Homebrew PCBs

I'm re-doing some components I previously created (in Eagle, but this
probably applies to other CAD pacakages as well).  The actual
components, MiniCircuits SBL-1 RF passive mixers require several
signal to be connectected externally.  This is an 8 pin through hole
device.

Two of the pins are for discrete signals.  Two other pins are for one
signal, and four pins are ground.  In Eagle, I've designated the
ground pins as SUP (supply) and the other four as I/O.  I would think
there should be a way to tie the two I/O pins together in the symbol
that are supposed to be connected together extenally, but I haven't
run across any symbols that tie pins together.  I have them tied
pictorally in the Symbol drawing.  Also, I'm not sure if pads can be
tied together in the Eagle Package for the device.  I can lay
additional pads down that overlay and graphically link the ones
defined for the pins, but they aren't logically connected when the
Device is defined; they are just sort of lying there.

Without tying the pins and pads together in the Symbol/Package/Device
definition, I have to remember that the two signal pins have to be
tied to the same external signal, and the four ground pins have to be
tied to ground, and not leave one or more unconnected.  It's not a
real big deal, just a convenience.

There is a note in the Eagle Help topic on pins that states if any pin
are defined on the Symbol as SUP (implying GND signal)that these will
be automatically connected to GND as a net if a Supply symbol is used
on the schematic; for example +12V, I presume. That's something else
that's news to me.  I've used Supply many times, and I've yet to see
any component automatically tie to GND.

Any ideas?

Ted

----- Original Message ----- 

From: "kilocycles" <kilocycles@...>
To: <Homebrew_PCBs@yahoogroups.com>
Sent: Saturday, March 18, 2006 4:00 PM
Subject: [Homebrew_PCBs] Pins and Pads for external connections


> I'm re-doing some components I previously created (in Eagle, but this
> probably applies to other CAD pacakages as well).  The actual
> components, MiniCircuits SBL-1 RF passive mixers require several
> signal to be connectected externally.  This is an 8 pin through hole
> device.
>
> Two of the pins are for discrete signals.  Two other pins are for one
> signal, and four pins are ground.  In Eagle, I've designated the
> ground pins as SUP (supply) and the other four as I/O.  I would think
> there should be a way to tie the two I/O pins together in the symbol
> that are supposed to be connected together extenally, but I haven't
> run across any symbols that tie pins together.  I have them tied
> pictorally in the Symbol drawing.  Also, I'm not sure if pads can be
> tied together in the Eagle Package for the device.  I can lay
> additional pads down that overlay and graphically link the ones
> defined for the pins, but they aren't logically connected when the
> Device is defined; they are just sort of lying there.
>
> Without tying the pins and pads together in the Symbol/Package/Device
> definition, I have to remember that the two signal pins have to be
> tied to the same external signal, and the four ground pins have to be
> tied to ground, and not leave one or more unconnected.  It's not a
> real big deal, just a convenience.
>
> There is a note in the Eagle Help topic on pins that states if any pin
> are defined on the Symbol as SUP (implying GND signal)that these will
> be automatically connected to GND as a net if a Supply symbol is used
> on the schematic; for example +12V, I presume. That's something else
> that's news to me.  I've used Supply many times, and I've yet to see
> any component automatically tie to GND.
>
> Any ideas?

In Pulsonix I can connect pins like that in the Footprint editor using a 
dummy net name, so I just have a four-pin schematic symbol - RF, IF, LO and 
GND. Perhaps you can do something like that in Eagle. Otherwise, you could 
just use additional pins on the symbol and connect them on the schematic.

Leon

Hi Ted,

I saw parts with hidden supply pins get connected, but trouble is, there 
are many ways to call pins, VDD, VCC,  GND, VSS.  And Eagle doesn't seem 
to have a way to "alias" them together when they should be.

Did you notice the GND@1 and GND@2 convention?  you might try the @ 
convention to tie your pins together.

