| 6502.org http://forum.6502.org/ |
|
| [31] Using the EAGLE Layout Editor http://forum.6502.org/viewtopic.php?f=7&t=289 |
Page 1 of 1 |
| Author: | Mike Naberezny [ Thu Mar 09, 2000 6:55 pm ] |
| Post subject: | [31.1] Using the EAGLE Layout Editor |
Our resident EAGLE software guru, Douglas Beattie, has some instructions to get you up and running with the EAGLE layout software below. I'd like everyone who wants to participate in the board design to get familiar with the package, and we can all work on it together. ------- There is now a 65XX library, including W65C816, on my WWW site. I encourage you to download EAGLE, from http://www.cadsoftusa.com/ or (in Germany) http://www.cadsoft.de/ - in the FREEWARE section, and "get your feet wet" with it. Install EAGLE Freeware for DOS or Windows 95/98/NT or Linux, and put 65XXX.LBR into the EAGLE directory. Menu:OPEN::Schematic, and give it a name (e.g. TEST.SCH) In the command window of the schematic, type USE 65XXX [enter] to use the library then type ADD [enter] to add a component and a dialog box will pop up. Select a device, such as W65C02P and it will pick one up, so you can place it into the schematic. Click on the schematic, somewhere in the (upper right) positive coordinates of the sheet... Now there is a component on the schem. Press ESC key, or type semicolon ; and [enter] again to end the command. Add other components in a similar way. For example, to add a '138 decoder, USE 74XX [enter] and then ADD 74138 [enter]. Or just ADD and select from the many 74xx devices available. Use the NET command to create a connection to pins on the device. For example NET [enter] and click on the A1 pin of the device. Right click will change the drag option (right-angle, 45-degree,etc.) and double-click to end the net. Use NET with an option (e.g. NET PHI2 [enter] ) to name the signal as you create it. Or type NAME [enter] and click on the net to give it a meaningful name. Or type NAME PHI2 and click on the net (preferred) To label the net, so you can see what it is use LABEL [enter] and click. You can also NAME a component and specify its VALUE.. for example, NAME U1 [enter] [click on G65SC02] VALUE 65C02-4_MHz [enter] [click on G65SC02] To create a board, type BOARD [enter] and it will prompt you, "create from schematic?" -- okay, then you have the board. MOVE (or MOV as most commands can be abbreviated) [enter] click on the component, place it where you want on the board, and then click again.. Right-click to rotate the component before you place. This is just for starters. 65XXX.LBR is available as a .ZIP file from my web site, at http://www2.whidbey.net/~beattidp/comput/x65tools/65xxxE1.zip ** ** ** ** ** ** ** ** ** ** ** ** ** ** Getting Started with Eagle -- Additional Information: You might want to re-configure the default user interface settings for EAGLE -- try this, then decide which is more comfortable for you: At the main EAGLE CONTROL PANEL, select the OPTIONS menu. Select USER INTERFACE Controls -- select "Pulldown Menu" only Command Menu -- select "Text" (or "None" once you know them well) Layout -- Black Background Schematic -- Black Background Help is HELP -- it's an Eagle command, and also available from the menus, so the help options can be on or off; I see no difference. Click OKAY and save user interface preferences, open a DEMO schematic; and see how it looks. That's the way the original Eagle 3.5 looked, before all the funny icons and white schematics -- I like it the old way, but you might not. Also, sizing the window and zooming is one of the things that frustrates people from the start, and they trash Eagle before even trying it.. the WINDOW command is easy to learn in about 2 minutes: WINDOW FIT [enter] puts everything on the design at maximum fit for viewing.. you can also abbreviate as WIN FIT ; WIN [enter] then click opposite diagonal corners then semicolon/enter, ( ; ) and [enter] -- this will zoom to anywhere in the visible area. WIN [enter] and click-hold at one corner of desired zoom area; drag to enlarge the window, then release the mouse. Similar effect as above. Some people prefer to click instead of drag (like me, usually). F3 and F4 keys by default will zoom in and out, by 2 and 0.5.. You can also say WIN 1.2 to scale inward or WIN .8 for outward, or any ratio you would like. The F5 key should center to where the mouse is; actually it seems to pan the window the same direction in which the mouse is offset from the middle of the window. (read that 3 times, 'cause that's the best I can explain it.) Move your mouse a little in the direction you want to pan and press F5, move a little, press F5 -- it's handy, but a bit more tricky to master. -- Douglas Beattie Jr. http://www2.whidbey.net/~beattidp/ |
