After reading a lot of articles on the web, I’m still unsure of how to properly make use of capacitors in my design, so I basically followed the Eagle tutorial and FTDI docs. I’m thinking I should probably have more bypass caps around the driver/inverter, but maybe the frequencies aren’t high enough to warrant more complexity?
Anyway, any feedback on the circuit, the board layout, anything… would be greatly appreciated!
You will get more people looking at your design if you put an image (gif, png or jpg) up instead of the eagle files. Even with eagle, it’s a pain to dl the files and then run eagle. Looking at images on line is so much easier. Use eagle’s file/export/image.
In general, put a bypass cap on every chip. Not 100% necessary but no hard if you do.
Also, I forgot to ask about this. In the DS for the UM232R (similar to the sparkfun breakout), they show 47pF caps on USBDP and USBDM (USB TX/RX lines), but other DS’s don’t show these caps. Any thoughts on that, and what the purpose of such caps would be on such inherently noisy lines.
I would put a polygon on both sides of the board and rename them to GND (i.e. make a ground “plane”). This will really clean up your layout, especially with the bottom being mostly gnd. You can get rid of almost all the top layer gnd lines and shorten the long trace from pin 23 of IC1.
I agree with increasing the width of the Vcc and Vbus tracks though 50 mil is probably more than you need - the most you can draw is 500 mA and I bet you aren’t requesting that so it’s 100 mA.
Also, I forgot to ask about this. In the DS for the UM232R (similar to the sparkfun breakout), they show 47pF caps on USBDP and USBDM (USB TX/RX lines), but other DS’s don’t show these caps. Any thoughts on that, and what the purpose of such caps would be on such inherently noisy lines.
Thanks!
Pete.
The 232RL should have those caps built into the IC its self. It is a “no external parts” type chip. Check its datasheet.
The USB lines should be run as a 90 ohm differential pair. You should have a ground plane anyways (but running a diff pair will require it). I’d recommend rotating IC1 180 degrees to allow for better routing of the USB lines. “U$1” is a lousy designator for a part. Get rid of all the right angle traces. Eww. Clean up the silkscreen - you have silkscreen covering your pads. Also - you seem to be using two different thicknesses of silkscreen for your text. That gives it a pretty unattractive, non-uniform look. I could be wrong about this - but I think it’d be best to ground the shield of your USB connector.
He’s using stock library parts in eagle. these are user submitted so there is little consistency. You can use Name to rename U$1 to IC2.
On legends over pads while not a serious problem, it is kind of ugly. Use smash to allow placement of name. You can also change size at that point.
On the USB lines and right angle issues, if this was a highspeed, it would be super important. As it is, this is probably a fairly low speed application. I’ve prototyped several USB designs on a solderless breadboard and they worked. Not recommended, though.
I like using 45 degree corners instead of 90. It looks much prettier.
One other thing. A number of your pads are off-grid. To get them to line up, try routing from (i.e. start there) rather than to them.
I agree - rotate the IC1 so the USB D+ and D- lines are very short. 90 deg would do it as well
The USB lines should be run as a 90 ohm differential pair. You should have a ground plane anyways (but running a diff pair will require it).
I don’t really understand what action item I should take from this statement. How would I run the USB lines “as a 90 ohm differential pair”? I know they are inherently a differential pair, but is there something specific I have to do in my layout?
The 232RL should have those caps built into the IC its self. It is a “no external parts” type chip. Check its datasheet.
Hmm… The UM232R uses the FT232RL, so I looked at the pin-out picture of the UM232R module in the datasheet, and you can see that the C1 and C3 caps on the board. They actually have these 47pF caps on USBDP and USBDM, not in the IC. I still don’t understand why they would be on the module, but not in the FT232RL datasheet’s suggested designs.
Btw, is your descriptive text on the top copper layer (right side of the board)? It looks far too small and will generate DRCs. Text in copper layers needs to be of larger size and have the ratio turned up to not generate 1mil traces.
Wild guess … Crustcrawler Project? (Hint was the 9.6V bus).
Heh, close. It’s a USB interface to the Robotis Bioloid/CM-5/AX-12 serial bus. They sell one, but it’s like $70 + shipping. I figured that’s a good enough reason to do it myself. I’ll probably end up spending more, but it’s a very approachable project for a newbie.
Philba:
I would put a polygon on both sides of the board and rename them to GND (i.e. make a ground “plane”). This will really clean up your layout, especially with the bottom being mostly gnd. You can get rid of almost all the top layer gnd lines and shorten the long trace from pin 23 of IC1.
I agree with increasing the width of the Vcc and Vbus tracks though 50 mil is probably more than you need - the most you can draw is 500 mA and I bet you aren’t requesting that so it’s 100 mA.
Wide supply tracks for ICs aren’t because of the continuous current they are carrying, it’s to minimise inductance and reduce the effects of transients. Switching outputs can have fast rise and fall times and can inject noise into the supply that can affect other parts of the circuit.
I had some enhanced google-fu tonight and stumbled up some good resources.
First is this [USB design guide PDF, which also happens to explain the 90 ohm differential pair comment from earlier.
Second, I found that searching for “EMC design guidelines” was one path to a goldmine of information that starts to gel the wealth of advice people have on layout. I found [this PDF particularly helpful.
Philba:
On legends over pads while not a serious problem, it is kind of ugly. Use smash to allow placement of name. You can also change size at that point.
I'm afraid you're quite mistaken on that. If the PCB fab does not remove the silkscreen off the pads (some don't, others only do if you ask, and others just do it) those pads will be left very difficult to solder and you'll get a terrible solder joint.
On the USB lines and right angle issues, if this was a highspeed, it would be super important. As it is, this is probably a fairly low speed application. I’ve prototyped several USB designs on a solderless breadboard and they worked. Not recommended, though.
Just because something has worked in the past does not mean it'll always work in the future. The right angle traces issue is mostly a cosmetic thing. But the diff pair is not and needs to be rectified.
There are lot of USB devices that don’t do anything special on the D+ and D- lines beyond making them short. Like I said for low speed it won’t matter.
As for the silk screen, the ink burns off. I agree he should fix it but it’s not a significant as you are making out.
Philba:
There are lot of USB devices that don’t do anything special on the D+ and D- lines beyond making them short. Like I said for low speed it won’t matter.
As for the silk screen, the ink burns off. I agree he should fix it but it’s not a significant as you are making out.
It burns off?
I’m afraid you’re mistaken on that one. Maybe that is true for some specific manufacturer’s silkscreen - but with most that stuff is on there for good. Reflowing the pad doesn’t affect silk on pads. The pads are coated in solder after the silkscreen is applied, not before, so the silkscreen is directly on the copper.
And again - because you’ve seen improper routing of USB lines work many times doesn’t mean it works every time. That’s an illogical argument. If we’re playing “rock paper scissors” and I throw a rock 10 times in a row - does that mean I’m going to throw it on the 11th time as well?