Time for my question,  I  just finished routing my board (by hand!), and 
I see that I  have vias that somehow have the wrong hole size?  They 
show up on the design rules check.  I have 12 mil signals and 24 mil 
power traces.  They need changed, but what's the spec?

Alan  KM6VV


kilocycles wrote:

> I'm re-doing some components I previously created (in Eagle, but this
> probably applies to other CAD pacakages as well).  The actual
> components, MiniCircuits SBL-1 RF passive mixers require several
> signal to be connectected externally.  This is an 8 pin through hole
> device.
> 
> Two of the pins are for discrete signals.  Two other pins are for one
> signal, and four pins are ground.  In Eagle, I've designated the
> ground pins as SUP (supply) and the other four as I/O.  I would think
> there should be a way to tie the two I/O pins together in the symbol
> that are supposed to be connected together extenally, but I haven't
> run across any symbols that tie pins together.  I have them tied
> pictorally in the Symbol drawing.  Also, I'm not sure if pads can be
> tied together in the Eagle Package for the device.  I can lay
> additional pads down that overlay and graphically link the ones
> defined for the pins, but they aren't logically connected when the
> Device is defined; they are just sort of lying there.
> 
> Without tying the pins and pads together in the Symbol/Package/Device
> definition, I have to remember that the two signal pins have to be
> tied to the same external signal, and the four ground pins have to be
> tied to ground, and not leave one or more unconnected.  It's not a
> real big deal, just a convenience.
> 
> There is a note in the Eagle Help topic on pins that states if any pin
> are defined on the Symbol as SUP (implying GND signal)that these will
> be automatically connected to GND as a net if a Supply symbol is used
> on the schematic; for example +12V, I presume. That's something else
> that's news to me.  I've used Supply many times, and I've yet to see
> any component automatically tie to GND.
> 
> Any ideas?
> 
> Ted
>

On Sat, 18 Mar 2006 19:41:25 +0100, Alan Marconett <KM6VV@...> wrote:

> Hi Ted,
>
>
> I saw parts with hidden supply pins get connected, but trouble is, there
>
> are many ways to call pins, VDD, VCC,  GND, VSS.  And Eagle doesn't seem
>
> to have a way to "alias" them together when they should be.
>
>
> Did you notice the GND@1 and GND@2 convention?  you might try the @
>
> convention to tie your pins together.
>

Hidden pins can be very annoying, i know the problem from orcad times. You  
can use a "supply block" for components that use hidden supply (imagine a  
quad opamp, i will havbe 4 opamp symbols inside and a supply block  
symbol). The supply blocks can be put together in one area of the  
schematic and connected in parallel to the supply and capacitors as  
required. This is not so clean looking as totally hidden supply, but IMO  
in a schematic that is used to create a PCB and does _not_ show each and  
every pin is worthless. Leaving out pins may be nice for some earlier  
design stage, but the PCB really needs a full schematic. I would expect  
eagle will allow to use supply blocks (every software that allows multiple  
symbols inside one component can do that, eagle is one of them i think).

If you use reference symbols instead of wires having all supply pins on  
the component symbol does not add much "clutter", and i actually prefer  
that over supply blocks. When i read the schematic thinking "which pin was  
supply again" i don't need to look at the component, see that it is say  
IC4, search IC4 amongst the supply blocks, and read the numbers, it will  
all be there in one place like a real-life component.


>
> Time for my question,  I  just finished routing my board (by hand!), and
>
> I see that I  have vias that somehow have the wrong hole size?  They
>
> show up on the design rules check.  I have 12 mil signals and 24 mil
>
> power traces.  They need changed, but what's the spec?
>

Depends on the drill sizes you can have. People seem to prefer several  
vias over one larger one for high current traces.

ST

Alan,
I just tried the new part in place of the old one.  Originally, when I
designed the symbol for it (it's an SBL-1 mixer), I just used the
standard "wagon wheel" for the symbol for it, the TUF-1, ADE-1 and a
homebrew version of the SBL-1.  Then, I realized when doing the first
board, I had no convenient way to connect the external grounds and the
two IF pins together (doh!).  I was trying to force wiring on the
board view, and I didn't care for that much.

