Homebrew PCBs

Does anyone know if it’s possible to tell Eagle that standard holes  
for through-hole components aren’t automatically attached to both top  
and bottom layers?  That seems to be the assumption, and I ended up  
with an isolated ground plane on my first board.  I fixed that easily,  
but I’m finding that I need to pay careful attention when laying out  
the board to ensure that I will have connected the layers together at  
a given hole where necessary.  For example, it’s easy to solder the  
leg of an IC to both layers without a socket, but if you *are* using a  
socket, you can only solder to the bottom layer (if the socket’s on  
top).

Thanks,
Brian

--
Brian Lalor / blalor@...
     You snooze, you lose
     Well I have snost and lost

I can't help you with the question about Eagle, but FWIW I don't think there is a way to do that in Kicad, which is the layout program I use. This is one reason why auto-routers have limitations; a lot of folks here do most or all of their layout manually. (Well -- manually as in telling the program where to put the trace; it's still a heck of a lot easier than the old press & stick manual process!)

One thing I have done to include a socket is to use a wire-wrap socket -- the long legs let you mount it as high as needed to be able to solder on the top side and still have it stick out the bottom -- in fact, you'll almost certainly wind up cutting the legs shorter to keep them from sticking out too far. This feels like a kludgy solution to me, but I have used it at the prototyping stage.

--- In Homebrew_PCBs@yahoogroups.com, Brian Lalor <blalor@...> wrote:

>
> Does anyone know if it's possible to tell Eagle that standard holes  
> for through-hole components aren't automatically attached to both top  
> and bottom layers?  That seems to be the assumption, and I ended up  
> with an isolated ground plane on my first board.  I fixed that easily,  
> but I'm finding that I need to pay careful attention when laying out  
> the board to ensure that I will have connected the layers together at  
> a given hole where necessary.  For example, it's easy to solder the  
> leg of an IC to both layers without a socket, but if you *are* using a  
> socket, you can only solder to the bottom layer (if the socket's on  
> top).
> 
> Thanks,
> Brian
> 
> --
> Brian Lalor / blalor@...
>      You snooze, you lose
>      Well I have snost and lost
>

I'm not sure how it can be done in eagle. In most any other layout
software you'd just define the padstack so it doesn't have a pad on
top where you can't solder. Since the pads in eagle are a separate
single layer that might be impossible for all I know. You might be
able to fake it by using SMD pads, but it would be one horrible
kludge, should fit right in with Eagle.

There's a list 'specially for Eagle, you might have more luck here:
eaglecad@yahoogroups.com

Regarding soldering on top side, It's possible for turned sockets,
which expose a little of the metal, but tricky.

ST

On Wed, Jan 20, 2010 at 8:00 PM, awakephd <a_wake@...> wrote:
> I can't help you with the question about Eagle, but FWIW I don't think there is a way to do that in Kicad, which is the layout program I use. This is one reason why auto-routers have limitations; a lot of folks here do most or all of their layout manually. (Well -- manually as in telling the program where to put the trace; it's still a heck of a lot easier than the old press & stick manual process!)
>
> One thing I have done to include a socket is to use a wire-wrap socket -- the long legs let you mount it as high as needed to be able to solder on the top side and still have it stick out the bottom -- in fact, you'll almost certainly wind up cutting the legs shorter to keep them from sticking out too far. This feels like a kludgy solution to me, but I have used it at the prototyping stage.
>
> --- In Homebrew_PCBs@yahoogroups.com, Brian Lalor <blalor@...> wrote:
>>
>> Does anyone know if it's possible to tell Eagle that standard holes
>> for through-hole components aren't automatically attached to both top
>> and bottom layers?  That seems to be the assumption, and I ended up
>> with an isolated ground plane on my first board.  I fixed that easily,
>> but I'm finding that I need to pay careful attention when laying out
>> the board to ensure that I will have connected the layers together at
>> a given hole where necessary.  For example, it's easy to solder the
>> leg of an IC to both layers without a socket, but if you *are* using a
>> socket, you can only solder to the bottom layer (if the socket's on
>> top).
>>
>> Thanks,
>> Brian
>>
>> --
>> Brian Lalor / blalor@...
>>      You snooze, you lose
>>      Well I have snost and lost
>>
>
>
>
>
> ------------------------------------
>
> Be sure to visit the group home and check for new Links, Files, and Photos:
> http://groups.yahoo.com/group/Homebrew_PCBsYahoo! Groups Links
>
>
>
>

On 20/01/2010 19:33, Stefan Trethan wrote:
> I'm not sure how it can be done in eagle. In most any other layout
> software you'd just define the padstack so it doesn't have a pad on
> top where you can't solder. Since the pads in eagle are a separate
> single layer that might be impossible for all I know. You might be
> able to fake it by using SMD pads, but it would be one horrible
> kludge, should fit right in with Eagle.
>
> There's a list 'specially for Eagle, you might have more luck here:
> eaglecad@yahoogroups.com
>
> Regarding soldering on top side, It's possible for turned sockets,
> which expose a little of the metal, but tricky.

