Filed under: Displays

Read | Permalink | Email this | Linking Blogs | Comments

x Before we get started, you might want to download our latest bundle of project files. Inside the zip file you'll find a copy of the connector library and the complete schematic we made last week.

Before we make the board, we'll double check for any wiring problems on the schematic. Clicking on Tools then Erc checks the schematic for electrical problems.

In this case, we're not using the T1 or R1 pins on the MAX232. The two power errors are because we didn't follow the EAGLE power and ground conventions. Again, no big deal. If you have any "nets" that aren't fully connected, you'll get warnings about them here. Even with our "errors" we're good to go.

To create the board, click the not so obvious 'board' button next to the drop down in the tool bar.

EAGLE will as you if you want to create the board from the schematic. Click Yes.

The new window will be black, with the various components sitting to the side. The white outline represents the actual PC board. Everything in this view is movable. If you make a mistake, remember that in EAGLE alt-backspace is undo. You get several undo steps, so feel free to mess around.

Drag the dock connector over to the edge of the board and place it. This is where the nice outline of the connector we created comes in handy. The yellow lines represent the connections that will be made to all the other components from the schematic.

Don't worry if you get this error. In the board view, it just means you tried to move or rotate a part off the board outline. Try it again placing it within the outline of the board. Alternatively, you can make the board really, really big and shrink it down later.

Play with the board layout until you get something you're happy with. We put all of the AV connections on one edge and the data connectors on the opposite. Take your time. Keep in mind that each yellow line will eventually become a trace. Life's easier if you remember the Ghost-Busters motto: Don't cross the streams.

In case you're wondering where the power connector is, we plan to use a spare firewire cable along with our iPod wall charger. That way we can't accidentally inject extra juice to our computer's FireWire ports.

Once you're happy, click Tools and Auto to pull up the options for routing the board. The auto router is one of the fantastic features of EAGLE. The software will play connect the dots to achieve a reasonably efficient trace layout. If it doesn't completely succeed the first time, don't worry. Keep reading.

To get the board to route completely, we had to take the grid to 15 mil. This is pretty fine, but we'll tweak the routing once the computer takes a shot at it. The option to set this pops up when the Auto command is used.

This is a slightly modified auto generated layout. At this point we'd made just a few changes. If you're curious, the fatter traces are replacements. We used them where they'd fit, and they'll be easier to etch later on. Red denotes top layer traces, blue the bottom.

A few tips on tweaking traces: With a trace selected, clicking the middle mouse button will change the layer that the trace lives on. To keep the signal, you'll need "via." Sometimes EAGLE will add them, but you may need to do it by hand.

Here we've moved all the through hole connections (but one) to the bottom layer for ease of construction. Laying out a nice PC board is really an art. This is our result after a few hours of tweaking until we were pretty happy. We made loads changes to the computer generated board. Don't be surprised if the ultimate version ends up a bit different.

Next time we'll bring all the pieces together and finish our super dock. The traces on our board are pretty fine for the usual home PC board making techniques; we'll test out a few and let you know what gives the best results for making your own. See you next week!

Permalink | Email this | Linking Blogs | Comments

Filed under: Features, Portable Audio

We've updated the the EAGLE library we provided last time, so grab the latest one. Download it and save it to the lbr directory under EAGLE's main program directory.

When you start up EAGLE, it should appear under Libraries. If you can see it there, you're good to go.

Create a new project from the File menu. This makes a new folder for the project to help keep things organized. The folder will show up under Projects in the control panel. Rename the new folder.

Select your iPod dock project folder, right click and select New > Schematic. A new schematic window will appear. It's untitled, but associated with the project we created. You'll get a chance to name it when you save the schematic.

Click on the Add button that looks like a logic gate with an arrow.

In the add window, scroll down to the ipod_con library and expand it. Select the IPOD-DOCK-CONNECTOR that we created in part 1 and click OK.

When you hit OK and the outline of the schematic will appear. Mouse over to a convenient area, like the right side and click once on the schematic. The connector will now appear with labeled pins galore.

