Re: [time-nuts] Schematic capture, anyone?
On Fri, 24 Feb 2012 10:41:37 -0800 Chris Albertson albertson.ch...@gmail.com wrote: A good feature to look for is autorouting. and design rule checking. Of course every engineer thinks he is smarter than this kind of software. Mostly he is but it is good to use software that simply will not allow some kinds of errors. Design rules generally are things like following the schematic and the geometry of traces and limits of the PCB fab like line widths. I've used rat's nest routing too. This allows you to place the parts on the PCB and then does the interconnects with as the crow flies traces that cross and can't possibly work but they are drawn in red. you click them one at a time and rout them. As you place components you can see the rats net and you move them around to minimize the crossings. I advice against the use of autorouting. It's not that the engineer is so much smarter than the router, but it's that the engineer has much more knowledge than the router to know what those wires carry and which ones should be short, which wide, which do not really matter if they have a small trip around the PCB... Of course, you can annotate the schematics with all that info in order to get the autorouter to the point it can beat you. But it'll take much longer than doing it yourself. The usual way i do routing, is to use rats nest place the parts and see whether i can route the important signals nicely. Then route those first. If the PCB is complex (either too many highly interconnected componets, or not enough space) i often do a first run to asses how the connections will look like when routed and after that a second run with adjusted placement. Attila inali -- Why does it take years to find the answers to the questions one should have asked long ago? ___ time-nuts mailing list -- time-nuts@febo.com To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts and follow the instructions there.
Re: [time-nuts] Schematic capture, anyone?
In case anyone is following my progress, I started with EAGLE. It works fine on the Mac. I can tell it's not quite native (it even has a man(1) page!), but it's no problem. One afternoon with the tutorial, and I have a schematic. It's not yet complete, but that's not Eagle's fault: I'm still thinking about that current-loop driver, and the whole thing isn't even to the breadboard stage. Off to buy an 8255A and assorted parts somewhere. ___ time-nuts mailing list -- time-nuts@febo.com To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts and follow the instructions there.
Re: [time-nuts] Schematic capture, anyone?
I use professionally. It was the best that our small company could afford. Here are some tips that will save you mucho grief. 1) This is the biggie. Make your own parts library. Then put any part that you have to create in that library. As well, put a copy of any standard library part in your library AFTER you've verified that the part, especially the footprint is valid. Then put that library under SubVersion or whatever version control system you use. I call my library 00johh.lbr. The 00 makes it appear first in the library list. 2) another biggie. Validate any part that you take from an Eagle library. They are recklessly careless with those parts. I've found silk screens on the solder side and even individual pins on the wrong side. I lost a board run only once because of this but it was enough to make me extremely paranoid. 3) LOOK AT YOUR GERBERS! It takes a pretty long while and it's tedious work (I print mine out on an 11X17 printer and check off every feature with a highlighter as I go) but it's vital. Eagle doesn't always produce Gerbers like the board appears on the screen. Especially if you get caught by #2 above. I use gerbv which is a Linux tool but I think there's a version for the mac's almost-unix OS. John On 02/26/2012 02:12 PM, Jim Hickstein wrote: In case anyone is following my progress, I started with EAGLE. It works fine on the Mac. I can tell it's not quite native (it even has a man(1) page!), but it's no problem. One afternoon with the tutorial, and I have a schematic. -- John DeArmond Tellico Plains, Occupied TN http://www.neon-john.com-- email from here http://www.johndearmond.com -- Best damned Blog on the net PGP key: wwwkeys.pgp.net: BCB68D77 ___ time-nuts mailing list -- time-nuts@febo.com To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts and follow the instructions there.
Re: [time-nuts] Schematic capture, anyone?
Hi Verifying Gerbers on a trace by trace basis for a moderately complex multi-layer design could take a very long time. If you can't trust the program to go from the screen to the Gerbers, I'd say - find a new program... A bug like that nullifies any value from schematic checking or DRC. Bob On Feb 26, 2012, at 5:36 PM, NeonJohn j...@neon-john.com wrote: I use professionally. It was the best that our small company could afford. Here are some tips that will save you mucho grief. 1) This is the biggie. Make your own parts library. Then put any part that you have to create in that library. As well, put a copy of any standard library part in your library AFTER you've verified that the part, especially the footprint is valid. Then put that library under SubVersion or whatever version control system you use. I call my library 00johh.lbr. The 00 makes it appear first in the library list. 2) another biggie. Validate any part that you take from an Eagle library. They are recklessly careless with those parts. I've found silk screens on the solder side and even individual pins on the wrong side. I lost a board run only once because of this but it was enough to make me extremely paranoid. 3) LOOK AT YOUR GERBERS! It takes a pretty long while and it's tedious work (I print mine out on an 11X17 printer and check off every feature with a highlighter as I go) but it's vital. Eagle doesn't always produce Gerbers like the board appears on the screen. Especially if you get caught by #2 above. I use gerbv which is a Linux tool but I think there's a version for the mac's almost-unix OS. John On 02/26/2012 02:12 PM, Jim Hickstein wrote: In case anyone is following my progress, I started with EAGLE. It works fine on the Mac. I can tell it's not quite native (it even has a man(1) page!), but it's no problem. One afternoon with the tutorial, and I have a schematic. -- John DeArmond Tellico Plains, Occupied TN http://www.neon-john.com-- email from here http://www.johndearmond.com -- Best damned Blog on the net PGP key: wwwkeys.pgp.net: BCB68D77 ___ time-nuts mailing list -- time-nuts@febo.com To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts and follow the instructions there. ___ time-nuts mailing list -- time-nuts@febo.com To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts and follow the instructions there.
Re: [time-nuts] Schematic capture, anyone?
I've used EAGLE for about ten years. I strongly agree with what NeonJohn wrote below. I don't know if it is still the case, but when I started using EAGLE all of the library parts were on metric spacing (including DIPs and SMDs). This causes all sorts of headaches when doing a layout on inch spacing; traces don't meet the pads. I ended up creating my own libraries using the EAGLE libraries as a guide. I had one main library (1_main.lbr) for standard parts and additional libraries of specialized parts for each project. Brent On 2/26/2012 3:36 PM, NeonJohn wrote: I use professionally. It was the best that our small company could afford. Here are some tips that will save you mucho grief. 1) This is the biggie. Make your own parts library. Then put any part that you have to create in that library. As well, put a copy of any standard library part in your library AFTER you've verified that the part, especially the footprint is valid. Then put that library under SubVersion or whatever version control system you use. I call my library 00johh.lbr. The 00 makes it appear first in the library list. 2) another biggie. Validate any part that you take from an Eagle library. ___ time-nuts mailing list -- time-nuts@febo.com To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts and follow the instructions there.
Re: [time-nuts] Schematic capture, anyone?
NeonJohn wrote: I use professionally. It was the best that our small company could afford. Here are some tips that will save you mucho grief. 1) This is the biggie. Make your own parts library. Then put any part that you have to create in that library. As well, put a copy of any standard library part in your library AFTER you've verified that the part, especially the footprint is valid. Then put that library under SubVersion or whatever version control system you use. I call my library 00johh.lbr. The 00 makes it appear first in the library list. This is exactly right. I create a separate library for each board and name them starting with ! so they appear first in the list. Rick ___ time-nuts mailing list -- time-nuts@febo.com To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts and follow the instructions there.
Re: [time-nuts] Schematic capture, anyone?