I redesigned a rectangular symbol with 4 pins on each side, and drew
the wagon wheel mixer symbol inside it at .0125" grid resolution, and
added the text to it.  Then I switched back to .1" resolution to make
sure the pins would connect on the schematic.  I renamed the pins fro
P$1 etc. to (in order, as the are one the actual device) RF, GND@1,
IF@1, IF@2, GND@2, GND@3, GND@4 and LO for pin #8.  By the way, as
expected, the "@1" doesn't show up on the symbol.  I set the pin to
display the nam on the symbol only, and it just shows RF GND IF IF 
and then GND GND GND LO coming back up the other side.

I just added them to the schematic of the product detector/audio
schematic I'm working on, and it looks good on the schematic and
board.  I disconnected the grounds temporarily to test that "auto net"
thing with a supply.  I added a +12V supply and connected it to a
transistor, and it didn't connect any of the grounds.  Then, I
arbitrarily connected the +12V to the LO pin, and again, no
auto-ground connection.  Maybe it will only do that if you have a part
with a voltage supply defining one of the pins, like maybe on a 7812
regulator, or something.  The regulators that are in the libraries
don't do that, however.

I'm the wrong person to ask about vias.  I just made my first ones, on
a board with some MMIC amplifier devices on the top ground plane side,
along with the PA transistor at the other end of the board.  I *think*
I'm doing it right; it added a via pad to the board, and I'll connect
it through with a piece of wire.  Click on DRC, and then read the
information regarding minimum drill for the Sizes and Restring tabs. 
I don't completely understand it (it's Eagle!), but the Japanese
tutorial suggested setting Restring at 40%.  I've had many situations
where I had DRC errors for drill size, but I just ignore them, since I
don't send the boards out for fabrication.  I don't even print the
boards from the program, which could show the drill holes. I export
them to .bmp files and edit them in Photoshop, adding text, making
pilot holes, and use the "Threshold" control of Photoshop to ge a pure
black and white image for printing.  It adds a considerable amount of
time to do it that way, but that's the way I've always done it.  Until
I figured out the "polygon gnd" thing, I even added fills using
Photoshop.  

As to the specs, well, I pretty much ignore those as well.  After I've
finished routing, I usually go back with the "Wrench" tool and
redefine the traces to a wider trace, typically .032", as long as it
still passes DRC.  I have seen specs for digital and mixed analog
layouts on some sites, along with specs for signals crossing under
other signals.  Obviously, signal trace widths and layer crossings are
extremely critical at VHF and UHF, where the foil traces are inductors
and capacitors.  I haven't seen any guidelines for HF, but I try to
use common sense.  I tie the top ground plane to the bottom foil layer
in several places, and I'm careful not to put a large trace across a
critical section where capacitance through the 1/16" thickness of a
board would be a problem.  For example, for those GHz-capable MMIC
amplifiers mounted on the top layer, I left the foil side of the board
blank underneath them and their circuitry to hopefully preclude VHF
oscillations.

When I get the other mixer device symbols corrected, I can send you a
copy of the small custom library they're in, if you want it.  I also
have some toroids in there (bifilar and trifilar FT37-43, etc., and
the Mouser 42IF123 IF can transformer that is used in several QRP rig
designs.  Also a board-mounted RCA jack that I found at a local
surplus house, to use for board-to-board connections with coax.

