) for a given component layout, but it's probably easier to just put in
> a few jumpers.

Because jumpers aren't the issue. Trying to fabricate a double sided board is.
The task is going to be complicated enough without having to try to get two
perfectly lined up sizes. Once I get comfortable with the PCB making process
then I'll try to tackle double sided boards.

>
> > 5) Specifically for Olin. Your PIC library is great. Would you object if I
> >    posted a copy of it (with proper attribution of course) on my PIC page?
>
> There's an Eagle PIC library?  I'd really like to see that.

Let me see if I can find that message in the archive:

It takes a bit of effort to get to though. That's why I asked Olin if I can
house a copy. But I don't think he got to the bottom of my original message.

Olin, can I put a copy of your PIC library, with proper attribution, on my
PIC page?

BAJ

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

2003\04\25@162931 by Ned Konz

flavicon
face
On Friday 25 April 2003 01:14 pm, Byron A Jeff wrote:
{Quote hidden}

No, all it does is make a net.

If you need somewhere to attach a wire, you'll have to put in a
testpoint or pad or SMD or something.

Look at the "wirepad" library, for instance.

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

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

2003\04\25@163140 by Picdude

flavicon
face
On Friday 25 April 2003 15:14, Byron A Jeff wrote:
> Ned, unfortunately I'm a real novice here. Please forgive me for being
> dense. I understand what you're saying above and will test that. However
> I'm asking a more fundamental question. I figured out how to create a power
> net. I see that it's possible to change that net class. What I can't figure
> out is how to create a physical point on the board to attach the power
> wire. See what I mistakenly thought was that putting a Vcc/Vdd/+5V and
> Vss/GND/0V power element on the schematic would create an actual attachment
> element on the board.
>
> So I guess I need to go look for a banana jack donut or somesuch to attach
> to the power nets.
>


I usually use a component called "PAD" or more specifically, LSP10, LSP11, LSP13, etc.  It's just a pad with a wire to your circuit, but with varying sizes.

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

2003\04\25@164019 by Olin Lathrop

face picon face
> Because jumpers aren't the issue. Trying to fabricate a double sided
> board is.

So don't fab the top layer.

> Let me see if I can find that message in the archive:
>
> It takes a bit of effort to get to though. That's why I asked Olin if I
> can house a copy. But I don't think he got to the bottom of my original
> message.
>
> Olin, can I put a copy of your PIC library, with proper attribution, on
> my
> PIC page?

I did respond to your other message.  I didn't see it either, so MSOE
probably stripped off the [EE] and I didn't notice.  It's probably in the
archives under OT or untagged, or whatever.

Anyway, yes you can post my Eagle PIC library, but I'd like a reference to
http://www.embedinc.com/pic associated with it.  I attached the latest
version to the other message.  Let me know if you can't retrieve it from
the archives.


*****************************************************************
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 RemoveMElistservEraseMEspamEraseMEmitvma.mit.edu with SET PICList DIGEST in the body

2003\04\25@164755 by Picdude

flavicon
face
On Friday 25 April 2003 15:20, Byron A Jeff wrote:
> Because jumpers aren't the issue. Trying to fabricate a double sided board
> is. The task is going to be complicated enough without having to try to get
> two perfectly lined up sizes. Once I get comfortable with the PCB making
> process then I'll try to tackle double sided boards.

Sure, if you can make a board single-sided, go ahead.  But I've found it almost impossible to layout any circuit I do with just one layer.  But I say go ahead and experiment with making a few double-sided via connections on the board.  You can route with top layer set to N/A as far as it will go, then either manually route the vias on the top layer, or turn the top layer back on and let it continue.  However, use really large vias just in case.  Feel free to use a 1/4" via if you feel comfortable, and just drill a .025 or whatever hole to fit the connection wire.