Hi You will indeed spend a lot of time learning any of the more powerful packages. The same is true about re-learning them if you don't work with them for a while. Unless you are going to do this at least once a month, there is such a thing as to powerful. Bob On Feb 24, 2012, at 8:56 PM, shali...@gmail.com wrote: Rick, Thanks for the comments on Eagle. I have been frustrated trying to learn Eagle for a small urgent project recently. I ended up using ExpressPCB and the attendant schematic capture. While it uses proprietary file format and is therefore locked to one vendor, it was surprisingly easy to use. I created a schematic and a double sided RF PWB in a couple of weeks with minimum reference to the documentation. That was my first PWB design. I intend to learn Eagle for future projects though, as I need the capability to generate Gerbers at least. I tried KiCAD but I found it unfriendly and I do not like the way the schematic symbols look (I like my resistors wiggly, not rectangular, call me old fashioned...) If someone only needs a simple schematic capture tool, ExpressSCH from ExpressPCB is hard to beat. You can easily edit or create new symbols and the printouts look good and professional. Didier KO4BB Sent from my BlackBerry Wireless thingy while I do other things... -Original Message- From: Rick Karlquist rich...@karlquist.com Sender: time-nuts-boun...@febo.com Date: Thu, 23 Feb 2012 17:21:39 To: Discussion of precise time and frequency measurementtime-nuts@febo.com Reply-To: rich...@karlquist.com, Discussion of precise time and frequency measurement time-nuts@febo.com Subject: Re: [time-nuts] Schematic capture, anyone? Jim Hickstein wrote: What do people use these days for schematic capture (and just possibly PCB worse, I prefer ANSI logic symbology over shovels-and-spades (or, really, over plain rectangles where you're expected to know what the part number means). I'll add another vote for Eagle. It is a German program written in Unix, and ported to Windows. Therefore, you select the action first then click on the object of the action. It takes some getting used to. There has been a pattern of PC layout companies getting cobbled up leaving you with an orphan program, or an upgrade to some very expensive program. Orcad and Protel go gobbled up. Eagle did too, but by a distributor, Newark. They just came out with a new improved version. You can finally draw arbitrary SMT footprints. I think that was the major limitation of the old version. You can of course draw your own symbols any way you like. I have been using Eagle for 5 years now and never looked back. One other drawback of Eagle is that it is difficult to move a design between computers, and there are issues with the way preferences are stored. If you use a part from a library in a design, you are forever locked into that library. Many other CAD systems have these issues. Mentor used to be terrible about having absolute path names, etc. Rick N6RK ___ time-nuts mailing list -- time-nuts@febo.com To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts and follow the instructions there. ___ time-nuts mailing list -- time-nuts@febo.com To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts and follow the instructions there. ___ time-nuts mailing list -- time-nuts@febo.com To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts and follow the instructions there.
Re: [time-nuts] Schematic capture, anyone?
I'll add my $0.01 (depreciated). I am working on a project with Eagle. I started with the Gnu cad stuff but like many free software projects, it has multiple user interfaces and clunks. I tired of it and switched to Eagle. Eagle also has quirks but has the ability to switch back and forth between schematic and layout. I have added parts with the XML format and while painful, it's not impossible. Also, the user library of scripts is very useful: there is one that converts the schematic to a SPICE netlist (suitable for LTSpice with a little massaging). If/when I need a larger board than the free version then I'll have to decide what to do. But for the time being, it's OK. (And, as I like to say, when it comes to advice, you get what you pay for). On Fri, Feb 24, 2012 at 2:49 AM, Chris Albertson albertson.ch...@gmail.com wrote: On Thu, Feb 23, 2012 at 10:52 PM, Charles P. Steinmetz charles_steinm...@lavabit.com wrote: I've been using LTspice for schematic capture and simulation at home. Will the PCB CAD tools being discussed (Eagle, DesignSpark, FreePCB, etc.) import netlists from LTspice? Or do folks prefer to do the schematic capture in a CAD tool and export that netlist to LTspice for simulation? LT Spice is basically just the normal Spice simulator with a schematic capture program acting as a front end. LTspice can export standard Spice net lists and can save to it's own file format too. The spice net lists don't have any graphical information and don't have footprints. I find I don't need to move data from a simulation to a design program because to rarely simulate exactly the target circuit. You usually have to Spice specific stuff components like signal generators or maybe some parasitic capacitance for realism. These parts only exist in a simulation not on the PCB. Chris Albertson Redondo Beach, California ___ time-nuts mailing list -- time-nuts@febo.com To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts and follow the instructions there. ___ time-nuts mailing list -- time-nuts@febo.com To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts and follow the instructions there.
Re: [time-nuts] Schematic capture, anyone?
On Feb 23, 2012, at 7:38 PM, Jim Hickstein wrote: What do people use these days for schematic capture (and just possibly PCB layout), for low-budget homebrew stuff? [snip] I'm a Mac shop, but can of course run Windows if need be. Basically there are only two reasonable choices for schematic capture on the Mac: Capilano's DesignWorks: http://www.capilano.com/dwm_features. Available only from the Mac App Store. VAMP's McCAD: http://www.mccad.com/ Years ago, DesignWorks fit my budget much better than McCAD, but today I think they both offer free versions that can handle small hobby projects. For PCB layout on the Mac: Osmond PCB http://www.osmondpcb.com/ Again, the Osmond free trial handles small hobby-sized boards. The price for the full version is quite reasonable. For spice, see http://www.macspice.com/ There are some open-source apps using cross-platform GUI frameworks that compile on the Mac: KiCad: http://kicad.sourceforge.net/wiki/Main_Page If you can stomach Xwindows applications, then there are many open-source applications such as the Chipmunk system: http://www.cs.berkeley.edu/~lazzaro/chipmunk/index.html Best regards, -Steve -- Steve Byan steveb...@me.com Littleton, MA 01460 ___ time-nuts mailing list -- time-nuts@febo.com To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts and follow the instructions there.
Re: [time-nuts] Schematic capture, anyone?
I have been using OrCad SDT and PCB 386+ since the middle 1980's. It is a DOS based classic, and runs very nicely using the DOSEMU emulator on linux. It also runs nicely on Windows machines using their various dosbox incantations. The full package is available in the files section of the yahoo DosOrCad group. It has no really important limitations, and is still being used commercially by hundreds of users... most of which occupy the DosOrCad group. One of the users I know used it to develop PC motherboards. -Chuck Harris Mark Kahrs wrote: I'll add my $0.01 (depreciated). I am working on a project with Eagle. I started with the Gnu cad stuff but like many free software projects, it has multiple user interfaces and clunks. I tired of it and switched to Eagle. ___ time-nuts mailing list -- time-nuts@febo.com To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts and follow the instructions there.
Re: [time-nuts] Schematic capture, anyone?
Add a vote on DipTrace. I like it a lot. The Schematics and PCB environments are well integrated. The library has thousands of components (generic and proprietary), and the free version will support up to 300 pins on two PCB layers. It runs on all versions of Windows starting at 2000 and also run on Mac OS X. It has support for other CAD file formats. http://www.diptrace.com/ Cheers, Bert, VE2ZAZ ___ time-nuts mailing list -- time-nuts@febo.com To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts and follow the instructions there.
Re: [time-nuts] Schematic capture, anyone?
If you can stomach Xwindows applications, then there are many open-source applications such as the Chipmunk system: I'm a UNIX guy, really. It so happens I can't use a Mac unless it has a 3-button mouse and between 9 and 16 xterms open at any given time. :-) And yet it can print! ___ time-nuts mailing list -- time-nuts@febo.com To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts and follow the instructions there.
Re: [time-nuts] Schematic capture, anyone?
Charles P. Steinmetz wrote: I've been using LTspice for schematic capture and simulation at home. Will the PCB CAD tools being discussed (Eagle, DesignSpark, FreePCB, etc.) import netlists from LTspice? Or do folks prefer to do the schematic capture in a CAD tool and export that netlist to LTspice for simulation? Best regards, Charles Beige Bag Spice is designed to interchange schematics with Eagle. I recently evaluated it against LTspice and decided to use LTspice on the basis that it is more important to get the right Spice tool than have schematic exchange capability. Whatever I am going to simulate, I can usually draw the schematic in 5 minutes anyway. LTspice is very retro, being just an engine with very little GUI. Anything beyond the simplest stuff is done by playing SPICE cards, which I used to do years ago, so I was already familiar with that paradigm. It was actually very refreshing, because I again felt like I was in control, not trying to figure out what the program was going to do. It's kind of like driving a car with a stick shift vs automatic. Rick N6RK ___ time-nuts mailing list -- time-nuts@febo.com To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts and follow the instructions there.
