Squirrels have fuzzy tails.
0 Members and 1 Guest are viewing this topic.
Hi,Not bad at all, if it's your first go PCBI have attached the PCB with some markings.Red dots where you have acid traps (inward corners <90° have a tendency to pocket some etchant that will react to moisture and degrade the PCB over time.Yellow dot where you have a flaw because you used the wrong component for IC1 - use the upright one instead.Connect the outer black pour to ground (in the schematic, rename your ground line to GND and when you have drawn the outline of the pour, rename that to GND too (and when it asks, select GND for the "total" name as well, for good measure).Purple... Remove any non-grounded pour, it will act as noise antennas.If you go down to a proper clearance, like 20 mil, there's a good chance that most will be grounded and anything above 32 mil of clearance should be for kindergarten kids anyway I'd enlargen the pads a bit, plenty of room and it makes it easier to make a good strong solder connection (the coppe foil of a narrow "ring" will lift very easy, if a component can be moved the tiniest bit down)If you are going to drill the board yourself, run the User Language Program (ULP, they're scripts really) called "Drill-aid" and when it asks for the drill size, set it to 0.5mm and you will get a fine "dot" that helps centering the drill. Don't set it smller, or some won't etch and too big, you loose the drill centering somewhat.C2 could be a 1206 or 0805 ceramic SMD mounted directly at the pins of the µcontroller on the solder side - then you could avoid the µwave resonant circuit that you have as is and get rid of a lurking potential problem, while getting the effect where it matters the most.SchematicIf you're using a plain old 7805, C3 is around 1000 times to large (make it 220n to 330n) and C1 is 10 times too large.These two caps should be mounted closer to the regulator, as close as possible, although C1 shouldn't be too near the heat from IC1 either, so around 5mm or so away.If you just used the drawing of the 7805 for a switcher, study the datasheet in this regard.You have a junction where none is needed (nor wanted) right above C2.When your circuit isn't larger than a single sheet, don't break it up with strange placements like on the left side of your schematic - if it's one circuit, show that it is, it will make it much easier for you to read 6 months from now. The power part can be a separate entity though.Move the line running through the pin numbers of J1 a couple of notches left.Don't take the power for the motors from the PCB, take it directly from the battery, to avoid influencing the logics.I'm not sure I follow the idea with separate connectors for each white and blue LED. Making a single connector and wire both (white or blue) LEDs to that will save you a connector pair - and the less you mount, the less can go wrong.In general (PCB overlay and schematic alike), "smash all" (ULP) the components and rearrange names and values to same orientation to make it easier to read.The above may sound as harsh critique, but if this is really your first Eagle attempt, it's very good!Never the less, there's always room for improvement and heeding the above advice will take you a good few steps further.
I don't quite get what the smash does, or how to use it
I also don't quite know what you mean about not pulling from the PCB
Regarding the power pulling
Don't take the power for the motors from the PCB,
Another question I just thought of if anyone could help me out, if I do draw directly from the battery, should I use a capacitor as well?
How do you remove the non grounder pour, the purple area?
Also, how do I enlarge the pads, I cannot figure that out either.
How does this look? I tried including the actual sch file, but it was above the max size.
I am going to leave in both forward LED's, so that I can make one light when left servo is running, and the other LED for the Right servo.
I modified power to only use 1, modified everything else you suggested, that I can figure out.
I don't quite get what the smash does, or how to use it, I hit the smash tool and then clicked on components, but they did not seem to do anything.
I also am not sure if I got my 5V going correctly to my 328P, I removed the junctions above the cap, but not sure I did this correctly.
I also don't quite know what you mean about not pulling from the PCB, do you mean I should run a battery off my board, directly to those pins, both positive and negative?
I hope you feel better.
The .sch file is more complete than the board, I kind of stopped that until I get the sch right first.
I think I understand how to use the cap close to the servos, but not exactly sure how to do it in the schematic.
I will try what you mention on the pads, makes sense.
I may have to try the hot cocoa and whiskey trick if get it. Hope you feel better soon!
I am pretty new to all of this stuff, and have learned pretty quickly that before I can get too deep into this hobby, I really need to nail down the basics.
Hi,You're welcome. Happy trails and Merry X-mas (we do the gift swapping tonight here in DK )
f you use the "Smash All" ULP
Not sure if I am missing it, but I am not seeing the attachment. Did you attach the file? Thanks!
Quotef you use the "Smash All" ULPWhat is the benefit of this over just doing it in the GUI?1) frame select everything2) click smash tool3) ctrl-right-click any one object in the selectionNow, everything's smashed, and it took 3 seconds.
I plan on completely re-doing the sch and the brd myself, not because this isn't awesome, it is, but because I feel like I need to do it myself before fabricating it, I will use yours as a guide.
I originally was planning on a reset button, I had it in the schematic, but I had a very hard time getting it on the board because of wiring, so I removed it, thinking for this bot it was not critical, I would like to include it if I can fit it on the board without any crazy jumpers, I am going to play around more.
I did not have a resistor on my power LED's because I was going to solder a 330ohm resistor to each LED, but this makes much more sense.
I don't see any resistors on the forward LED's, so I am going to include one for each, like you did for the power LED, rather than soldering directly to the LED, I will attempt to arrange it so that I can use the same 330ohm resistor for all 3 LED mounts.
It looks like you are including a surface mount cap for c3 under the ATMega 328P, I never would have thought of this, very interesting and very helpful for creating the board, just have to learn to solder surface mount components now!
If I am not so courageous as to solder mount, I am assuming I can just mount this cap outside the chip, and run my +5V around k3, k5 and k11 to get there, this would clearly not be as elegant, but I would think it would work.
