Homebrew_PCBs

>Now I am trying to figure out how to make a copper-filled polygon in
>the red layer.

--- In Homebrew_PCBs@yahoogroups.com, "alan00463" <alan00463@...> wrote:
>

>
> I completed my schematic capture with the freeware version of EAGLE
> and have begun board layout. I am enjoying it, although I still have
> to learn which layers correspond to the physical layers on the PCB.
> I am just keeping all my traces in the red layer. I think that
> corresponds to the copper trace side of the board.
>

--- In Homebrew_PCBs@yahoogroups.com, "alan00463" <alan00463@...> wrote:
>
> I completed my schematic capture with the freeware version of EAGLE
> and have begun board layout. I am enjoying it, although I still have
> to learn which layers correspond to the physical layers on the PCB.
> I am just keeping all my traces in the red layer. I think that
> corresponds to the copper trace side of the board.
>
> Now I am trying to figure out how to make a copper-filled polygon in
> the red layer. I figured out how to make a closed polygonal figure
> with the trace command.
>
> But my polygons aren't filled. They're hollow. Or is that just
> the way they look on the computer screen?
>
> I looked in the HELP. Apparently I have to set the 'fill mode' to
> SOLID for this operation. How do I do that? Also, how do I set
> the line width for this operation?
>
> Alan
>

>quotes. Then, you select the new drop-down information that appears
>on the menu bar...the layer, width, fill type, isolation and spacing
>(defining how much unfilled area you want around the traces and pads).
> Then you draw the polygon, and click on the ratsnest (green X) symbol
>beside the autoroute symbol.
>
>
>

>Back to the subject of surface mount devices. I did a single layer
>board, and one of the chips (a passive RF mixer, actually, in an SMD
>package) I wanted to use, I wanted to place on the bottom foil layer
>to keep the board single-sided. I had to make a custom variant of the
>device with the pins essentially upside down in the symbol and the
>pads redefined in the package to the bottom layer in order to do that.
> I did a lot of hunting around in the Japanese tutorial on that one :)
>
>
>

>I had to make a custom variant of the
>device with the pins essentially upside down in the symbol and the
>pads redefined in the package to the bottom layer in order to do that.

>

>But my polygons aren't filled. They're hollow. Or is that just
>the way they look on the computer screen?

>
> I completed my schematic capture with the freeware version of EAGLE

>
> >But my polygons aren't filled. They're hollow. Or is that just
> >the way they look on the computer screen?
>
> Are you trying to do something like this by any chance;
>
> http://www.pbase.com/image/57044297/large
>
> In case you are then it's not done by filling several polygons, in
> fact it's done by filling a single polygon. "Copper pours" is one term
> used for the activity.
>

--- In Homebrew_PCBs@yahoogroups.com, "derekhawkins" <eldata@...> wrote:
>
> >I had to make a custom variant of the
> >device with the pins essentially upside down in the symbol and the
> >pads redefined in the package to the bottom layer in order to do that.
>
> You should be able to place SMD devices on either top or bottom layer.
> Just mirror the standard component by clicking on the mirror icon (or
> edit/mirror) then left clicking the device. If you keep left clicking
> the device you'll see it switch layers for each click. It's as easy as
> that.
>
> --- In Homebrew_PCBs@yahoogroups.com, "kilocycles" <kilocycles@>
> wrote:
> >
>

>Next, I want to learn how to toggle the
>visibility of any particular layer (ON and OFF)

>I don't understand how that copper pour is
>done using a single polygon.

--- In Homebrew_PCBs@yahoogroups.com, "alan00463" <alan00463@...> wrote:
>

>I'll have to try that; it would be extremely convenient to do that
>kind of flip for SMDs onto the bottom layer!

>

--- In Homebrew_PCBs@yahoogroups.com, "alan00463" <alan00463@...> wrote:
>
> --- In Homebrew_PCBs@yahoogroups.com, "derekhawkins" <eldata@> wrote:
> >
> > >But my polygons aren't filled. They're hollow. Or is that just
> > >the way they look on the computer screen?
> >
> > Are you trying to do something like this by any chance;
> >
> > http://www.pbase.com/image/57044297/large
> >
> > In case you are then it's not done by filling several polygons, in
> > fact it's done by filling a single polygon. "Copper pours" is one
term
> > used for the activity.
> >
> I just did two simple layouts using point-to-point traces between
> through-hole components. Next, I want to learn how to toggle the
> visibility of any particular layer (ON and OFF).
>
> No, I never considered doing anything like that until you posted the
> pic. After seeing the pic, I am interested in trying that technique
> for a future board. I don't understand how that copper pour is
> done using a single polygon. I will take a look at the Japanese
> website and see if that helps my understanding.
>
> I'm glad you made me aware of this alternate layout technique.
>

>You would typically want to do this prior to the polygon fill, of
>course, to maintain your set clearance around the traces.

>

> You can do this trace by trace (segments of traces actually) by
> clicking on the wrench symbol, setting the desired trace width, and
> then one by one, clicking on the trace segments you want to change.
> You would typically want to do this prior to the polygon fill, of
> course, to maintain your set clearance around the traces.
>
> Cheers,
> Ted

--- In Homebrew_PCBs@yahoogroups.com, "derekhawkins" <eldata@...> wrote:
>
> >I'll have to try that; it would be extremely convenient to do that
> >kind of flip for SMDs onto the bottom layer!
>
> This board has SMD components (albeit basic) on the bottom layer as you
> can see;
>
> http://www.pbase.com/eldata/image/46673206/large
>
> Thru hole devices can be mirrored the same way.
>
> --- In Homebrew_PCBs@yahoogroups.com, "kilocycles" <kilocycles@>
> wrote:
> >
>

--- In Homebrew_PCBs@yahoogroups.com, "alan00463" <alan00463@...> wrote:
>
> --- In Homebrew_PCBs@yahoogroups.com, "kilocycles" <kilocycles@> wrote:
>
> > You can do this trace by trace (segments of traces actually) by
> > clicking on the wrench symbol, setting the desired trace width, and
> > then one by one, clicking on the trace segments you want to change.
> > You would typically want to do this prior to the polygon fill, of
> > course, to maintain your set clearance around the traces.
> >
> > Cheers,
> > Ted
>
> Ted,
>
> Your comments on setting trace widths were EXTREMELY helpful to me.
> This is my first layout. I do want to leave lots of copper on the
> trace side of the board. I tried your technique using the wrench icon
> and it worked great!
>
> Thanks to all who replied to this newbie.
>
> Thanks,
> Alan
>

----- Original Message -----
From: "Alan King" <alan@...>
> Try turning on the tplace layer, placing your SMT device, then use
> that little mirror tool on it, right below the move and beside rotate.
> It's in the tutorial PDF somewhere, the 4.1 or so new version is when I
> got it as I recall..

I don't think that works for SMT parts, Alan. It works fine for
through-hole, but I've never been successful in flipping surface mount
parts. Maybe a limitation of the freebie?

>----- Original Message -----
>From: "Alan King" <alan@...>
>
>
>> Try turning on the tplace layer, placing your SMT device, then use
>>that little mirror tool on it, right below the move and beside rotate.
>>It's in the tutorial PDF somewhere, the 4.1 or so new version is when I
>>got it as I recall..
>>
>>
>
>I don't think that works for SMT parts, Alan. It works fine for
>through-hole, but I've never been successful in flipping surface mount
>parts. Maybe a limitation of the freebie?
>
>
>

>I don't think that works for SMT parts, Alan.