Re: [time-nuts] Schematic capture, anyone?
I'm a UNIX guy, really. It so happens I can't use a Mac unless it has a 3-button mouse and between 9 and 16 xterms open at any given time That's me also, The Mac is taking the place of the high-end Silicon Graphics O2 that I used to like. One more Schematic capture program I like that is different from the others is xcircuit. http://opencircuitdesign.com/xcircuit/ This one is aimed at publication. It is actually a Postscript graphic editor and all the schematic symbols are little snippets of Postscript. The goal of the program is publication quality schematics but it can also export a net list. It's extenable with scripts and plays well with other EDA systems. I build some things (Guitar amps, studio type audio) with vacuum tubes so one of my criteria is that any schematic capture software has to handle vacuum tubes well as well as micro-controllers and op amps. would never use a PCB on a tube project. xcircuit does what it claims to do. That said Eagle has some advantages too and so does gEDA nad KiCad and the others. I stay away from software that runs only on Windows http://opencircuitdesign.com/xcircuit/ Chris Albertson Redondo Beach, California ___ time-nuts mailing list -- time-nuts@febo.com To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts and follow the instructions there.
Re: [time-nuts] Schematic capture, anyone?
Hi One very basic question to ask yourself: Do you want / need a program that checks the schematic against the layout? It's a feature that probably isn't needed for a really simple circuit. It's something that will save you a hundred dollars (one PCB run) pretty quick on things of even moderate complexity. You can indeed do the schematic on the back of an envelope and do the layout from that. Print out the layout and get out the colored pencils. Color this here and that there as you check it. Been there done that. Gets old pretty quick. Next basic question: How big are the built in / available libraries? If not built in are they free or an extra cost option? All of these programs have the very basic stuff in them. Even simple designs seem to get past the basics pretty fast. RF connectors, regulators, stuff from Mini Circuits, something gets in there. Even a big library won't have everything. Doing two things instead of ten is a lot less tiring. The library thing goes to both ends. Having a schematic with a bunch of numbered boxes in it isn't very helpful. Having a layout made up of a random bunch of pads makes changes (and checking) tough. Again, loose one PCB run to a mistake and you have paid for a license to some of these programs or the library upgrade. No, I'm not trying to sell you on any specific program. I'm just trying to complicate the decision process. It's better to look at all the issues before you spend a couple months learning how a package works than to run through three or four packages (and a years worth of agony). Bob -Original Message- From: time-nuts-boun...@febo.com [mailto:time-nuts-boun...@febo.com] On Behalf Of Jim Hickstein Sent: Thursday, February 23, 2012 7:39 PM To: time-nuts@febo.com Subject: [time-nuts] Schematic capture, anyone? What do people use these days for schematic capture (and just possibly PCB layout), for low-budget homebrew stuff? It's been so long since I did this, I still own a T-square and a pile of contemporary relics like rules and triangles. I'll get out my pencil sharpener if I have to. But really, this must be a solved problem by now. For less than $300? I only need TTL, not striplines or any black magic like that. I'm a Mac shop, but can of course run Windows if need be. And to make matters worse, I prefer ANSI logic symbology over shovels-and-spades (or, really, over plain rectangles where you're expected to know what the part number means). This comes from exposure to Control Data, who were big on it back in the day. I even used to be on the mailing list of the standards committee. I suppose that all sank without a trace? If it's still controversial, I apologize in advance for trolling. ___ time-nuts mailing list -- time-nuts@febo.com To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts and follow the instructions there. ___ time-nuts mailing list -- time-nuts@febo.com To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts and follow the instructions there.
Re: [time-nuts] Schematic capture, anyone?
Hi Bob: I'll second the usefulness of checking the layout against the schematic. The early versions of ExpressPCB did not have schematic capture and even on very simple boards I ended up making patches. http://www.expresspcb.com/ Now when you're doing the layout you can turn on checking and all the pads for the currently active note light up in a different color. By stepping through all the nodes you can confirm that they are all connected to each other. I've been using ExpressPCB for a long time and for what I'm doing it's the most effective in terms of my time. The down side is that their free software is proprietary to their process. You don't get to shop vendors. In exchange you get a very simple and easy to learn interface and an extensive library of standard parts. It's also easy to add a custom part. For me the learning curve for working with something like Eagle and the different file types and conventions is not worth the time. I use the schematic capture to draw schematics for things where I'm not going to make a board. Have Fun, Brooke Clarke http://www.PRC68.com http://www.end2partygovernment.com/Brooke4Congress.html Bob Camp wrote: Hi One very basic question to ask yourself: Do you want / need a program that checks the schematic against the layout? It's a feature that probably isn't needed for a really simple circuit. It's something that will save you a hundred dollars (one PCB run) pretty quick on things of even moderate complexity. You can indeed do the schematic on the back of an envelope and do the layout from that. Print out the layout and get out the colored pencils. Color this here and that there as you check it. Been there done that. Gets old pretty quick. Next basic question: How big are the built in / available libraries? If not built in are they free or an extra cost option? All of these programs have the very basic stuff in them. Even simple designs seem to get past the basics pretty fast. RF connectors, regulators, stuff from Mini Circuits, something gets in there. Even a big library won't have everything. Doing two things instead of ten is a lot less tiring. The library thing goes to both ends. Having a schematic with a bunch of numbered boxes in it isn't very helpful. Having a layout made up of a random bunch of pads makes changes (and checking) tough. Again, loose one PCB run to a mistake and you have paid for a license to some of these programs or the library upgrade. No, I'm not trying to sell you on any specific program. I'm just trying to complicate the decision process. It's better to look at all the issues before you spend a couple months learning how a package works than to run through three or four packages (and a years worth of agony). Bob -Original Message- From: time-nuts-boun...@febo.com [mailto:time-nuts-boun...@febo.com] On Behalf Of Jim Hickstein Sent: Thursday, February 23, 2012 7:39 PM To: time-nuts@febo.com Subject: [time-nuts] Schematic capture, anyone? What do people use these days for schematic capture (and just possibly PCB layout), for low-budget homebrew stuff? It's been so long since I did this, I still own a T-square and a pile of contemporary relics like rules and triangles. I'll get out my pencil sharpener if I have to. But really, this must be a solved problem by now. For less than $300? I only need TTL, not striplines or any black magic like that. I'm a Mac shop, but can of course run Windows if need be. And to make matters worse, I prefer ANSI logic symbology over shovels-and-spades (or, really, over plain rectangles where you're expected to know what the part number means). This comes from exposure to Control Data, who were big on it back in the day. I even used to be on the mailing list of the standards committee. I suppose that all sank without a trace? If it's still controversial, I apologize in advance for trolling. ___ time-nuts mailing list -- time-nuts@febo.com To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts and follow the instructions there. ___ time-nuts mailing list -- time-nuts@febo.com To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts and follow the instructions there. ___ time-nuts mailing list -- time-nuts@febo.com To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts and follow the instructions there.
Re: [time-nuts] Schematic capture, anyone?
On Fri, Feb 24, 2012 at 9:52 AM, Brooke Clarke bro...@pacific.net wrote: Now when you're doing the layout you can turn on checking and all the pads for the currently active note light up in a different color. By stepping through all the nodes you can confirm that they are all connected to each other. A good feature to look for is autorouting. and design rule checking. Of course every engineer thinks he is smarter than this kind of software. Mostly he is but it is good to use software that simply will not allow some kinds of errors. Design rules generally are things like following the schematic and the geometry of traces and limits of the PCB fab like line widths. I've used rat's nest routing too. This allows you to place the parts on the PCB and then does the interconnects with as the crow flies traces that cross and can't possibly work but they are drawn in red. you click them one at a time and rout them. As you place components you can see the rats net and you move them around to minimize the crossings. -- Chris Albertson Redondo Beach, California ___ time-nuts mailing list -- time-nuts@febo.com To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts and follow the instructions there.
