Puma board for FreeEMS

[jharvey]

The silk screen work, is tedious and painful, but when it comes to assembly, it's worth it. I suspect once you've had a chance to catch you breath, you might give it another once over. I find it handy to turn off the hidden layers, copper layers, and any layer that's not silk screen. Then for a final check, I plot the Gerber, and look at it with GerbView. I open the silkscreen, then append the solder mask, then turn off DCcodes. This will be what's actually seen by the silk screen process. GerbView is monochrome, where the design phase is multi color. Simply seeing it in one color, can show some problems that aren't as noticeable in the multi-colored environment.

I see several items you will likely not be happy with, relative to the silk screen. Several areas have tent's, these in theory should work (assuming the mfg allows them), but the via(s) often create an uneven surface (with a hole in the middle) which causes a poor/inconsistent silk screen. I'd recommend trying to keep of the vias if you can. Here are some other more specific areas you might want to look at.

-- P90 is overlapped by D91's component outline. This will cause the P90 indicator to go away.
-- Q17 2N6044 has large text and it over laps other text. Also similar for the LM1914 / U28 and Q1
-- Perhaps rotate C122 such that it fits between the pads. Remember the pads/solder mask will also mask the silk screen, preventing the silkscreen from printing.
-- The 10A from F1 seems to have wandered a bit.
-- "LED" near D49 and D45
-- R181 and R178
-- Q18 and Q19 PNP and NPN designators could probably go hidden, or moved. They currently get overlapped by the footprint silk screen like P90
-- There's a good chance designators like R250 can fit between the pads. Or changing R249 to match R250's placement might also help some. I guess it's a bit of a toss up about if the designator should be between the pads or not. On one hand you should only need the designator to ensure you're assembling it correct. On another hand, diag and modifications are easier if you can read the designator.
-- CONN_20X2 can probably go hidden.
-- You might want to put on a revision number, or some kind of name somewhere. Some way to identify this vs another build. I often do this in the copper, as you know that will be etched. This can be handy where a DIYer might not do the silk screen.
-- Perhaps some lines to separate the circuits into their respective areas. Kind of a box that indicates these components are the RPM input, ect.
-- Perhaps you want to draw the pin out for P74 and other specific net names. For example, when in the field, is P3 for Q1? You'll have trouble noticing it's for the fuse. Putting the net name next to P3, would be handy later on.

One thing I try to do if space and such permits, is to include the value of components like resistors and caps. This can be handy when doing diagnostics. If you have a cap or resistor, and you put your meter on it, it makes for a nice verification. However, it also increases the complexity of the silkscreen and could slow down assembly. So it's a bit of a toss up about what is best. Figured I'd toss it out there as a food for thought item. I often put things like R15 between the pads and 1K just out side near the pads. To find the parts for diagnostics purposes, I usually have KICAD open, and click the part. It high lights and I find it based on visual placement.

X3 doesn't look to hard to me. The case on the XTAL might be a bit larger than the silkscreen indicates, which might make it a bit of a pain to get the other components in there. I would recommend populating the XTAL before resistors an caps. Perhaps move C96 and C97 down a bit to give it more clearance.

About that non-conductive ground ring, you can probably put that on the top layer, and punch one via near the boards primary gnd.

[Fred]

Jared, thanks for your input on this! I appreciate your thorough approach :-)

BIG +1 on the version/name/model/revsion on the board, essential really. +1 on doing it with copper too.

It's about now that I confess to not having opened kicad and looked at this at all, just what you guys post screeny and generated pic wise. I read every post, though :-)

Without a version on the board, how can I list it in the official hw compat/feature spreadsheet/guide? :-)

You might want to consider putting a url of some sort on it too? Just a thought.

"Puma 0.987" or whatever is essential really! Good spotting Jared!

Fred.

[nitrousnrg]

I'm very thankful too, I get sloppy after some time, tending to think "ok, good enough". Then, the next day many things look awful.

About the version... don't worry. I received the mail from the manufacturer, I expect some more fluid communication now. What I want is to put a "Puma logo" (Puma and a couple of feline eyes, or something like that), and a version number. For this board, its just "proto1", clearer than v0.012. After all, with 2 or 3 spins well get to a 1.0 version I guess, no need to be v0.xxxxxx at this beta stage. But, the thing is, I want that in the solder mask, and kicad automates the generation of that mask. So, I hope the mfg can put the graphics it that layer. I'll let you know. I also want to remove mask from some vias for testing, and beneath the CPU for a lower the thermal resistance.