--- In Homebrew_PCBs@yahoogroups.com, "Mike Young" <mikewhy@...> wrote:
>

>Parts is parts in Eagle

--- In Homebrew_PCBs@yahoogroups.com, Alan King <alan@...> wrote:
>

>
> >I don't think that works for SMT parts, Alan.
>
> Eagle would be crap if it didn't. I use that feature often;
>
> One layer;
> http://www.pbase.com/eldata/image/57091286/large
>
> The other;
> http://www.pbase.com/eldata/image/57091263/large

>I think this means the polygons were electrically isolated from the
>traces.

>There must be some way to merge

>

----- Original Message -----
From: "Alan King" <alan@...>
To: <Homebrew_PCBs@yahoogroups.com>
Sent: Friday, March 10, 2006 10:31 PM
>>I don't think that works for SMT parts, Alan. It works fine for
>>through-hole, but I've never been successful in flipping surface mount
>>parts. Maybe a limitation of the freebie?
>>
> I used Eagle for quite some time knowing it worked on through hole and
> not realizing it was how to do SMT parts myself until I finally did the
> tutorial with 4.1. Try again, it works fine. Pads and pins are on the
> same edit window in the library editor, there simply are no SMT or
> through hole parts in Eagle, it understands no difference. There is
> only whether there is a pin touching both layers or an smd at any
> particular point, which has no bearing on flip working or not.. Parts
> is parts in Eagle, it is the chicken nugget mecca of the CAD world..

It worked like a charm after turning on tOrigins. :) I didn't test
exhaustively, but it appears only the origin cross is selectable for mirror.
Otherwise, it flips something else nearby. (I mutter a lot when I use Eagle,
so this isn't anything new or bad. It's just one more thing to keep in mind
and mutter at.)

>but it appears only the origin cross is selectable for mirror.

>
> ----- Original Message -----
> From: "Alan King" <alan@...>
> To: <Homebrew_PCBs@yahoogroups.com>
> Sent: Friday, March 10, 2006 10:31 PM
> >>I don't think that works for SMT parts, Alan. It works fine for
> >>through-hole, but I've never been successful in flipping surface

> >>parts. Maybe a limitation of the freebie?
> >>
> > I used Eagle for quite some time knowing it worked on through

> > not realizing it was how to do SMT parts myself until I finally

> > tutorial with 4.1. Try again, it works fine. Pads and pins are

> > same edit window in the library editor, there simply are no SMT

> > through hole parts in Eagle, it understands no difference.

> > only whether there is a pin touching both layers or an smd at any
> > particular point, which has no bearing on flip working or not..

> > is parts in Eagle, it is the chicken nugget mecca of the CAD

>
> It worked like a charm after turning on tOrigins. :) I didn't test
> exhaustively, but it appears only the origin cross is selectable

> Otherwise, it flips something else nearby. (I mutter a lot when I

> so this isn't anything new or bad. It's just one more thing to

> and mutter at.)
>

--- In Homebrew_PCBs@yahoogroups.com, "jriggen55" <jriggen55@...> wrote:
>
> Several months ago I was looking for a PCB design and layout software
> package. I wanted to draw the schematic and lay out the PCB. A
> friend at work told me about CadSoft Eagle. I found that they had a
> freeware version so I got it.
---snip---
> I was able to muddle through the process and finally got my schematic
> and PCB completed. It seemed to be an uphill battle all the way. It
> seemed that few of the processes in Eagle are intuitive at all but
> rather some obscure method that is difficult to discover and equally
> difficult to remember.
>
> I then went on to my second project which needed a larger circuit
> board. It wouldn't fit within the constraints of Eagle freeware
> version, so I started looking for another software package and found
> DipTrace.
>
> As with Eagle, DipTrace comes with a tutorial and libraries. I went
> through the tutorial and while reading, realized that the processes
> and techniques in DipTrace seemed very intuitive in nature. Quite
> different from Eagle. I then started on my project. I was amazed at
> the size of the supplied libraries. I found all but a couple of my
> components in the supplied libraries. For the few components I could
> not find, it was easy to create them in DipTrace.
>
> Comparing DipTrace to Eagle is like comparing night and day. Going
> from point A to point B can be done in both, but the trip is so-o-o
> much easier in DipTrace.
>
> Help with DipTrace is also very readilly available. They've got a
> yahoo group called 'diptr'. The DipTrace staff is very involved with
> all of the discussions on the group and you get quick answers to all
> of your questions.
>
> My bottom line is:
> If you're looking for PCB software, give DipTrace a try.
> If you use Eagle, give DipTrace a try.
> If you're fed up with Eagle, give DipTrace a try.
---snip---

> My bottom line is:
> If you use Eagle, give DipTrace a try.
> Jim

> In Homebrew_PCBs@yahoogroups.com, "jriggen55" wrote:
> > My bottom line is:
> > If you use Eagle, give DipTrace a try.
> > Jim
>
> Thanks from here too Jim! I'm always on the lookout for an
> alternative. I can't say I'm "fed up" with Eagle. I've actually gotten
> to where I'm quite comfortable with it, and all the features I'm not
> yet using are becoming useful and necessary, one at a time.
>
> Alan, I know you've bought the entry level Eagle bundle already, but
> if the "next level" you're talking about moving to, is referring to
> the Eagle "version" pricing, I'm trusting you'll carefully consider
> any limitations and alternatives. After struggling through some of
> it's "less than intuitive" interfacing, and becoming comfortable with
> it, that's really my only remaining gripe about the whole thing. There
> was a nice discussion here a few weeks ago on it. I've always seen the
> board size thing as ultimately being sort of an unnecessary "road
> block" for those using it for my purposes.
>
> I hang out in a DIY audio forum, where Eagle is the app of choice, and
> all the available boards are forcefully "squashed" into the freeware
> size restraints. It actually makes it a lot harder (or impossible) for
> most DIY etchers to print and etch simple circuits, which may have
> easily fit on a larger board, especially with the larger "control"
> parts like pots,buttons,etc.
>
> I admit, I don't know enough about that industry to know what they
> could afford to change in that area, but there has to be something. I
> was thinking that maybe if they limited some of the more
> "professional" features, like the milling and multi-layer functions,
> for those who obviously wouldn't be etching at home, it may allow for
> a size-unlimited, lower priced version, which would be too difficult
> to use commercially. (dunno??)
>
> If you agree with any of that, please drop them an email. I'm sure
> they get it a lot. I'm hoping they're the sort of company who won't
> disregard any customers who openly admit that they don't intend to
> eventually move into a career in the PCB field.
>
> Take Care,
>
> George

>
> My bottom line is:
> If you're looking for PCB software, give DipTrace a try.
> If you use Eagle, give DipTrace a try.
> If you're fed up with Eagle, give DipTrace a try.
>
> Have a Great day.
>
> Jim
>

>The board size is probably DESIGNED as a roadblock intentionally. BUT I
>think it's really GOOD marketing to make at least one level of "full
>product" available so that potential users can give it a good tryout. Also
>
>Yeah, it's a shame to have to "squash" a good design down into too small an
>area, but it keeps one on one's toes!
>
>
>

>

> I've finally settled on the EASY to master ABACOM products SPLAN and
> SPRINT LAYOUT. (Both come in under the price of DIPTRACE, so it's
> comparable) In my opinion, it's the perfect tool for HOMEBREW.

>
>

>
> I also used AUTOTRAXEDA, though it never stopped feeling like a

> and after $95 and little improvment in release... I let it fade

> as only marginally useful. Making your own parts is a snap with
> AUTOTRAXEDA, BTW.
>

>Hard to figure a way where people can't cheat easily.

