Post by thread:[EE] Eagle question

Hello, I need to make (home-make) a 2 layered PCB design...It's gonna be about 12x9 cm. I'm using 5 DIP ICs, lots of resistors, lots of TO92 transistors, LEDs, etc. My question is: How do I tell the autorouter not to route my DIP ICs in the top layer...I mean, DIP ICs, if placed in the top layer, need to be soldered in the opposite (bottom) layer...right?...so why does eagle begins traces from some IC's pads in the top layer and some other traces in the bottom layer...? Thanks for your time Julio -- http://www.piclist.com hint: To leave the PICList spam_OUTpiclist-unsubscribe-requestTakeThisOuTmitvma.mit.edu>

On Wednesday, May 21, 2003, at 14:55 Australia/Sydney, Julio Jumpa wrote: > How do I tell the autorouter not to route my DIP ICs in the top > layer...I > mean, DIP ICs, if placed in the top layer, need to be soldered in the > opposite (bottom) layer...right? Correct. > ...so why does eagle begins traces from some > IC's pads in the top layer and some other traces in the bottom > layer...? Because EAGLE assumes (correctly) that if you have a 2 layered board, then each signal layer is available for tracks. If its a home made board there is no reason why you can't just solder top and bottom of the ICs Otherwise, if you insist on NOT allowing EAGLE to route to ONLY the ICs, then you can draw a polygon around the IC pads on the trestrict (I think) layer. Regards, Sean -- http://www.piclist.com hint: To leave the PICList .....piclist-unsubscribe-requestKILLspam@spam@mitvma.mit.edu>

If its a home made board there is no reason why you can't just solder top and bottom of the ICs Well, sockets make this nearly impossible, for instance. Other components are inherently difficult to solder on both sides (relays and displays are particularly nasty...) Otherwise, if you insist on NOT allowing EAGLE to route to ONLY the ICs, then you can draw a polygon around the IC pads on the trestrict (I think) layer. That's correct. This is actually a real PITA. If you draw a large rectangle around the DIP, it will prevent the autorouter from routing topside traces between the pins or under the DIP, which would be desirable. You can put polygons on each pin, but that takes a while and the DRC will complain about the top-level PADS being in tRestrict. Apparently the correct solution is to draw a small rectangle using "wires" in tRestrict around each pin. Grr.. IMO, it better to route (automatically or manually) everything you can (and hopefully all of your "troublesome" pins) on the bottom layer, and then route (probably manually) the remaining connection on the top layer, more or less as if you were doing a single-sided board with jumpers. (But this in turn results in a board that is a bit "weird" should you get it professionally manufactured - I understand from a previous discussion that it's "nice" if there's an equal area of traces on each side of the board.) BillW -- http://www.piclist.com hint: To leave the PICList piclist-unsubscribe-requestKILLspammitvma.mit.edu>

Bill, > Well, sockets make this nearly impossible, for instance. Yeah, fair enough. Don't use them, myself. > Other components are inherently difficult to solder on both sides > (relays and displays are particularly nasty...) Yeah, I'm spoilt with through-hole plating on all my prototype boards. But he did say just the ICs. Looks like I was able to help him out anyway! ;-) Cheers, Sean -- http://www.piclist.com hint: To leave the PICList .....piclist-unsubscribe-requestKILLspam.....mitvma.mit.edu>

Hi J(h)ulio, > I need to use sockets for ICs, so, it's gonna be kind of difficult to > solder > the socket on the top layer. Yes. Understand. > the polygon on the trestrinct layer solved the problem > thank you very much No worries, mate! As soon as I clicked "Send", I was worried I had written the wrong layer. I had to go out, so I couldn't fire up EAGLE to check. Glad it worked! Cheer, Sean -- http://www.piclist.com hint: To leave the PICList EraseMEpiclist-unsubscribe-requestspam_OUTTakeThisOuTmitvma.mit.edu>

> Well, sockets make this nearly impossible, for instance. Not if you use the "turned pin" type sockets. These are the only ones I will use anyway, having had horrible experiences with cheaper ones, and the happen to have a significant length of pin exposed that allows you to solder on the top side. They also make excellent "pin savers" for IC's that require frequent removal, such as EPROM's going into a UV eraser. -- http://www.piclist.com hint: To leave the PICList piclist-unsubscribe-requestspam_OUTmitvma.mit.edu>

De: "Julio Jumpa" <@spam@juliojumpaKILLspaminfonegocio.net.pe> Para: "pic microcontroller discussion list" <KILLspamPICLISTKILLspamMITVMA.MIT.EDU> Asunto: Re: [EE] Eagle question Fecha: Miircoles, 21 de Mayo de 2003 02:17 a.m. hi, I need to use sockets for ICs, so, it's gonna be kind of difficult to solder the socket on the top layer. the polygon on the trestrinct layer solved the problem thank you very much Julio ----- Original Message ----- From: "Sean Alcorn - PIC Stuff" <RemoveMEpicstuffTakeThisOuTSDALCORN.COM> To: <spamBeGonePICLISTspamBeGoneMITVMA.MIT.EDU> Sent: Wednesday, May 21, 2003 1:32 AM Subject: Re: [EE] Eagle question -- http://www.piclist.com hint: To leave the PICList TakeThisOuTpiclist-unsubscribe-requestEraseMEspam_OUTmitvma.mit.edu>

> Hello, > I am an avid user of EAGLE, but one thing has eluded me. Is there a > way to turn off the little origin cross hairs for text in the > schematic editor? It makes the documents look somewhat bad having a > little plus sign next to every line of text. > Glenn Not that I know of. However unless there is some kind of issue with your particular printer drivers, that origin marker doesn't show up on a print. The torigin and borigin layer markers will unless you turn off that layer. Rob

>> I am an avid user of EAGLE, but one thing has eluded me. Is there a >> way to turn off the little origin cross hairs for text in the >> schematic editor? It makes the documents look somewhat bad having a >> little plus sign next to every line of text. >> I don't see the crosshairs on either print output OR image export of schematics. Are you talking about just on the active display? BillW

> I am an avid user of EAGLE, but one thing has eluded me. Is there a > way to turn off the little origin cross hairs for text in the > schematic editor? It makes the documents look somewhat bad having a > little plus sign next to every line of text. It shouldn't come up when you print out the schematic... If it does you can always try Export.Image, which works fine for me. on the board you can hide the white croshair by hiding the Torigin and Borigin layers (type "disp -torig -borig"). Good luck, Christian VA2CBW

Yes, I meant on the active display, since I was doing screen captures. I will try image export, it sounds like a better way of doing things anyway. Thanks all, Glenn On 4/23/05, William Chops Westfield <RemoveMEwestfwTakeThisOuTmac.com> wrote: {Quote hidden}> >> I am an avid user of EAGLE, but one thing has eluded me. Is there a > >> way to turn off the little origin cross hairs for text in the > >> schematic editor? It makes the documents look somewhat bad having a > >> little plus sign next to every line of text. > >> > I don't see the crosshairs on either print output OR image export of > schematics. > Are you talking about just on the active display? > > BillW > > -

I have a standard 2.54mm 3 pin header on an Eagle Schematic. Pin1 Gnd, Pin2, Supply, Pin3 to Pic Pin, I would like to add 2 rows of 3, on the board, so it would be like a small proto area in case I need to connect a wire or add a cap or resistor to smooth out a signal. So, GND would be connected to the two pins in front of it on the board like a solderless bread board. What symbol would this be ? Should I just use a jumper symbol or can you draw something like this on the schematic ? Thanks in advance, Kevin

The simplest way is adding vias in the PCB. No schematic need. Vasile On 11/29/05, Kevin <kbenEraseME.....dca.net> wrote: {Quote hidden}> I have a standard 2.54mm 3 pin header on an Eagle Schematic. > Pin1 Gnd, Pin2, Supply, Pin3 to Pic Pin, I would like to add > 2 rows of 3, on the board, so it would be like a small > proto area in case I need to connect a wire or add a cap or > resistor to smooth out a signal. So, GND would be connected > to the two pins in front of it on the board like a > solderless bread board. What symbol would this be ? Should > I just use a jumper symbol or can you draw something like > this on the schematic ? > > Thanks in advance, > Kevin > > > -

On Tue, 29 Nov 2005, Vasile Surducan wrote: > The simplest way is adding vias in the PCB. No schematic need. > > Vasile > > On 11/29/05, Kevin <EraseMEkbendca.net> wrote: > > I have a standard 2.54mm 3 pin header on an Eagle Schematic. > > Pin1 Gnd, Pin2, Supply, Pin3 to Pic Pin, I would like to add > > 2 rows of 3, on the board, so it would be like a small > > proto area in case I need to connect a wire or add a cap or > > resistor to smooth out a signal. So, GND would be connected > > to the two pins in front of it on the board like a > > solderless bread board. What symbol would this be ? Should > > I just use a jumper symbol or can you draw something like > > this on the schematic ? > > > > Thanks in advance, > > Kevin > > > > Yes, I could try that, however, Olin has this on his quick proto board. www.embedinc.com/products/qprot01/qprot2.pdf I am looking for something similiar to sheet 6. Unfortunately, it is in pdf format, so I do not know how he did it on the schematic ?