Re: [time-nuts] Schematic capture, anyone?
I suggested expresspcb earlier and all thats been said is on target. General ease of use. What is however tricky is if you need to create a symbol. Lets say a particular PIC micro. It is cumbersome to adapt one that exists and I am unsure as to why. But that said its is pretty easy to use overall. I do plan to try a few others suggested here. Like most of us I am a small board/project kind O time-nut and since most of my stuff is really one off do point to point and really just want to document what on earth I actually did. I do think this thread has been pretty good as a overall state of the industry today. I want to go hunting for libraries since that does seem to be pretty key. Regards Paul. WB8TSL On Fri, Feb 24, 2012 at 12:52 PM, Brooke Clarke bro...@pacific.net wrote: Hi Bob: I'll second the usefulness of checking the layout against the schematic. The early versions of ExpressPCB did not have schematic capture and even on very simple boards I ended up making patches. http://www.expresspcb.com/ Now when you're doing the layout you can turn on checking and all the pads for the currently active note light up in a different color. By stepping through all the nodes you can confirm that they are all connected to each other. I've been using ExpressPCB for a long time and for what I'm doing it's the most effective in terms of my time. The down side is that their free software is proprietary to their process. You don't get to shop vendors. In exchange you get a very simple and easy to learn interface and an extensive library of standard parts. It's also easy to add a custom part. For me the learning curve for working with something like Eagle and the different file types and conventions is not worth the time. I use the schematic capture to draw schematics for things where I'm not going to make a board. Have Fun, Brooke Clarke http://www.PRC68.com http://www.**end2partygovernment.com/**Brooke4Congress.htmlhttp://www.end2partygovernment.com/Brooke4Congress.html Bob Camp wrote: Hi One very basic question to ask yourself: Do you want / need a program that checks the schematic against the layout? It's a feature that probably isn't needed for a really simple circuit. It's something that will save you a hundred dollars (one PCB run) pretty quick on things of even moderate complexity. You can indeed do the schematic on the back of an envelope and do the layout from that. Print out the layout and get out the colored pencils. Color this here and that there as you check it. Been there done that. Gets old pretty quick. Next basic question: How big are the built in / available libraries? If not built in are they free or an extra cost option? All of these programs have the very basic stuff in them. Even simple designs seem to get past the basics pretty fast. RF connectors, regulators, stuff from Mini Circuits, something gets in there. Even a big library won't have everything. Doing two things instead of ten is a lot less tiring. The library thing goes to both ends. Having a schematic with a bunch of numbered boxes in it isn't very helpful. Having a layout made up of a random bunch of pads makes changes (and checking) tough. Again, loose one PCB run to a mistake and you have paid for a license to some of these programs or the library upgrade. No, I'm not trying to sell you on any specific program. I'm just trying to complicate the decision process. It's better to look at all the issues before you spend a couple months learning how a package works than to run through three or four packages (and a years worth of agony). Bob -Original Message- From: time-nuts-boun...@febo.com [mailto:time-nuts-bounces@**febo.comtime-nuts-boun...@febo.com] On Behalf Of Jim Hickstein Sent: Thursday, February 23, 2012 7:39 PM To: time-nuts@febo.com Subject: [time-nuts] Schematic capture, anyone? What do people use these days for schematic capture (and just possibly PCB layout), for low-budget homebrew stuff? It's been so long since I did this, I still own a T-square and a pile of contemporary relics like rules and triangles. I'll get out my pencil sharpener if I have to. But really, this must be a solved problem by now. For less than $300? I only need TTL, not striplines or any black magic like that. I'm a Mac shop, but can of course run Windows if need be. And to make matters worse, I prefer ANSI logic symbology over shovels-and-spades (or, really, over plain rectangles where you're expected to know what the part number means). This comes from exposure to Control Data, who were big on it back in the day. I even used to be on the mailing list of the standards committee. I suppose that all sank without a trace? If it's still controversial, I apologize in advance for trolling. __**_ time-nuts mailing list -- time-nuts@febo.com To unsubscribe, go to https
Re: [time-nuts] Schematic capture, anyone?
Rick, Thanks for the comments on Eagle. I have been frustrated trying to learn Eagle for a small urgent project recently. I ended up using ExpressPCB and the attendant schematic capture. While it uses proprietary file format and is therefore locked to one vendor, it was surprisingly easy to use. I created a schematic and a double sided RF PWB in a couple of weeks with minimum reference to the documentation. That was my first PWB design. I intend to learn Eagle for future projects though, as I need the capability to generate Gerbers at least. I tried KiCAD but I found it unfriendly and I do not like the way the schematic symbols look (I like my resistors wiggly, not rectangular, call me old fashioned...) If someone only needs a simple schematic capture tool, ExpressSCH from ExpressPCB is hard to beat. You can easily edit or create new symbols and the printouts look good and professional. Didier KO4BB Sent from my BlackBerry Wireless thingy while I do other things... -Original Message- From: Rick Karlquist rich...@karlquist.com Sender: time-nuts-boun...@febo.com Date: Thu, 23 Feb 2012 17:21:39 To: Discussion of precise time and frequency measurementtime-nuts@febo.com Reply-To: rich...@karlquist.com, Discussion of precise time and frequency measurement time-nuts@febo.com Subject: Re: [time-nuts] Schematic capture, anyone? Jim Hickstein wrote: What do people use these days for schematic capture (and just possibly PCB worse, I prefer ANSI logic symbology over shovels-and-spades (or, really, over plain rectangles where you're expected to know what the part number means). I'll add another vote for Eagle. It is a German program written in Unix, and ported to Windows. Therefore, you select the action first then click on the object of the action. It takes some getting used to. There has been a pattern of PC layout companies getting cobbled up leaving you with an orphan program, or an upgrade to some very expensive program. Orcad and Protel go gobbled up. Eagle did too, but by a distributor, Newark. They just came out with a new improved version. You can finally draw arbitrary SMT footprints. I think that was the major limitation of the old version. You can of course draw your own symbols any way you like. I have been using Eagle for 5 years now and never looked back. One other drawback of Eagle is that it is difficult to move a design between computers, and there are issues with the way preferences are stored. If you use a part from a library in a design, you are forever locked into that library. Many other CAD systems have these issues. Mentor used to be terrible about having absolute path names, etc. Rick N6RK ___ time-nuts mailing list -- time-nuts@febo.com To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts and follow the instructions there. ___ time-nuts mailing list -- time-nuts@febo.com To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts and follow the instructions there.
Re: [time-nuts] Schematic capture, anyone?