Pulsonix has a plated/unplated option for all pads.

Leon

I don't think that would actually do it in this case.

What is required is to eliminate or disconnect the pad on the top
side. Basically edit the padstack so that for this component there is
no copper pad on the top layer and no throughhole plating.

How is this done in PSX by the way, I can't seem to figure it out there either?

ST

On Wed, Jan 20, 2010 at 9:47 PM, Leon Heller <leon355@...> wrote:

>
> Pulsonix has a plated/unplated option for all pads.
>
> Leon
>

On 20/01/2010 21:07, Stefan Trethan wrote:
> I don't think that would actually do it in this case.
>
> What is required is to eliminate or disconnect the pad on the top
> side. Basically edit the padstack so that for this component there is
> no copper pad on the top layer and no throughhole plating.
>
> How is this done in PSX by the way, I can't seem to figure it out there either?

When the pad is added to the footprint you simply select <topside> or 
<bottomside> instead of <through board>.

Leon

Ok in Pulsonix this is done by editing technology, pad styles, and
doing a "by layer" definition. This is badly documented and maybe the
most difficult thing I tried to find so far. Took me almost 20
minutes, but it does work just fine. Once you know how it's a matter
of a few seconds. The pad properties dialog does not in any way hook
you up with the technology settings, which is a shame, they should put
a button there.

In Altium Designer it was just a matter of clicking the pad and then
editing the padstack. Easy to find in a couple of seconds even for
someone who has never used the software like myself. Might just be the
most intuitive thing I have tried with that darn confusing hunk of
software.

In Target 3001 it was just a matter of doubleclicking the pad and
selecting the layer, or defining a padstack. Easy to do since I know
it was there but would be just as intuitive for someone who doesn't
know. After all if you want to change the pad layers you try clicking
that pad first thing.

Now on to Eagle. Finding how to do it there, if it is possible at all,
might just take me longer than I'm willing to spend on this trial.

ST

On Wed, Jan 20, 2010 at 10:07 PM, Stefan Trethan <stefan_trethan@...> wrote:
> I don't think that would actually do it in this case.
>
> What is required is to eliminate or disconnect the pad on the top
> side. Basically edit the padstack so that for this component there is
> no copper pad on the top layer and no throughhole plating.
>
> How is this done in PSX by the way, I can't seem to figure it out there either?
>
> ST
>
> On Wed, Jan 20, 2010 at 9:47 PM, Leon Heller <leon355@...> wrote:
>
>>
>> Pulsonix has a plated/unplated option for all pads.
>>
>> Leon
>>
>

No can do, it doesn't put the hole in then. Tried that first thing.

ST

On Wed, Jan 20, 2010 at 10:53 PM, Leon Heller <leon355@...> wrote:

> When the pad is added to the footprint you simply select <topside> or
> <bottomside> instead of <through board>.
>
> Leon
>

On 20/01/2010 21:56, Stefan Trethan wrote:
> No can do, it doesn't put the hole in then. Tried that first thing.

The hole might not be visible, but it will be in the drill file!

Leon

On 20/01/2010 22:19, Leon Heller wrote:
> On 20/01/2010 21:56, Stefan Trethan wrote:
>> No can do, it doesn't put the hole in then. Tried that first thing.
>
> The hole might not be visible, but it will be in the drill file!

I just checked and it isn't. I'll ask Pulsonix about it.

Leon

On Jan 20, 2010, at 2:33 PM, Stefan Trethan wrote:

> There's a list 'specially for Eagle, you might have more luck here:
> eaglecad@yahoogroups.com

I joined that list, and one of the first posts I saw was yours on this  
topic! :-)  I’ll be looking forward to seeing if anyone comes up with  
an answer.  I searched the archives there briefly and did see a post  
from ’08 where someone seemed to be asking a similar question without  
a very positive response.  It’s not a massive problem, but it would be  
nice not to have to think about it…

Brian

--
Brian Lalor / blalor@...
     Humanity is rife with enterprising idiots whose final words may  
well have
     been "hold my beer and watch this."

Well, you got me interested. We have the same thing in a couple of our
designs (with the SMD pad fake) but thinking about it that is really
not a good solution.

There's also a german post on another forum, they couldn't help that
guy either so it doesn't look promising.