Kevin, As far as I can tell, Olin has just used some pin headers from the PINHEAD library in EAGLE (he may not have used EAGLE) and connected his VCC and GND to the headers. I've used this on many boards and it seems to work fine. Is this what you were asking? Sorry, I don't think I completely understood your original question. Hope this helps -Tarun. On 11/29/05, Kevin <RemoveMEkbenEraseMEEraseMEdca.net> wrote: {Quote hidden}> > On Tue, 29 Nov 2005, Vasile Surducan wrote: > > > The simplest way is adding vias in the PCB. No schematic need. > > > > Vasile > > > > On 11/29/05, Kevin <RemoveMEkbenspam_OUTKILLspamdca.net> wrote: > > > I have a standard 2.54mm 3 pin header on an Eagle Schematic. > > > Pin1 Gnd, Pin2, Supply, Pin3 to Pic Pin, I would like to add > > > 2 rows of 3, on the board, so it would be like a small > > > proto area in case I need to connect a wire or add a cap or > > > resistor to smooth out a signal. So, GND would be connected > > > to the two pins in front of it on the board like a > > > solderless bread board. What symbol would this be ? Should > > > I just use a jumper symbol or can you draw something like > > > this on the schematic ? > > > > > > Thanks in advance, > > > Kevin > > > > > > > Yes, I could try that, however, Olin has this on his quick > proto board. > www.embedinc.com/products/qprot01/qprot2.pdf > I am looking for something similiar to sheet 6. > Unfortunately, it is in pdf format, so I do not know how he > did it on the schematic ? > >

Tarun Grover wrote: > As far as I can tell, Olin has just used some pin headers from the > PINHEAD library in EAGLE No way. The Cadsoft libraries suck. Besides, a pin header wouldn't solve this problem. > (he may not have used EAGLE) I did use Eagle. ****************************************************************** Embed Inc, Littleton Massachusetts, (978) 742-9014. #1 PIC consultant in 2004 program year. http://www.embedinc.com/products

Olin, On Tue, 29 Nov 2005 14:25:09 -0500, Olin Lathrop wrote: {Quote hidden}> Tarun Grover wrote: > > As far as I can tell, Olin has just used some pin headers from the > > PINHEAD library in EAGLE > > No way. The Cadsoft libraries suck. Besides, a pin header wouldn't solve > this problem. > > > (he may not have used EAGLE) > > I did use Eagle. Tease! I've been meaning to ask how you did the 5-strips in Eagle, because I haven't managed to solve it. Is there a demon trick that you've discovered, or something obvious that I've missed? They appear in the schematic, so I don't think it's done at the board stage, so how do you tell Eagle to connect pins for a single component together? Cheers, Howard Winter St.Albans, England

Howard Winter wrote: > Tease! I've been meaning to ask how you did the 5-strips in Eagle, > because I haven't managed to solve it. Is there a demon trick that > you've discovered, or something obvious that I've missed? They appear > in the schematic, so I don't think it's done at the board stage, so how > do you tell Eagle to connect pins for a single component together? You put copper where you want it in the package definition, then raise the blast shields when running DRC. ****************************************************************** Embed Inc, Littleton Massachusetts, (978) 742-9014. #1 PIC consultant in 2004 program year. http://www.embedinc.com/products

Maybe a dumb question, I have a motor chip MC33887, which has a few features, like current use of motor. I wanted to define two gnd classes one for powering the motor and one for the current sense. This would make it easier to auto route, since the motor current would be on a 40 mil route and the motor current sense would be on a 20 mil route trace. Does this make sense to do ? Is it possible to define two ground classes for one chip ? Thanks, Kevin

Kevin wrote: > Is it possible to define two ground classes for one chip ? Classes (Eagle) have nothing to do with chips (devices), just nets. Each net can only have one class. ****************************************************************** Embed Inc, Littleton Massachusetts, (978) 742-9014. #1 PIC consultant in 2004 program year. http://www.embedinc.com/products

> > Maybe a dumb question, I have a motor chip MC33887, which > has a few features, like current use of motor. I wanted to > define two gnd classes one for powering the motor and one > for the current sense. This would make it easier to auto > route, since the motor current would be on a 40 mil route > and the motor current sense would be on a 20 mil route > trace. Does this make sense to do ? Is it possible to > define two ground classes for one chip ? > > Thanks, > Kevin

On Jan 9, 2006, at 4:56 AM, Olin Lathrop wrote: >> Is it possible to define two ground classes for one chip ? > > Classes (Eagle) have nothing to do with chips (devices), just nets. > Each net can only have one class. You CAN have several "power" "direction" pins with different names, such as "AGND", "PGND", "LGND", and so on (and then AGND@2, etc.) Connecting multiple "different" signals to the same copper on the PCB or net on a schematic seems to be one of the "FAQ" issues for Eagle users; various sorts of zero-ohm resistors tend to be used. BillW

On Mon, 9 Jan 2006, Olin Lathrop wrote: > Kevin wrote: >> Is it possible to define two ground classes for one chip ? > > Classes (Eagle) have nothing to do with chips (devices), just nets. Each > net can only have one class. Isn't this why 'zero ohm jumper' parts using overlapping pads or traces are configured into Eagle libraries ? Peter

Peter wrote: > Isn't this why 'zero ohm jumper' parts using overlapping pads or traces > are configured into Eagle libraries ? I don't know, but that's why I have a library of "shorts". ****************************************************************** Embed Inc, Littleton Massachusetts, (978) 742-9014. #1 PIC consultant in 2004 program year. http://www.embedinc.com/products

On Mon, 9 Jan 2006, David VanHorn wrote: > > > > > > Isn't this why 'zero ohm jumper' parts using overlapping pads or traces > > are configured into Eagle libraries ? > > > It's an easy hack, and works with most programs. It's what I use with the > old DOS orcad. The program never sees the nets as connected. > -- Thanks for the repsonses, I should have enough info to do what I need. ~Kevin

On Mon, 9 Jan 2006, David VanHorn wrote: >> >> >> Isn't this why 'zero ohm jumper' parts using overlapping pads or traces >> are configured into Eagle libraries ? > > > It's an easy hack, and works with most programs. It's what I use with the > old DOS orcad. The program never sees the nets as connected. What about DRC ? Do you put a via at the joint to shut it up ? That should connect the networks and Eagle complains about such things. Peter

On Mon, 9 Jan 2006, Olin Lathrop wrote: > Peter wrote: >> Isn't this why 'zero ohm jumper' parts using overlapping pads or traces >> are configured into Eagle libraries ? > > I don't know, but that's why I have a library of "shorts". Ok, so do I, but Eagle does not like it when one connects nets in the PCB. What is the trick to avoid that ? Do you have an actual part that looks like a 'jumper' or something and whose pattern has overlapping traces ? Doesn't DRC/ERC complain about that ? Peter

Peter wrote: > Do you have an actual part that > looks like a 'jumper' or something and whose pattern has overlapping > traces ? Yes, my shorts look like a slightly thicker line in the schematic. > Doesn't DRC/ERC complain about that ? Not ERC, but DRC does. ****************************************************************** Embed Inc, Littleton Massachusetts, (978) 742-9014. #1 PIC consultant in 2004 program year. http://www.embedinc.com/products

Peter wrote: {Quote hidden}>On Mon, 9 Jan 2006, Olin Lathrop wrote: > > > >>Peter wrote: >> >> >>>Isn't this why 'zero ohm jumper' parts using overlapping pads or traces >>>are configured into Eagle libraries ? >>> >>> >>I don't know, but that's why I have a library of "shorts". >> >> > >Ok, so do I, but Eagle does not like it when one connects nets in the >PCB. What is the trick to avoid that ? Do you have an actual part that >looks like a 'jumper' or something and whose pattern has overlapping >traces ? Doesn't DRC/ERC complain about that ? > >Peter > > As William already mentionned, a 0 ohm SMD is used. Gaston

Gaston Gagnon wrote: > As William already mentionned, a 0 ohm SMD is used. But then you actually have to place a 0ohm "resistor" on the board at production time. ****************************************************************** Embed Inc, Littleton Massachusetts, (978) 742-9014. #1 PIC consultant in 2004 program year. http://www.embedinc.com/products

Remember what ERC and DRC are for....to warn YOU that something is wrong and could be a problem. In some packages, you get a warning for parts that are overlapping, but if thats OK (say a connector who's ears are above the 0201 part below it) then don't worry about it. Same with ERC from Eagle, I get ERC saying that something is too close to something else, but the ratsnest is fine so thats the end result....interpret the reports and determine if what you are seeing really is an issue. For connecting two ground...digital and analog, I always find its a good idea to put something there....zero ohm, ferrite beat....but a package so you can experiment if you do have issues. --------------------------------- Yahoo! Photos – Showcase holiday pictures in hardcover Photo Books. You design it and we’ll bind it!

