prototype pcb design

Hi JonSea, thank you very much for this analysis, I wouldn't have been able to see this by myself.
So, the tracks and via's should be less wide, ok that can be arranged. Now the soldermask: your last comment "..don't think it's what you are expecting.": in what sense do you mean? I probably do not understand the meaning of the last pictures.

Conclusion: version 4, not the first, is to be used, but the via's and the copper track have to be made narrower.. Is that correct?

Drill holes: not present but I assume that is because the drill layer is not shown?

Thks a lot!
Erik

One issue with the via's: they are not meant if a single sided board is needed without hole plating, right? So if the first version (with the "package" definition) is not really right, how should I proceed?

I asked Elecrow, they can provide non-plated holes. I am however not sure if that is possible with version 4?

Erik

Let's start with the last question first. At Elcrow, you won't save anything by building a single layer board compared to a 2-layer board. If you do make a single layer board, I don't know if they plate the holes by default.

This is similar to the board you showed originally with non-plated holes. The one advantage of non-plated holes are that it's easier to unsolder leads from the board because there's no solder connection inside the holes. The solder is only on top of the copper. This type of board could be cheaper to have made, but this is not the case at Elecrow.



The board below has plated holes, and incidentally is 48 cents at Elecrow. The advantages are it's easier to solder since solder flows into the holes and makes a solid connection and you can make easy connections by soldering a fine wire between pads on either the top or bottom.


My preferred style would be a layout like this board, with groups of holes connected together with traces. A 16mil (mil = thousandth of inch, not millimeter) or 24mil trace between grouped pads is plenty wide enough. The green color on the above board is soldermask. It pretty much repels solder, so inadvertantly bridging pads is more difficult.

The pads on the above board are also solder-plated, which is what you'll get from Elecrow; it's better than the bare copper of the first board shown because it resists tarnishing, which makes soldering difficult.


As far as pad size goes...it depends! Standard square header pins fit in a 0.04" drilled hole, allowing for plating thickness. That's probably a safe size for most components on a protoboard but check the manufacture's recommended "pcb footprint" (or look in Eagle libraries) for parts you might use to see what's recommended.

As to which is better, it depends on what you want. I pretty much make a mess of protoboards when I use them!

Here's a couple examples of boards I've had made...almost always from Elecrow by the way.

Just a couple of points about non-through plated holes. It is quite true that it is easier to remove components from non-through plated holes, but:

The trace, without through plating, is not so firmly attached to the substrate.

Also the trace will more easily detach from the substrate, due to high temperature, when you heat the solder to remove a component.

Only some basic observations.

spec

Not to beat a dead horse, but if you want to make exactly the board you originally showed, here's how to do it. I had to think about how to make it with non-plated holes.

1. Draw the outline of the pad group in the Tplace layer. It's 0.3" x 0.1".


2. Position HOLES (not pads) at 0.1" centers.


3. Draw a copper rectangle in the bottom layer, allowing clearance around the edges. I inset it 0.125" from each side.


4. Draw the same size rectangle in the Bstop layer 30. It's shown as a cross-hatch here. This keeps solder mask from the rectangular area and gives you solder mask between each copper block.


5. Lay out the desired array in Eagle.


6. Save the file and run the cam job to create the Gerber files. This picture shows the top silkscreen layer and the bottom copper.


7. And the top silkscreen plus the bottom soldermask; remember, the solder mask layer shows where the openings are.


Now you have a variety of options.

Creating a Gerber NPTH (non-plated through hole) layer isn't an included option in the cam processor, but it's simple. This picture shows what layers you need to include. It will give you an error that says "holes" are included but not "drills" - this is just to show the fab house which holes aren't plated. The drills are specified by the Excellon drill file.

This is great! I will get to this the coming days, have the boards made and I send you one if you give me your address.
Grts, Erik

EEVBlog Dave just published a great video, How is a PCB Made?.

The video shows the steps in making one of his PCBs. You will be amazed at all the steps required to make a circuit board that can cost you as little as a buck or two.

JonSea said:

EEVBlog Dave just published a great video, How is a PCB Made?.

The video shows the steps in making one of his PCBs. You will be amazed at all the steps required to make a circuit board that can cost you as little as a buck or two.

Click to expand...

Fascinating.

spec