[HELP] for Express PCB experts (marshall shredmaster inside)

[HeaD]

Hey everyone!

A few days ago I found a schematic (thanks to Hanglow) for a marshall shredmaster clone. I've heard often talk about Express PCB, so I decided to give it a try, and I drew up the schematics with Express SCH and linked it to PCB. Now I'm able to see all the links between every pins but I cannot figure out how to make a "clean" PCB scheme. Please can someone help me whit this simple scheme or give me some advices to create and optimize a PCB?

Here is my schematics: http://www.savefile.com/files/1806048

[R O Tiree]

I used the library components and then modified some of them so that:

Electro caps' radiuses are accurate to the ones in my parts bins.

Resistors and diodes can be 0.4" or 0.3" lead spacing, laying flat, or 0.2" or 0.1" spacing standing upright.

Metal film box caps of various sizes.

Ceramic caps with 0.1" and 0.2" spacing.

Create Pot pads - Lay down 3 0.080" pads with 0.035" holes in a line, 0.1" apart, then group them, assign pin numbers 1, 2, 3, then double click the component you just made and type "R" in the part name, then save the custom component. I called it (boring) "Pot Pads".

There are no transistors in this schem, but be careful when you create a project that has them. TO92 cases are not all the same pinout, for example, so create different ones for the different pinouts of the ones in your parts bins. Consult the datasheets that are available free online. You'll also need to create schem symbols for each type as well, just as you did for the TL074.

Armed with this info, you place all the parts on the ExpressPCB page outside the box and assign part IDs.  Now lay down a 0.05" track down the left hand side, along the bottom and up the right hand side for 0V. Then lay a similar rail along the top of the box which is your +9V supply and place a 0.080" pad with a 0.035" hole somewhere on each supply rail. You can move it around later. Place the TL074 in the middle of the board area with it "vertical" and pin 1 top/left.

Move the parts from outside the box into their quarter of the board. You see how each stage has components associated with it? The Input stage lives top right (pins 12, 13, 14) the next stage on the schem lives bottom right, and so on. Now start clicking on pins to see what lights up blue. Often, you can see very clearly how to get a compact layout for the individual circuit "blocks" straight away. I can usually avoid jumpers by laying resistors flat, or make things really compact by standing them up.

For the voltage divider sub-circuit, lay a track under the opamp from pin 3 to pin 10, then extend it up so you can connect R18 and D3 up towards the +9V rail and from their junction C17 to ground rail. Run R19 from the Vref (+5V in your schem) track to the ground rail. You can now lay in R9 to pin 6, D1 and D2 needs to come off that as well, etc, etc. See what I mean about laying flat resistors instead of jumpers? And R10 and C10 can use 0.1" spacing (upright for the resistor), because they're only going from pin 6 to pin 7.

Once you have it all laid out roughly, you can start tightening things up, reducing the spacing between components, rotating parts, exchanging a 0.3" spaced resistor for an upright, or vice versa, if that makes it easier, etc. Eventually, you should end up with a compact layout.

Hope all that helped. I could give more detailed advice on this layout if I had the values of all the components? That would give me the sizes you'd need for the caps. Perhaps you could enter the values in the schem and then provide me with the link?