| Author |
Message |
Lofi Ninja
Joined: Oct 25, 2008
Posts: 143
Location: Jupiter
|
 Posted: Thu Jan 15, 2009 11:08 am Post subject:
 I want to learn how to make pcb layouts... |
  |
|
Hellooo..
I would like to learn how to make PCB layouts..
Which program?
I'm using Windows XP btw.
Any guides?
Thanks!
_________________
www.youtube.com/user/lofininja |
|
|
Back to top
|
|
 |
ericcoleridge
Joined: Jan 16, 2007
Posts: 889
Location: NYC
|
| Posted: Thu Jan 15, 2009 11:26 pm Post subject:
|
|
|
I'm trying to learn how to layout PCBs also. I downloaded this free software:
DIY Layout Creator |
|
|
Back to top
|
|
|
gubbeper
Joined: Oct 10, 2005
Posts: 50
Location: Sweden
|
| Posted: Fri Jan 16, 2009 12:11 am Post subject:
|
|
|
I haven't made any advanced layouts my self, but I found these videos really helpful in getting started with Eagle:
http://tangentsoft.net/elec/movies/
Good luck.
_________________
/Per
I'm on Twitter |
|
|
Back to top
|
|
|
LetterBeacon
Joined: Mar 18, 2008
Posts: 454
Location: London, UK
|
| Posted: Fri Jan 16, 2009 5:17 pm Post subject:
|
|
|
| What a useful site! Thanks a lot for the link! |
|
|
Back to top
|
|
|
R.G.
Joined: Feb 10, 2009
Posts: 2
Location: Austin TX
|
| Posted: Tue Feb 10, 2009 11:35 am Post subject:
|
|
|
I wrote a book explaining how to think about, prepare for, and then lay out through-hole PCBs for the beginner. It's sold through Small Bear Electronics.
The approach is not specific to any one PCB layout program, and concentrates on the kind of things that a beginner will run into immediately, as well as some more advanced concepts.
Let me pre-apologize if this sounds like offensive self advertisement. I wrote this mainly as a service for the beginner at guitar effects layouts. The quantity sold is not large, I don't handle the sales, and I don't make that much money from it. So far no one has complained that it wasn't useful in starting up at PCB layout, and there have been many positive responses.
It's there if you're interested. |
|
|
Back to top
|
|
|
Rykhaard
Joined: Sep 02, 2007
Posts: 1290
Location: Canada
|
| Posted: Tue Feb 10, 2009 12:12 pm Post subject:
|
|
|
| R.G. wrote: | I wrote a book explaining how to think about, prepare for, and then lay out through-hole PCBs for the beginner. It's sold through Small Bear Electronics.
The approach is not specific to any one PCB layout program, and concentrates on the kind of things that a beginner will run into immediately, as well as some more advanced concepts.
Let me pre-apologize if this sounds like offensive self advertisement. I wrote this mainly as a service for the beginner at guitar effects layouts. The quantity sold is not large, I don't handle the sales, and I don't make that much money from it. So far no one has complained that it wasn't useful in starting up at PCB layout, and there have been many positive responses.
It's there if you're interested. |
Now THAT is cool to read about! I haven't any troubles in laying out my own PCBs for "poor man's surface mount" (no thru-hole at all, except for the 0.156" Molex power connector). But I'd love to read about examples in laying things out, as my layouts are still somewhat unorganized looking, outside of the chips themselves. 
Shall see what cost of it is. If it's cheap enough, I'll order it when I place my next order with SmallBear.  |
|
|
Back to top
|
|
|
haxster
Joined: Feb 01, 2006
Posts: 246
Location: MONTEREY PARK, CA 91754
G2 patch files: 2
|
| Posted: Wed Jun 03, 2009 1:16 pm Post subject:
|
|
|
Abacom Sprint PCB layout is a good 2 Layer software that is not as intensive as Eagle/CAD. It is very easy to use also.