On Tue, 10 Jan 2006, Gaston Gagnon wrote: {Quote hidden}> Peter wrote: > >> On Mon, 9 Jan 2006, Olin Lathrop wrote: >> >> >>> Peter wrote: >>> >>>> Isn't this why 'zero ohm jumper' parts using overlapping pads or traces >>>> are configured into Eagle libraries ? >>>> >>> I don't know, but that's why I have a library of "shorts". >>> >> >> Ok, so do I, but Eagle does not like it when one connects nets in the PCB. >> What is the trick to avoid that ? Do you have an actual part that looks >> like a 'jumper' or something and whose pattern has overlapping traces ? >> Doesn't DRC/ERC complain about that ? >> >> Peter >> > As William already mentionned, a 0 ohm SMD is used. > Gaston Ok, thanks. I was thinking about the overlapping traces as Olin wrote. Hmm. Would a *very* short 0 ohm resistor be a ERC violation ? I do not expect Eagle to be smart enough to get away with that but it does not hurt to ask ... thanks, Peter

On Wed, 11 Jan 2006, alan smith wrote: {Quote hidden}> Remember what ERC and DRC are for....to warn YOU that something is > wrong and could be a problem. In some packages, you get a warning for > parts that are overlapping, but if thats OK (say a connector who's > ears are above the 0201 part below it) then don't worry about it. > Same with ERC from Eagle, I get ERC saying that something is too close > to something else, but the ratsnest is fine so thats the end > result....interpret the reports and determine if what you are seeing > really is an issue. > > For connecting two ground...digital and analog, I always find its a > good idea to put something there....zero ohm, ferrite beat....but a > package so you can experiment if you do have issues. Good ideas to keep in mind. Thanks. Peter

On 1/11/06, Olin Lathrop <RemoveMEolin_piclistTakeThisOuTspamembedinc.com> wrote: > Peter wrote: > > Do you have an actual part that > > looks like a 'jumper' or something and whose pattern has overlapping > > traces ? > > Yes, my shorts look like a slightly thicker line in the schematic. > > > Doesn't DRC/ERC complain about that ? > > Not ERC, but DRC does. There is a trick for this. Use a standard two pin whatever as a jumper. After the board is ready and you don't need anymore the drc feature change in library the two pin device with a short circuit and update the lib. Voilla. cheers, Vasile

Vasile Surducan wrote: > There is a trick for this. Use a standard two pin whatever as a > jumper. After the board is ready and you don't need anymore the drc > feature change in library the two pin device with a short circuit and > update the lib. Voilla. Hmm. As long as you actually remember to do it. ****************************************************************** Embed Inc, Littleton Massachusetts, (978) 742-9014. #1 PIC consultant in 2004 program year. http://www.embedinc.com/products

On Jan 12, 2006, at 1:16 PM, Olin Lathrop wrote: >> After the board is ready and you don't need anymore the drc >> feature change in library the two pin device with a short >> circuit and update the lib. Voilla. > > Hmm. As long as you actually remember to do it. > If you don't remember, you have to install a jumper; shouldn't be TOO big a deal... So can you just do this with an alternate package and a "change package" command on your jumper? Or two separate libraries and and "update shorts = shorts-w-gaps" command? That'd be pretty easy to script or ULP into a general purpose "pre-production" script... Nice... BillW

On 1/12/06, Olin Lathrop <EraseMEolin_piclistspamspamBeGoneembedinc.com> wrote: > Vasile Surducan wrote: > > There is a trick for this. Use a standard two pin whatever as a > > jumper. After the board is ready and you don't need anymore the drc > > feature change in library the two pin device with a short circuit and > > update the lib. Voilla. > > Hmm. As long as you actually remember to do it. There are many other shits on Eagle. For instance if you have more than 300-400 components and about of 1500- routes or more, even if you keep off the polygon processing, it works like a snail on 1GHz processor. I'm wasting my patience... cheers, Vasile

William Chops Westfield wrote: > So can you just do this with an alternate package and a "change > package" command on your jumper? Or two separate libraries and > and "update shorts = shorts-w-gaps" command? That'd be pretty > easy to script or ULP into a general purpose "pre-production" > script... Nice... If you're going to do that (and I'm still uneasy about this), you have to make sure nothing gets routed between the pads of the package. At least put Trestrict and Brestrict rectangles in the package definition. ****************************************************************** Embed Inc, Littleton Massachusetts, (978) 742-9014. #1 PIC consultant in 2004 program year. http://www.embedinc.com/products

On Thu, 12 Jan 2006, Vasile Surducan wrote: {Quote hidden}> On 1/11/06, Olin Lathrop <RemoveMEolin_piclistKILLspamembedinc.com> wrote: >> Peter wrote: >>> Do you have an actual part that >>> looks like a 'jumper' or something and whose pattern has overlapping >>> traces ? >> >> Yes, my shorts look like a slightly thicker line in the schematic. >> >>> Doesn't DRC/ERC complain about that ? >> >> Not ERC, but DRC does. > > There is a trick for this. Use a standard two pin whatever as a jumper. > After the board is ready and you don't need anymore the drc feature > change in library the two pin device with a short circuit and update > the lib. Voilla. Does this change propagate to the current project ? When I reopen it or whenever ? This could be a good solution. Make a smd 'zero ohm' part, call it 'tbs' (to be shorted) and when done actually substitute the library in which it is defined with another where the library part is actually shorted, reopen the project, and verify that the board does not do anything stupid, then CAM it ? This sounds like a Rube Goldberg solution (like so many others ...). But will it work ? Vasile, when you change the library, does it affect all the projects that use it ? What if they are open (the projects) ? thanks, Peter

On Thu, 12 Jan 2006, Olin Lathrop wrote: > Vasile Surducan wrote: >> There is a trick for this. Use a standard two pin whatever as a >> jumper. After the board is ready and you don't need anymore the drc >> feature change in library the two pin device with a short circuit and >> update the lib. Voilla. > > Hmm. As long as you actually remember to do it. This could be scripted I think. No ? Peter

> when you > change the library, does it affect all the projects that use > it ? No, only when you do an update (either of that specific library or of all libraries). A .brd file contains a *copy* of the relevant library part, which is updated only when you do an update. You can even create a library from a .brd! Wouter van Ooijen -- ------------------------------------------- Van Ooijen Technische Informatica: http://www.voti.nl consultancy, development, PICmicro products docent Hogeschool van Utrecht: http://www.voti.nl/hvu

>> Hmm. As long as you actually remember to do it. > > This could be scripted I think. No ? How do you script rembering to run the script? Wouter van Ooijen -- ------------------------------------------- Van Ooijen Technische Informatica: http://www.voti.nl consultancy, development, PICmicro products docent Hogeschool van Utrecht: http://www.voti.nl/hvu

On Jan 13, 2006, at 10:44 AM, Wouter van Ooijen wrote: >> This could be scripted I think. No ? > > How do you script rembering to run the script? Default to having shorted shorts. Replace the DRC command with a "script rundrc" command or user buttom. You don't need to remember to short the shorts, you just need to remember to unshort them for purposes of running the DRC... BillW

On 1/13/06, Wouter van Ooijen <wouterSTOPspamspam_OUTvoti.nl> wrote: > > when you > > change the library, does it affect all the projects that use > > it ? > > No, only when you do an update (either of that specific library or of > all libraries). A .brd file contains a *copy* of the relevant library > part, which is updated only when you do an update. > > You can even create a library from a .brd! How? Vasile

On Fri, 13 Jan 2006, Wouter van Ooijen wrote: >> when you >> change the library, does it affect all the projects that use >> it ? > > No, only when you do an update (either of that specific library or of > all libraries). A .brd file contains a *copy* of the relevant library > part, which is updated only when you do an update. > > You can even create a library from a .brd! Aha! Thanks, this is useful. Is this fully recursive ? <g> Peter

Eagle questions: When performing auto route, is it possible to disallow diagonal tracks. ? When performing auto route is it possible to force all red tracks to be in one direction, and all blue track in the other direction, and to have this 100% enforced ? Is it possible to see the names of the pins of an IC, when I click on the pin, I get the of the entire IC rather than the name of the pin?

Will wrote: > Eagle questions: You're asking a lot of basic Eagle questions in a short time. While we're willing to help, you also have to do your part and *** READ THE MANUAL *** > When performing auto route, is it possible to disallow diagonal tracks. Yes. > When performing auto route is it possible to force all red tracks to be > in one direction, and all blue track in the other direction, No, you can't set these parameters by display color. You can set a preferred direction by layer, though. > and to have this 100% enforced? No, but it can be a strong suggestion. ****************************************************************** Embed Inc, Littleton Massachusetts, (978) 742-9014. #1 PIC consultant in 2004 program year. http://www.embedinc.com/products

> You're asking a lot of basic Eagle questions in a short time. While we're > willing to help, you also have to do your part and > > *** READ THE MANUAL *** > I did not find these things, but I _will_ try again. > > When performing auto route, is it possible to disallow diagonal tracks. > > Yes. > > > When performing auto route is it possible to force all red tracks to be > > in one direction, and all blue track in the other direction, > > No, you can't set these parameters by display color. You can set a > preferred direction by layer, though. I thought color and layer are the same thing Red=layer1 Blue=layer16 Basically, because I am using a strip board, all my tracks are in one direction. I can remove tracks with a face cutter, but I can't do diagonal, and all tracks in opposite direction must be implemented as a wire component on the "red" side. > > > and to have this 100% enforced? > > No, but it can be a strong suggestion. I really must enforce this, as I am using a vero board, there is no other way.