I am trying to calculate how big of a capacitor I really need for c5. I am using 2 HS-311's, and they say at no load operating, they drain 180mA each. From what I have read, a standard hobby servo can draw up about 1 amp at startup, so for two that would be 2amps. So, 22uF would be the bottom of the range Admin recommends in his Electronics tutorial, of 1-10uF for every Amp. I am assuming there is some science/art in selecting between 22 and 220uF in this case.
In the schematic, it looks like the +5V that runs through r1 and c4 is connected to Pin 1 (PC6) but on the board it looks like they are almost but not quite touching on the pad of c4 and the pad for r1, was this an oversight or intentional? I think I need to run a wire between the two pads.
With K5, I am curious to why you chose to place the pins the way you did, I would have assumed that A5 would go in the middle of k5, and ground, and +5V on the outer pins for the potentiometer.This will work just fine, I am just curious as I would have done it a bit different.
For the non-grounder pour, I did not see you restrict anything on your board. I am playing round with layer 42, and I see how it works, it's very cool. My question on this is, what is the rule of thumb for removing? Do I remove as much area where the ground is not needed, as possible? The noise factor makes complete sense, so to me I would think I would want to make sure ground has paths to get wherever it needs to go, but no more than that.
I see on your board you do have a .07 width wire going from the cap to the servo for +UB. Is this how you would recommend it, or should I take this wire off the board, and actually use say 24 gauge wire from the +cap to each servo pin?
I am sorry for so many questions, [...]
If you don't mind a 2 pin connector in a slightly odd place, it should be easy.Personally, I'd rather include a few jumpers, than having to use double sided PCB on home etched boards, but while I won't recommend homemade double sided PCB for a beginner, with a little experience it's perfectly doable. If you get the PCB made in a PCB fab-house, on the other hand, it's best to go with double sided PCB, even if one side is more or less a ground plane.
Yeah, always double check anything coming from a fever ridden brain I should have put resistors on all LEDs of course.
Not sure whether you mean "use the same resistor" or "use the same value"?If you have a parallel combination of LEDs, the value should be halved,but it's better to get each a resistor, or any initial unbalance between them will usually widen - in severe cases to an extent where one of them hog all, or most of, the current.
2 pin wire mounted female "headers" are a perfect fit for conventional LEDs btw.
The 1206 size is huge and it is very easy to solderTo solder them, tin one of the pads.Using tweezers, tin one end of the cap lightly.Position the cap over the pads (tinned end on tinned pad).Pres down lightly on the middle of it, while you reheat the solder.Then solder other end adding a very light amount of (rosin core) solder.Finally redo the first, adding aeither the smallest amount of solder or, even better, some fluss.
Here's a photo of a remote I made for my DSLR, none of the SMD's are as large as a 1206, as I build it into a cigarette lighter that had a white LED originally, so space was a commodity. It ain't exactly pretty and I even pinched off a corner of the microcontroller, but it's hidden inside the lighter anyway and it works aces - covers the same distance as the original remote (which has got no lighter) costing around $30-$40. Cost me the ~$0.35 microcontroller, the rest was recycled from junk
Not sure why you want to change the +5V trace?If you keep it as is, just mount a regular cap right where the lettering on the PCB says "100n" now, with one hole directly next to pin 22 (gnd) and one next to pin 20 (assuming a 2 unit pin distance).
Admittedly, I just copied C2 (in the schematic part) to get C5 and left it with its original value.The science behind selecting a value for the servo buffer-cap is more a matter of experience, coupled with knowing the specifics of a given project, as it depends on things like: Battery used, wiring gauge/trace width and how much voltage sag you'll accept.A rule of thumb is only as good as the thumbs (or factors) involved. I usually don't skimp on buffer capacitance, but initially select what my gut tells me for a given application and then measure the sag under the most adverse conditions to see if more is needed.The lower the impedance of battery, wiring and traces, the less capacitance is needed.Without knowing what's outside the board, I'd go up to 470µF or even 1000µF if space allows.
That is what gives the best wiring - ground at the outside, +5V in the middle and the I/O at the pin nearest the controller. When wired to the pot via a connector, it doesn't matter which is which, but it's sometimes make or break for a clean PCB layout.I'll blame it on the fever that I didn't swapped the positions of K10 and K11 as well, as is, it's inconsistent and with the swap, the +5V would have had a straight trace, rather than the angled one.
I didn't have to restrict anything, as all of the pour is connected. If you name the pour the same as the net you want it to be (GND here), it will tell you something like "Polygons may be broken", if it cannot connect all of the pour.
Either way will work. Traces that carries a certain amount of current should always be tinned and with high currents a copper wire or -braid (eg. the shield braid in antenna cable, or similar) should be soldered onto the trace (watch for shorts) - fluss is a good thing with braid.
I will attempt to arrange it so that I can use the same 330ohm resistor for all 3 LED mounts.
QuoteI will attempt to arrange it so that I can use the same 330ohm resistor for all 3 LED mounts.One small detail, depending on how you meant this sentence:The same kind of 330 ohm resistor will work fine.The *same* 330 ohm resistor will not work fine, if more than one LED is on at the same time (such as the power and forward, say.) The reason is that the voltage drop across the resistor equals resistance times current. When two LEDs are lit and both currents go through the resistor, it will give you a different voltage drop, and thus, the two LEDs will be dimmer than a single LED would be when using the same resistor.The reason I say "different" and not "double" is that the voltage/current function of the LEDs is non-linear.If you want a single component, biasing any number of LEDs appropriately, use a Zener with the appropriate voltage drop, assuming the LEDs all need the same voltage.