Ted 

--- In Homebrew_PCBs@yahoogroups.com, Alan Marconett <KM6VV@...> wrote:
>
> Hi Ted,
> 
> I saw parts with hidden supply pins get connected, but trouble is,
there 
> are many ways to call pins, VDD, VCC,  GND, VSS.  And Eagle doesn't
seem 
> to have a way to "alias" them together when they should be.
> 
> Did you notice the GND@1 and GND@2 convention?  you might try the @ 
> convention to tie your pins together.
> 
> Time for my question,  I  just finished routing my board (by hand!),
and 
> I see that I  have vias that somehow have the wrong hole size?  They 
> show up on the design rules check.  I have 12 mil signals and 24 mil 
> power traces.  They need changed, but what's the spec?
> 
> Alan  KM6VV
> 
> 
> kilocycles wrote:
> > I'm re-doing some components I previously created (in Eagle, but this
> > probably applies to other CAD pacakages as well).  The actual
---snip---

Stefan,
I'm not sure how to do that in Eagle  Once I get the supply pins to
show up, using the "invoke" command, I don't think the pins are
repositionable.  One thing I noticed when I first started playing
around with DipTrace is that it worked somewhat differently.  For
example, the first op amp I added, when I went to add the second
section, the symbol with the same pin numbers showed up, instead of
the higher pin numbers, as U1b. I think I remember being able to put
the supply pins on either section, once I got the sections
straightened out.

I'll have to do some more investigating; maybe now is a good time to
read the "Schematic Creating" tutorial by the guy from Japan.

Ted 

--- In Homebrew_PCBs@yahoogroups.com, "Stefan Trethan"
<stefan_trethan@...> wrote:
>
> On Sat, 18 Mar 2006 19:41:25 +0100, Alan Marconett <KM6VV@...> wrote:
> 
> > Hi Ted,
> >
> >
> > I saw parts with hidden supply pins get connected, but trouble is,
there
> >
> > are many ways to call pins, VDD, VCC,  GND, VSS. 
> >
> 
> Hidden pins can be very annoying, i know the problem from orcad
times. You  
> can use a "supply block" for components that use hidden supply
(imagine a  
> quad opamp, i will havbe 4 opamp symbols inside and a supply block  
> symbol). The supply blocks can be put together in one area of the  
> schematic and connected in parallel to the supply and capacitors as  
> required. This is not so clean looking as totally hidden supply, but
IMO  
> in a schematic that is used to create a PCB and does _not_ show each
and  
> every pin is worthless. Leaving out pins may be nice for some earlier  
> design stage, but the PCB really needs a full schematic. I would
expect  
> eagle will allow to use supply blocks (every software that allows
multiple  
> symbols inside one component can do that, eagle is one of them i think).
> 
> If you use reference symbols instead of wires having all supply pins
on  
> the component symbol does not add much "clutter", and i actually
prefer  
> that over supply blocks. When i read the schematic thinking "which
pin was  
> supply again" i don't need to look at the component, see that it is
say  
> IC4, search IC4 amongst the supply blocks, and read the numbers, it
will  

> all be there in one place like a real-life component.
> 

> 
> ST
>

On Sat, 18 Mar 2006 22:12:56 +0100, kilocycles <kilocycles@...>  
wrote:

> Stefan,
>
> I'm not sure how to do that in Eagle  Once I get the supply pins to
>
> show up, using the "invoke" command, I don't think the pins are
>
> repositionable.  One thing I noticed when I first started playing
>
> around with DipTrace is that it worked somewhat differently.  For
>
> example, the first op amp I added, when I went to add the second
>
> section, the symbol with the same pin numbers showed up, instead of
>
> the higher pin numbers, as U1b. I think I remember being able to put
>
> the supply pins on either section, once I got the sections
>
> straightened out.
>
>
> I'll have to do some more investigating; maybe now is a good time to
>
> read the "Schematic Creating" tutorial by the guy from Japan.
>
>
> Ted


A quick look at the first result  
<http://www.testech-elect.com/cadsoft/tour13.htm> for "eagle creating  
library parts" on google shows it can do multiple symbols in one component  
and it even shows a power symbol beeing used. Now this page is crap, and  
it only shows this animated picture, but it _does_ show it is possible, so  
you should be able to find the details elsewhere. So if you want to use  
separate power symbols that should be fine, and it also shouldn't be a  
problem to put the power pins on one of the regular symbols.