> Alan Marconett wrote:
>
>
>>The board size is probably DESIGNED as a roadblock intentionally. BUT I
>>think it's really GOOD marketing to make at least one level of "full
>>product" available so that potential users can give it a good tryout. Also
>>
>>Yeah, it's a shame to have to "squash" a good design down into too small an
>>area, but it keeps one on one's toes!
>>
>>
>>
>
>
>
> The fact is, it does unduly penalize those who would want relatively
> simple schematics but need larger unused areas. It'd be nice if you
> could design everything on the small board, but then break the rules and
> spread things out as needed, only after the area rule break you can't
> add new parts. Problem is then you could simply load up the small
> board, break the rules, then do what you want. Hard to figure a way
> where people can't cheat easily. Complexity limit as in others is just
> as bad, you also can't deeply test things without a lot of parts..
>
> But that leads to exactly what it needs, an area * complexity limit.
> Stay below the bounds and you can do what you want, for larger size
> boards you are limited to a maximum complexity. That would allow the
> people with the $49 version to do exactly what is overly limited, making
> larger size boards that simply need spacing for large components but are
> still rediculously simple and should hardly qualify as needing the $200
> per module version. And if you had to choose at the outset for larger
> board or small board but no complexity limit, that should be easy enough
> to program in.
>
> Alan
>
> PS: Lately I sort of feel like I've gone straight from the round table
> to the Alan convention..
>

>Hi Alan K, !
>
>I take your point! Better then nothing, I suppose. I like your "area *
>complexity" algorithm. But I think they've been using this for what, 6+
>years now? Must work for them.
>
>

>--- In Homebrew_PCBs@yahoogroups.com, Alan King <alan@...> wrote:
>
>
>>Hard to figure a way where people can't cheat easily.
>>
>>
>active members, to allow for a sort of "student" discount. I don't
>think most people talking about toner transfers, DIY etch tanks, or
>GPL-based web projects, are looking at making enough money to
>constitute a few hundred dollars for their circuit apps. I've seen
>
>
>

>I'm sure I'll sound like a cheapskate to someone here, but I think the
>prices Pete mentioned are plenty, for some of us "eternally non-
>profit" types. Maybe $150 or below, for a full featured app, ideally
>even $100 or below. I still think there are some critical "commercial"
>functions they could target, without attacking the board size or
>number of parts. Even just a limit to double-sided boards would likely
>
>
>

>I also still believe that if the limits,etc. force some people
>elsewhere, and they remain fairly "non-profit", I can't see any reason
>why they would return to pay a few hundred later on, and have to re-
>learn whatever the current Eagle is, after growing accustomed to an
>alternative. Probably not the outcome they have in mind.
>
>
>

>With the "harmless" freeware version, they have the option of jumping
>right over something they could actually have afforded, which might
>suit all their needs just the same.
>
>which smaller developers couldn't begin to compete with. Needless to
>say, it pretty much ruined the market for quite a few younger audio
>packages.
>
>
>

On Thu, 16 Mar 2006 01:18:26 +0100, Alan King <alan@...> wrote:

>
>
> The fact is, it does unduly penalize those who would want relatively
>
> simple schematics but need larger unused areas. It'd be nice if you
>
> could design everything on the small board, but then break the rules and
>
> spread things out as needed, only after the area rule break you can't
>
> add new parts. Problem is then you could simply load up the small
>
> board, break the rules, then do what you want. Hard to figure a way
>
> where people can't cheat easily. Complexity limit as in others is just
>
> as bad, you also can't deeply test things without a lot of parts..
>
>
> But that leads to exactly what it needs, an area * complexity limit.
>
> Stay below the bounds and you can do what you want, for larger size
>
> boards you are limited to a maximum complexity. That would allow the
>
> people with the $49 version to do exactly what is overly limited, making
>
> larger size boards that simply need spacing for large components but are
>
> still rediculously simple and should hardly qualify as needing the $200
>
> per module version. And if you had to choose at the outset for larger
>
> board or small board but no complexity limit, that should be easy enough
>
> to program in.
>
>
> Alan

----- Original Message -----
From: "Stefan Trethan" <stefan_trethan@...>
To: <Homebrew_PCBs@yahoogroups.com>
Sent: Thursday, March 16, 2006 8:41 AM
Subject: Re: [Homebrew_PCBs] Re: freeware CAD EAGLE -> (Alan Marconett)


> Which is why i bought Target, which has a pin limit.
> I can make boards as large as i like, but the number of pins is limited.
>
> Has disadvantages also, but i prefer it over size limit.
>

PCB-Pool has a full version of Target on their web site, but I don't think
it generates Gerber and drill files. They can make PCBs directly from the
Target PCB files.

Both Easy-PC and Pulsonix have lower-cost pin-limited versions which allow
boards of any size.

Leon

>
> PCB-Pool has a full version of Target on their web site, but I don't
> think
>
> it generates Gerber and drill files. They can make PCBs directly from the
>
> Target PCB files.

> Both Easy-PC and Pulsonix have lower-cost pin-limited versions which
> allow
>
> boards of any size.

>
> --- In Homebrew_PCBs@yahoogroups.com, "Pete" <pwillard@> wrote:
> >
> ...
> > I've finally settled on the EASY to master ABACOM products SPLAN and
> > SPRINT LAYOUT. (Both come in under the price of DIPTRACE, so it's
> > comparable) In my opinion, it's the perfect tool for HOMEBREW.
>
> So, you are going to add links to their website in the Links section,
> right? ;')
>
> Steve Greenfield

> -----Original Message-----
> On Behalf Of Alan King
> >
> Well it works, but it could work better even for them. They appear to
> be very Euro-centric, and targeting commercial outfits etc since that's
> who buys in Europe. I don't think they really have a proper concept of
> just how many individuals would afford it themselves in the US etc if
> the pricing and capabilities were properly matched to individual needs.
> As it is it's $400 for a double beginner size board setup, for schematic
> and layout. If that was more like $200, they would sell way more than
> 2x as many, even though it would still be priced at 2x of a lot of the
> competition.. $400 simply puts it out of the purchase realm of many
> people who'd manage to afford $150 or $200, and there are way more
> people in that category here than in Europe, I don't think they really
> understand that idea very well..
>
> What it really needs is simply a map. A chart or graphic map of which
> copy or move etc function to use under which circumstances would greatly
> advance ease of use for most people. Similarly a chart for what to do
> for the various library operations would make way more sense than all
> the different descriptions. Though of it a week ago when the library
> discussions came up, simply don't have time to do it myself right now..
>
> Alan
>

>

>
> A Yahoo list for Eagle would be nice!
>

>> A Yahoo list for Eagle would be nice!
>
>>
>
>
> Given the percentage of Eagle-related posts made to this group over
>
> the past few days, the level of interest indicates to me that somebody
>
> could start one and it would instantly become a very active group.
>
> (The folks at CadSoft might even want to get involved.)
>
>
>
> Regards, Bob
>
>

>
> Which is why i bought Target, which has a pin limit.
> I can make boards as large as i like, but the number of pins is limited.
>
> Has disadvantages also, but i prefer it over size limit.
>
> ST
>
>
> On Thu, 16 Mar 2006 01:18:26 +0100, Alan King <alan@...> wrote:
>
> >
> >
> > The fact is, it does unduly penalize those who would want relatively
> >
> > simple schematics but need larger unused areas.