> > > > > When performing auto route is it possible to force all > red tracks to > > > be in one direction, and all blue track in the other direction, > > > > No, you can't set these parameters by display color. You can set a > > preferred direction by layer, though. > > I thought color and layer are the same thing > Red=layer1 > Blue=layer16 > Basically, because I am using a strip board, all my tracks > are in one direction. I can remove tracks with a face cutter, > but I can't do diagonal, and all tracks in opposite direction > must be implemented as a wire component on the "red" side. > You can change the colors and even layer names so it would not be a good idea to refer to traces by color. Referring to them by layer number would be best. > > > > > > and to have this 100% enforced? > > > > No, but it can be a strong suggestion. > > I really must enforce this, as I am using a Vero board, there > is no other way. Olin is right in that it isn't a 100% hard and fast rule for the autorouter (which isn't that great to begin with) but if you are patient with it and go back post-autoroute and clean up it will be fine. If you are going to the trouble of routing a circuit board, why not just skip the Vero board altogether and have a "real" PCB made. Lots of inexpensive sources, Olimex, barebones, pcbexpress and the list goes on. Or even etch it yourself, or get a used PCB mill from eBay. Cadsoft used to have a nice tutorial file on their page. It makes a good companion to the manual. Rob

Will wrote: > I thought color and layer are the same thing > Red=layer1 > Blue=layer16 No, that's just the default mapping. For example, my GRID_BRD ULP changes these to shades of gray for making an assembly drawing. I also have a script COLORS_BOARD that puts the colors back to the defaults I'm used to. ****************************************************************** Embed Inc, Littleton Massachusetts, (978) 742-9014. #1 PIC consultant in 2004 program year. http://www.embedinc.com/products

> Olin is right in that it isn't a 100% hard and fast rule for the > autorouter (which isn't that great to begin with) but if you are patient > with it and go back post-autoroute and clean up it will be fine. I still can't find how to disallow diagonal lines... > > If you are going to the trouble of routing a circuit board, why not just > skip the Vero board altogether and have a "real" PCB made. Lots of > inexpensive sources, Olimex, barebones, pcbexpress and the list goes on. > Or even etch it yourself, or get a used PCB mill from eBay. > > Cadsoft used to have a nice tutorial file on their page. It makes a > good companion to the manual. Because even the cheap ones will be more expensive than a vero board, and I am not into production, so why would I want to waste my time on professional boards? > > Rob

> > > > Olin is right in that it isn't a 100% hard and fast rule for the > > autorouter (which isn't that great to begin with) but if you are > > patient with it and go back post-autoroute and clean up it will be > > fine. > > I still can't find how to disallow diagonal lines... You do it by setting the "cost" for each of the autoroute passes (Busses, Route, Optimize1, etc) Key cost variables will be NonPref, ChangeDir, OrthStep, DiagStep, ExtStep, BonusStep. I don't know what version of Eagle you have but for mine (4.13 professional) this is all covered starting on page 137 of the printed manual. {Quote hidden}> > > > > If you are going to the trouble of routing a circuit board, why not > > just skip the Vero board altogether and have a "real" PCB > made. Lots > > of inexpensive sources, Olimex, barebones, pcbexpress and the list > > goes on. Or even etch it yourself, or get a used PCB mill from eBay. > > > > Cadsoft used to have a nice tutorial file on their page. > It makes a > > good companion to the manual. > > Because even the cheap ones will be more expensive than a > vero board, and I am not into production, so why would I want > to waste my time on professional boards? At what rate do you value your time? If you value it at $0/hr then a Vero board will be less expensive. But if you value your time at something like $30/hr or $50/hr then spending time cutting pads and fiddling with the Vero board and the autorouter settings can be more expensive than a ~$40 2 layer board. And you aren't restricting yourself to PTH parts or trying to find clever ways to mount SMT parts on a Vero board. But your time is your own so do as you wish. Rob

> Because even the cheap ones will be more expensive than a vero > board, and I am not into production, so why would I want to > waste my time on professional boards? waste your time => use veroboard waste your money => use a PCB house Personally (or should that be: professionally?) I use plug-in breadboards for a first attempt, if and when it works I Eagle/Olimex (there should be a verb for that). Wouter van Ooijen -- ------------------------------------------- Van Ooijen Technische Informatica: http://www.voti.nl consultancy, development, PICmicro products docent Hogeschool van Utrecht: http://www.voti.nl/hvu

Will wrote: > I still can't find how to disallow diagonal lines... Set the cost for diagonal steps and non-preferred direction really high. You have to make sure the preferred direction for that layer is set to what you want, of course. > Because even the cheap ones will be more expensive than a vero > board, and I am not into production, What is a Vero board? I can't picture something between a breadboard and an arbitrary circuit board where routing in Eagle is still a useful thing. If these tracks are already existing, how is routing in Eagle going to help. > so why would I want to waste my time on professional boards? Since you've already decided that it's a waste of time it leads me to believe any advice I would give in this area would also be a waste of time, so I won't. ****************************************************************** Embed Inc, Littleton Massachusetts, (978) 742-9014. #1 PIC consultant in 2004 program year. http://www.embedinc.com/products

Eagimex or eaglimex -Adam On 3/8/06, Robert Young <KILLspamrwybeakerspamBeGonehotmail.com> wrote: {Quote hidden}> > > > Personally (or should that be: professionally?) I use plug-in > > breadboards for a first attempt, if and when it works I > > Eagle/Olimex (there should be a verb for that). > > > > Stepping of the precipice at the edge of the on-topic cliff... > > Ealimex? > > Oligle? > > Rob > -

Wouter van Ooijen wrote: {Quote hidden}>> Because even the cheap ones will be more expensive than a vero >> board, and I am not into production, so why would I want to >> waste my time on professional boards? >> > > waste your time => use veroboard > waste your money => use a PCB house > > Personally (or should that be: professionally?) I use plug-in > breadboards for a first attempt, if and when it works I Eagle/Olimex > (there should be a verb for that). > > Wouter van Ooijen > > -- ------------------------------------------- > Van Ooijen Technische Informatica: http://www.voti.nl > consultancy, development, PICmicro products > docent Hogeschool van Utrecht: http://www.voti.nl/hvu > > > The problem with that, is that there isn't always an non-smd component available. I recently became interrested in FPGA's which are all smd components. That won't fit in a breadboard.

{Quote hidden}>-----Original Message----- >From: EraseMEpiclist-bouncesEraseMEmit.edu [@spam@piclist-bounces@spam@spam_OUTmit.edu] >Sent: 08 March 2006 16:54 >To: Microcontroller discussion list - Public. >Subject: Re: [EE] Eagle question > > >Will wrote: >> I still can't find how to disallow diagonal lines... > >Set the cost for diagonal steps and non-preferred direction >really high. You have to make sure the preferred direction for >that layer is set to what you want, of course. > >> Because even the cheap ones will be more expensive than a >vero board, >> and I am not into production, > >What is a Vero board? I can't picture something between a >breadboard and an arbitrary circuit board where routing in >Eagle is still a useful thing. If these tracks are already >existing, how is routing in Eagle going to help. Veroboard is a brand name for stripboard, very popular (or used to be) in Europe, but apparently virtualy unheard of in the US. Regards Mike ======================================================================= This e-mail is intended for the person it is addressed to only. The information contained in it may be confidential and/or protected by law. If you are not the intended recipient of this message, you must not make any use of this information, or copy or show it to any person. Please contact us immediately to tell us that you have received this e-mail, and return the original to us. Any use, forwarding, printing or copying of this message is strictly prohibited. No part of this message can be considered a request for goods or services. =======================================================================

On Mar 8, 2006, at 9:36 AM, Paul van der Linden wrote: > The problem with that, is that there isn't always an non-smd component > available. I recently became interrested in FPGA's which are all smd > components. That won't fit in a breadboard. > SMD components won't fit on a veroboard, either (certainly not WELL, anyway.) Getting Eagle to (nearly) generate veroboard layout/routes would be a reasonably useful thing, IMO. But I don't expect it would be easy. I have some eagle PCBs made BASED on veroboard layouts; perhaps I'll give it a try... BillW

> > I still can't find how to disallow diagonal lines... > > Set the cost for diagonal steps and non-preferred direction really high. > You have to make sure the preferred direction for that layer is set to what > you want, of course. But I don't understand which one, I get a popup windows with many tabs such as general, busses, route, optimize1, ..2 ..3 ..4 all those tab windows have a diagstep parameter. I tried increasing the value from 3 to 30, and all I got was that now everything goes diagonally. Then I tried setting it to zero, and again, all routes are diagonal? > > > Because even the cheap ones will be more expensive than a vero > > board, and I am not into production, > > What is a Vero board? I can't picture something between a breadboard and an > arbitrary circuit board where routing in Eagle is still a useful thing. If > these tracks are already existing, how is routing in Eagle going to help. I am using eagle to print the top view (red print) onto the board, this will show me where to put my parts, where to put the "red" wires, and where to cut wires on the other side. It gives the vero a prefessional look. > > > so why would I want to waste my time on professional boards? > > Since you've already decided that it's a waste of time it leads me to > believe any advice I would give in this area would also be a waste of time, > so I won't. What I meant was that I prefere to use a vero because I only have a few components and just one small IC, it should be done in a few hours.