|
| Author: | uli_E [ Sun Jul 30, 2000 3:13 pm ] |
| Post subject: | [31.2] Using the EAGLE Layout Editor |
EAGLE is an excellent tool for what it costs. I recommend its use even if it will only be used for schematic interchange. There are no limits on schematic size, so you can draw and swap whatever you like, though it's not likely you'll be able to route a PCB for every schematic, since they don't all fit on the 80x100mm board to which the freeware version intended for hobbyist use allows. 80x100 mm is not a bad size for the typical hobby project, though , and I've developed circuits for the 6502 that fit nicely on that size board. A 6502 with an oscillator, a 64Kx8 SRAM, 65kx8 EPROM, and quite a bit of discrete MSI latches and buffers for I/O will easily fit. Now, routing them is another issue. I have, in the recent past not made up boards, but merely wire-wrapped my circuits. There's one thing that would interest me, however. I'd like to know precisely what I have to do in order to make the PCB router autorout using only one layer. I've read a couple of notes about that but have had no success in making it do what I want. Any suggestions? Uli |
|
| Author: | GARTHWILSON [ Fri Jan 26, 2001 3:41 am ] |
| Post subject: | [31.3] Using the EAGLE Layout Editor |
If you find any inexpensive autorouters that are worth anything at all, I'm sure many of us would be interested. Where I worked last, we had OrCad. Its autorouting was a horendous disaster. Sometimes there would even be two adjacent IC pins that were supposed to be connected together, with nothing in the way, and the autorouter would take off in exactly the wrong direction, wander around, and then say "you can't get there from here." Other times that it was successful, it would impress us all at how carefully it chose the scenic route. I have resigned myself to the idea that to do an efficient routing job, or to get the job done at all on a really dense board, it must be done by hand. I virtually always route it while I'm placing parts (instead of later), since optimum placement and optimum routing cannot be separated. They affect each other. About your last comment-- I've never heard of an autorouter that would put in jumpers, have you? That would be interesting. |
|
| Author: | uli_E [ Fri Jan 26, 2001 4:45 am ] |
| Post subject: | [31.4] Using the EAGLE Layout Editor |
I've not found an inexpensive one better than EAGLE. I do use the OrCAD stuff, though nothing after 1992, when they went to Windows. I've had good luck with their old PCBII and the PCB386+, though that was by the standards of the early '90's. I haven't looked at their products since then. I suspect that if you fiddle with the "rules" a bit you may be able to get better performance out of OrCAD, but maybe not. As for the Eagle router and the jumpers, if you raise the "cost" of using the component side of the board enough, there will be few enough routes on that side that you can stick in jumpers if you prefer to make your boards at home. If you're not in a big hurry, there are places in east-central Europe that will make you a nominally 8" x 10" board, 16 layers, solder masked, with silkscreen and gold plating for about $30. If you don't mind that it takes the USPS 20 days to route mail from any European origin except the UK, you can save quite a bit of dough. Of course there's always $$Fed$$Ex$$. I surely wish it were easier (possible) to find the parts you need when composing a schematic in Eagle. I put together one old circuit about the size of a business card with standard through-hole parts, which was a circuit I used to sell back in the '80's, and routed it with Eagle. Though it's not terribly dense or complicated ( a 40-pin DIP, a 20, a 16, and a pair of 14's along with a 40-pin cable mass-termination header ) it autorouted completely if not with a minimum of holes, in about 5 seconds. Needless to say, I was impressed! I took two weeks doing that job back in '81. Now that OrCAD's part of Cadence, I think people will forget about it completely. Uli |
|
| Author: | saipan59 [ Sat Jan 27, 2001 10:59 pm ] |
| Post subject: | [31.5] Using the EAGLE Layout Editor |
What happened to the "PCB project" from last year? Notes related to it seem to be gone from both this conference, and from 6502.org. Has the idea been dropped? Pete |
|
| Author: | Mike Naberezny [ Wed Feb 07, 2001 10:02 pm ] |
| Post subject: | [31.6] Using the EAGLE Layout Editor |
Recently Ted Melton approached me with the same questions. If there is sufficient interest we should continue with the project. |
|
| Page 1 of 1 | All times are UTC |
| Powered by phpBB® Forum Software © phpBB Group http://www.phpbb.com/ |
|