I'm designing a custom Arduino with Fritzing and have some questions about UNO schematic.
I will send the design to Fritzing Labs to get the PCBs.
I need a "easy-soldering" PCB
Power source:
D1. What diode must I use? I will use a 9v wall adapter with barrel conector
PC1-47u; PC2-47u; C2-100n. What kind of capacitor are these ones?
MC33269D or NCP1117ST50 or what regulator?
In general: What capacitors do I need for the power source and clock (22p ones)
Other:
There is a 100n capacitor between VCC/AVCC and GND/AGND. I will use the analog inputs as digital inputs. Do I need this capacitor?
this will not answer your question directly, but may help you design an easy to use board.
Take a look at http://www.nanode.eu/ .They have built an adruino without using any surface mount items.
This particular board does not have a barrel jack - but easy to add, and does not include any USB (atmega8?) capabilities (uses a FTDI cable).
If you use a "store bought" ATmega328P, you will need a programmer to install the bootloader or your code
In general: What capacitors do I need for the power source and clock (22p ones)
The 22pf capacitors are needed for the crystal to start oscillation.
There is a 100n capacitor between VCC/AVCC and GND/AGND. I will use the analog inputs as digital inputs. Do I need this capacitor?
These are filtering capacitors for the power supply; you most likely do want these or you could experience some erratic behaviour.
Can I use a ceramic resonator with built-in capacitors instead of a crystal and two capacitors?
Will be it accurate enough to have rs485/modbus communications?
I've built many a custom boards with a 328P on-board with an Arduino bootloader. There's really nothing special about it. As long as you understand the information in the Atmel's datasheet, you can use your own parts to build another clone in any way, shape, or form that you would want to.
At the minimum, you need filtering caps on the power input, and a crystal with caps, or resonator. After that, you customize it to your needs. I like to add caps on the VCC lines to the IC itself. If you are using a regulator, again, it's up to you what you want to use. I've driven these things with both through hole as well as SMD parts. Whether you want to drive it at 3V3 or 5V is entirely up to you and what your design requires.
Whenever I start a new project, I always breadboard it first, even if the final product will be using all SMD parts. Doesn't matter. From that point of view, I can take that entire breadboard, stick it on a PCB and I would have exactly what you're trying to do. In fact, I've attached an image that shows the various stages of my most recent project. You can see the whole setup in breadboard form, and the final product using mostly SMD parts. I could've just as easy take the breadboard as is and made that the final product.
[quote author=Jose Francisco link=topic=85064.msg636696#msg636696 date=1325171694]
D1. What diode must I use? I will use a 9v wall adapter with barrel conector[/quote]
This is a "reverse protection" diode. Decide for yourself if you think you might accidentally plug in a 9V adapter that is backwards. If not, you don't need one.
PC1 and PC2 are aluminum electrolytic capacitors. These are "bulk storage" caps. If they weren't surface mount, you'd recognize them as being in nearly any power supply. Make sure you use caps rated at least 18V or more (2X your expected supply voltage.)
[quote author=Jose Francisco link=topic=85064.msg636696#msg636696 date=1325171694]
In general: What capacitors do I need for the power source and clock (22p ones)[/quote]
Next to the chip use Ceramic capacitors (0.1uF). Near the power jack the 47u Aluminum Electrolyic.
The two caps for the crystal should be ceramic and anything in the range of 18-22pF.
[quote author=Jose Francisco link=topic=85064.msg636696#msg636696 date=1325171694]
There is a 100n capacitor between VCC/AVCC and GND/AGND. I will use the analog inputs as digital inputs. Do I need this capacitor?[/quote]
That cap is there to filter noise out of AREF. You are probably okay to not use it. However, I'd suggest adding it in case you want analog input capability down the road.
1N4001 will do just fine, or leave it out as James says.
Yes, definitely. It's not there just for the analog reference, it's the decoupling capacitor for the whole chip.
Yes, if it is a 3-terminal ceramic resonator (the 2-terminal ones needs caps just like a crystal). Accuracy of ceramic resonators is normally +/- 0.5% which is good enough for serial comms.
When drawing use your power and ground symbols where applicable, it cuts down on extra lines in the drawing making it more legible. Avoid drawing lines by the crow's flight, route them horizontal and vertical, make circuit lines cross at 90degree angles. Any intersection that is a connection gets a junction symbol(the large black dot). I know I sound bitchy, but I remark for your own benefit as well as for those who you are trying to enlist help from. A clean drawing can eliminate lots of errors. Speaking of errors mark all un-connected pins as such usually a red 'X'. This helps you to not leave out things too. Most PCB editors complain of unconnected pins when transitioning from schematic to a net list for routing, as it is part of the DRC (Design Rules Check).
ajofscott:
What is IC4, as in the part number? Your pinout does not strike me as a typical 4 channel line reciever.
MAX3097. It's a 3 channel line receiver for encoders.
CrossRoads:
What are the optoisolaters connected to? If there is no pullup's on the other side of J4 pins 2-3-4) you wont see any change on the outpuuts.
The optoisolators are connected to a variable frequency drive and it has internal resistors. This part is fully tested.
The circuit was tested in a hand-made shield with arduino. Now I want to make a board with an atmega328 and Fritzing.
I have made some changes and the project will be updated in Fritzing web.
JoeO:
You need to use a wider copper run for power and ground. How wide? Check your prototype for current draw then go from there.
You should put a decoupling cap next to each IC. You have more than enough room on the board.
Whatever the supply current to a chip you want wide Vcc and ground traces - this keeps the stray inductance low (this allows the decoupling capacitors to do their job best. In fact you only really need the wide traces between chip and nearby decoupling cap.
A ground-plane is a good idea anyway (especially if using analog signals). If the Vcc trace from chip to decoupling cap can run opposite ground-plane and be short then this is ideal. If ground-plane isn't possible, try to make a lattice of (wide) ground traces that cover the board area.
Typically you'd have the power traces 2 to 3 times the width of signal traces (this is also helpful to humans as it makes it easier to see what's what on the board).
