OpenServo.com

[mpthompson]

OK, I finally have something to show for many hours of work.

http://www.openservo.com/moin.cgi/PrintedCircuit2

This design has all components that are indicated in the schematic. I haven't yet done a thorough inspection so it wouldn't surprise me if there are significant errors at this point. I tried to keep signal traces reasonably thick (0.010"" is the narrowest) with the power traces being extra thick (0.015"" to 0.025"").

I'm not too happy where I had to place the large 33uF capacitor. Hopefully I'll be able to rework it a bit.

I'm trying to keep the board suitable for a full board design that is soldered directly to a motor and a half-board design suitable for servos such as the Hitec HS-645MG and the Blue Bird BMS-620.

-Mike

[mpthompson]

I created a parts placement diagram to illustrate how the parts would fit on my version of the PCB here:

http://www.openservo.com/moin.cgi/PartsPlacement2

I already discovered I'm missing R8 which I'll need to add to the PCB.

-Mike

[RifRaf]

took a few pulled apart servos (mainly hitec though full size boards and 2/3 size) with me driving today and had a few thoughts:
1. can the 33uF cap be replaced with a through hole tantalum to be able to move it out the way a bit, the thoughhole will use alot less board space as well for pads even though it goes through board

2. the connects to the servo pot do not have to be through hole or even located in a row, placing then in convenient sections will help layout and make room on other side of pcb. motor connects for small pcb can be done the same way or 2 small through hole pads in the best locations

3. as every 0.1mm counts on this board do we all agree that this board size will fit most standard servos
http://rifraf.rememberit.com.au/openservo/servo-pcb.gif
am sure you guys have been though this but i want to be clear before i try again. the yellow is board size and the copper is maximum area for traces or parts to be placed, definatly parts maybe traces can be against the plastic housing ok?

4. 10mil traces as the thinnest sounds better to me. and the 15mil power traces will handle the current fine as well. may try do an eagle design based around that next time Mike. btw. do you guys prefer talking in mm, inches or mil? being in australia we use all so am happy to work in the units most comforatble to the rest of you.

[mpthompson]

I'll check into the tantalum capacitors. My intention is for the 4.7uF to be tantalum and it makes sense that the 33uF be tantalum as well. It's been a while since I checked into capacitors and the board space wasn't as tight on the earlier version of the servo.

The through holes for potentiometer on the PCB is simply for me to support the Futaba S3003 easily. These are very cheap servos I buy in quantity for testing. They disassemble very nicely and Futaba doesn't have the tendency to put hot glue over everything such as HiTec does. Creating a variation of the PCB design without through holes would be fine as most other servos seem to have wires rather than leads from the potentiometer.

Rather than focusing on a particular PCB shape at this time, I think the primary focus should be on a layout that is flexible enough to be adapted to most any PCB shape. The final shape of the PCB will always likely be left to the enduser making their own OpenServo for their own needs. If we are successful, I imagine we will soon have a whole library of PCBs that people can choose from that all conform to the basic design and work with the OpenServo software. I'm interested in your drawing because it is another data point to tell us how tight things have to be to fit standard servos. I'll check your measurements against what I have so far. I hope this approach makes sense.

I'm OK with metric or English units. Being the US I tend to think in inches and such, but I can easily deal with both types of units. Metric adds an international flavor to the project .

-Mike

[ginge]

Great looking PCB, Mike!

I printed one out to scale to see if the parts that are available to my locale fit ok.

The only components that I had trouble firring in was the H bridge diodes. The footprint of the ones I had to use are slightly wider.

I will create an eagle version of the official design, and commit to CVS

Barry

[ginge]

Just a quick question regarding the components...

did you change the package sizes on the components, as I am having trouble finding the smaller component sizes you used. Can you do a parts list?

Cheers
Barry

[ginge]

Is there any merit to putting a xtal on the PCB. I have read the extra precision is worth it when using the ADC.

As we are going down the route of signal filtering using caps, why not go the extra mile.