> >
> > board or small board but no complexity limit, that should be easy

> >
> > to program in.
> >
> >
> > Alan
>

>
>
>
> How 'bout <http://groups.yahoo.com/group/eaglecad/>
> 500 members and all.
>

> Sorry, Stefan, I stand corrected. I had just assumed that there wasn't
>
> one based on the number of Eagle posts being made here. I should have
>
> done a search.
>
>
>
> Regards, Bob

>
> On Thu, 16 Mar 2006 19:26:56 +0100, Bob_xyz <bob_barr@...> wrote:
>
> > Sorry, Stefan, I stand corrected. I had just assumed that there wasn't
> >
> > one based on the number of Eagle posts being made here. I should have
> >
> > done a search.
> >
> >
> >
> > Regards, Bob
>
>
> nothing to be sorry about, i didn't know before either.
> I personally don't feel eagle posts are off topic, are they?
> 'course, as there is a special group for it you might find better
> responses there.
> I'd still like to read eagle related posts, especially if the

> can be applied more generally to other packages.
>

> Not specifically directed to Stefan; just convenient to use his post
>
> for a general response
>
>
> The free version of DipTrace has no limit on board size, but is
>
> "complexity limited" by a 250 pin maximum, which is fairly generous.
>
> I did a receiver IF system using all discrete components in Eagle,
>
> which pretty much filled the board, and the pin count was 215.
>
> DipTrace would be especially good for boards that need large foil
>
> traces, physical separation and have physically large components, such
>
> as power supplies with board mounted transformers and large
>
> computer-grade electrolytic caps.
>
>
> Cheers,
>
> Ted KX4OM

----- Original Message -----
From: "Stefan Trethan" <stefan_trethan@...>
To: <Homebrew_PCBs@yahoogroups.com>
Sent: Thursday, March 16, 2006 11:15 AM
Subject: Re: [Homebrew_PCBs] Re: freeware CAD EAGLE ->
(Alan Marconett)


> Not specifically directed to Ted, but also directed
> to him:
>
> I made a new table in the database section listing
> diffent PCB layout
> packages.
> Have a look, and if you have the time fill in what's
> missing.
> If there are any ideas for changes or to add
> something (we can not have
> more than 10 columns) please tell us now before there
> are many entries.
>
>
> <http://groups.yahoo.com/group/Homebrew_PCBs/database?method=reportRows&tbl=7>
>
> I set it so that every member can edit entries, i
> thought it would be
> better to allow changes easily than have the added
> security.
>
> It can be time consuming to add entries, especially
> if there are many
> license variants. There is a easy pricedure to speed
> this up:
> Enter one license version via the add record
> function. Then select export
> table. Copy this text into a text editor and remove
> all lines but the one
> of the entry you just made. Copy this line as often
> as there are other
> license variants. Edit those lines with all the data.
> Select the lines
> with the additional variants, and copy to clipboard.
> In the browser use
> import records to add them. Works like a charm, but
> do not use commas in
> your entries like i did, because otherwise there will
> be a / added for
> each comma 'cause is also used as field separator.
>
> I hope this works out, if it does one can even sort
> the table by price
> etc..
> Do let me know any ideas for changes so we get it
> perfect before too many
> records are in.
>
> ST
>
>
>
>
> On Thu, 16 Mar 2006 19:17:55 +0100, kilocycles
> <kilocycles@...>
> wrote:
>
>> Not specifically directed to Stefan; just convenient
>> to use his post
>>
>> for a general response
>>
>>
>> The free version of DipTrace has no limit on board
>> size, but is
>>
>> "complexity limited" by a 250 pin maximum, which is
>> fairly generous.
>>
>> I did a receiver IF system using all discrete
>> components in Eagle,
>>
>> which pretty much filled the board, and the pin
>> count was 215.
>>
>> DipTrace would be especially good for boards that
>> need large foil
>>
>> traces, physical separation and have physically
>> large components, such
>>
>> as power supplies with board mounted transformers
>> and large
>>
>> computer-grade electrolytic caps.
>>
>>
>> Cheers,
>>
>> Ted KX4OM
>
>
>
>
> 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
>
>
>
>
>
>
>

>
> On Thu, 16 Mar 2006 19:26:56 +0100, Bob_xyz <bob_barr@...> wrote:
>
> > Sorry, Stefan, I stand corrected. I had just assumed that there wasn't
> >
> > one based on the number of Eagle posts being made here. I should have
> >
> > done a search.

> nothing to be sorry about, i didn't know before either.
> I personally don't feel eagle posts are off topic, are they?
> 'course, as there is a special group for it you might find better
> responses there.
> I'd still like to read eagle related posts, especially if the

> can be applied more generally to other packages.

>
> >> A Yahoo list for Eagle would be nice!
> >
> >>
> >
> >
> > Given the percentage of Eagle-related posts made to this group over
> >
> > the past few days, the level of interest indicates to me that somebody
> >
> > could start one and it would instantly become a very active group.
> >
> > (The folks at CadSoft might even want to get involved.)
> >
> >
> >
> > Regards, Bob
>
> How 'bout <http://groups.yahoo.com/group/eaglecad/>
> 500 members and all.
>
> ST

> As many CAD packages and users as there are out there,
>
> how about placing some of the user generated special
>
> parts in the library files to save the rest of us from
>
> re-inventing them? (old DOS OrCad user).
>
>
> Norm
>
> W6NIM

> Subject: [Homebrew_PCBs] Re: freeware CAD EAGLE -> (Alan Marconett)
>
> Not specifically directed to Stefan; just convenient to use his post
> for a general response :)
>
> The free version of DipTrace has no limit on board size, but is
> "complexity limited" by a 250 pin maximum, which is fairly generous.
> I did a receiver IF system using all discrete components in Eagle,
> which pretty much filled the board, and the pin count was 215.
> DipTrace would be especially good for boards that need large foil
> traces, physical separation and have physically large components, such
> as power supplies with board mounted transformers and large
> computer-grade electrolytic caps.
>
> Cheers,
> Ted KX4OM
>

> Hi Alan K, !
>
> I take your point! Better then nothing, I suppose. I like your "area *
> complexity" algorithm. But I think they've been using this for what, 6+
> years now? Must work for them.
>
> I'm getting the hang of the library, I made two parts (PIC18F2520 and
> MAX232) by copying parts and making the changes I wanted. Nice! One
> more part to copy/paste, and I'll have all the power straightened out.
> I seem to recall an "alias" function, must be for a different program.
>
> A Yahoo list for Eagle would be nice!

>Alan Marconett(KM6VV@...) is reported to have said:
>
>
>>A Yahoo list for Eagle would be nice!
>>
>>
>
>To learn more about the eaglecad group, please visit
>http://groups.yahoo.com/group/eaglecad
>
>
>:-) HTH, YMMV, HAND :-)
>
>Wayne
>
>

On Fri, 17 Mar 2006 02:15:08 +0100, davelandnni <daveland@...> wrote:

> I think that Eagle and others should adopt a $per board strategy for
>
> causal users like us. They could make a single board license file
>
> that costs say $20 and gives you unlimited features for that single
>
> board (locked to that PCB file on your PC). You go to the web site
>
> and paypal $20 and they send you the license file good for one
>
> board. The license file "dies" after you run your CAM process for
>
> the 5th time on the board ( 4 tries to get it right). The license
>
> file would also be suspended if you try and delete too many parts and
>
> make another board from the design (cheating). You could then beg for
>
> forgiveness and get a re-instatement.