Some programs have a separate function to insert the remaining symbols  
(with the higher pin numbers). For example in Target i have to use "insert  
rest of component" if i stop placing midway through it. If i don't  
terminate the place command they will be generated correctly with the next  
set of pin numbers.

It is also worthwile to read up properly on library part creation before  
you start, for example exchange gate commands can usually only be used if  
you prepared the component properly (this allows you to swap whole sets of  
pins with identical function to make routing easier).

ST

Hi Ted,

I looked at the provided examples, and got the diameter/drill of the 
vias on it.  .048 /.032 drill.  seems to work.

Sounds like GND@1 is working for you.  A little confusing how they are 
placed/removed.  Hard to get rid of them after you've placed them! 
Finally did ripup followed by ratsnest and DRC commands.  I get a big X 
where the via was, and it finally goes away.  But all are fine now after 
being replaced.  DRC is good.

What else should I play with after I pretty it up a bit?

Alan  KM6VV


kilocycles wrote:

> Alan,
> I just tried the new part in place of the old one.  Originally, when I
> designed the symbol for it (it's an SBL-1 mixer), I just used the
> standard "wagon wheel" for the symbol for it, the TUF-1, ADE-1 and a
> homebrew version of the SBL-1.  Then, I realized when doing the first
> board, I had no convenient way to connect the external grounds and the
> two IF pins together (doh!).  I was trying to force wiring on the
> board view, and I didn't care for that much.
> 
> I redesigned a rectangular symbol with 4 pins on each side, and drew
> the wagon wheel mixer symbol inside it at .0125" grid resolution, and
> added the text to it.  Then I switched back to .1" resolution to make
> sure the pins would connect on the schematic.  I renamed the pins fro
> P$1 etc. to (in order, as the are one the actual device) RF, GND@1,
> IF@1, IF@2, GND@2, GND@3, GND@4 and LO for pin #8.  By the way, as
> expected, the "@1" doesn't show up on the symbol.  I set the pin to
> display the nam on the symbol only, and it just shows RF GND IF IF 
> and then GND GND GND LO coming back up the other side.
> 
> I just added them to the schematic of the product detector/audio
> schematic I'm working on, and it looks good on the schematic and
> board.  I disconnected the grounds temporarily to test that "auto net"
> thing with a supply.  I added a +12V supply and connected it to a
> transistor, and it didn't connect any of the grounds.  Then, I
> arbitrarily connected the +12V to the LO pin, and again, no
> auto-ground connection.  Maybe it will only do that if you have a part
> with a voltage supply defining one of the pins, like maybe on a 7812
> regulator, or something.  The regulators that are in the libraries
> don't do that, however.
> 
> I'm the wrong person to ask about vias.  I just made my first ones, on
> a board with some MMIC amplifier devices on the top ground plane side,
> along with the PA transistor at the other end of the board.  I *think*
> I'm doing it right; it added a via pad to the board, and I'll connect
> it through with a piece of wire.  Click on DRC, and then read the
> information regarding minimum drill for the Sizes and Restring tabs. 
> I don't completely understand it (it's Eagle!), but the Japanese
> tutorial suggested setting Restring at 40%.  I've had many situations
> where I had DRC errors for drill size, but I just ignore them, since I
> don't send the boards out for fabrication.  I don't even print the
> boards from the program, which could show the drill holes. I export
> them to .bmp files and edit them in Photoshop, adding text, making
> pilot holes, and use the "Threshold" control of Photoshop to ge a pure
> black and white image for printing.  It adds a considerable amount of
> time to do it that way, but that's the way I've always done it.  Until
> I figured out the "polygon gnd" thing, I even added fills using
> Photoshop.  
> 
> As to the specs, well, I pretty much ignore those as well.  After I've
> finished routing, I usually go back with the "Wrench" tool and
> redefine the traces to a wider trace, typically .032", as long as it
> still passes DRC.  I have seen specs for digital and mixed analog
> layouts on some sites, along with specs for signals crossing under
> other signals.  Obviously, signal trace widths and layer crossings are
> extremely critical at VHF and UHF, where the foil traces are inductors
> and capacitors.  I haven't seen any guidelines for HF, but I try to
> use common sense.  I tie the top ground plane to the bottom foil layer
> in several places, and I'm careful not to put a large trace across a
> critical section where capacitance through the 1/16" thickness of a
> board would be a problem.  For example, for those GHz-capable MMIC
> amplifiers mounted on the top layer, I left the foil side of the board
> blank underneath them and their circuitry to hopefully preclude VHF
> oscillations.
> 
> When I get the other mixer device symbols corrected, I can send you a
> copy of the small custom library they're in, if you want it.  I also
> have some toroids in there (bifilar and trifilar FT37-43, etc., and
> the Mouser 42IF123 IF can transformer that is used in several QRP rig
> designs.  Also a board-mounted RCA jack that I found at a local
> surplus house, to use for board-to-board connections with coax.
> 
> Ted