Of all the ways I've tried to line up both sides, the best and most reliable I've found is to add a few holes (approx 1/8") at the corners of the board, make 3 transparencies (I actually use clear inkjet window decals since they're self-stick) -- one for the top, and 2 for the bottom.  Put the bottom one in place first and drill those corner holes.  Discard that transparency.  Now use the other two and align with the holes you drilled.  You can look up at it thru a line and you'll see the hole-center marks over each other.  Adjust until they're perfectly aligned.  Then expose the board, etch, etc and then drill the component holes.  I've tried the fold-into-an envelope method of aligning the layers, also tried making a pocket out of an L-shaped piece of scrap PCB with the transparencies pre-stuck and pre-aligned on, but none gave me as easy and repeatable results as the drill-the-corner-holes method.

Cheers,
-Neil.

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

2003\04\25@172455 by William Chops Westfield

face picon face
   1) I'm looking for one small eagle tip. How in the heck do you create
   a power bus? I've used a few of the numerous tutorials out there to
   layout my first board (a 16F628, 3 resistors, and an LED). But I'm
   clueless as to how to create a physical representation of the power
   supply buses. Just draw a thick line?

In the schematic editor or the PCB editor?  In schematics, power traces are
generally hidden as not being very interesting.  On the PCB, you just use
"route" with a thick trace width.  I usually find it useful to manually
route the power bus (with thick traces) even if I expect to autoroute the
rest of the traces.  You can also use the "class" feature to assign a
different track width to different signals, in which case the autorouter
will use the larger width automatically.  It won't make a nice neat grid,
though, and it routes the wider traces first.


   2) More Eagle. Is there any way to force the autorouter to generate a
   single sided board only? Even after forcing the cost of the top side to
   99, sometimes it will still generate a top side trace or two.

You can set the top layer in the autoroute menu to "N/A", in which case it
won't be used at all.  There is also a set of autorouter design rules in:
   ftp://ftp.cadsoft.de/pub/userfiles/misc/1layer.ctl
that attempts to do a bit better by trating the top layer like jumpers.


   3) Any standards as to line thickness and pad size for novice boardmakers.

I use a mininum track width of .6mm, and increase the pad size using
a "restring" parameter of 40% (default is 25%)  Usually, I go through
after everything has routed and increase track widths or draw polygons
so that there is as much copper left behind as possible.  (But part of
that is because I'm using an LPKF router that is going to leave copper
behind anyway.)  I'm envisioning a ULP that does this automatically,
but i'm not sure it's QUITE possible.


   4) Final Eagle. Has anyone tried any tricks for creating larger boards
   by segmenting and cut/pasting the smaller boards into a larger board?

I discovered that the restriction is on PART placement, and I have at least
one board designed (with the freeware version) where I managed to squeeze
all the PARTS into the allowed area, but the TRACES go a bit outside. :-)
Of course, you can make stackable boards with actual connectors and such.

You can fit an awful lot of silicon on the freeware area, but larger
components (relays, etc) can be a bit of  pain...

You ARE aware of the "new" "hobbyist license", right?  Four layers, all
three "components", 160x100mm (6.5 x 4.08 inches), non-profit use only
for only $125.  (OK, you already commented that $125 was too much.  But
comparitively speaking, that's VERY reasonable.)  So that makes three
levels of license aimed at small users:
       Freeware:   $000.00  two-layers, 80x100mm, non-profit use only
       Light:      $ 49.00  two-layers, 80x100mm, commercial use OK.
       Non-profit: $125.00  four layers, 100x160mm, non-profit use only.

You could also generate a bunch of scaled libraries (1/5 size?) and scale
them up during printing, if you're really desparate.

Cadsoft's Eagle newsgroups are a good resource.  I hope they continue to
offer the freeware and low cost versios - you can just WATCH them get
deluged with "stupid questions" (ie ones that are already answered several
times in the archives) from people who are clear that they probably won't
every be buying a copy.  (OTOH, the "user community" is helpful as well.)