--- In Homebrew_PCBs@yahoogroups.com, "Alan Marconett" <KM6VV@...> wrote:
>
> Hi Ted,
>
> That doesn't seem very high. I easily exceeded that in the little PIC
> design I'm doing. Connectors eat up a lot of pins I guess. Digital
> probably has more pins typically then analog. I'm at maybe 350-400 now.
> But then this is really my first PCB project (that I'm laying out)
in a long
> time.
>
---snip---
> > The free version of DipTrace has no limit on board size, but is
> > "complexity limited" by a 250 pin maximum, which is fairly generous.
> > I did a receiver IF system using all discrete components in Eagle,
> > which pretty much filled the board, and the pin count was 215.
> > DipTrace would be especially good for boards that need large foil
> > traces, physical separation and have physically large components, such
> > as power supplies with board mounted transformers and large
> > computer-grade electrolytic caps.
> >
> > Cheers,
> > Ted KX4OM

> Wayne Topa wrote:
>
> >Alan Marconett(KM6VV@...) is reported to have said:
> >
> >
> >>A Yahoo list for Eagle would be nice!
> >>
> >>
> >
> >To learn more about the eaglecad group, please visit
> >http://groups.yahoo.com/group/eaglecad
> >
> >
> >:-) HTH, YMMV, HAND :-)
> >
> >Wayne
> >
> >
>
> I see you aren't a card carrying member of AUA.. (Acronym Users
> Anonymous)

> Alan
>
> I see you on CADCAMEDMDRO and now I see you here... You get around!!
>
> I think that Eagle and others should adopt a $per board strategy for
> causal users like us. They could make a single board license file
> that costs say $20 and gives you unlimited features for that single
> board (locked to that PCB file on your PC). You go to the web site
> and paypal $20 and they send you the license file good for one
> board. The license file "dies" after you run your CAM process for
> the 5th time on the board ( 4 tries to get it right). The license
> file would also be suspended if you try and delete too many parts and
> make another board from the design (cheating). You could then beg for
> forgiveness and get a re-instatement.
>
> With the internet it is easy for them to add the "spyware" needed to
> insure the license file is not copied and used by someone else. Just
> use the MAC or IP address of the machine as the "key".
>
> IF they had this... I would already have spent $200 with them and not
> have to think about moving to a competative package... they would
> have sucked me in!!
>
> DAve
>

>
> Alan,
> That's right, it isn't very high for digital circuitry. A 16F877 and
> a few other supporting ICs will run the count up in a hurry. That's
> why I mentioned that my 215-pin design was discrete components only.
> The design was the IF system in Figure 6.50 of "Experimental Methods
> for RF Design", the one using two pairs of J310 JFETs in cascoded
> arrangement. There are a lot of components in that design, and I had
> about a 1 square inch open area left on the 3 x 4 Eagle board when I
> was finished.
>
> I manually routed the board as I went, by the way. I added the
> components for a functional section to the schematic, for example the
> JFET pairs and associated circuitry for the board signal input from
> the crystal filter, laid them out on the board in a logical position,
> and routed; then I moved on to the next section, etc., following the
> signal flow from the schematic in the figure.
>
> Doing it that way made it pretty easy to tweak the routing when I had
> all of the components on the board, without having to unsnarl any
> oddball paths created by autorouting. I found that when I'd rip up a
> few tracks to move components around a bit, I could just hit the
> autoroute icon, and it would redo the routes pretty much as I wanted.
>
> Originally, I laid the board out with two 12 volt feeds, and some
> jumpers from the on-board regulator for Vcc to various points in the
> cicuit, but as it turned out, I was able to lay down tracks for most
> of the power feeds to the functional sections by the time I was finished.
>
> I did this board with a ground plane for the component side. To avoid
> having to mill clearance holes for non-grounded through-hole component
> leads, I exported the board image as a BMP file, and using the layer
> feature in Photoshop (freeware Paint.net will do layers, too), I
> manually added circular clearance holes for the ground plane side.
> After I printed the bottom layer tracks and ironed, I drilled a few
> holes in through-component lead pads to line up the holes, and then
> aligned the ground plane printout by holding the board up to the
> light. Then I ironed the ground plane pattern onto the PCB.
>
> I found that when I reheated the board while ironing on the ground
> plane/component side, some of the bottom layer tracks' toner
> transferred to the pad I was using as a surface for ironing. Next
> time I do a double-sided board, I think I'll etch the tracks side
> (masking the other side with electrical tape), drill my registration
> holes, and then iron the ground plane side. It shouldn't be necessary
> to do it that way. Under my old process of applying the toner to
> Press-n-Peel Blue with a copier, that reverse-transfer wouldn't have
> happened. P-n-P is so tough when it's applied with a copier, you just
> about have to sand it off (or use acetone, as I learned after many
> boards :) ). Now that I'm using my Brother 2040 laser printer for
> toner transfer, I have real problems in getting the toner to stick to
> the board in the first place, which has been much discussed here in
> this group.
>
> 73,
> Ted KX4OM
> www.kx4om.com
>

> I like the idea
> of MILLING isolation traces for a board.

>
> Alan Marconett wrote:
>
> > I like the idea of MILLING isolation traces for a board.
>
> I've considered that as well (on my CNC Taig), but haven't
> gotten around to trying anything other than using it to drill
> the holes. Having done a number of boards with chemical
> etching and knowing how simple it is, I haven't gotten up
> the initiative to try milling one yet.
>
> If you explore the option, would you mind posting details here?

>
> Alan Marconett wrote:
>
> > I like the idea
> > of MILLING isolation traces for a board.
>
> I've considered that as well (on my CNC Taig), but haven't gotten around
> to trying anything other than using it to drill the holes. Having done
> a number of boards with chemical etching and knowing how simple it is, I
> haven't gotten up the initiative to try milling one yet.
>
> If you explore the option, would you mind posting details here?
>
> Thanks
> Dave K
>
>

>
> The URL below show the floating Z-head I developed for
> mechanical etching:
>
> <http://gramlich.net/projects/mill_lathe/index.html#The_Floating_Z_Head>
>
> The mechanical etching bits come from Think and Tinker:
>
> <snip>
> -Wayne
>

>The drawbacks of mechanical etching is that the bits are
>expensive ($6-10 each) and wear out after approximately
>500-1000 linear inches of mechanical etching. As usual,
>there are no plated through holes, but that is fairly
>typical of the Home Brew PCB crowd.
>
>
>

>Alan King(alan@...) is reported to have said:
>
>
>>Wayne Topa wrote:
>>
>>
>>
>>>Alan Marconett(KM6VV@...) is reported to have said:
>>>
>>>
>>>
>>>
>>>>A Yahoo list for Eagle would be nice!
>>>>
>>>>
>>>>
>>>>
>>>To learn more about the eaglecad group, please visit
>>>http://groups.yahoo.com/group/eaglecad
>>>
>>>
>>>:-) HTH, YMMV, HAND :-)
>>>
>>>Wayne
>>>
>>>
>>>
>>>
>> I see you aren't a card carrying member of AUA.. (Acronym Users
>>Anonymous)
>>
>>
>
>Nah
>
>HTH=Hope This Helps, YMMV=Your Mileage May Vary, HAND=Have A Nice Day
>
>Wayne
>
>
>

On Thursday 09 March 2006 09:52 am, alan00463 wrote:
> I completed my schematic capture with the freeware version of EAGLE
> and have begun board layout.   I am enjoying it, although I still have
> to learn which layers correspond to the physical layers on the PCB. 
> I am just keeping all my traces in the red layer.   I think that
> corresponds to the copper trace side of the board.
>
> Now I am trying to figure out how to make a copper-filled polygon in
> the red layer.   I figured out how to make a closed polygonal figure
> with the trace command.
>
> But my polygons aren't filled.    They're hollow.   Or is that just
> the way they look on the computer screen? 
>
> I looked in the HELP.    Apparently I have to set the 'fill mode' to
> SOLID for this operation.    How do I do that?   Also, how do I set
> the line width for this operation?
>
> Alan
>
>
>
>
>
>
> 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/
>
>
>
>
> SPONSORED LINKS
> Electrical engineering degree online Electrical engineering degree
> Printed circuit board Electrical engineering Electrical engineering
> course Electrical engineering graduate school
>
>
> YAHOO! GROUPS LINKS
>
>
>  Visit your group "Homebrew_PCBs" on the web.
>  
>  To unsubscribe from this group, send an email to:
>  Homebrew_PCBs-unsubscribe@yahoogroups.com
>  
>  Your use of Yahoo! Groups is subject to the Yahoo! Terms of Service.
>
>
>  
>
> Message transport security by GatewayDefender
> 9:52:44 AM ET - 3/9/2006

On Thursday 09 March 2006 06:19 pm, kilocycles wrote:

> I did a lot of hunting around in the Japanese tutorial on that one :)

>With the internet it is easy for them to add the "spyware" needed to
>insure the license file is not copied and used by someone else. Just
>use the MAC or IP address of the machine as the "key".