The only problem is the library is small, so you will need to draw out your own parts you use which is easy. |
|
|
Back to top
|
|
|
Tim Servo
Joined: Jul 16, 2006
Posts: 924
Location: Silicon Valley
Audio files: 11
|
| Posted: Fri Jun 05, 2009 1:54 pm Post subject:
I want to learn how to make pcb layouts... |
|
|
I can highly recommend KiCAD as a PCB layout program. It can generate printouts if you etch your own boards, or Gerber files if you have them professionally done. It has a reasonable library of parts, and doesn't have any size restrictions (might be limited to four layers, but if you need more than that, you're probably laying out PCBs for a living using a high-end CAD tool). The best part? It's FREE!
http://kicad.sourceforge.net/wiki/forums.html/Main_Page
Note: I'm not affiliated with KiCAD in any way, but I have used this program to lay out all the Magic Smoke PCBs, in addition to a couple of commercial PCBs done for others. Despite a few quirks, I am very pleased with this program.
As far as rules for laying out a board, here are a few I use:
1) Breadboard your circuit first and make sure it works. I've been bitten by some small problem every time I've skipped this step. Even then, it's possible to have an error on your PCB, but breadboarding the circuit is a really good first step.
2) Make a few paper and pencil sketches to roughly plan the placement of ICs and major components. Look at the signal flow and try to arrange things for the shortest paths and to reduce cross overs (especially for audio signals).
3) Try to keep all ICs oriented the same way, and facing in the same direction. This makes the board easier to build and reduces the chances that an IC will get inserted backwards. I usually put my ICs horizontally, with pin 1 in the lower left. Commercial PCBs are done this way to reduce errors and to make automated component insertion easier.
4) Try to keep all Rs and Cs facing the same way. Again, this makes the board easier to build and is done on commercial boards to speed assembly. I usually put my Rs and Cs oriented vertically, although I sometimes violate this rule if I need to use a component to jump over an area with especially tricky routing. I'll only do this for a few components, and only to avoid having to place a jumper. Of course, this is a much easier rule to stick to if you're doing a double sided board, but it is still worth keeping in mind.
5) PUT DOWN YOUR POWER AND GROUND TRACKS FIRST! Again, this is easier to live with on a double sided board, but you really do want the supply lines to be as short and fat as possible. If you leave the power and ground traces to the last, you'll inevitably have to compromise and route them all over the place. Also, don't forget to add pads for bypass caps for every IC. Even is you don't end up needing them, I'd rather have the pads and not use them.
I think that's about all for now, but that should be enough for a start 
Tim (getting shorter and fatter as we speak) Servo |
|
|
Back to top
|
|
|
e-grad
Joined: Sep 12, 2008
Posts: 142
Location: Berlin
|
| Posted: Thu Jun 11, 2009 6:24 am Post subject:
|
|
|
| Tim, thanks for taking your time to share your experience in detail. Highly appreciated. |
|
|
Back to top
|
|
|
R.G.
Joined: Feb 10, 2009
Posts: 2
Location: Austin TX
|
| Posted: Fri Jul 10, 2009 6:00 am Post subject:
Re: I want to learn how to make pcb layouts... |
|
|
I've done a lot of layout, over a 30 year period, and what follows is just my personal experiences and opinion.
| Tim Servo wrote: | I can highly recommend... The best part? It's FREE!
... Despite a few quirks, I am very pleased with this program.
|
I've used many different programs for PCB layout. The essentials are that it
- be able to work in layers
- be able to easily select and work only on one layer at at time
- be able to place on a grid easily
Making Gerber is necessary for pro fabbing, but everything else is negotiable. Everything. I've done layouts for high volume production with pads on mylar.
| Quote: | | 1) Breadboard your circuit first and make sure it works. I've been bitten by some small problem every time I've skipped this step. Even then, it's possible to have an error on your PCB, but breadboarding the circuit is a really good first step. |
It's not a really good step - it's crucial. Going right to PCB is ingenuous at best.