ST

On Thu, Jan 21, 2010 at 5:00 AM, Brian Lalor <blalor@...> wrote:
> On Jan 20, 2010, at 2:33 PM, Stefan Trethan wrote:
>
>> There's a list 'specially for Eagle, you might have more luck here:
>> eaglecad@yahoogroups.com
>
> I joined that list, and one of the first posts I saw was yours on this
> topic! :-)  I’ll be looking forward to seeing if anyone comes up with
> an answer.  I searched the archives there briefly and did see a post
> from ’08 where someone seemed to be asking a similar question without
> a very positive response.  It’s not a massive problem, but it would be
> nice not to have to think about it…
>
> Brian
>
> --
> Brian Lalor / blalor@...
>     Humanity is rife with enterprising idiots whose final words may
> well have
>     been "hold my beer and watch this."
>
>
>
>
> ------------------------------------
>
> Be sure to visit the group home and check for new Links, Files, and Photos:
> http://groups.yahoo.com/group/Homebrew_PCBsYahoo! Groups Links
>
>
>
>

Leon,

I think it believes you are making a SMD pad if you put it on top or
bottom layer alone and ignores the drill.

In any case the correct way is to define a padstack, which works just fine.

ST

On Thu, Jan 21, 2010 at 12:10 AM, Leon Heller <leon355@...> wrote:

> I just checked and it isn't. I'll ask Pulsonix about it.
>
> Leon
>
>

On 21/01/2010 06:22, Stefan Trethan wrote:
> Leon,
>
> I think it believes you are making a SMD pad if you put it on top or
> bottom layer alone and ignores the drill.
>
> In any case the correct way is to define a padstack, which works just fine.

I tried the latter, it worked OK.

I did ask Pulsonix about it. As you say, it assumes it's an SMD pad.

Leon

Brian Lalor wrote: 
> Does anyone know if it\u2019s possible to tell Eagle that standard holes  
> for through-hole components aren\u2019t automatically attached to both top  
> and bottom layers? 

There is this simple, long used, funny English acronym: RTFM. Was a bit
over used by open source communities, and became unfriendly to newbies.
Maybe STFG/GIYF/JFGI should replace it now. 

> I ended up with an isolated ground plane on my first board.  

http://www.cadsoft.de/faq.htm.en#06013001


If you want to use the autorouter for single layer, some people use
tRestrict layer (41) to avoid top tracks.

How about RTFQ? ;-)
The section you linked to doesn't answer the question.
Please re-read the question and check if it really does fit. Perhaps i
just missed something.

To clarify again, I want to remove the upper pad on _some_ components
only. Others still need it, so setting the upper restring to zero in
design rules won't work.

Thanks

ST

On Thu, Jan 21, 2010 at 3:49 PM, Simao Cardoso <simaocardoso@...> wrote:
> Brian Lalor wrote:
>> Does anyone know if it’s possible to tell Eagle that standard holes
>> for through-hole components aren’t automatically attached to both top
>> and bottom layers?
>
> There is this simple, long used, funny English acronym: RTFM. Was a bit
> over used by open source communities, and became unfriendly to newbies.
> Maybe STFG/GIYF/JFGI should replace it now.
>
>> I ended up with an isolated ground plane on my first board.
>
> http://www.cadsoft.de/faq.htm.en#06013001
>
>
> If you want to use the autorouter for single layer, some people use
> tRestrict layer (41) to avoid top tracks.
>
>
>
> ------------------------------------
>
> Be sure to visit the group home and check for new Links, Files, and Photos:
> http://groups.yahoo.com/group/Homebrew_PCBsYahoo! Groups Links
>
>
>
>

Stefan Trethan wrote:

> The section you linked to doesn't answer the question.

> >> I ended up with an isolated ground plane on my first board.

Don't know how happen, should been this:
http://www.cadsoft.de/faq.htm.en#07021201


But i think this is a wrong question problem. To use bottom single layer
don't even print the top layer. To use the autorouter for single sided
or easy homemade double sided there is the tRestrict trick. But
generally is done by manual routing. How they say it, 90% placement 10%
routing? 

Simao

Ok, I did cosider if the URL might have skipped.
Now it points to 15. How to Create Power Planes, for Example for GND?
That explains the remove islands option, which is good but does not
solve the problem in this particular case, at least on it's own.

We still don't understand each other completely, let's try again. ;-)

We want to use both layers, it is mostly a two layer board. There are
traces running on both layers and many components are connected on
both layers. However some components should only be connected at one
side, for Brian because he can't solder the top side on some parts
that cover the pad and has no PTH, and for me because I need to have
no top pad on some components for production reasons (wires are
soldered there later).

No I don't know how to define the padstack so that there's a pad on
the bottom but no pad on the top. I can only set global design rules
for all pads at once.