--- In Homebrew_PCBs@yahoogroups.com, "Alan Marconett" <KM6VV@...> wrote:
>
> Hi Ted,
>
> That IS a lot of parts for a discrete RF design! I can see how
working back
> and forth on the schematic and layout would be an ideal way to get good
> routes. Do you already have a parts layout in mind before you do
this? I
> got into the habit of laying out wire-wrap projects by inserting WW
sockets
> into prototype board beforehand to get an idea of the layout. Discrete
> parts as well. But then I would solder ALL of the sockets down
first. This
> "tightly interactive" annotation between schematic and layout is great!
>
> On this board I found that the "flying wires" and parts profiles made it
> fairly easy to initially get all of the packages down and roughly
> orientated. Quite a difference from working with a bag of WW sockets!
>
> I won't be using a ground plane, but it's nice to learn how you've
done it.
> Hopefully I'll be able to MILL isolation traces, but I may also try
> Press-n-Peel Blue, just to be able to compare the results.
>
> I have been wondering how much of the board to manually route, and
when to
> just let the auto-router do it. Last night I got my first exposure to
> routing power traces by hand, and watching the flying wires
disappear after
> a net was routed (and the rat's nest updated). CUTE! I thought I'd run
> into a snag when I routed a ground trace from an IC over to a servo
ground.
> I couldn't delete my added route! But I found out that if I ripped
it up
> (back to an air line) that the rat's nest update would then delete
the bit I
> wanted (I already had the two nodes connected; I didn't want a
ground loop).
> I also found out how to rip up the entire board, which I needed!
>
> 73's,
>
> Alan KM6VV
>
> >
> > Alan,
> > That's right, it isn't very high for digital circuitry. A 16F877 and
> > a few other supporting ICs will run the count up in a hurry. That's
> > why I mentioned that my 215-pin design was discrete components only.
> > The design was the IF system in Figure 6.50 of "Experimental Methods
> > for RF Design", the one using two pairs of J310 JFETs in cascoded
> > arrangement. There are a lot of components in that design, and I had
> > about a 1 square inch open area left on the 3 x 4 Eagle board when I
> > was finished.
> >
> > I manually routed the board as I went, by the way. I added the
> > components for a functional section to the schematic, for example the
> > JFET pairs and associated circuitry for the board signal input from
> > the crystal filter, laid them out on the board in a logical position,
> > and routed; then I moved on to the next section, etc., following the
> > signal flow from the schematic in the figure.
---snip---

> I did autorouting almost exclusively when I first started with Eagle.
>
> The rat's nest simply looked impossible. One thing I use a lot while
>
> routing, either auto or manual, is "show ground"...click eye icon and
>
> type gnd in the command line text box. That helps in that I know
>
> which end of the component to focus on; i.e., the signal end, and
>
> whether or not I need to reorient it. The triangular
>
> emitter-base-collector transistors drive me batty, trying not to have
>
> to run a signal through the triangle. The pad clearances are pretty
>
> close as it is on a TO-92. Also, I'll use the "i" info icon to show
>
> what signal I'm dealing with, and check the schematic.

----- Original Message -----
From: "Stefan Trethan" <stefan_trethan@...>
To: <Homebrew_PCBs@yahoogroups.com>
Sent: Saturday, March 18, 2006 11:37 PM
Subject: Re: [Homebrew_PCBs] Re: freeware CAD EAGLE -> (Alan Marconett)


>I _SO_ agree with you!
> I suggested different color settings for the "rubber bands" of signals to
> the developers of my PCB software, they even called me back, but wouldn't
> quite see the value in the function as much as i would have liked.
> Orcad has this option, and it is dead useful to color ground and VCCs
> differently.
> A good placement means half the work, probably more, so this feature
> really helps. Of course you can select and highlight a net in most any
> software, but having them on special colors permanently beats that by a
> lot.

Pulsonix, of course, lets nets be assigned any colour. I tend not to use
the feature, though, and just highlight the net I am routing, for critical
nets.

Leon

>
>
> Pulsonix, of course, lets nets be assigned any colour. I tend not

> the feature, though, and just highlight the net I am routing, for

> nets.
>

----- Original Message -----
From: "Bob_xyz" <bob_barr@...>
To: <Homebrew_PCBs@yahoogroups.com>
Sent: Sunday, March 19, 2006 6:04 AM
Subject: [Homebrew_PCBs] Re: freeware CAD EAGLE -> (Alan Marconett)


> --- In Homebrew_PCBs@yahoogroups.com, "Leon Heller" <leon.heller@...>
> wrote:
>>
>>
>> Pulsonix, of course, lets nets be assigned any colour. I tend not
> to use
>> the feature, though, and just highlight the net I am routing, for
> critical
>> nets.
>>
>
> Can you different colors for individual net names, such as red for
> Vcc, green for ground, and another color for the other nets? That
> sounds like a very handy feature.

In fact, each net could have its own colour! Apart from the basic colours
(56 of them) one can define one's own custom colours via R,G and B and hue,
saturation and luminosity values.

Leon

> Alan,
> Sometimes I have an idea of the layout beforehand, but sometimes I
> don't. Generally, I'll put a voltage regulator circuit in a section
> of the board that minimizes the wire length to the switch on the
> panel, or to the dc socket on the back panel, however the circuit is
> configured. Same for RF output; I'd prefer to have it at he back of
> the board. In the case of this IF board, the input from the crystal
> filters comes in at the 3" wide left end of the board, because the
> switchable SSB/CW filters I'll be using will be on a sub-board. They
> will be fed by the RF input filter/RF amp/mixer/post-mixer amp board,
> and obviously I want the input to that board near the back of the
> case, but it's not as critical, since it's simply an antenna
> connection through coax. I'd like to try to minimize the number of
> wires and cables I have flying over the PC boards, though.
>
> When I did the SKN Special trans-receiver, If you take a look at the
> web site, I printed out correct-reading images of the boards and glued
> them to cardboard, and did the final planning by shuffling them
> around. I had to reposition the VFO compartment to the side under the
> top lip of the case after I modified the low pass filter to a better
> design that turned out to need more length. I was watching "Rides"
> the other night, and they were converting Jay Leno's Toronado to rear
> wheel drive, and then "oops...we forgot the air conditioner...now
> where do we put that?" It ended up in the trunk. Sometimes planning
> will carry you only so far!
>
> I did autorouting almost exclusively when I first started with Eagle.
> The rat's nest simply looked impossible. One thing I use a lot while
> routing, either auto or manual, is "show ground"...click eye icon and
> type gnd in the command line text box. That helps in that I know
> which end of the component to focus on; i.e., the signal end, and
> whether or not I need to reorient it. The triangular
> emitter-base-collector transistors drive me batty, trying not to have
> to run a signal through the triangle. The pad clearances are pretty
> close as it is on a TO-92. Also, I'll use the "i" info icon to show
> what signal I'm dealing with, and check the schematic.
>
> I aim to minimize the length of the signal paths whenever possible.
> With autorouting, especially if you have it set on a less intelligent
> setting like 20, as opposed to 50, the signal paths may end up being 3
> or 4 abreast, running around the edge of the board. That's annoying,
> when the components they are trying to connect are only 1 inch apart.
> Often, you can reposition a couple of resistors to allow the track to
> run beneath one, bisecting it, and eliminate one signal running around
> the edge of the board. It takes some juggling around. The routing on
> the SKN Special receiver board became a whole lot simpler once I put
> in the multiple power connection points. The tradeoff of much more
> sane RF paths vs. a few extra connections to the +12V jack was easy to
> make, in that case.
>
> 73,
> Ted
> www.kx4om.com
>