There is an equally critical second step missing: define any external-world placements or mechanical limits before you do any other layout operation. The layout of components especially for analog parts and circuits flows outwards from mechanical constraints of control placement and board size limits, not the other way round. The only possible exception is if you are willing to box it up in an enclosure that is free to be so big that you can put anything inside. In my experience, anything I'd want to use later has at least some kind of physical constraints; lay these down FIRST.
| Quote: | | 2) Make a few paper and pencil sketches to roughly plan the placement of ICs and major components. Look at the signal flow and try to arrange things for the shortest paths and to reduce cross overs (especially for audio signals). |
I agree with looking at signal flow, but look at signal flow in terms of partitioned sub-circuits. Every non-IC layout is done in terms of IC based subcircuits. Mentally cut your whole circuit into subcircuits of manageable size, about one IC plus directly linked parts, and place these in a signal flow. Except for the hugest boards or the smallest circuits, there will usually be some overlaps involved. Go to a U-, S, or Z pattern to keep like nearest like; where you have to make a choice, group like-signal-levels together and like-impedance-levels together. Isolate high impedance inputs like any FET gate from any high-signal-level sources.
| Quote: | 3) Try to keep all ICs oriented the same way, and facing in the same direction. ...
4) Try to keep all Rs and Cs facing the same way. ...
|
More importantly, orient all physical-orientation parts the same way; all ICs the same way, all electro caps the same way, all diodes the same, way, all transistors the same way. I agree - random orientations is like leaving little hidden traps sitting around to wander into.
| Quote: | | 5) PUT DOWN YOUR POWER AND GROUND TRACKS FIRST! Again, this is easier to live with on a double sided board, but you really do want the supply lines to be as short and fat as possible. If you leave the power and ground traces to the last, you'll inevitably have to compromise and route them all over the place. |
This one is not straightforward, and it qualifies for something you think about right after physical constraints. For audio circuits, best power and ground distribution is star distribution per subcircuit. This is a sufficient (if not strictly necessary) solution to enforce that you get no power supply crosstalk or interaction from power impedances. Beyond that, you need to control where power and ground currents flow by isolating them on point-to-point traces. This is critical in, for instance, power amplifier and power supply circuits more than low signal. As frequency increases, power and expecially grounding changes. At RF and for fast logic (over 1MHz, which isn't all that fast, I guess) go to ground planes. Even at audio, use local guard rings and ground planing to isolate high inpedance points.
All that is preparatory to saying: for audio circuits of smallish size (perhaps under ten opamp packages), placing power and ground first is not mandatory and is counterproductive to generating tight layouts. To a first approximation, power and ground should be ignored for placement. Power and ground go everywhere, so there is no net positive or negative effect to considering them in placement.
Once you get subcircuits placed (on the signal flow, within the physical constraints) then route power and ground. It helps if your layout package can highlight all the pads on one net - like ground - so you can gather ground points locally within a subcircuit, then plot (in the sense of scheming) how you want your ground return to work.
I should say "ground returnS" because there are at least two kinds of ground that you should distinguish. These are reference ground and what i call sewer ground. Reference ground is what carries the system-wide zero-voltage reference voltage. This is used to compare signal voltages against, and is used for things like referencing inputs. Sewer ground is what returns the "used electricity" back to the power supply for recycling. The choice of the word "sewer" is deliberate. That ground is contaminated with current spikes, random signal variations, class AB currents, and so on. If you mix up the two grounds, you are contaminating your inputs with the sewage, getting crosstalk and the sincere possibility of oscillation.
Highlighting the ground net, and to a lesser extent the power net lets you isolate ground-current induced effects. To the extent that reference ground carries zero current, as it should, all reference grounds can be connected up at random, no scheme for how they're routed. The need for fat, wide traces on sewer ground and its pairing with power traces is an attempt to provide a low-inductance, low-resistance path for sewer ground currents to minimize problems with ground offsets when the local sewer ground is used for input reference; this style of routing power and ground was developed during the TTL logic era and back-applied to high speed opamps. TTL needed it because of the high transition currents and opamps needed it because of the intermixing of reference and sewer ground.
So break ground (and power, where you use power to generate references) into reference ground and sewer ground. Route them separately back to the power supply.
Local decoupling is there to provide a bucket of current for sudden power needs which cannot be supplied by the power supply because of impedance between the IC/active device and the power supply proper. It is best thought of as "what to do until I can get some current through the power supply inductance". |
|
|
Back to top
|
|
|
|
Forum index » DIY Hardware and Software » The layout factory
FAQ
Calendar
Search
Memberlist
Usergroups
Register
Profile
Log in to check your private messages
Log in
Chat Room