Alan,
It's just plain weird the way Eagle leaves detritus behind when you
remove something, or fix a DRC error like not enough clearance between
pads and traces.  I'd like to discover a way to turn on the drill
holes for exporting the image as a .bmp file.  That must be possible,
because some time ago I made a part, and the drill holes always showed
in the pads on the board for that part.  It also had too large a drill
diameter for the pads, so maybe that was Eagle's way of reminding me
of that fact.

Here's some other silliness to avoid: some of the packages used for
HC-49 crystals and other components in some of the libraries have a
crosshatch area surrounding them.  I used to manually edit out those
areas in Photoshop until I discovered they can be turned off!  They
are on one of the layers; near the end of the list, I forget right
now, and I'm downstairs on the laptop, not at the big machine.

If you haven't discovered it yet, there is a "solpad" library.  You
can add connection points on the schematic for off-board components
like power feeds, front-panel pots, etc.  They will show up as pads on
the board, fly-wired to whatever component on the schematic you've
connected them to.  Very useful; I use them as jumper points on
single-sided boards as well.  They can be renamed and re-valued like
any other part on the schematic, such as "J1"  "Audio_Out".

Ted

--- In Homebrew_PCBs@yahoogroups.com, Alan Marconett <KM6VV@...> wrote:
>
> Hi Ted,
> 
> I looked at the provided examples, and got the diameter/drill of the 
> vias on it.  .048 /.032 drill.  seems to work.
> 
> Sounds like GND@1 is working for you.  A little confusing how they are 
> placed/removed.  Hard to get rid of them after you've placed them! 
> Finally did ripup followed by ratsnest and DRC commands.  I get a big X 
> where the via was, and it finally goes away.  But all are fine now
after 
> being replaced.  DRC is good.
> 
> What else should I play with after I pretty it up a bit?
> 
> Alan  KM6VV
---snip---

Hi Tod,

I thought I'd look at the Excellon files, they should have the hole 
data.  Somewhere is a program to convert that to Gcode.  Just having the 
coordinates and drill sizes should do it.  If I can import points into 
Vector CAD/CAM, I can generate a Gcode program.

So that's what that was on my HC-49 crystal!  I turned off the vrestrict 
layer, and the extra went away.  Didn't seem to help anyway, I had a via 
(that I've since moved) encroaching into this area.

Just tried a solpad.  Must be a test pad?  I almost forgot to add some 
test points.

It seems to get harder to find the un-routed signals at the very end. 
Is there a way to make them stand out, or determine their net name?