Michael Rigby-Jones wrote: > Veroboard is a brand name for stripboard, very popular (or used to be) > in Europe, but apparently virtualy unheard of in the US. But doesn't that have pads prewired in strips of 5 or whatever. How is routing anything in Eagle going to help? Isn't the OP going to manually connect the strips? ****************************************************************** Embed Inc, Littleton Massachusetts, (978) 742-9014. #1 PIC consultant in 2004 program year. http://www.embedinc.com/products

On 3/8/06, Olin Lathrop <spamBeGoneolin_piclistKILLspamembedinc.com> wrote: > What is a Vero board? I can't picture something between a breadboard and an > arbitrary circuit board where routing in Eagle is still a useful thing. If > these tracks are already existing, how is routing in Eagle going to help. It's a one layer PCB with holes on 0.1" centers covering the board. The copper side is all vertical (or all horizontal) traces. If you develop your PCB layout with all vertical traces on the bottom, and all horizontal traces on the top, then you can make any PCB with veroboard and jumpers (to implement the top layer). You cut through traces on the bottom to break them into shorter runs. As with any complex PCB design this can be tedious to design by hand, so restricting an autorouter to produce designs that can be easily implemented on veroboard makes sense. A good example of veroboard construction can be had here: http://www.smspower.org/smsreader/prepare.html -Adam

Paul van der Linden wrote: >> Personally (or should that be: professionally?) I use plug-in >> breadboards for a first attempt, if and when it works I Eagle/Olimex >> (there should be a verb for that). > > The problem with that, is that there isn't always an non-smd component > available. I recently became interrested in FPGA's which are all smd > components. That won't fit in a breadboard. You can always use an adapter board. Although personally, I only breadboard small "risky" parts of a design. Since we usually check the schematic and the PCB layout carefully, there are only one or maybe two mistakes in the first prototype. I prefer to cut traces and greenwire the PCB, rather than breadboard a complex design on a breadboard. As Wouter mentioned, it's always a tradeoff between time and money. Best regards, Vitaliy

M. Adam Davis wrote: > A good example of veroboard construction can be had here: > http://www.smspower.org/smsreader/prepare.html I still don't understand. These pictures show strips on one side and nothing on the other. So the bare side is going to be implemented with jumpers anyway which are not restricted to any particular direction and can cross over each other, unlike routing in an Eagle plane. The OP said this was a "simple" one-off test, so why not just wire it by hand? He'd be done by now. Or go all the way and make a PCB. How is anything on one of these boards going to have the "professional" look he says he wants? ****************************************************************** Embed Inc, Littleton Massachusetts, (978) 742-9014. #1 PIC consultant in 2004 program year. http://www.embedinc.com/products

On 3/8/06, Wouter van Ooijen <.....wouterspam_OUTvoti.nl> wrote: > > Because even the cheap ones will be more expensive than a vero > > board, and I am not into production, so why would I want to > > waste my time on professional boards? > > waste your time => use veroboard > waste your money => use a PCB house waste your money once => buy your inhouse PCB maker device > > Personally (or should that be: professionally?) I use plug-in > breadboards for a first attempt, if and when it works I Eagle/Olimex > (there should be a verb for that). Eaglex or poor's man pcb house ? greetings, Vasile

>> waste your time => use veroboard >> waste your money => use a PCB house > > waste your money once => buy your inhouse PCB maker device waste your health => make your own PCBs? Wouter van Ooijen -- ------------------------------------------- Van Ooijen Technische Informatica: http://www.voti.nl consultancy, development, PICmicro products docent Hogeschool van Utrecht: http://www.voti.nl/hvu

> The problem with that, is that there isn't always an non-smd > component > available. I recently became interrested in FPGA's which are all smd > components. That won't fit in a breadboard. For an FPGA with 100+ pins a breadboard might not be a good idea (note: trimming the message you reply to is definitely a good idea!). But in general SMD components can be used in breadboards with an appropriate SMD-to-DIP PCB. If none exist you can always Ealimex one. Wouter van Ooijen -- ------------------------------------------- Van Ooijen Technische Informatica: http://www.voti.nl consultancy, development, PICmicro products docent Hogeschool van Utrecht: http://www.voti.nl/hvu

>But doesn't that have pads prewired in strips >of 5 or whatever. No they are continuous strips the length of the board. >How is routing anything in Eagle going to help? I don't really think it is, but I guess it allows him to draw the circuit and attempt to do a layout with only vertical and horizontal traces. Not sure that it will do efficient traces though. >Isn't the OP going to manually connect the strips? Yes, what he is looking to do is have the bottom layer as the copper strips on the board, and the top layer as the jumper wires. So what he needs to do is set the thing to 0.1" pitch for each, but I suspect he is going to have to use insulated wire anyway. I cannot figure out how other components are going to get laid out either, unless he has a heap of footprints for C's and R's with different hole spacings on the footprints. Otherwise there will be excess jumpers to work to standard footprints.

On 3/9/06, Wouter van Ooijen <TakeThisOuTwouter.....TakeThisOuTvoti.nl> wrote: > >> waste your time => use veroboard > >> waste your money => use a PCB house > > > > waste your money once => buy your inhouse PCB maker device > > waste your health => make your own PCBs? good :) Notice I didn't said "homebrew". I said inhouse (with proffesional tools). Vasile

> >> waste your time => use veroboard > >> waste your money => use a PCB house > > > > waste your money once => buy your inhouse PCB maker device > > waste your health => make your own PCBs? > > waste your mind => go into design, engineering and > programming.. xxx000 of course 'go into' is bad, you should use a structured programming construct! Wouter van Ooijen -- ------------------------------------------- Van Ooijen Technische Informatica: http://www.voti.nl consultancy, development, PICmicro products docent Hogeschool van Utrecht: http://www.voti.nl/hvu

On Mar 9, 2006, at 4:33 AM, Vasile Surducan wrote: > waste your money once => buy your inhouse PCB maker device > When stripboard WORKS, I think it tends to go faster than easier than any actual PCB manufacturing process. (The holes are pre-drilled, the "cuts" made tend to be fewer than the holes you'd have to drill on a real PCB, and there's no etch step at all.) (I HAVE the inhouse PCB maker device (an LPKF), and while it's quicker than going out, I wouldn't want to race someone with a finished stripboard design from "design done" to "assembled board.") BillW

On Wed, 8 Mar 2006, Olin Lathrop wrote: > Michael Rigby-Jones wrote: >> Veroboard is a brand name for stripboard, very popular (or used to be) >> in Europe, but apparently virtualy unheard of in the US. > > But doesn't that have pads prewired in strips of 5 or whatever. How is > routing anything in Eagle going to help? Isn't the OP going to manually > connect the strips? If one forces the layout program to make only vertical connections on the component side and only horizontal on the layout side, with a sizeable modulus (=0.1"), then one can 'convert' the resulting layout into traces to be cut on the back and wire bridges to be put in on the front. There exists a layout program that generates layouts specifically for Veroboards (in color). I do not remember what it is called. Peter

On 3/9/06, William Chops Westfield <TakeThisOuTwestfwKILLspamspammac.com> wrote: > > On Mar 9, 2006, at 4:33 AM, Vasile Surducan wrote: > > > waste your money once => buy your inhouse PCB maker device > > > When stripboard WORKS, I think it tends to go faster than easier > than any actual PCB manufacturing process. This time I think you wrong. How many packages may be used these days on 2.54 (100mil) raster. I'm talking about real electronics on SMD or microwave with high desities and high frequencies. http://www.lpkf.com/products/rapid-pcb-prototyping/circuit-board-plotter/protomat-s-series/s62/index.htm you have a demo movie about speed there greetings, Vasile

When I change some pad diameters and pad holes of say a crystal, they look OK relative to other pads etc on my board layout. When I print my board layout, the pads and pad holes for the crystal do not reflect my changes? Also, I still don't get the restring parameter..Can the problem above be due to an incorrect restring parameter value? Any help would be appreciated --Grahame

It's a bug. You have to run drill-aid.ulp. or to switch to a *real* CAD package. Vasile On 9/21/06, grammmvic <.....grammmvicRemoveMEbigpond.com> wrote: {Quote hidden}> When I change some pad diameters and pad holes of say a crystal, they look > OK relative to other pads etc on my board layout. > > > > When I print my board layout, the pads and pad holes for the crystal do not > reflect my changes? > > > > Also, I still don't get the restring parameter..Can the problem above be due > to an incorrect restring parameter value? > > > > Any help would be appreciated > > > > --Grahame > > -

