I need PCB design tips

[nelson]

I am designing a PCB from an EH clone theory schematic, I have finished a beta version, but its too large and uses too many jumpers.

does anyone have any good tips on how to design a good PCB from a schematic?

[R.G.]

Yeah... lots... but I can't get someone to print the book. I've been through two supposed "custom printers" now and although they didn't get to keep my money, they also didn't print the things.

I guess I have to go back to duplex printing them.

[mikeb]

I am designing a PCB from an EH clone theory schematic, I have finished a beta version, but its too large and uses too many jumpers.

does anyone have any good tips on how to design a good PCB from a schematic?

Go away and design 100 other layouts first, then come back to this one - it will be much better!

Seriously though - study layouts that are available (I learnt by studying RGs, he's got quite an obvious 'style' that is very neat and works well for 'signal flowing through from input to output' FX pedals), and copy bits'n'pieces. Experience counts for a lot. Don't expect to get 'good' ones at your first go.

There are lots more tips - I'm sure you can find someone searching through the forum. And get RGs book when/if possible.

Mike

[nelson]

I think I am getting there, its getting smaller lol. I guess I will just have to learn via trial and error.


I think this one is preferable over the echoflanger which was my other choice. I will post up the beta 2 version, or maybe I will stick it up on a website, I have webspace doing nothing.

[pjwhite]

Although you're probably not going to build a large number of these boards, one way to approach the problem is to assume that you are.  Google "Design for manufacture" for some ideas.

Hole sizes: Use the right hole size for each part*.  Data sheets will give you dimensions of IC pins, resistor leads, etc.  Take the tolerance of the part and the tolerance of the hole size into account.  A typical hole size for resistors, capacitors and IC leads would be 0.032 inch.  Jacks, connectors, switches, etc. will generally have larger leads and require larger holes.  If any parts have square or otherwise non-round leads, be sure to use the largest diagonal dimension to calculate the round hole size.  Some jacks and switches have flat pins that would fit best in a slot.  A 50 x 200 slot is better than a 200 mil diameter round hole for a 40 x 180 mil flat pin.  It will give better supprt to the part and use less solder.  Board manufacturers can make slots (by drilling a series of small holes, or by using a router).

* Going a little bit larger is usually OK, and can save money by reducing the number of different tools needed to drill the board.  Going _way_ larger is not recommended because soldering starts to become more difficult when component leads are rattling around in a hole that's too big.

Pad sizes: Use pads that are significantly larger than the holes in them.  You don't want slight errors in hole placement to drill through the edge of a pad, and you need enough copper around the hole to make a good solder joint.  On the other hand, pads that are too large tend to suck the heat away and make soldering difficult.  Try 80 mil (0.080 inch) circles or 80 x 150 mill ovals for IC pads as a starting point.  Jacks, switches and other components that will be subject to outside forces should have larger pads to anchor them securely (using the correct hole sizes also help to secure these parts)..

Trace widths:  In general, use the widest traces that you can.  For this type of board, I'd say an absolute minimum trace width would be 12 mils (0.012 inch), with 50 to 100 mils used for power traces.

Trace spacing: Use generous spacing between all lines and pads.  12 mils (0.012 inch)  or more would be a typical minimum spacing for this type of board.

Trace routing: In general, try to use the most direct routes possible.  Avoid running traces between adjacent pads on an IC, and if you have no other choice, be sure to observe trace width and spacing rules.  Route your power traces first, and try to use a "star" pattern, where power is distributed to your various components with one trace feeding each IC from a single power distribution point.  This would apply to your positive (and negative) power supplies, as well as ground.

Part placement:  All ICs should be oriented in the same direction where possible.  Leave enough clear space around components for probing.  Keep in mind the body dimensions of all components.  Electrolytic capacitors are notorious for coming in various diameters for the same value.  If you have any parts that will generate significant heat (voltage regulators, large resistors, etc) be sure to allow plenty of elbow room around them.  Include space for heat sinks where necessary.  Lay out all parts on a 0.100 inch grid where possible, and pots and switches should be placed in an aesthetically pleasing and symmetrical arrangement where they will come through the front panel of the box.  
Look at the schematic and place components together logically.  On op-amp circuits, place feedback resistors close to the input pins of the IC.  On input sections and other places with low level signals, keep the layout tight.  Power supply bypass capacitors should go as close to their ICs as possible, keeping placement rules in mind.

Some of these tips seem contradictory.  That's where the art comes in.

[Dirk_Hendrik]

Some comments from own experience:

On the above (excellent) post one comment. Having all ic's in the same direction will avoid mistakes when putting them in their sockets. Other than that there's no need. If the design becomes simpler by rotating this can be an option.

NEVER overrule the design rule checker. An error is easy made. With a few overrules the chance is large that one of these overrules justified.

From my own experience: keep connections between high resistance locations (such as Opamp and fet inputs as short as possible. These are the locations where you pick up hum and other noise.

Lay out long lines (from one side to the other side of the board for example) first. These are the hardest to route when all short connections have consumed up space. Solving short connections later is way easier.

As for the power supply lines. In contradiction of the previous post I usually save those for last. When using wire bridges in the supply lines very often one bridge can connect a lot of points needed to connect. With other connections this wire only makes 1 to a few connection. This saves time in mounting the wires.

If a component need to be at a certain location just dump it there, regardless of other traces and components and start fixxing up after that. Let the design rule checker work for you (instead of being annoying) and tell you where you are wrong. Working like this saved me hours.

Don't make loops. View all traces individually (by turnng off the others) to check this.

Be aware that the last 10% to be routed  consumes by far the most time.

STOP in time. When you just can't get those last connections done try again the next day. Chances are big you'll manage then easily.

[nelson]

WOW, some good stuff here, thanks guys. I have managed to condense from my original design, its still to big, 19cm across, I will continue to condense it.

this is definately something that needs ALOT of practice.

if anyone wants to see my efforts drop me an email, I will ship it off in jpg format.

[guitar_dave]

Very good advise offered in this thread.....well done.

Don't underestimate this statement made by a previous poster....

"STOP in time. When you just can't get those last connections done try again the next day. Chances are big you'll manage then easily."

Wish I had a dollar for everytime I was working on a design late at night and run into that "problem trace" that you just cant see how your going to route it.   This best thing to do is just leave it alone....and come back later to take a fresh look at it.

(Or you could just turn the autorouter on and hope for the best..lol...just kidding).