Alan  KM6VV


kilocycles wrote:

> Alan,
> It's just plain weird the way Eagle leaves detritus behind when you
> remove something, or fix a DRC error like not enough clearance between
> pads and traces.  I'd like to discover a way to turn on the drill
> holes for exporting the image as a .bmp file.  That must be possible,
> because some time ago I made a part, and the drill holes always showed
> in the pads on the board for that part.  It also had too large a drill
> diameter for the pads, so maybe that was Eagle's way of reminding me
> of that fact.
> 
> Here's some other silliness to avoid: some of the packages used for
> HC-49 crystals and other components in some of the libraries have a
> crosshatch area surrounding them.  I used to manually edit out those
> areas in Photoshop until I discovered they can be turned off!  They
> are on one of the layers; near the end of the list, I forget right
> now, and I'm downstairs on the laptop, not at the big machine.
> 
> If you haven't discovered it yet, there is a "solpad" library.  You
> can add connection points on the schematic for off-board components
> like power feeds, front-panel pots, etc.  They will show up as pads on
> the board, fly-wired to whatever component on the schematic you've
> connected them to.  Very useful; I use them as jumper points on
> single-sided boards as well.  They can be renamed and re-valued like
> any other part on the schematic, such as "J1"  "Audio_Out".
> 
> Ted
> 
> --- In Homebrew_PCBs@yahoogroups.com, Alan Marconett <KM6VV@...> wrote:
> 
>>Hi Ted,
>>
>>I looked at the provided examples, and got the diameter/drill of the 
>>vias on it.  .048 /.032 drill.  seems to work.
>>
>>Sounds like GND@1 is working for you.  A little confusing how they are 
>>placed/removed.  Hard to get rid of them after you've placed them! 
>>Finally did ripup followed by ratsnest and DRC commands.  I get a big X 
>>where the via was, and it finally goes away.  But all are fine now
> 
> after 
> 
>>being replaced.  DRC is good.
>>
>>What else should I play with after I pretty it up a bit?
>>
>>Alan  KM6VV
> 
> ---snip---
> 
> 
> 
> 
> 
> Be sure to visit the group home and check for new Links, Files, and Photos:
> http://groups.yahoo.com/group/Homebrew_PCBs
> 
> If Files or Photos are running short of space, post them here:
> http://groups.yahoo.com/group/Homebrew_PCBs_Archives/ 
> Yahoo! Groups Links
> 
> 
> 
>  
> 
> 
> 
>

Hello Alan,

  Monday, March 20, 2006, 1:15:45 AM, you wrote:

> Hi Tod,

> I thought I'd look at the Excellon files, they should have the hole 
> data.  Somewhere is a program to convert that to Gcode.  Just having the
> coordinates and drill sizes should do it.  If I can import points into
> Vector CAD/CAM, I can generate a Gcode program.

> So that's what that was on my HC-49 crystal!  I turned off the vrestrict
> layer, and the extra went away.  Didn't seem to help anyway, I had a via
> (that I've since moved) encroaching into this area.

> Just tried a solpad.  Must be a test pad?  I almost forgot to add some
> test points.

> It seems to get harder to find the un-routed signals at the very end.
> Is there a way to make them stand out, or determine their net name?

> Alan  KM6VV

<snip>

Some time ago I wrote Exellon->G-code converter you can find it on the
kellyware.com

In  the  mean  time,  I  have  to resort some issues with my ISP and I
willput  different versions as freeware on-line. Link willbe posted to
the group.

The  limitation  of  the converter is that id does not like suppressed
zeroes,it requires both leading and trailing zeroes
-- 
 Best regards,
ø¤º°``````````````````````````````````````````````````````°º¤ø
ZAS ElMed                        | mailto:zastos@...
szr za proizvodnju i odrzavanje  | http://www.zas-elmed.co.yu
    medicinske i industrijske    | 
    elektronike i automatike     | Tel/Fax: (011) 344-0748
                                 | 
 Zoran A. Scepanovic             |     Mob: (063) 609-993
º¤ø,¸¸¸¸¸¸¸¸¸¸¸¸¸¸¸¸¸¸¸¸¸¸¸¸¸¸¸¸¸¸¸¸¸¸¸¸¸¸¸¸¸¸¸¸¸¸¸¸¸¸¸¸¸¸,ø¤º

*********
Investment in reliability will increase until it exceeds the probable cost of errors,
  or until someone insists on getting some useful work done.
*********

Please be advised what was said may be absolutely wrong, and hereby this disclaimer follows.  I reserve the right to be wrong and admit it in front of the entire world.