On Sep 21, 2006, at 3:33 AM, Vasile Surducan wrote: >> When I change some pad diameters and pad holes of say a crystal, >> they look OK relative to other pads etc on my board layout. >> >> When I print my board layout, the pads and pad holes for the >> crystal do not reflect my changes? >> > It's a bug. In what version? (and what version is the OP running?) and exactly how are you changing the diameters, and how are you printing? It seems to work OK for me, running 4.15 on MacOSX, changing package pad sizes with restring and via hole sizes with "change drill." BillW

Works for me also. Real CAD package? Hmmm......define real. SmartWork was real but not a very good one. PADs is real, but has issues.... Every package has quirks...just have to know them. William Chops Westfield <RemoveMEwestfwspamBeGonemac.com> wrote: On Sep 21, 2006, at 3:33 AM, Vasile Surducan wrote: >> When I change some pad diameters and pad holes of say a crystal, >> they look OK relative to other pads etc on my board layout. >> >> When I print my board layout, the pads and pad holes for the >> crystal do not reflect my changes? >> > It's a bug. In what version? (and what version is the OP running?) and exactly how are you changing the diameters, and how are you printing? It seems to work OK for me, running 4.15 on MacOSX, changing package pad sizes with restring and via hole sizes with "change drill." BillW

Use the "mirror" function. It's the fourth down button from the top left corner of the left sidebar. Cheers, Zik On 11/22/06, Martin K <spamBeGonemartin-distlists@spam@spam_OUTnnytech.net> wrote: > All, > I have been trying to figure out how to move an SMD part from the top > layer to the bottom layer. I'm sure it's described somewhere but I can't > find out how it is done. > I'd appreciate the help. > Thanks, > Martin Klingensmith > -

Thanks a lot Jinx, Zik, David, and future replies. I wouldn't have guessed the mirror function changed layers. -- Martin K David P. Harris wrote: {Quote hidden}> Martin K wrote: > > >> All, >> I have been trying to figure out how to move an SMD part from the top >> layer to the bottom layer. I'm sure it's described somewhere but I can't >> find out how it is done. >> I'd appreciate the help. >> Thanks, >> Martin Klingensmith >> >> >> > Use mirror. > > David > >

I've been designing my first SMT PCB. I forgot I could use both sides for components so you just shrunk my board in half :). It's so small it's just amazing. I'm being careful to stick with 1206 components and a 10f PIC. since I'll be hand-soldering it. Is there a way to make the silk screen labels smaller though? The labels are as big as the components and overlapping each other quite badly. From: "Martin K" <TakeThisOuTmartin-distlistsspamnnytech.net> Sent: Tuesday, November 21, 2006 6:51 PM > Thanks a lot Jinx, Zik, David, and future replies. > I wouldn't have guessed the mirror function changed layers.

You're welcome :-) I'm sticking to 1206 parts as well because they are much easier to place by hand than the smaller parts. I have a bad habit of getting 0805 parts offset a little bit so they short out. SMT diodes and caps save a lot of space. Good luck. -- Martin K Jason wrote: {Quote hidden}> I've been designing my first SMT PCB. I forgot I could use both sides for > components so you just shrunk my board in half :). It's so small it's just > amazing. I'm being careful to stick with 1206 components and a 10f PIC. > since I'll be hand-soldering it. > > Is there a way to make the silk screen labels smaller though? The labels > are as big as the components and overlapping each other quite badly. > > > From: "Martin K" <martin-distlistsEraseMEnnytech.net> > Sent: Tuesday, November 21, 2006 6:51 PM > > > >> Thanks a lot Jinx, Zik, David, and future replies. >> I wouldn't have guessed the mirror function changed layers. >> > > >

I've had no problem doing 0603 components reliably. It gets difficult when you try QFN parts. Those require a stencil and must be reflowed, or put the heat gun to them. Something I've found that works for me is pre-tinning the pads on the board so you can apply the part, put heat to the pin and it should wick the solder up the pin giving you a satisfactory joint. On 11/21/06, Martin K <RemoveMEmartin-distlistsEraseMEspam_OUTnnytech.net> wrote: {Quote hidden}> > You're welcome :-) > I'm sticking to 1206 parts as well because they are much easier to place > by hand than the smaller parts. I have a bad habit of getting 0805 parts > offset a little bit so they short out. > SMT diodes and caps save a lot of space. > > Good luck. > -- > Martin K > > Jason wrote: > > I've been designing my first SMT PCB. I forgot I could use both sides > for > > components so you just shrunk my board in half :). It's so small it's > just > > amazing. I'm being careful to stick with 1206 components and a 10f PIC. > > since I'll be hand-soldering it. > > > > Is there a way to make the silk screen labels smaller though? The > labels > > are as big as the components and overlapping each other quite badly. > > > > > > From: "Martin K" <@spam@martin-distlistsRemoveMEEraseMEnnytech.net> > > Sent: Tuesday, November 21, 2006 6:51 PM > > > > > > > >> Thanks a lot Jinx, Zik, David, and future replies. > >> I wouldn't have guessed the mirror function changed layers. > >> > > > > > > > -

Shawn Wilton wrote: > I've had no problem doing 0603 components reliably. It gets difficult > when > you try QFN parts. Those require a stencil and must be reflowed, or put > the > heat gun to them. Something I've found that works for me is pre-tinning > the > pads on the board so you can apply the part, put heat to the pin and it > should wick the solder up the pin giving you a satisfactory joint. Have you tried baking your PCBs, instead of hand-soldering? We use a regular $20 toaster oven at work, and it works perfectly for prototypes and single boards. Sure beats soldering SSOPs by hand. :) Best regards, Vitaliy

On Wed, 22 Nov 2006 09:56:21 -0800, Shawn Wilton wrote: > I've had no problem doing 0603 components reliably. It gets > difficult when you try QFN parts. Those require a stencil and must > be reflowed, or put the heat gun to them. Something I've found > that works for me is pre-tinning the pads on the board so you can > apply the part, put heat to the pin and it should wick the solder > up the pin giving you a satisfactory joint. If you know you're going to hand solder the QFN parts, it helps a lot to make the pads extend beyond the body an extra 0.02 to 0.025" in your PCB layout. It gives you more pad to hit with a very small tip when soldering. One other trick that works is to use 2 or 4 vias in the center "power pad" of the device. Solder the pins as you normally would and then solder the pad from the back side of the PCB. This only works if the vias are not connected to an internal ground plane, then you'd have to reflow them to get sufficient heating to solder the pad. I've also had really good luck soldering small prototype PCBs in my SMD "reflow skillet". It works really well for QFN packages. If you don't know what the SMD reflow skillet is all about, you can check it out at: http://www.sparkfun.com/commerce/present.php?p=Reflow%20Skillet Matt Pobursky Maximum Performance Systems

You have to make/buy stencils though and get the solder paste right? That would be pretty convenient if I was making many boards. -- Martin K Vitaliy wrote: {Quote hidden}> Shawn Wilton wrote: > >> I've had no problem doing 0603 components reliably. It gets difficult >> when >> you try QFN parts. Those require a stencil and must be reflowed, or put >> the >> heat gun to them. Something I've found that works for me is pre-tinning >> the >> pads on the board so you can apply the part, put heat to the pin and it >> should wick the solder up the pin giving you a satisfactory joint. >> > > Have you tried baking your PCBs, instead of hand-soldering? We use a regular > $20 toaster oven at work, and it works perfectly for prototypes and single > boards. Sure beats soldering SSOPs by hand. :) > > Best regards, > > Vitaliy > >

Yeah, that's actually how I do it. But sometimes you have to rework a part, hence the pad tinning. It's just too much time and work to reflow a board for one part when it's double sided. :-) On 11/22/06, Vitaliy <EraseMEpiclist.account@spam@gmail.com> wrote: {Quote hidden}> > Shawn Wilton wrote: > > I've had no problem doing 0603 components reliably. It gets difficult > > when > > you try QFN parts. Those require a stencil and must be reflowed, or put > > the > > heat gun to them. Something I've found that works for me is pre-tinning > > the > > pads on the board so you can apply the part, put heat to the pin and it > > should wick the solder up the pin giving you a satisfactory joint. > > Have you tried baking your PCBs, instead of hand-soldering? We use a > regular > $20 toaster oven at work, and it works perfectly for prototypes and single > boards. Sure beats soldering SSOPs by hand. :) > > Best regards, > > Vitaliy > > -

Yes. Stencils come in two varieties. Mylar, and Stainless steel. The stainless is by far the way to go, but those are around $150-$200 a piece versus $50 for the mylar stencil. If you're pin pitch is large enough, then you can go Mylar. I would not attempt making my own stencil. Solder paste will do many small (3"x4") boards. I have done probably 30 boards for various projects and I'm down no more than 1/4 of my first jar of paste. On 11/22/06, Martin K <@spam@martin-distlistsspam_OUT.....nnytech.net> wrote: {Quote hidden}> > You have to make/buy stencils though and get the solder paste right? > That would be pretty convenient if I was making many boards. > -- > Martin K > > Vitaliy wrote: > > Shawn Wilton wrote: > > > >> I've had no problem doing 0603 components reliably. It gets difficult > >> when > >> you try QFN parts. Those require a stencil and must be reflowed, or > put > >> the > >> heat gun to them. Something I've found that works for me is > pre-tinning > >> the > >> pads on the board so you can apply the part, put heat to the pin and it > >> should wick the solder up the pin giving you a satisfactory joint. > >> > > > > Have you tried baking your PCBs, instead of hand-soldering? We use a > regular > > $20 toaster oven at work, and it works perfectly for prototypes and > single > > boards. Sure beats soldering SSOPs by hand. :) > > > > Best regards, > > > > Vitaliy > > > > > -