Ok, now with the silkscreen:

First of all, I'm plotting only references, not values.
Just like you, I shut down the front layer, back layer, but also values (Render tab, at the right of Layer). I'd like to have the values, but it'd quite a pain. Anyway,
I placed some references between the pads of a couple of resistors, just to try. If that works, R's and C's can to have both ref and value.

Net names for the connectors is an excellent idea, I like it.

Separate circuits with lines is good too. You did it, and while moving everything around I ended deleting them. Its a good time to bring them back.

By now I believe I've corrected most -if not all- of your advices, at least regarding resistors, caps, and overlapping references. This night I'm naming the connectors pins.

About the ring... I'm not sure about how effective it is, if we have a whole ground plane 1.6mm beneath the ring.

Pushing up as soon as the connectors are labeled :-) Thanks again!

[jharvey]

I get sloppy after some time, tending to think "ok, good enough". Then, the next day many things look awful.

I hear you there. After spending several hours changing the font size, it's gets daunting. I've done the same, and I would agree that stepping back and taking a bit of breath, then getting back to it, is a huge help. I would guess that future release of KICAD will include a bulk text size change option. For now it's a very manual process, or you have to make your own library, such that you can change the default text size, then import the foot print. One option is to change the foot print, then push it to the current board. It's a bit of a hidden approach, but it can be a helpful approach.

What I want is to put a "Puma logo"

I haven't figured out how to do graphics yet. I also haven't look closely. I'll be interested in what you come up with. Also you might want to do the graphics and revision number stuff in both silk screen and copper. The silk screen is easy to read, while the copper is more robust against solvents, abrasions and such.

Oh also, about the black board, you are probably on a good idea. Black will absorb and radiate better then other colors. So Black has some thermal benefits as well.

About the ring... I'm not sure about how effective it is, if we have a whole ground plane 1.6mm beneath the ring.

It's a bit hard to say. The goal is to capture RF energy, the ring will have different inductive and capacitive properties. The plane would be more capacitive, while the ring will be more inductive. In the end, it's not much more than a stab. I saw you had some space on the top layer, so I tossed out the recommendation. I'm not sure how effective it will be either.

[jharvey]

One thought about the graphic, I see GerbView can export to PCBNew. This is typically used if you get a gerber file, and you want to make it into a modifiable netlist attached to a schematic, ect. However, It may allow you to create a graphic with another tool, then import the graphic this way. Just a thought.

Also when you get the latest and greatest up there, let me know and I'll look at it again.

[nitrousnrg]

Oh, let me copy a mail from kicad-developers

Hello,

I've created a quick script to convert an image into a module file for a
PCB. I know there is a program built into Kicad, but it wasn't working
correctly for me, and has no options for adjusting the size of the
output module. This script I wrote is quick and dirty, but has been
working well for me. It is not very optimized, as it converts each input
pixel into one output "pixel" of a configurable size in the module. It
doesn't merge adjacent pixels or anything like that.

The converter is available both as a "web app" and as a standalone
script. For more details: http://img2mod.wayneandlayne.com/

Its a fantastic tool. Just beware that the module generated could be a couple of MB in size. Its unbearable to work with, just add the image as a last step.

Abut the pcb, I'm not liking the costs/lead times/capabilities of local manufacturers. I had good references about http://www.ourpcb.com from guys from Argentina. I'm quoting there to give it a try.

[jharvey]

Great, I read the PCB cost as $83ish for 3 20in^2, and the image script is great to know about, I'll look forward to seeing the image you come up with.

[nitrousnrg]

Good news, I modified the python script posted above to create pads instead of drawings. Now, I can draw in a copper layer, and the soldermask is created automatically. That bring us the possiblity to put a golden logo with black background (assuming gold plating and a black mask)

The modified script is /puma/PCB-modules/img2mod.py, and its going to be pushed up as soon as I finish labeling the connectors. It took me a couple of hours to label the BDM connector ¬¬.

In theory the guys from ourpcb should reply in 24hs, I'm expecting something around $83. Not sure if I asked for 2 boards or 3, though.

Ok, hands on the logo now.

[nitrousnrg]

This is the deal with ourpcb:

Tooling: $75
Each board: $3
E-testing: free
immersion gold: $35
Shipping: $40

1.6mm thick, 1oz copper (fine for testing, it may get thicker later)

Apparently I asked for 2 boards, so it would be $156 (usd). If each costs $3 I'm going for 3 or 4.

I like it, the houses I contacted from Argentina turned out quite crappy (no mask colors, no gold for less than 50 boards, expensive, etc)

[Fred]

Marcos, for postage + 3 bucks each, can I have a few for xmas?