The Kobiconn RCA connectors we purchased from Mouser aren't in the standard EAGLE libraries. Fortunately, there are a few RCA style connectors. To make your life a bit easier, we created the missing parts and added them to our iPod connector library.

For the iPod connector, we built the EAGLE parts from scratch. By using the search feature in EAGLE we found a couple of existing RCA connectors and copied the package and schematic of the WB0R1. By setting the grid to 0.01 inches we were able to quickly modify the package outline, pads and drill holes to match our parts. We printed the layout and compared our parts to the print. We then tweaked it until the layouts matched up nicely. Your success may vary, but using this method we managed created the correct patterns within three or four iterations for both parts.

Adding audio and video to the schematic goes very quickly. Add two of the single RCA connectors and one triple RCA from the latest ipod_con library. We named the single RCAs R.Audio-in and L.Audio-in. The triple connector will provide audio and video out. Use the Net tool (not the misleadingly named 'wire' tool) to connect the pins of the RCAs to the iPod pins.

We love that EAGLE runs on Mac OS, Linux and Windows, but it's not perfect. Our biggest frustration occurs when the wires just don't connect to the pins. To fix the problems, we use the arrow tool and grab the part in question and pull it to the side. If there's a broken connection, placing the objects pin back over the unconnected wire will usually take care of it.

Fortunately for us, a USB connector similar to ours exists in the EAGLE libraries. Use the add tool and select the PN61729 USB connector in the con-berg library. Place it on the schematic and rotate it so the pins can be connected easier.

The pinout shown above is from the USB page at pinouts.ru. With this, we can wire up our USB connector to the iPod connector.

With the pinout, wiring up the connector is trivial. Just use the net tool and connect the pins.

There's also a similar FireWire connector to the Molex one we ordered. It's not in the Molex library though, it's in the con-cypressindustries library. Go ahead and add this connector to your schematic.

The FireWire page at pinouts.ru gives us this. Again, we just match up the pins to the iPod connector.

Wire up the FireWire connector using the net tool. Don't forget to connect both power and both ground pins.

The iPod serial port is designed to talk to TTL devices like microcontrollers. We want to access it with a standard PC RS-232 serial port. To translate TTL to RS-232 we'll use the ever handy Dallas Semiconductor Max 232 family. The Max-232 works great and uses just a few external capacitors as charge pumps.

This TTL to serial converter circuit from ipodlinux.org shows a standard MAX232 based circuit. Just ignore the pin numbers on the iPod side. Those are for the accessory serial port next to the headphone jack. For our dock connector, we'll connect:

• pin 10 on the MAX232 to pin 12 of the iPod
• pin 9 of the MAX232 to pin 13 of the iPod
• pin 16 of the MAX232 to pin 18 of the iPod

Use the add tool and type in MAX232 in the search box. The capacitors don't really need to be polarized, so we didn't worry about it.

You might notice the lack of power pins on the MAX232. EAGLE places these separately. Click the invoke button, and then click the MAX232.

Select the VCC-GND option, hit OK. Now you can place the pins in a convenient location.

Wire up the power to the iPod dock connector. If you pay attention, you'll see a wiring mistake in this picture that we had to fix.

We're almost done. Just the DB9 connector and the serial enable resistor.

A search for D finds a suitable Sub-D 9 pin connector in the library.

Now we wire up pins 2, 3 and 5 to the MAX232 per the wiring diagram.

The last bit of wiring is a 500K Ohm resistor. First we pick one with a suitable package design.

Then wire up the resistor between the serial enable and the ground at pin 1. The value of the resistor tells the iPod what sort of accessory is connected.

If you're not interested in playing with the iPod using the serial port of a computer, you might want to replace the max-232 circuit with one like the iPod to T&A Remote adapter. It uses a PIC micro-controller to send serial commands to the ipod. The PIC programming (and circuit) could be adapted to add things like hard buttons to the dock, your own infrared remote or an external text display showing the current song.

Finally! Our schematic is finished. Next we'll be fixing any problems, creating the board and building our own super dock. Stay tuned!