First off if you prefer the American style zig-zag resistors or maybe circles around your transistors, all of them allow you to edit symbols and most have alternate symbol libraries. I think xciruit wil make the best looking schematics and it can be used along side other software http://opencircuitdesign.com/xcircuit/index.html One feature to look for is BOM management. You should be able to not only label a cap as C24 but say it's value, who makes it, manufacture part number the maybe even the distributer's part number The other thing is backwards references. So you can change a part int e PCB layout and have the schematic change On Fri, Feb 24, 2012 at 5:56 PM, shali...@gmail.com wrote: Rick, Thanks for the comments on Eagle. I have been frustrated trying to learn Eagle for a small urgent project recently. I ended up using ExpressPCB and the attendant schematic capture. While it uses proprietary file format and is therefore locked to one vendor, it was surprisingly easy to use. I created a schematic and a double sided RF PWB in a couple of weeks with minimum reference to the documentation. That was my first PWB design. I intend to learn Eagle for future projects though, as I need the capability to generate Gerbers at least. I tried KiCAD but I found it unfriendly and I do not like the way the schematic symbols look (I like my resistors wiggly, not rectangular, call me old fashioned...) If someone only needs a simple schematic capture tool, ExpressSCH from ExpressPCB is hard to beat. You can easily edit or create new symbols and the printouts look good and professional. Didier KO4BB Sent from my BlackBerry Wireless thingy while I do other things... -Original Message- From: Rick Karlquist rich...@karlquist.com Sender: time-nuts-boun...@febo.com Date: Thu, 23 Feb 2012 17:21:39 To: Discussion of precise time and frequency measurementtime-nuts@febo.com Reply-To: rich...@karlquist.com, Discussion of precise time and frequency measurement time-nuts@febo.com Subject: Re: [time-nuts] Schematic capture, anyone? Jim Hickstein wrote: What do people use these days for schematic capture (and just possibly PCB worse, I prefer ANSI logic symbology over shovels-and-spades (or, really, over plain rectangles where you're expected to know what the part number means). I'll add another vote for Eagle. It is a German program written in Unix, and ported to Windows. Therefore, you select the action first then click on the object of the action. It takes some getting used to. There has been a pattern of PC layout companies getting cobbled up leaving you with an orphan program, or an upgrade to some very expensive program. Orcad and Protel go gobbled up. Eagle did too, but by a distributor, Newark. They just came out with a new improved version. You can finally draw arbitrary SMT footprints. I think that was the major limitation of the old version. You can of course draw your own symbols any way you like. I have been using Eagle for 5 years now and never looked back. One other drawback of Eagle is that it is difficult to move a design between computers, and there are issues with the way preferences are stored. If you use a part from a library in a design, you are forever locked into that library. Many other CAD systems have these issues. Mentor used to be terrible about having absolute path names, etc. Rick N6RK ___ time-nuts mailing list -- time-nuts@febo.com To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts and follow the instructions there. ___ time-nuts mailing list -- time-nuts@febo.com To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts and follow the instructions there. -- Chris Albertson Redondo Beach, California ___ time-nuts mailing list -- time-nuts@febo.com To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts and follow the instructions there.
[time-nuts] Schematic capture, anyone?
What do people use these days for schematic capture (and just possibly PCB layout), for low-budget homebrew stuff? It's been so long since I did this, I still own a T-square and a pile of contemporary relics like rules and triangles. I'll get out my pencil sharpener if I have to. But really, this must be a solved problem by now. For less than $300? I only need TTL, not striplines or any black magic like that. I'm a Mac shop, but can of course run Windows if need be. And to make matters worse, I prefer ANSI logic symbology over shovels-and-spades (or, really, over plain rectangles where you're expected to know what the part number means). This comes from exposure to Control Data, who were big on it back in the day. I even used to be on the mailing list of the standards committee. I suppose that all sank without a trace? If it's still controversial, I apologize in advance for trolling. ___ time-nuts mailing list -- time-nuts@febo.com To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts and follow the instructions there.
Re: [time-nuts] Schematic capture, anyone?
Jim... There is a free package called Eagleware that you might find suitable. Or maybe it is just Eagle; it's been a while. A little quality time with Google should find it for you easily. It is for Windows, but there might be a Mac version as well. Tom Holmes, N8ZM Tipp City, OH EM79 -Original Message- From: time-nuts-boun...@febo.com [mailto:time-nuts-boun...@febo.com] On Behalf Of Jim Hickstein Sent: Thursday, February 23, 2012 7:39 PM To: time-nuts@febo.com Subject: [time-nuts] Schematic capture, anyone? What do people use these days for schematic capture (and just possibly PCB layout), for low-budget homebrew stuff? It's been so long since I did this, I still own a T-square and a pile of contemporary relics like rules and triangles. I'll get out my pencil sharpener if I have to. But really, this must be a solved problem by now. For less than $300? I only need TTL, not striplines or any black magic like that. I'm a Mac shop, but can of course run Windows if need be. And to make matters worse, I prefer ANSI logic symbology over shovels-and-spades (or, really, over plain rectangles where you're expected to know what the part number means). This comes from exposure to Control Data, who were big on it back in the day. I even used to be on the mailing list of the standards committee. I suppose that all sank without a trace? If it's still controversial, I apologize in advance for trolling. ___ time-nuts mailing list -- time-nuts@febo.com To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts and follow the instructions there. ___ time-nuts mailing list -- time-nuts@febo.com To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts and follow the instructions there.
Re: [time-nuts] Schematic capture, anyone?
Nowadays you can simply download the design software for free from the fab houses. Try PCB 123 from sunstone.com Good shop, reasonable prices for quick protos. bye, Said In a message dated 2/23/2012 16:39:12 Pacific Standard Time, j...@jxh.com writes: What do people use these days for schematic capture (and just possibly PCB layout), for low-budget homebrew stuff? It's been so long since I did this, I still own a T-square and a pile of contemporary relics like rules and triangles. I'll get out my pencil sharpener if I have to. But really, this must be a solved problem by now. For less than $300? I only need TTL, not striplines or any black magic like that. I'm a Mac shop, but can of course run Windows if need be. And to make matters worse, I prefer ANSI logic symbology over shovels-and-spades (or, really, over plain rectangles where you're expected to know what the part number means). This comes from exposure to Control Data, who were big on it back in the day. I even used to be on the mailing list of the standards committee. I suppose that all sank without a trace? If it's still controversial, I apologize in advance for trolling. ___ time-nuts mailing list -- time-nuts@febo.com To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts and follow the instructions there. ___ time-nuts mailing list -- time-nuts@febo.com To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts and follow the instructions there.
Re: [time-nuts] Schematic capture, anyone?
Eagle all the way. It's free and the documentation is good enough to get you by. There is a huge hobbiest following as well if you get stuck. Definitely read the tutorial on creating parts. It'll be nearly impossible to wing. The free version has some limits. 80mmx100mm boards, 2 layers, and I think 2 schematic sheets. -Bob On Thu, Feb 23, 2012 at 5:46 PM, saidj...@aol.com wrote: Nowadays you can simply download the design software for free from the fab houses. Try PCB 123 from sunstone.com Good shop, reasonable prices for quick protos. bye, Said In a message dated 2/23/2012 16:39:12 Pacific Standard Time, j...@jxh.com writes: What do people use these days for schematic capture (and just possibly PCB layout), for low-budget homebrew stuff? It's been so long since I did this, I still own a T-square and a pile of contemporary relics like rules and triangles. I'll get out my pencil sharpener if I have to. But really, this must be a solved problem by now. For less than $300? I only need TTL, not striplines or any black magic like that. I'm a Mac shop, but can of course run Windows if need be. And to make matters worse, I prefer ANSI logic symbology over shovels-and-spades (or, really, over plain rectangles where you're expected to know what the part number means). This comes from exposure to Control Data, who were big on it back in the day. I even used to be on the mailing list of the standards committee. I suppose that all sank without a trace? If it's still controversial, I apologize in advance for trolling. ___ time-nuts mailing list -- time-nuts@febo.com To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts and follow the instructions there. ___ time-nuts mailing list -- time-nuts@febo.com To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts and follow the instructions there. ___ time-nuts mailing list -- time-nuts@febo.com To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts and follow the instructions there.
Re: [time-nuts] Schematic capture, anyone?
On Thu, Feb 23, 2012 at 4:38 PM, Jim Hickstein j...@jxh.com wrote: What do people use these days for schematic capture (and just possibly PCB layout), for low-budget homebrew stuff? Eagle is popular. It is a commercial product but there is a free version that limits you to smallish PCBs. If you out grow it the next step up is not that much more than free. http://www.cadsoftusa.com/ here is a very complete, if not up to date list http://en.wikipedia.org/wiki/Comparison_of_EDA_software Of the free systems gEDA and KiCAD have large active user bases. Chris Albertson Redondo Beach, California ___ time-nuts mailing list -- time-nuts@febo.com To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts and follow the instructions there.
Re: [time-nuts] Schematic capture, anyone?