Martin K wrote: > You have to make/buy stencils though and get the solder paste right? > That would be pretty convenient if I was making many boards. > -- > Martin K Cash Olsen <http://www.zianet.com/erg/ShopSolderPaste.html> sells small quantities of solder paste in small syringes for prototyping. You manually apply it to each pad instead of using a stencil. He also describes an economical heat embossing gun that can be purchased at craft supply stores that can be used to so some rework/reflow operations for those on a budget. Tim

> On 11/22/06, Martin K <spamBeGonemartin-distlistsEraseMEnnytech.net> wrote: >> You have to make/buy stencils though and get the solder paste right? >> That would be pretty convenient if I was making many boards. Shawn Wilton wrote: {Quote hidden}> Yes. Stencils come in two varieties. Mylar, and Stainless steel. The > stainless is by far the way to go, but those are around $150-$200 a piece > versus $50 for the mylar stencil. If you're pin pitch is large enough, > then > you can go Mylar. I would not attempt making my own stencil. > > Solder paste will do many small (3"x4") boards. I have done probably 30 > boards for various projects and I'm down no more than 1/4 of my first jar > of > paste. No, we do not use stencils, because normally we only make one or two prototypes before a design goes into production. So I just take the syringe, and apply solder paste direcly to each pad. And the small syringe of solder paste that we bought from Digikey seems to last forever. See this page: http://www.seattlerobotics.org/encoder/200006/oven_art.htm Best regards, Vitaliy

I do exactly the same with a syringe of Kester and a hotplate. -marc On 11/22/06, Vitaliy <piclist.accountspamBeGonegmail.com> wrote: {Quote hidden}> > On 11/22/06, Martin K <RemoveMEmartin-distlists@spam@spamBeGonennytech.net> wrote: > >> You have to make/buy stencils though and get the solder paste right? > >> That would be pretty convenient if I was making many boards. > > Shawn Wilton wrote: > > Yes. Stencils come in two varieties. Mylar, and Stainless steel. The > > stainless is by far the way to go, but those are around $150-$200 a piece > > versus $50 for the mylar stencil. If you're pin pitch is large enough, > > then > > you can go Mylar. I would not attempt making my own stencil. > > > > Solder paste will do many small (3"x4") boards. I have done probably 30 > > boards for various projects and I'm down no more than 1/4 of my first jar > > of > > paste. > > No, we do not use stencils, because normally we only make one or two > prototypes before a design goes into production. So I just take the syringe, > and apply solder paste direcly to each pad. And the small syringe of solder > paste that we bought from Digikey seems to last forever. > > See this page: http://www.seattlerobotics.org/encoder/200006/oven_art.htm > > Best regards, > > Vitaliy > > > -

Has anyone had any luck with BGAs? I'd love to use a BGA in a project I have coming up but I'll be forced to use something else if I can't solder it. Has anyone tried the "reflow skillet" with 200+ ball BGAs for instance? Cheers, Zik On 11/23/06, Tim <.....tim.n9puz@spam@EraseMEgmail.com> wrote: {Quote hidden}> Martin K wrote: > > You have to make/buy stencils though and get the solder paste right? > > That would be pretty convenient if I was making many boards. > > -- > > Martin K > > Cash Olsen <http://www.zianet.com/erg/ShopSolderPaste.html> sells > small quantities of solder paste in small syringes for prototyping. > You manually apply it to each pad instead of using a stencil. > > He also describes an economical heat embossing gun that can be > purchased at craft supply stores that can be used to so some > rework/reflow operations for those on a budget. > > Tim > > -

Oh man. I do NOT have the patience for doing a few hundred pads with a syringe...<cringe> On 11/22/06, Vitaliy <.....piclist.accountRemoveMEgmail.com> wrote: {Quote hidden}> > > On 11/22/06, Martin K <.....martin-distlistsSTOPspam@spam@nnytech.net> wrote: > >> You have to make/buy stencils though and get the solder paste right? > >> That would be pretty convenient if I was making many boards. > > Shawn Wilton wrote: > > Yes. Stencils come in two varieties. Mylar, and Stainless steel. The > > stainless is by far the way to go, but those are around $150-$200 a > piece > > versus $50 for the mylar stencil. If you're pin pitch is large enough, > > then > > you can go Mylar. I would not attempt making my own stencil. > > > > Solder paste will do many small (3"x4") boards. I have done probably 30 > > boards for various projects and I'm down no more than 1/4 of my first > jar > > of > > paste. > > No, we do not use stencils, because normally we only make one or two > prototypes before a design goes into production. So I just take the > syringe, > and apply solder paste direcly to each pad. And the small syringe of > solder > paste that we bought from Digikey seems to last forever. > > See this page: http://www.seattlerobotics.org/encoder/200006/oven_art.htm > > Best regards, > > Vitaliy > > > -

Shawn Wilton wrote: > Oh man. I do NOT have the patience for doing a few hundred pads with a > syringe...<cringe> Have you ever tried it? It sounds scary, but consider that it's faster than soldering the same number of pads. And 300 pads at 1 second/pad is only 5 minutes. FINE, do it *very* slowly and carefully at first, 3 seconds per pad. Still only 15 minutes. Doing fine-pitch ICs is the easiest of all: you don't apply the paste to each pad individually, just squeeze it toothpaste-style from pad 1 to pad 20. Vitaliy

David P Harris wrote: > Marc Nicholas wrote: >>I do exactly the same with a syringe of Kester and a hotplate. > > Tell us more... See Sparkfun's website: http://www.sparkfun.com/tutorial/ReflowToaster/reflow-hotplate.htm#Hot-Plate I haven't actually tried the hot plate, but what this guy says makes sense: http://openhardware.net/Misc_Stuff/ToasterSMD/#donotfry "I don't like fry pans! I suggest that you don't even bother with this technique. I am convinced that the electric fry pan method is nothing more than a convection heat method to melt the solder with some conductive heating of the PCB to act as a preheater. From what I remember about my test with a 5inch X 8inch board, on the electric stove with a large aluminum slab to place the PCB on, is the smell of charred fiberglass resin! Use the toaster oven technique, it is so much easier and you can control the heat more precisely than with an electric skillet. Also, if you notice, the boards that Sparkfun is using on the skillet are relatively small boards? I believe this is why they are getting convection heat to melt the paste." Plus, a toaster oven is safer. Would you want a fry pan on your desk? I have enough burns from my 30W soldering iron, thank you. Best regards, Vitaliy

You're not understanding. I don't hand solder either. I don't have the patience. On 11/23/06, Vitaliy <piclist.accountEraseME@spam@gmail.com> wrote: {Quote hidden}> > Shawn Wilton wrote: > > Oh man. I do NOT have the patience for doing a few hundred pads with a > > syringe...<cringe> > > Have you ever tried it? > > It sounds scary, but consider that it's faster than soldering the same > number of pads. And 300 pads at 1 second/pad is only 5 minutes. FINE, do > it > *very* slowly and carefully at first, 3 seconds per pad. Still only 15 > minutes. > > Doing fine-pitch ICs is the easiest of all: you don't apply the paste to > each pad individually, just squeeze it toothpaste-style from pad 1 to pad > 20. > > Vitaliy > > -

Well, for couple of SMD stuff it worth the effort of these kind of techniques for sure. I was just wondering that I may be a slow on this a bit but I can't produce faster than let's say 6 pieces in an hour soldering only one SOT23-6, a 0402 capacitor and 12 awg23 cables or connectors as a surface mounted ie to soldering pads by my bare hands. Most of the time spending with checking, double checking if there is a shortcut or open legs using a 6x and a 20x magnifier. So I was just thinking that a hotplate may not help on speeding this much further as I still have to do the QA? I would trust more on a company who has the proper machine, what do you recon? Thanks, Tamas On 11/24/06, Shawn Wilton <RemoveMEblack9spamBeGonegmail.com> wrote: {Quote hidden}> > You're not understanding. I don't hand solder either. I don't have the > patience. > > > On 11/23/06, Vitaliy <spamBeGonepiclist.accountKILLspam@spam@gmail.com> wrote: > > > > Shawn Wilton wrote: > > > Oh man. I do NOT have the patience for doing a few hundred pads with > a > > > syringe...<cringe> > > > > Have you ever tried it? > > > > It sounds scary, but consider that it's faster than soldering the same > > number of pads. And 300 pads at 1 second/pad is only 5 minutes. FINE, do > > it > > *very* slowly and carefully at first, 3 seconds per pad. Still only 15 > > minutes. > > > > Doing fine-pitch ICs is the easiest of all: you don't apply the paste to > > each pad individually, just squeeze it toothpaste-style from pad 1 to > pad > > 20. > > > > Vitaliy > > > > --