Permalink | Email this | Linking Blogs | Comments

Filed under: Features, Portable Audio

In this first part we'll be shopping for parts and preparing to design the super dock. The idea of building a dock with every connection available has been around for a while. It came up on the iPodLinux forums long ago and more recently a prototyping version was featured on Hack-A-Day. To find out just what the dock connector has to offer, we checked out pinouts.ru. Twenty five of thirty pins on the connector are used to deliver line level audio in, out, composite video out, a TTL level serial port, 3.3 volts out (handy for powering accessories), Firewire and USB.


The most challenging part to acquire is the actual iPod dock connector. Others have sacrificed cables, but new connectors are easier to work with. We picked up ours from Ridax on the iPodLinux forums, but lately Spark Fun Electronics started to carry them. (Spark Fun is out of stock today, but they assured us that more are coming in very soon) The connector we used is actually designed for making cable assemblies. The tabs are very small, and you'll probably turn into Smeagol go nuts trying to solder to them.


For the rest of the connectors, we visited Mouser electronics. Here's what we bought (Mouser's part numbers are listed):

• 538-53460-0621 6 pin 1394 PCB Connector
• 571-7877801 'B' USB Connector
• 161-4223 3 way RCA Phono Jack: Red, White and Yellow
• 152-3309  D-Sub 9 pin Connector
• 161-0096-E Red PCB Phono Jack
• 161-0097 Black PCB Phono Jack
  

Firewire and USB were pretty easy, we just searched for PCB mount variants of each. The 9 pin D-Sub connector is for the serial port. For audio and video out, we selected the three connector RCA jack with the red, white and yellow connectors. Mouser was out of the dual read an black RCA connectors, so we bought a single red and black (ok, it should have been white) one to finish the order up. We already had blank printed circuit boards and some MAX 232s and 233s in our parts bin to convert the TTL level signals to RS-232 serial. Oh, and you might want to season your recipe with a power connector or two.


To try our hand at soldering wires to the tiny connector, we made this handy travel charger just before a long, long, long plane ride. (The TSA guys actually laughed at it) Trust us, wiring this up took some patience. Forum user holto2go suggests placing a small piece of paper between the pins to ease soldering.


Because we want to use all of the pins, we decided to mount the connector directly to a pc board. A small screw driver was used to slightly spread the pins of the connector, and it fit very snugly around the edge of our board.


We considered using a fine tip sharpie to lay out the connector lines, but there's still alot of  board design left to do, and it's not very clean looking. In the end, we decided to lay out the custom connector in the latest version of our favorite freeware layout software: EAGLE.


To get started on the custom connector we measured the pins of the connector with our digital calipers. It's pretty challenging to measure the tiny connectors with much accuracy, but our measurements gave us a great place to start. We're going to skimp on some of the details because Instructables has a nice how-to on making your own parts in EAGLE.


To get the width of the pins just right, we printed out test rows with our laser printer and compared it to the pins on the connector.


We found that a .016 inch thick SMD pad was the right width, and starting with a grid size of .0205 inches we made test layouts of 15 pins, printed them out on a laser printer and compared the width to the actual part. Through a few iterations we settled on a grid that was .0195 inches wide. To provide plenty of surface area, we made the pads a generous  .140 inches wide. The pads alternate red and blue to indicate the top and bottom of the board. To make it look good, we added an approximation of what the dock connector looks like. Lastly we numbered the pads in order with the name command.


Next we made a simple schematic layout. It's just a box with the 25 active connector pins. Then we named each pin. We did a couple of repeats, because EAGLE doesn't want to link a schematic pin to two physical pins.


To bring together the symbol and the package layouts, we created a new device called the ipod-dock-connector. Within the package definition we associate the pins on the physical package with the pins in the schematic version. Now all the really tedious stuff is finished and we can start laying out the actual connections.

If you want to start playing around with your own dock designs, you can download the library we created for EAGLE here. Just place it in the "lbr" directory under the main EAGLE program directory. We'll continue the project in next week's in Part II. We'll be designing the dock and laying out the board using EAGLE. From there we'll make our own PC board and complete the super dock faster than you can say "iPod on fire."

Permalink | Email this | Linking Blogs | Comments