--- In Homebrew_PCBs@yahoogroups.com, Alan Marconett <KM6VV@...> wrote:
>
> Hi Ted,
>
> I haven't done any layouts for HF. Last time, I think it was
probably a
> tube circuit. Ok, maybe some simple single side circuit laid out
with tape.
>
> I went to your website, but couldn't find the SKN xcvr.
>
> Although I did a few sample autoroutes on my board, I just "kept going"
> after getting the the pwr routed. Wasn't that hard! The board was
> fairly simple, 'tho.
>
> And I came to appreciate why boards (digital anyway) are often routed
> one direction on top, and a cross direction on the bottom. It keeps
the
> paths open, and minimizes vias.
>
> Alan KM6VV
---snip---

>
> Hi Alan,
> The SKN transceiver is "A 30 meter transceiver for Straight Key Night"
> under the "Completed Projects" setion, 1st item listed. The direct
> link would be http://www.kx4om.com/Projects/SKNXCVR/30mxcvr.html.
>
> The site may have been in flux when you looked. I did some
> considerable re-writing of that page last night, changing the wording
> from a project description in progress, so the html code was flying
> back and forth from my laptop to the server, and the internal links
> were changing.
>
> My latest frustration with Eagle is pad design, or lack of it. I'm
> doing an RF amplifier circuit that has two MMICs in it for
> preamplification prior to the PA. Of course, there are no library
> components for the Mini-Circuits MAR-6, or Agilent MSA-0386, etc,. so
> I had to design them. The problem is, the spec for the two opposing
> ground pad sections (think 4-bladed ceiling fan; input, output, and 2
> grounds)are horizontally wide, rounded edges, with 8 through-holes to
> the bottom layer of the board, to distribute the capacitance to the
> ground plane. The best I could do for the Package was to lay down the
> surface mount pads, and draw using the polygon tool on the outer 1/3
> of the two ground pads. Now, after adding the part to the schematic,
> DRC on the board tells me I have a clearance problem between the
> ground pads and the rectangular polygons! Duh...they're suppost to be
> connected, but as my questions from last week remain, Eagle expects
> one and one only "pad" connected to each pin. Nothing else must touch.
>
> As I told a friend in an e-mail earlier today, that's why I export my
> Eagle boards to Photoshop, so I can do anything I want to with them!
>
> It's hard to imagine doing digital work without CAD, even at the DIL
> page level. I actually do have a manual wire-wrap tool and a spool of
> wire, but I've never used it. To tell you the truth, I'm not very
> good at perf-boad soldered lead construction, either. I have a couple
> of basic problems: layout visualization (I keep running off the end of
> the board), and bending those leads and running wiring in a sane
> manner. Doing "Ripup All" is so much easier! I've done a little bit
> of "ugly" construction, and that's a very fast way to buid, and I've
> done a bit of Manhattan, which is kind of tedious to me. Until I
> recently got back into homebrewing the last couple of years, most of
> my work involved drilling chassis and mounting tube sockets and
> terminal strips. That's quite a gap in time from working with 6146
> beam power tetrodes to MMIC amplifiers the size of a piece of buckshot!
>
> CUL,
> Ted

>I enjoy the CAD work as well. I've mostly used it for designing parts for
>my steam engine models.
>
> http://www.hobbitengineering.com/
>
>

--- In Homebrew_PCBs@yahoogroups.com, "Alan Marconett" <KM6VV@...> wrote:
>
> Hi Ted,
>
> OK, I found it! Quite impressive! I wish I had the time (and
knowledge)
> for advanced RF projects.
>
> I enjoy the CAD work as well. I've mostly used it for designing
parts for
> my steam engine models.
>
> http://www.hobbitengineering.com/
>
> But now it's PCB time! I do have a collection of parts for a PCB
router,
> I'd like to get that up and running.
>
> I've got DeskPCB from IMService, and I'm experimenting with
importing Gerber
> files into it. I suspect some of the parts I used (or made/altered)
have
> pads or outlines on the WRONG layer, as not everything is coming through
> correctly! More library work.
>
> I did find that by adding only a few lines (blocks) of Gcode, I
could get
> Vector CAD/CAM to backplot a Excellon file. And I got rid of the
offset,
> thanks to a reply on this list!
>
> CUL8R,
>
> Alan KM6VV
>
> >
> > Hi Alan,
> > The SKN transceiver is "A 30 meter transceiver for Straight Key Night"
> > under the "Completed Projects" setion, 1st item listed. The direct
> > link would be http://www.kx4om.com/Projects/SKNXCVR/30mxcvr.html.
> >
> > The site may have been in flux when you looked. I did some
> > considerable re-writing of that page last night, changing the wording
> > from a project description in progress, so the html code was flying
> > back and forth from my laptop to the server, and the internal links
> > were changing.
> >
> > My latest frustration with Eagle is pad design, or lack of it. I'm
> > doing an RF amplifier circuit that has two MMICs in it for
> > preamplification prior to the PA. Of course, there are no library
> > components for the Mini-Circuits MAR-6, or Agilent MSA-0386, etc,. so
> > I had to design them. The problem is, the spec for the two opposing
> > ground pad sections (think 4-bladed ceiling fan; input, output, and 2
> > grounds)are horizontally wide, rounded edges, with 8 through-holes to
> > the bottom layer of the board, to distribute the capacitance to the
> > ground plane. The best I could do for the Package was to lay down the
> > surface mount pads, and draw using the polygon tool on the outer 1/3
> > of the two ground pads. Now, after adding the part to the schematic,
> > DRC on the board tells me I have a clearance problem between the
> > ground pads and the rectangular polygons! Duh...they're suppost to be
> > connected, but as my questions from last week remain, Eagle expects
> > one and one only "pad" connected to each pin. Nothing else must
touch.
> >
> > As I told a friend in an e-mail earlier today, that's why I export my
> > Eagle boards to Photoshop, so I can do anything I want to with them!
> >
> > It's hard to imagine doing digital work without CAD, even at the DIL
> > page level. I actually do have a manual wire-wrap tool and a spool of
> > wire, but I've never used it. To tell you the truth, I'm not very
> > good at perf-boad soldered lead construction, either. I have a couple
> > of basic problems: layout visualization (I keep running off the end of
> > the board), and bending those leads and running wiring in a sane
> > manner. Doing "Ripup All" is so much easier! I've done a little bit
> > of "ugly" construction, and that's a very fast way to buid, and I've
> > done a bit of Manhattan, which is kind of tedious to me. Until I
> > recently got back into homebrewing the last couple of years, most of
> > my work involved drilling chassis and mounting tube sockets and
> > terminal strips. That's quite a gap in time from working with 6146
> > beam power tetrodes to MMIC amplifiers the size of a piece of
buckshot!
> >
> > CUL,
> > Ted
>