On Thu, Feb 23, 2012 at 4:46 PM, saidj...@aol.com wrote: Nowadays you can simply download the design software for free from the fab houses. Yes, but in many cases these have problems like (1) They save the design in a format that forces to to use ONLY that fab house to make the PCB. You really, really want to be able to save in a standard file format and (2) many of these programs only run on Windows so you can notshare your designs except to Windows users. Basically just watch out that many of these free programs only run in a closed environment. The better software lets you save the schematic to several different industry standard formats formats Chris Albertson Redondo Beach, California ___ time-nuts mailing list -- time-nuts@febo.com To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts and follow the instructions there.
Re: [time-nuts] Schematic capture, anyone?
There are a bunch of choices, some free and some limited to working with a certain PCB shop, but I like Eagle (http://www.cadsoftusa.com) because, among other things, it's cross-platform running on Windows, Mac, and Linux (I use the Linux version). There's a free version and a couple of steps of paid versions which allow larger board sizes and more layers. John Jim Hickstein said the following on 02/23/2012 07:38 PM: What do people use these days for schematic capture (and just possibly PCB layout), for low-budget homebrew stuff? It's been so long since I did this, I still own a T-square and a pile of contemporary relics like rules and triangles. I'll get out my pencil sharpener if I have to. But really, this must be a solved problem by now. For less than $300? I only need TTL, not striplines or any black magic like that. I'm a Mac shop, but can of course run Windows if need be. And to make matters worse, I prefer ANSI logic symbology over shovels-and-spades (or, really, over plain rectangles where you're expected to know what the part number means). This comes from exposure to Control Data, who were big on it back in the day. I even used to be on the mailing list of the standards committee. I suppose that all sank without a trace? If it's still controversial, I apologize in advance for trolling. ___ time-nuts mailing list -- time-nuts@febo.com To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts and follow the instructions there. ___ time-nuts mailing list -- time-nuts@febo.com To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts and follow the instructions there.
Re: [time-nuts] Schematic capture, anyone?
DesignSpark PCB: http://www.designspark.com/knowledge/pcb Being free and having no limitations like Eagle, I think you can try it... ___ time-nuts mailing list -- time-nuts@febo.com To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts and follow the instructions there.
Re: [time-nuts] Schematic capture, anyone?
On Thu, Feb 23, 2012 at 5:09 PM, Elio Corbolante elio...@gmail.com wrote: DesignSpark PCB: http://www.designspark.com/knowledge/pcb Being free and having no limitations like Eagle This looks interesting but the download is a .exe file for Windows Does anyone know if it works with Wine? Yes I know I could try and see but many times it takes many hours to find problems. Chris Albertson Redondo Beach, California ___ time-nuts mailing list -- time-nuts@febo.com To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts and follow the instructions there.
Re: [time-nuts] Schematic capture, anyone?
Jim Hickstein wrote: What do people use these days for schematic capture (and just possibly PCB worse, I prefer ANSI logic symbology over shovels-and-spades (or, really, over plain rectangles where you're expected to know what the part number means). I'll add another vote for Eagle. It is a German program written in Unix, and ported to Windows. Therefore, you select the action first then click on the object of the action. It takes some getting used to. There has been a pattern of PC layout companies getting cobbled up leaving you with an orphan program, or an upgrade to some very expensive program. Orcad and Protel go gobbled up. Eagle did too, but by a distributor, Newark. They just came out with a new improved version. You can finally draw arbitrary SMT footprints. I think that was the major limitation of the old version. You can of course draw your own symbols any way you like. I have been using Eagle for 5 years now and never looked back. One other drawback of Eagle is that it is difficult to move a design between computers, and there are issues with the way preferences are stored. If you use a part from a library in a design, you are forever locked into that library. Many other CAD systems have these issues. Mentor used to be terrible about having absolute path names, etc. Rick N6RK ___ time-nuts mailing list -- time-nuts@febo.com To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts and follow the instructions there.
Re: [time-nuts] Schematic capture, anyone?
Hi, Comments on their downloads page indicate that it runs under Wine. I havent tried it though. Cheers. On Thursday, February 23, 2012 05:18:06 PM Chris Albertson wrote: On Thu, Feb 23, 2012 at 5:09 PM, Elio Corbolante elio...@gmail.com wrote: DesignSpark PCB: http://www.designspark.com/knowledge/pcb Being free and having no limitations like Eagle This looks interesting but the download is a .exe file for Windows Does anyone know if it works with Wine? Yes I know I could try and see but many times it takes many hours to find problems. Chris Albertson Redondo Beach, California ___ time-nuts mailing list -- time-nuts@febo.com To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts and follow the instructions there. -- Mike McCauley mi...@open.com.au Open System Consultants Pty. Ltd 9 Bulbul Place Currumbin Waters QLD 4223 Australia http://www.open.com.au Phone +61 7 5598-7474 Fax +61 7 5598-7070 Radiator: the most portable, flexible and configurable RADIUS server anywhere. SQL, proxy, DBM, files, LDAP, NIS+, password, NT, Emerald, Platypus, Freeside, TACACS+, PAM, external, Active Directory, EAP, TLS, TTLS, PEAP, TNC, WiMAX, RSA, Vasco, Yubikey, MOTP, HOTP, TOTP, DIAMETER etc. Full source on Unix, Windows, MacOSX, Solaris, VMS, NetWare etc. ___ time-nuts mailing list -- time-nuts@febo.com To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts and follow the instructions there.
Re: [time-nuts] Schematic capture, anyone?
Good eve, I must be the exception... I've tried Eagle, most recently about three months back. I can't stand it. I find it, for my purposes, to be about as intuitive as a Salvador Dali painting. I've not yet tried DesignSpark, but it looks very promising. Personally, I use an old version of OrCAD (9-dot-something, I think). Happy tweaking. *** REPLY SEPARATOR *** On 23-Feb-12 at 18:38 Jim Hickstein wrote: What do people use these days for schematic capture (and just possibly PCB layout), for low-budget homebrew stuff? snippage It's been so long since I did this, I still own a T-square and a pile of contemporary relics like rules and triangles. I'll get out my pencil sharpener if I have to. But really, this must be a solved problem by now. For less than $300? I only need TTL, not striplines or any black magic like that. I'm a Mac shop, but can of course run Windows if need be. And to make matters worse, I prefer ANSI logic symbology over shovels-and-spades (or, really, over plain rectangles where you're expected to know what the part number means). This comes from exposure to Control Data, who were big on it back in the day. I even used to be on the mailing list of the standards committee. I suppose that all sank without a trace? If it's still controversial, I apologize in advance for trolling. ___ time-nuts mailing list -- time-nuts@febo.com To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts and follow the instructions there. -=-=-=-=-=-=-=-=-=-=-=- Bruce Lane, Owner Head Hardware Heavy, Blue Feather Technologies -- http://www.bluefeathertech.com kyrrin (at) bluefeathertech do/t c=o=m If Salvador Dali had owned a computer, would it have been equipped with surreal ports? ___ time-nuts mailing list -- time-nuts@febo.com To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts and follow the instructions there.
Re: [time-nuts] Schematic capture, anyone?
