My first attempt in layout design. Any opinions?

[ytsestef]

Done and DONE!
Most 100μF/16V are 6.3mm diameter, the smallest I found is 5mm. But it doesn't matter that much because there's a lot of space above it for some bending  although I don't think it will be necessary.

As for the ground plane, like I mentioned before, something went wrong the first time around, I tried again and got the desired result (I think...)
I think I get closer each time, this has been really helpful, thanks a lot guys. What do you think of it now?

PS: Maybe we (meaning some experienced guy) should do some PCB design meta thread. And even some PCB making ones (exposure/etching/drilling etc)

 

[wtmnmf]

I'd clean up the silkscreen layer.  Learn how to edit and reposition the component references so that they don't overlap, read in a consistent orientation when possible, etc., even if you won't be silkscreening the board.  You need an easy to read silk layer just for reference. You may want to put some of the component info in the copper layer, especially for the polar caps.

I see a number of places where the 90's could still be removed and a number of 'T' connections that could be avoided by going to a pad instead of the middle of a trace.

The connections to the ground plane do not look like they have adequate thermal relief, which will make soldering difficult.  On a single sided board this is not as big an issue, but it's good to work on the little stuff when it is not so important and develop good habits.  When you have plated through holes and inner layers, etc., it can be tough to get a good connection and even tougher to remove a component without thermal relief.

Make sure that any pots or other panel mounted components are placed properly with reference to the edge of the board.  Better to give a little extra clearance than to have to add washers later. Make a 1:1 check plot and put the components on it to be sure.

You may also want to add registration marks in the copper layer at the edges for cutting the board.

You will want to learn to edit and create component footprints soon, as no layout software will come with everything that you need, and many footprints might be close but could be a lot better with a little tweak.

Oh, as mentioned before, get good at using DRC and when you go to a board house you can make sure that DRC matches their parameters.  You can play with PCB express and see how violation of cost, like using a hole that is smaller than required, can drive the price up.

Looks like you have the basics down and it's just about finessing it now

 

[volker]

Most of it has already been said, you really made a good progress. Stick to the 45°s. Still some improvements, for example: Q2 base to C1, P2 to R1.

Concerning the ground plane, I should have been a bit clearer. 'ripup gnd' obviously only works only if your ground net is named 'gnd'. So look up the name in your schematic and it should work. Then draw the polygon and name it the same. To check if it's connected the right way type 'show name_of_your_ground'. Also do ERC and DRC.

To avoid big areas without copper, play around with the isolate and width settings of the polygon. 10 or 12 mil should be enough. Or you could move C1 a bit down to open the way. You see where this goes.

Another thing you could do is up the size of the pads a bit, if you're going to etch and drill that board yourself they will be pretty tiny. Go to DRC -> Restring and gradually increase them.


Volker


edit: I just took a look at the videos at tangentsoft.net. The tutorial for the ground plane pretty much explains it all. TT#7 and TT#8 are probably worth the while too to cover the basics.