> Subject: [Homebrew_PCBs] Re: freeware CAD EAGLE
>
> Alan,
> Now I understand why you want to mill your PC boards! Those are very
> nice looking engines. I have a fascination for mechanical technology,
> especially engines and steam. The National Museum of American History
> is my favorite Smithsonian museum. Plus, I'm something of a railfan.
> I arranged to have our QRP to the Field annual operating event last
> year at the Southeastern Railway Museum. It was fun operating from a
> caboose!
>
> Speaking of mechanical technology, have you seen Rich Meiss's work
> with Morse keys? I have a link to his three sites on my page, and I
> just received a CD from him yesterday. He's going to have his stuff
> at Four Days in May this year at Dayton. With your skills and
> equipment, I imagine you could turn out some darned nice stuff as
> well, if you had the time.
>
> My problem is 1) the lack of funds to put into the lathes and other
> tools I'd need to do mechanical work like both you and he do (I'd have
> to sell all of my ham radio gear), and 2) lack of good shop skills and
> experience. The good thing about Rich's simpler designs is that they
> can be done with a hacksaw and belt sander, and I've ben out pricing
> belt 1" / combo belt sanders.
>
> As far as building radio equipment, I'd like to be fully homebrew
> eventually. The 15 meter SSB/CW transmitter and its peripherals like
> a VFO stabilizer circuit and PIC-based counter/display is taking up my
> time right now. Then, I'll get back on the 17/12 meter SSB
> transceiver based on the Belthorn SSB IF board you saw on the site. I
> have an SW-80+ kit to build with the local QRP club next month, and I
> have a 40 meter homebrew version as separate VFO, receiver and
> transmitter boards ready to build, done in Eagle.
>
> I sold all my modern equiqment last spring when I got back into the
> hobby, and I bought several old Heathkit monobanders and three AC
> power supplies to restore and sell. Eventually, the HW-101 that is my
> primary QRO rig will probably go, as well. I have a full set of
> Heathkit HF oscillator crystals, SSB and CW filters, a power
> transformer and filter choke from an SB-401, and an LMO. Eventually
> that's going into a chassis as a solid state up to the driver and
> finals 5-band rig.
>
> 73,
> Ted

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

[much snippage]

> For now, I intend to get going on PCB's. And there's the
> PCB router parts that are taking up space and not being
> useable... yet.

Just a thought. If you want, you are welcome to borrow
my floating Z head assembly for a Sherline. I've got too
many projects on my plate right now, to reactive the
mechanical etching project.

Let me know,

-Wayne

[eve more snippage]

>
> --- In Homebrew_PCBs@yahoogroups.com, "Alan Marconett" <KM6VV@...> wrote:
>
> [much snippage]
>
> > For now, I intend to get going on PCB's. And there's the
> > PCB router parts that are taking up space and not being
> > useable... yet.
>
> Just a thought. If you want, you are welcome to borrow
> my floating Z head assembly for a Sherline. I've got too
> many projects on my plate right now, to reactive the
> mechanical etching project.
>
> Let me know,
>
> -Wayne

--- In Homebrew_PCBs@yahoogroups.com, "Alan Marconett" <KM6VV@...> wrote:
>
> HI Ted,
>
> Thanks for the kind words!
>
> Yes, I'm fascinated with the simple, elegant steam engine designs of the
> past. Not so much on the RR's, but that may develop later...
>
> I have a little QRP paddle, and I've drawn it up. I've also taken a
GOOD
> look at some of the really nice keys out there. I believe I could
design
> and build a reasonable hand key. Just too many other interesting
things to
> do!
>
> I have a few small CW transmitters in the closet that I intend to
restore.
> A Johnston and a Heathkit.
>
> For now, I intend to get going on PCB's. And there's the PCB router
parts
> that are taking up space and not being useable... yet.
>
> I'm still making minor improvements in my board layout, and in the
parts I
> incorporated into my design. Seems they don't look equally well when it
> comes to exporting Gerber files from Eagle. Outlines which must be
on the
> wrong layers, funny pad sizes/shapes. And now it appears that I'm a
"little
> too big" in my layout (pushing the envelope), I've lost part of my
board!
>
> I'm using DeskPCB to do generate the isolation toolpaths, and export
in DXF.
> This allows me to import into Vector CAD/CAM and examine it thoroughly.
>
> Can I re-center the border on my board? Just erase and redraw it?
>
> 73's,
>
> Alan KM6VV
---snip---

> Alan,
> I'm not quite sure what you mean when you say recenter the border. On
> a few occasions, I've manage to lose one of the border lines on my
> board, on-screen anyway. I don't know how, I just accidentally
> deleted it, probably while deleting a polygon.
>
> You can recenter or otherwise move the whole layout, or a part of the
> layout, in effect changing the distance to the border or edge of the
> board, by grouping and moving it. The Group icon is the larger of
> the two open/closed brackets-looking things on the left. Select that,
> then turn on all of your normal layers, and draw a rectangle around
> all the components you need to group and move. They will turn red and
> black highlghted on-screen. Then click the Move icon, and use
> RIGHT-CLICK to drag the layout to wherever you want it.
>
> By the way, I figured out how to make multipart ICs yesterday. I was
> working on a 74HC4053 MUX/DEMUX (actually, three single pole double
> throw switches with 5V logic control lines). I wanted each switch
> section to appear where it needed to be in the schematic, rather than
> having all net wires coming in to a 16-pin symbol. Op amps are done
> the same way. I drew each switch section symbol with its pins and
> saved it under a name, beginning with 74HC4053A (note-I changed the
> pin names to the actual pin numbers of the DIP package). The next
> section was then 74HC4053B, etc. The last section was the ground,
> supply, and two other pins that are usually tied to ground. The
> kicker is to assign the first symbols pins as swap level 0, the second
> swaplevel 1, etc (that's a drop-down box).
>
> When creating the 74HC4053 device, import first the 74HC4053A symbol,
> and look at the drop-down boxes at the upper left. Keep this one at
> swaplevel 0, and make sure addlevel is "Next". Then, import the next
> symbol with its set of pins, and set swaplevel to 1, and addlevel to
> "next". Just put the second symbol right on top of the first. The
> third switch section will be swaplevel 2, addlevel "next". The 4th
> section is the power section, and it's swaplevel 3, but assign
> addlevel or "Always" if you want it to always be shown on the diagram.
> If you want it to show only when you type "Invoke" to show power
> sections on the diagram, set addlevel to "Must". (I used always). Put
> it somewhere beside the pile of 3 switch section symbols on the screen.
>
> Then create the device by clicking on "New" to bring up the package, a
> 16-pin DIP. Then "Connect" to synchronize the symbol pins with the
> actual pad numbers one by one. That's easy if you've changed the pin
> names to match. Finish the device by assigning a default designator,
> U or IC or whatever, add a description, and save the library.
>
> When you call the part into the schematic, the first switch section
> will appear, along with the power section. Click again, and the
> second section will appear, again, and the third will appear. Now, if
> you're using the device to switch between two LC filter sections, one
> narrow and one wide band, for example, you can drag one section to the
> input, and drag one to the output. You can mirror one of the sections
> so it's facing the filters in the correct orientation. The schematic
> looks a lot cleaner and easier to read.
>
> By the way, this IC draws only 4 uA, as opposed to the 16 to 50 mA or
> more of a sensitive relay. Steve Weber, KD1JV used the device to do
> the bidirectional mixer switching in his Minimalisist SSB transceiver.
> I've been using it in my designs ever since.
>
> Ted
> --- In Homebrew_PCBs@yahoogroups.com, "Alan Marconett" <KM6VV@...> wrote:
>
>>HI Ted,
>>