I have drawm up a power supply on eagle, on bread board it all works fine, but when i did a single layer pcb it didn't. Now one thing i noticed if i use autoroute the current doesn't seem to take the same path as it does on breadboard, it seems to run here and there... does this matter?
1) Your schematic and board don't seem to match. For example there are 6 diodes on the board and only 4 on the schematic. Also, the input power connector seems to have all three pins connected on the board and only 2 connected on the schematic.
2) Have you verified the schematic and layout pin connections for all the library components you have used against the component data sheets for the parts you are using? It might seem strange, but I have seen an error here cause lots of problems.
3) As some of the other responders have indicated, you should be using larger traces for a power supply. You would also have better luck keeping the traces short, by manually routing something this simple. You might have to add a wire jumper here or there, but that is better than letting the autorouter run a trace all around the board as it did for the input to your 7812. If you really must use Eagle's autorouter, you should define a Net Class for your power traces before turning the autorouter loose.
4) You might also try the Eagle news groups (eagle.support.eng or eagle.userchat.eng). Since your circuit isn't a top secret design, consider posting copies of your Eagle .brd and .sch files to make it easier for other Eagle users to help you. At least that way, one could turn off the silkscreen layer to see where the traces really go.
Good luck. I'd be interested to hear what the problem was when you find it.
First, I see an error on the schematic - the AC ground should come from pin 2 of the connector, not pin 3.
The board layout seems to have six diodes, but there are only four on the schematic???
The board layout is poor - the capacitors at the input and output of the regulators should be placed very close to the regulators - you want short fat tracks between the hot side of the capacitors and the regulator, and between the ground side of the capacitors and the regulator. I can't see how you get from C2+ to IC2-in.
Autorouters can be useful, but they can also seriously mess up the routing - things may be connected, but the tracks will go all over the countryside. Strangely, they will often do a worse job on a simple board like this than on a more complex board.
I don't know if Eagle has an auto-placer - but if so, don't bother with it. Autoplacers were invented to appease the marketing department, and rarely do anything useful, even on high-end CAD systems.
I don't know what currents you expect to have on this board, but as a matter of course, I would use .050, or even .100, tracks in a power supply. There is lots of room on the board for Really Big tracks.
A comment on schematic drawing conventions - I consider it Bad Practice to have 4-way junctions on a schematic - if the connection dots go fuzzy (as they will after a few photocopies), it will be unclear whether C1- and C5+ are just connected to each other, or if they are also connected to ground. I would move the whole -12 regulator section right one grid position, so that you only have 3-way connections - that would make it perfectly clear that C1- and C5+ connect to ground.
Peter Bennett, VE7CEI
peterbb4 (at) interchange.ubc.ca
I see that I was not replying directly to the OP due to the poor cropping of the post you replied to with a curt "NO". Sorry about that. and your tag line was in the way. Checking it made me question the need for the original post. I see now that your RUDE response was because you missed the problem and wanted to strike out in anger at someone.
"Chris" schreef in bericht news:jI6jd.60245$ email@example.com...
Printlayout is almost an art in itself and an autorouter is all but an artist. This print is bad in two ways: The placement of some components is wrong and the traces are improperly drawn and to thin. I don't want to cover the whole print but I'll give some examples.
- The trace from the cathode D1 branches. One trace goes to the capacitors, the other to the regulator. That's wrong. The trace should go from the diode to the capacitors and then from the capacitors to the regulator.
- The 100nF decoupling capacitors should be near the regulators. Especially a 7912 can go oscillate like hell when not carefully decoupled. Check the datasheets for it.
An autorouter is not the correct tool to design printed circuit boards like this. Its rules do not care for the rules of even this simple power suply design.
Outgoing mail is certified Virus Free.
Checked by AVG anti-virus system (http://www.grisoft.com).
My name is Graham Knott and I teach Electronics and Microcomputing in a third rate school at Cambridge Regional College, situated in the city of Cambridge, England. I need you money so send me $20 USD for my little reader.
Send money to:
Graham Knott 27, Edinburgh Road Cambridge CB4 1QR UK phone 01223 502751
On Sat, 6 Nov 2004 17:26:21 -0600 in sci.electronics.basics, "James T. White" wrote,
This strikes me as very odd. In my experience, that's the sort of thing Eagle gets right 100% of the time. You draw the schematic, then tell Eagle to "create board from schematic". It gives you a created board file with all the parts, and airwires for all the net-connections. However you proceed to move the parts around and route the connections, the airwires don't go away until you are done.
Chris, A lot of good stuff from James. There is a school of thought on etching PCBs that says the less copper you etch away, the more ecomomical the design; make 'em as fat as clearance allows. (Your etchant lasts longer.) Beefier copper is rarely a bad idea.
BTW, the EAGLE Autorouter never impressed me
--not even on a shortest-route basis. As petrus said, to do a good job, an autorouter has to know a lot of rules about physics and the more you do before turning it loose, the better it does.