I favor ExpressPCs free schematic generation and board layout But Now I have a whole new list to go looking for. More time-nuts trouble ahead. Regards Paul On Thu, Feb 23, 2012 at 8:36 PM, Bruce Lane kyr...@bluefeathertech.comwrote: Good eve, I must be the exception... I've tried Eagle, most recently about three months back. I can't stand it. I find it, for my purposes, to be about as intuitive as a Salvador Dali painting. I've not yet tried DesignSpark, but it looks very promising. Personally, I use an old version of OrCAD (9-dot-something, I think). Happy tweaking. *** REPLY SEPARATOR *** On 23-Feb-12 at 18:38 Jim Hickstein wrote: What do people use these days for schematic capture (and just possibly PCB layout), for low-budget homebrew stuff? snippage It's been so long since I did this, I still own a T-square and a pile of contemporary relics like rules and triangles. I'll get out my pencil sharpener if I have to. But really, this must be a solved problem by now. For less than $300? I only need TTL, not striplines or any black magic like that. I'm a Mac shop, but can of course run Windows if need be. And to make matters worse, I prefer ANSI logic symbology over shovels-and-spades (or, really, over plain rectangles where you're expected to know what the part number means). This comes from exposure to Control Data, who were big on it back in the day. I even used to be on the mailing list of the standards committee. I suppose that all sank without a trace? If it's still controversial, I apologize in advance for trolling. ___ time-nuts mailing list -- time-nuts@febo.com To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts and follow the instructions there. -=-=-=-=-=-=-=-=-=-=-=- Bruce Lane, Owner Head Hardware Heavy, Blue Feather Technologies -- http://www.bluefeathertech.com kyrrin (at) bluefeathertech do/t c=o=m If Salvador Dali had owned a computer, would it have been equipped with surreal ports? ___ time-nuts mailing list -- time-nuts@febo.com To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts and follow the instructions there. ___ time-nuts mailing list -- time-nuts@febo.com To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts and follow the instructions there.
Re: [time-nuts] Schematic capture, anyone?
Bruce, You are not alone. After 20 years of OrCAD, currently using 9.1, I agree completely. Eagle just seemed...weird. (I should add that I'm a RPN calculator fan - where one chooses data before selecting the operator.) That said, I will probably learn to use Eagle, as that seems to be the darling of the DIY and Sparkfun type folks. Bob LaJeunesse From: Bruce Lane kyr...@bluefeathertech.com To: Discussion of precise time and frequency measurement time-nuts@febo.com Sent: Thu, February 23, 2012 8:36:54 PM Subject: Re: [time-nuts] Schematic capture, anyone? Good eve, I must be the exception... I've tried Eagle, most recently about three months back. I can't stand it. I find it, for my purposes, to be about as intuitive as a Salvador Dali painting. I've not yet tried DesignSpark, but it looks very promising. Personally, I use an old version of OrCAD (9-dot-something, I think). Happy tweaking. *** REPLY SEPARATOR *** On 23-Feb-12 at 18:38 Jim Hickstein wrote: What do people use these days for schematic capture (and just possibly PCB layout), for low-budget homebrew stuff? snippage It's been so long since I did this, I still own a T-square and a pile of contemporary relics like rules and triangles. I'll get out my pencil sharpener if I have to. But really, this must be a solved problem by now. For less than $300? I only need TTL, not striplines or any black magic like that. I'm a Mac shop, but can of course run Windows if need be. And to make matters worse, I prefer ANSI logic symbology over shovels-and-spades (or, really, over plain rectangles where you're expected to know what the part number means). This comes from exposure to Control Data, who were big on it back in the day. I even used to be on the mailing list of the standards committee. I suppose that all sank without a trace? If it's still controversial, I apologize in advance for trolling. ___ time-nuts mailing list -- time-nuts@febo.com To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts and follow the instructions there. -=-=-=-=-=-=-=-=-=-=-=- Bruce Lane, Owner Head Hardware Heavy, Blue Feather Technologies -- http://www.bluefeathertech.com kyrrin (at) bluefeathertech do/t c=o=m If Salvador Dali had owned a computer, would it have been equipped with surreal ports? ___ time-nuts mailing list -- time-nuts@febo.com To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts and follow the instructions there. ___ time-nuts mailing list -- time-nuts@febo.com To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts and follow the instructions there.
Re: [time-nuts] Schematic capture, anyone?
I mostly use Target3001: http://server.ibfriedrich.com/wiki/ibfwikien/index.php?title=Main_Page It's commercial, but there are six different editions starting as low as 59€, with digital+analog, schematics, PCB, autorouting, simulation, it's multilingual (German/English/French), and there is even a free evaluation version somewhat limited in PCB size and pins numbers, but nevertheless worth trying. They are also very responsive. I also tried DesignSparks, which is free, but a lot less powerfull. Just a satisfied user, standard disclaimers apply ! :-) Jean-Louis On 24/02/2012 01:52, paul swed wrote: I favor ExpressPCs free schematic generation and board layout But Now I have a whole new list to go looking for. More time-nuts trouble ahead. Regards Paul On Thu, Feb 23, 2012 at 8:36 PM, Bruce Lanekyr...@bluefeathertech.comwrote: Good eve, I must be the exception... I've tried Eagle, most recently about three months back. I can't stand it. I find it, for my purposes, to be about as intuitive as a Salvador Dali painting. I've not yet tried DesignSpark, but it looks very promising. Personally, I use an old version of OrCAD (9-dot-something, I think). Happy tweaking. *** REPLY SEPARATOR *** On 23-Feb-12 at 18:38 Jim Hickstein wrote: What do people use these days for schematic capture (and just possibly PCB layout), for low-budget homebrew stuff? snippage It's been so long since I did this, I still own a T-square and a pile of contemporary relics like rules and triangles. I'll get out my pencil sharpener if I have to. But really, this must be a solved problem by now. For less than $300? I only need TTL, not striplines or any black magic like that. I'm a Mac shop, but can of course run Windows if need be. And to make matters worse, I prefer ANSI logic symbology over shovels-and-spades (or, really, over plain rectangles where you're expected to know what the part number means). This comes from exposure to Control Data, who were big on it back in the day. I even used to be on the mailing list of the standards committee. I suppose that all sank without a trace? If it's still controversial, I apologize in advance for trolling. ___ time-nuts mailing list -- time-nuts@febo.com To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts and follow the instructions there. -=-=-=-=-=-=-=-=-=-=-=- Bruce Lane, Owner Head Hardware Heavy, Blue Feather Technologies -- http://www.bluefeathertech.com kyrrin (at) bluefeathertech do/t c=o=m If Salvador Dali had owned a computer, would it have been equipped with surreal ports? ___ time-nuts mailing list -- time-nuts@febo.com To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts and follow the instructions there. ___ time-nuts mailing list -- time-nuts@febo.com To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts and follow the instructions there. -- Jean-Louis Oneto OCA GeoAzur - Avenue Nicolas Copernic 06130 Grasse - France e-mail: jean-louis.on...@obs-azur.fr ___ time-nuts mailing list -- time-nuts@febo.com To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts and follow the instructions there.
Re: [time-nuts] Schematic capture, anyone?
Jim Hickstein said the following on 02/23/2012 07:38 PM: What do people use these days for schematic capture (and just possibly PCB layout), for low-budget homebrew stuff? It's been so long since I did this, I still own a T-square and a pile of contemporary relics like rules and triangles. I'll get out my pencil sharpener if I have to. But really, this must be a solved problem by now. For less than $300? I only need TTL, not striplines or any black magic like that. I'm a Mac shop, but can of course run Windows if need be. And to make matters worse, I prefer ANSI logic symbology over shovels-and-spades (or, really, over plain rectangles where you're expected to know what the part number means). This comes from exposure to Control Data, who were big on it back in the day. I even used to be on the mailing list of the standards committee. I suppose that all sank without a trace? If it's still controversial, I apologize in advance for trolling. I suggest the pair Tinycad + freepcb. Both are free, without restrictions on size or the number of layers (nowadays, it is next to impossible to use the fine pitch chips with less then four layers). It is very easy to design your own symbols in Tinycad, and I suggest you do that. Freepcb has a large number of standard footprints, and it easy do design your own, if required. FWIW, I use the batchpcb service for four layers boards - fast and cheap for small designs. tinycad.sourceforge.net www.freepcb.com batchpcb.com Geraldo Lino de Campos gera...@decampos.net ___ time-nuts mailing list -- time-nuts@febo.com To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts and follow the instructions there.
Re: [time-nuts] Schematic capture, anyone?