BillW

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

2003\04\25@173749 by William Chops Westfield

face picon face
   > Change the net class if you want so when you route it it'll make a
   > thicker wire. Don't draw lines, instead route segments from airwires.

   Ned, unfortunately I'm a real novice here. Please forgive me for being
   dense.  I understand what you're saying above and will test
   that. However I'm asking a more fundamental question. I figured out
   how to create a power net. I see that it's possible to change that net
   class. What I can't figure out is how to create a physical point on
   the board to attach the power wire. See what I mistakenly thought was
   that putting a Vcc/Vdd/+5V and Vss/GND/0V power element on the
   schematic would create an actual attachment element on the board.

Ahh.  One of my most frequently used personally-defined library elements is
something I call "wire", which is one pin and one pad.  It gets used for
all sorts of offboard connection including switches and testpoints, but the
most common is one "wire" for VCC, and one for GND.  You can use existing
two-pin connectors as well, but it's hard to find one you like the looks
up, and you lose some routing flexibility.

I also got tired of dealing with umpty-hundred different transistors and
create NPN-generic and PNP-generic parts, each available in assorted common
packages and pinouts.  The "generic" name can easilly be overridden in the
editors to specify a particular part.

BillW

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

2003\04\25@180245 by Dave King

flavicon
face
>
>Cadsoft's Eagle newsgroups are a good resource.  I hope they continue to
>offer the freeware and low cost versios - you can just WATCH them get
>deluged with "stupid questions" (ie ones that are already answered several
>times in the archives) from people who are clear that they probably won't
>every be buying a copy.  (OTOH, the "user community" is helpful as well.)
>
>BillW

You mean the real GOOD questions like the one guy who was asking how
come his cracked copy wouldn't load the files and if anyone had a better crack
for it?

That reminds me one of these days I need to call tech support and ask how to
keep the coffee cup holder from retracting....


Dave

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

2003\04\25@200832 by William Chops Westfield

face picon face
   > you can just WATCH them get deluged with "stupid questions"

   You mean the real GOOD questions like the one guy who was asking
   how come his cracked copy wouldn't load the files and if anyone
   had a better crack for it?

Wow.  I didn't see THAT one.  But no, actually.  There will always be
complete jerks, and some of them will have paid the full price and think
that intitles them to be jerks.

The two questions that come to mind were "how do I route a single sided
board?" and "how do I move my components to the other side of the board."

It's not quite a case of failure to RTFM; the freeware doesn't come with
a manual, just a tutorial and online help.  They're OK, but not great.

BillW

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

2003\04\25@214123 by Dave King

flavicon
face
At 05:07 PM 25/04/03, you wrote:
>     > you can just WATCH them get deluged with "stupid questions"
>
>     You mean the real GOOD questions like the one guy who was asking
>     how come his cracked copy wouldn't load the files and if anyone
>     had a better crack for it?
>
>Wow.  I didn't see THAT one.  But no, actually.  There will always be
>complete jerks, and some of them will have paid the full price and think
>that intitles them to be jerks.

Yah that ones worth printing and framing ;-]

>The two questions that come to mind were "how do I route a single sided
>board?" and "how do I move my components to the other side of the board."
>
>It's not quite a case of failure to RTFM; the freeware doesn't come with
>a manual, just a tutorial and online help.  They're OK, but not great.
>
>BillW

If you rummage around the site there is a PDF version of the manual
available for download.

Dave

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

2003\04\26@092126 by erholm (QAC)

flavicon
face
You mean something else than the "Tutorial" (aprox 390kb) ?
You don't happen to have a link ?

B.t.w, I think this "http://www.hobby-elec.org/e_eagle.htm"
is a usable introduction-guide to Eagle. It did solve some
initial problems for me at least...

Jan-Erik Soderholm.


Dave King wrote (about a manual to Eagle) :

> If you rummage around the site there is a PDF version of the manual
> available for download.

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

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