Shawn Wilton wrote (top posting fixed): >> > Oh man. I do NOT have the patience for doing a few hundred pads with a >> > syringe...<cringe> >> >> Have you ever tried it? >> >> It sounds scary, but consider that it's faster than soldering the same >> number of pads. And 300 pads at 1 second/pad is only 5 minutes. FINE, do >> it >> *very* slowly and carefully at first, 3 seconds per pad. Still only 15 >> minutes. > > You're not understanding. I don't hand solder either. I don't have the > patience. But you do have the patience to order the stencils, and wait for several days for them to arrive in the mail? Even for a small board, with only a few SMDs? You're right -- I'm not understanding. :) Vitaliy

Tamas Rudnai wrote: > Well, for couple of SMD stuff it worth the effort of these kind of > techniques for sure. I was just wondering that I may be a slow on this a > bit > but I can't produce faster than let's say 6 pieces in an hour soldering > only > one SOT23-6, a 0402 capacitor and 12 awg23 cables or connectors as a > surface > mounted ie to soldering pads by my bare hands. Most of the time spending > with checking, double checking if there is a shortcut or open legs using a > 6x and a 20x magnifier. So I was just thinking that a hotplate may not > help > on speeding this much further as I still have to do the QA? I would trust > more on a company who has the proper machine, what do you recon? With enough practice, it's possible to solder very high-pitch parts and not get a solder bridge. The nice thing about the reflow process, is that parts tend to center themselves on the pads due to surface tension. Also consider that you can bake several boards at a time, so you save yourself a lot of time and effort by not having to hand-solder each pad. If you need to make more than a few boards, Shawn's suggestion to use a stencil starts to make sense. Whenever we need more than a few prototypes built, we use Advanced Assembly. They're pricey, though -- last time we paid $50+ per board for 10 small boards. Best regards, Vitaliy

The stencil arrives when the boards and parts arrive. On 11/24/06, Vitaliy <piclist.accountspam_OUT@spam@gmail.com> wrote: {Quote hidden}> > Shawn Wilton wrote (top posting fixed): > >> > Oh man. I do NOT have the patience for doing a few hundred pads with > a > >> > syringe...<cringe> > >> > >> Have you ever tried it? > >> > >> It sounds scary, but consider that it's faster than soldering the same > >> number of pads. And 300 pads at 1 second/pad is only 5 minutes. FINE, > do > >> it > >> *very* slowly and carefully at first, 3 seconds per pad. Still only 15 > >> minutes. > > > > > You're not understanding. I don't hand solder either. I don't have the > > patience. > > But you do have the patience to order the stencils, and wait for several > days for them to arrive in the mail? Even for a small board, with only a > few > SMDs? > > You're right -- I'm not understanding. :) > > Vitaliy > > -

stencilsunlimited, or advancedpcb. Doesn't take more than a few days to get a stencil. I order the stencil on Monday, and I have it by Wednesday or Thursday at the latest. On 11/27/06, Vitaliy <spamBeGonepiclist.account@spam@gmail.com> wrote: {Quote hidden}> > Shawn Wilton wrote: > > The stencil arrives when the boards and parts arrive. > > Hmmm... that's interesting. If you don't mind me asking, what company do > you > use? > > Best regards, > > Vitaliy > > -

I probably have this miscatagorized, and apologize if this is so. I have EAGLE Lite 4.16r2, and I've been working with getting a feel for it. Does anyone have suggestions for using EAGLE to produce PCB artwork that I can etch myself? -- Paul Anderson VE3HOP RemoveMEwackyvorlonEraseMEKILLspamgmail.com http://www.oldschoolhacker.com

Is your question on: 1: Using Eagle - Can't help much there, just finished first board with FREEPCB, but probably best to make a schematic first, I'll try TinyCad for next board, then import to the FREEPCB the netlist. View Gerbers with GC-PREVUE and/or VIEWMATE, and print output from there. Previously used Autocad to make print output. 2: From the end of Eagle to getting ready to etch: Need Laser printer or copier (not any other process including inkjet) on glossy paper, iron on to clean board. (and I'm simplifing a little) 3: The etching process: Ferric chloride seems better than Sulfuric acid and Hydrigen Peroxide. Caution the process gives off some chlorine. In the workshop the chlorine will combine with any iron it finds causing rusting! Say what area you need help. Paul Anderson wrote: > I probably have this miscatagorized, and apologize if this is so. I > have EAGLE Lite 4.16r2, and I've been working with getting a feel for > it. Does anyone have suggestions for using EAGLE to produce PCB > artwork that I can etch myself? > >

On 1/8/07, Carl Denk <spamBeGonecdenkspam_OUTRemoveMEalltel.net> wrote: > Is your question on: > 1: Using Eagle - Can't help much there, just finished first board with > FREEPCB, but > probably best to make a schematic first, I'll try TinyCad for next > board, then import to the FREEPCB the netlist. View Gerbers with > GC-PREVUE and/or VIEWMATE, and print output from there. Previously used > Autocad to make print output. > > It would be the first I need help with. Still learning the program, though it seems to be better than some of the others I've tried. -- Paul Anderson VE3HOP .....wackyvorlonRemoveMEgmail.com http://www.oldschoolhacker.com

> I probably have this miscatagorized, and apologize if this is so. I > have EAGLE Lite 4.16r2, and I've been working with getting a > feel for it. Does anyone have suggestions for using EAGLE to > produce PCB artwork that I can etch myself? You can output the board as a monochrome .tiff from the CAM Processor. This can then be printed onto a transparency for UV exposure or onto paper for the iron-on transfer method. Many people here have experimented with this (perhaps not directly from Eagle though but from other drawing packages) and there are Yahoo groups and similar for home-brew etching methods

On Jan 8, 2007, at 6:01 PM, Paul Anderson wrote: > have EAGLE Lite 4.16r2, and I've been working with getting a feel for > it. Does anyone have suggestions for using EAGLE to produce PCB > artwork that I can etch myself? > I made an "Instructable" on just that topic: http://www.instructables.com/id/EZVIGHUBGCEP287BJB/ I also did a couple of general tutorials aimed specifically at EAGLE beginners: Schematic entry: www.instructables.com/id/EXU9BO166NEQHO8XFU/ Schematic to PCB: http://www.instructables.com/id/EZ3WN1QUKYES9J5X48/ And someone else did one on creating library parts: http://www.instructables.com/id/ERHQQ180Y3EP286NQY/ BillW

On 1/8/07, Paul Anderson <wackyvorlon@spam@gmail.com> wrote: > I probably have this miscatagorized, and apologize if this is so. I > have EAGLE Lite 4.16r2, and I've been working with getting a feel for > it. Does anyone have suggestions for using EAGLE to produce PCB > artwork that I can etch myself? If it's the Windows version, what's wrong with File/Print? I get great results from 4.16r1 with an inkjet printer and transparancies as follows: Display only the layer/pads you want artwork for Select the File/Print menu item Select Black under style, scale factor 1 Hit the Page... button and turn off Caption, fiddle with border and alignment to put the image where you want it*, hit OK. Hit the Printer... button and set paper type and printer resolution (trial and error here, you'll have to experiment with these settings whatever method you use for printing your artwork), hit OK Make sure the right paper/transparancy is in the printer and hit OK *for small designs, I re-use transparancies and print the image in a blank area... this does require some care at not getting finger prints all over the transparancy while using it... I had poor results with the Linux version, BUT that was due to the printer driver being stuck in a draft mode. I've not tried since I fixed the printer settings, but see no reason it wouldn't do as well as the Windows version now. Orin.

Hi Paul, Not an Eagle-specific tip, but: Make copies of the library parts you are going to use, and change the pad types of your through-hole parts to "annular". That's the type of pad that has a hole in the center. When you drill the board, it'll act like a center punch and keep the drill bit centered. Cheerful regards, Bob Paul Anderson wrote: > I probably have this miscatagorized, and apologize if this is so. I > have EAGLE Lite 4.16r2, and I've been working with getting a feel for > it. Does anyone have suggestions for using EAGLE to produce PCB > artwork that I can etch myself? >

On 1/8/07, Bob Blick <EraseMEbblickRemoveMESTOPspamsonic.net> wrote: > Hi Paul, > > Not an Eagle-specific tip, but: > > Make copies of the library parts you are going to use, and change the > pad types of your through-hole parts to "annular". That's the type of > pad that has a hole in the center. When you drill the board, it'll act > like a center punch and keep the drill bit centered. Yes, I do the equivalent on Eagle, but for the whole board... In the board editor, under the Options/Set... menu item, select the Misc tab and select the Real button under Display mode (the alternative is No drills). Orin.

>> Make copies of the library parts you are going to use, and change the >> pad types of your through-hole parts to "annular". That's the type of >> pad that has a hole in the center. When you drill the board, it'll act >> like a center punch and keep the drill bit centered. >> THere's also an EAGLE ULP "drill-aid" that will generate pseudo-pads within the pads and vias that have a smaller internal diameter. BillW