[Non-text portions of this message have been removed]

HI Zoran,

Thanks for the URL!  I'll check it out.  And I'll be watching for anything
you care to post in the files.

Alan  KM6VV

> On Behalf Of Zoran A. Scepanovic
> 
> Hello Alan,
> 
>   Monday, March 20, 2006, 1:15:45 AM, you wrote:
> 
> > Hi Tod,
> 
> > I thought I'd look at the Excellon files, they should have the hole
> > data.  Somewhere is a program to convert that to Gcode.  Just having the
> > coordinates and drill sizes should do it.  If I can import points into
> > Vector CAD/CAM, I can generate a Gcode program.
> > <snip>
>  
> > Alan  KM6VV
> 
> <snip>
> 
> Some time ago I wrote Exellon->G-code converter you can find it on the
> kellyware.com
> 
> In  the  mean  time,  I  have  to resort some issues with my ISP and I
> willput  different versions as freeware on-line. Link willbe posted to
> the group.
> 
> The  limitation  of  the converter is that id does not like suppressed
> zeroes,it requires both leading and trailing zeroes
> --
>  Best regards,
>
>  Zoran A. Scepanovic

HI again Zoran!

I just ran Eagle 4.1 and generated an Excellon file from my project!  I
don't recall if you said you use Eagle, but I've got a few questions on my
results!

First, I suspect Eagle's Units of 1/10000 Inch are not what you're using (I
suspect you use 1mil, 1/1000"?).  No big deal, I can import the gcode file
into Vector CAD/CAM and re-scale it.  I also noticed that you rapid (G00) at
Z = 0 level.  I can work around this, but if I'm not mistaken, current
practice is often to set surface = 0.  Maybe it's different in the PCB
world.

BUT EAGLE is what's confusing me!  I have five holes, only used for the four
corners, and the center.

T07
X4687Y2006
X24687Y17006
X4687Y32006
X44687Y32006
X44687Y2006


One hole is at (0,0) the EXACT origin!  The other corners are (4,0)  (4,3)
and (0,3) as you might expect (read by cursor on the board.  Center hole is
at (2,1.5).  So clearly there is an offset in these coordinates!  And an
UGLY one at that! (X 2.4687, Y 1.7006)

Your program faithfully passes the locations through with the noted scaling.

The CAM processor offsets are set to 0 and 0.  

Anyone know why there are offsets in the Excellon file?

I did learn that I had a few odd-sized vias or pads that I want to replace!

Alan  KM6VV
P.S.  While on your site I noticed the "Max Stepper" board (and a PC
program?)  What can you tell me about that?  Is it now in production?  Is
the protocol to talk to the board published?  I currently use an 18F452 on a
demo board to drive ONE stepper motor.

http://www.kellyware.com

> 
> Some time ago I wrote Exellon->G-code converter you can find it on the
> kellyware.com
> Zoran

>Anyone know why there are offsets in the Excellon file?

I suspect this happens if the pos.Coord option under Style in the CAM 
Processor is checked. Uncheck it and process the job again. It 
probably applies an offset to prevent negative coordinates when that 
option is checked.

--- In Homebrew_PCBs@yahoogroups.com, "Alan Marconett" <KM6VV@...> 
wrote:

Hi Derek,

Yes!  That was it!

X0Y0
X20000Y15000
X0Y30000
X40000Y30000
X40000Y0

Thanks!

Alan  KM6VV

> 
> >Anyone know why there are offsets in the Excellon file?
> 
> I suspect this happens if the pos.Coord option under Style in the CAM
> Processor is checked. Uncheck it and process the job again. It
> probably applies an offset to prevent negative coordinates when that
> option is checked.
>