I'll add another vote for Eagle. It is a German program written in Unix, and ported to Windows. Therefore, you select the action first then click on the object of the action. It takes some getting used to. There has been a pattern of PC layout companies getting cobbled up leaving you with an orphan program, or an upgrade to some very expensive program. Orcad and Protel go gobbled up. Eagle did too, but by a distributor, Newark. They just came out with a new improved version. You can finally draw arbitrary SMT footprints. I think that was the major limitation of the old version. You can of course draw your own symbols any way you like. I have been using Eagle for 5 years now and never looked back. One other drawback of Eagle is that it is difficult to move a design between computers, and there are issues with the way preferences are stored. If you use a part from a library in a design, you are forever locked into that library. Many other CAD systems have these issues. Mentor used to be terrible about having absolute path names, etc. It's worth noting as well that Eagle has just moved to a more open XML-based format for their data files. Assuming they've done a good job (I have no experience with the new version yet), I wouldn't be surprised to see it become the lingua franca of EDA, with a lot of third-party support in the future. Eagle is quirky but it's also inexpensive, reliable, and highly functional, making it accessible to a lot of users at a lot of different levels. Their new public file formats could be a major selling point. I use Sunstone for PCBs myself, but I don't use PCB 123 because I don't want the board house to 'own' my data. In most serious projects you spend a lot of time not only drawing schematics and routing traces, but also building part definitions and writing various scripts. This all adds up to a long-term commitment to whatever tool you select. In most cases you should use Eagle or another program that can generate standard RS-274X Gerbers, and you should always double-check those Gerbers in a third-party viewer before hitting the big green button. The free GEDA Gerber viewer (gerbv) is pretty good; there are plenty of others. All that being said, Eagle V6 is brand new, and historically it's been painful to use brand new major versions of Eagle. Everything went smoothly on a recent project with the last version of Eagle V5, but if you look back at CadSoft's support forum posts dating from the initial V5 release era, there were a lot of unhappy campers. The downside of the new XML file formats is that migrating back to V5 will be difficult or impossible, so you should take some time to be sure that V6 is really ready for your application before going with it. I can't overemphasize how important it is to read their support forums to learn what to expect with any new Eagle version, and what to watch out for. -- john ___ time-nuts mailing list -- time-nuts@febo.com To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts and follow the instructions there.
Re: [time-nuts] Schematic capture, anyone?
I used Eagle for years, but can't say I really warmed to it. I recently changed to DipTrace. Their pricing model seems to work better for me (large but sparse boards in Eagle require $$$ license) as it's based on pin count, not board size. It's really hard to quantify usability, but I no longer find myself dreading drafting a symbol from scratch and things work more like how I would expect them to work. I watched their video demo, found that it made a lot of sense to me, tried it, and was hooked. http://www.diptrace.com/ Scott On Feb 23, 2012, at 6:38 PM, John Miles wrote: I'll add another vote for Eagle. It is a German program written in Unix, and ported to Windows. Therefore, you select the action first then click on the object of the action. It takes some getting used to. There has been a pattern of PC layout companies getting cobbled up leaving you with an orphan program, or an upgrade to some very expensive program. Orcad and Protel go gobbled up. Eagle did too, but by a distributor, Newark. They just came out with a new improved version. You can finally draw arbitrary SMT footprints. I think that was the major limitation of the old version. You can of course draw your own symbols any way you like. I have been using Eagle for 5 years now and never looked back. One other drawback of Eagle is that it is difficult to move a design between computers, and there are issues with the way preferences are stored. If you use a part from a library in a design, you are forever locked into that library. Many other CAD systems have these issues. Mentor used to be terrible about having absolute path names, etc. It's worth noting as well that Eagle has just moved to a more open XML-based format for their data files. Assuming they've done a good job (I have no experience with the new version yet), I wouldn't be surprised to see it become the lingua franca of EDA, with a lot of third-party support in the future. Eagle is quirky but it's also inexpensive, reliable, and highly functional, making it accessible to a lot of users at a lot of different levels. Their new public file formats could be a major selling point. I use Sunstone for PCBs myself, but I don't use PCB 123 because I don't want the board house to 'own' my data. In most serious projects you spend a lot of time not only drawing schematics and routing traces, but also building part definitions and writing various scripts. This all adds up to a long-term commitment to whatever tool you select. In most cases you should use Eagle or another program that can generate standard RS-274X Gerbers, and you should always double-check those Gerbers in a third-party viewer before hitting the big green button. The free GEDA Gerber viewer (gerbv) is pretty good; there are plenty of others. All that being said, Eagle V6 is brand new, and historically it's been painful to use brand new major versions of Eagle. Everything went smoothly on a recent project with the last version of Eagle V5, but if you look back at CadSoft's support forum posts dating from the initial V5 release era, there were a lot of unhappy campers. The downside of the new XML file formats is that migrating back to V5 will be difficult or impossible, so you should take some time to be sure that V6 is really ready for your application before going with it. I can't overemphasize how important it is to read their support forums to learn what to expect with any new Eagle version, and what to watch out for. -- john ___ time-nuts mailing list -- time-nuts@febo.com To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts and follow the instructions there. ___ time-nuts mailing list -- time-nuts@febo.com To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts and follow the instructions there.
Re: [time-nuts] Schematic capture, anyone?
Hi Jim, for many years (over 20) I have used protel (now altium) autotrax- not that I am recommending it to you, but it is a very simple and intuitive program to use and I base my opinion of all the others on it. All the more modern ones I have tried are, for the most part, from fairly, to extremely, counter-intuitive. Until I came across Target 3001. http://server.ibfriedrich.com/wiki/ibfwikien/index.php?title=Main_Page It took me only a an hour or so to produce my first board with the free version using the autorouter and schematic capture, which for me is a very short learning curve! What I was also impressed with is the 3d image of the board which you can rotate to check component clearances, etc. Like Bruce, I persevered with eagle for a while, even got some boards out if, but it was bloody hard work, and about as counter-intuitive as they come so I gave up on that. Having said all that, load 'em all on your machine and have a play- different strokes for different folks. On 2012-02-24 11:38, Jim Hickstein wrote: What do people use these days for schematic capture (and just possibly PCB layout), for low-budget homebrew stuff? It's been so long since I did this, I still own a T-square and a pile of contemporary relics like rules and triangles. I'll get out my pencil sharpener if I have to. But really, this must be a solved problem by now. For less than $300? I only need TTL, not striplines or any black magic like that. -- Cheers, Ken vk7...@users.tasmanet.com.au www.vk7krj.com 'It seems hard to sneak a look at God's cards. But that He plays dice and uses telepathic methods is something that I cannot believe for a single moment.' (Einstein's famous quote on Quantum theory) ___ time-nuts mailing list -- time-nuts@febo.com To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts and follow the instructions there.
Re: [time-nuts] Schematic capture, anyone?
I've been using LTspice for schematic capture and simulation at home. Will the PCB CAD tools being discussed (Eagle, DesignSpark, FreePCB, etc.) import netlists from LTspice? Or do folks prefer to do the schematic capture in a CAD tool and export that netlist to LTspice for simulation? Best regards, Charles ___ time-nuts mailing list -- time-nuts@febo.com To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts and follow the instructions there.
Re: [time-nuts] Schematic capture, anyone?
On Thu, Feb 23, 2012 at 10:52 PM, Charles P. Steinmetz charles_steinm...@lavabit.com wrote: I've been using LTspice for schematic capture and simulation at home. Will the PCB CAD tools being discussed (Eagle, DesignSpark, FreePCB, etc.) import netlists from LTspice? Or do folks prefer to do the schematic capture in a CAD tool and export that netlist to LTspice for simulation? LT Spice is basically just the normal Spice simulator with a schematic capture program acting as a front end.LTspice can export standard Spice net lists and can save to it's own file format too. The spice net lists don't have any graphical information and don't have footprints. I find I don't need to move data from a simulation to a design program because to rarely simulate exactly the target circuit. You usually have to Spice specific stuff components like signal generators or maybe some parasitic capacitance for realism. These parts only exist in a simulation not on the PCB. Chris Albertson Redondo Beach, California ___ time-nuts mailing list -- time-nuts@febo.com To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts and follow the instructions there.