I don't use the autorouter as a general rule, I find it useless and as
you say 90% is placement, I think a further 9% is cleanup and I might
as well do that 1% left for the autorouter myself.

The restrict area could work well for Brian because it would prevent
the powerplane and any trace from connecting and leaving an island.
Since Brain doesn't need the pads itself to go away that would seem
like a good solution. Put a top restrict circle on each pad in the
library for the parts you can't solder and you should be good to go.

I don't think there is any solution for myself, other than faking it
with a SMD pad on the bottom side, a hand drawn round pad surrounding
it, and a mounting hole to get it drilled.

ST

On Thu, Jan 21, 2010 at 6:51 PM, Simao Cardoso <simaocardoso@...> wrote:
> Stefan Trethan wrote:
>
>> The section you linked to doesn't answer the question.
>
>> >> I ended up with an isolated ground plane on my first board.
>
> Don't know how happen, should been this:
> http://www.cadsoft.de/faq.htm.en#07021201
>
>
> But i think this is a wrong question problem. To use bottom single layer
> don't even print the top layer. To use the autorouter for single sided
> or easy homemade double sided there is the tRestrict trick. But
> generally is done by manual routing. How they say it, 90% placement 10%
> routing?
>
> Simao
>
>
>
> ------------------------------------
>
> Be sure to visit the group home and check for new Links, Files, and Photos:
> http://groups.yahoo.com/group/Homebrew_PCBsYahoo! Groups Links
>
>
>
>

Stefan Trethan wrote: 
> 
> 
> We still don't understand each other completely, let's try again. ;-)

Sorry the unnecessary confusion, i miss it completely, don't know the
answers.

> no top pad on some components for production reasons (wires are
> soldered there later).
> 

I ended avoiding wires soldered on PCB, they easily break. If i have to
do it without a connector, i solder one pinhead (those used with
jumpers) and them solder the wire to it. And use those termo retractable
rubber tubes (don't know the English name) around pinhead, solder and at
least on 1cm of wire. Much work but this way it really lasts even with
wires movement. 

Simao

On 21/01/2010 19:08, Simao Cardoso wrote:
> Stefan Trethan wrote:
>>
>>
>> We still don't understand each other completely, let's try again. ;-)
>
> Sorry the unnecessary confusion, i miss it completely, don't know the
> answers.
>
>> no top pad on some components for production reasons (wires are
>> soldered there later).
>>
>
> I ended avoiding wires soldered on PCB, they easily break. If i have to
> do it without a connector, i solder one pinhead (those used with
> jumpers) and them solder the wire to it. And use those termo retractable
> rubber tubes (don't know the English name) around pinhead, solder and at
> least on 1cm of wire. Much work but this way it really lasts even with
> wires movement.

Heat-shrink tubing?

Leon

On Jan 21, 2010, at 1:16 PM, Stefan Trethan wrote:

> Now it points to 15. How to Create Power Planes, for Example for GND?
> That explains the remove islands option, which is good but does not
> solve the problem in this particular case, at least on it's own.

That’s a useful nugget to have tucked away, but it still doesn’t help  
in this case.  The island is made up of a pad and a section of ground  
plane on the bottom layer, but that pad is for a socket, and I can’t  
access the pin for the socket on the *top* layer.  If the hole were  
plated, I wouldn’t have the island.

> The restrict area could work well for Brian because it would prevent
> the powerplane and any trace from connecting and leaving an island.
> Since Brian doesn't need the pads itself to go away that would seem
> like a good solution. Put a top restrict circle on each pad in the
> library for the parts you can't solder and you should be good to go.

This is the approach I’m going to try, now.

--
Brian Lalor / blalor@...

"[Pickup trucks] are, to the world of cars, what Mexican food is to  
the world of cuisine. They exist, they are popular in Texas, and, er,  
that’s it." -- Jeremy Clarkson

On Jan 21, 2010, at 7:14 PM, Brian Lalor wrote:

>> The restrict area could work well for Brian because it would prevent
>> the powerplane and any trace from connecting and leaving an island.
>> Since Brian doesn't need the pads itself to go away that would seem
>> like a good solution. Put a top restrict circle on each pad in the
>> library for the parts you can't solder and you should be good to go.
>
> This is the approach I’m going to try, now.

Even better, it appears that I can just draw a rectangle on the  
tRestrict layer in the layout editor.  I don’t need to modify the  
component itself!  Woo hoo!  Still not a perfect solution, but at  
least I can specify regions on a per-layer basis that I know I can’t  
get to.

Thanks, everyone!

--
    __   ____
   / /  / __/ Brian Lalor           "If you still have gas, you're not  
lost."
  / _ \/__ \  blalor@...             -- Jacques Strappe
/_.__/____/  http://bravo5.org/