Barry

[mpthompson]

Barry,

I'll start a parts list tonight and start doubling checking things for size and fit.

The 1N4148W diodes I'm using are the same as those used on the original OpenServo. I'm also using the same pad size on the PCB. A link to the datasheet can be found here: http://www.openservo.com/moin.cgi/Datasheets

Looking at the board again I may have made the space around the diodes a little too tight as they are a little wide. I'll print out the circuit on a laser printer to test fit some pieces and double check spacing between the diodes and MOSFETs.

I'll need to double check the size of the inductors and the 4.7 uF cap as well.

Regarding a crystal, I just don't see where it could fit on the board. However, I haven't really investigated it. With a crystal the CPU can be driven to 16 or 20 MHz and it would indeed be quite fast. At this point, I'll leave it as an exercise to someone else to create a layout with a crystal. I'm kinda itching to get back to the software development with a few working servos. Porting the software was a cinch compared to the PCB layout .

By the way, I don't want to necessarily imply there is any official design of the OpenServo. However, at this point there are distinct advantages to have a common reference design as we work out the early details to get to a circuit proven to work. I certainly appreciate your work with Eagle.

If the designs start to diverge let's at least give them names and their own sections under the Wiki so it clear to people that there are distinct, but similar designs they can choose from for the OpenServo.

-Mike

[RifRaf]

the consistant layout is a good idea, seems that so far we agree Mikes design is the one to work on. have nearly got it routed in eagle as well though have the same issues that Barry has with part sizes, already on the previous version i edited a few smt pads because they seem alot bigger than the expresspcb software pads on some parts. just one thing i did notice though with the diodes, the Minimelf package 1n4148 (digikey LL4148DICT-ND) is higher power, shorter and cheaper, though a bit fatter, may be an option? has the 8 pin header idea been shelved for now? personally i think the edge connector is cute but you guys have had more experience actually using them

[mpthompson]

I updated the files on the following to pages with updated images. Basically putting a little more space between parts and correcting a few errors I found such as the mitting R8. It's not 100% yet, but getting close.

http://www.openservo.com/moin.cgi/PrintedCircuit2
http://www.openservo.com/moin.cgi/PartsPlacement2

Is there an image format I can convert these drawings to that would be more suitable for examining?

I'll be putting together a parts list tonight and starting to verify the sizing and placement of items. The large 33uF capacitor is still bothering me, but I'll probably have to live with it for now. I'll look into using a smaller tantalum capacitor if possible.

Regarding the ExpressPCB pad sizes. After getting the first OpenServo board made I went back and adjusted some pad sizes based on what worked better for me for hand soldering. I think a number of pads were made smaller. Also, I created pads for some components based on suggestions from the datasheets. That may explain some of the weird sizing you see in my design.

After I get things straightened out under ExpressPCB and have placed an an order for some boards, I'll start looking at Eagle.

For me the edge connector seems to work well with the servos I've been working with. They are convient for getting the board bootstrapped (making the little adapter card is pretty easy) and for solding the SDA/SCL/V+/GND wires to when putting a servo together. An 8 pin header could work, but you would need the header in place for bootstrapping, but probably don't want it in place for normal servo operation.

Rifraf, I checked the size of my current design against the measurements in the drawing you provided. My layout is too long by about 1 to 2 millimeters. Things are kind of tight, but there are probably a few things we can do to make the layout work better for that board configuration. Convert the potentiometer to pads as you suggested and make the power lines use 0.15"" traces rather than the thicker 0.25"" traces I'm currently using.

-Mike

[mpthompson]

Some of the problems I see in my current design are:

The large capacitor C10. Hopefully we can find a smaller capacitor.

The signal that snakes under D3 and Q3 bothers me. It's a pretty tricky signal to route. Any other ideas? If we can tolerate a via under the ATmega8 things could get a little easier.

The trace that cuts under R7. This is probably a little easier to fix than the one under Q3 and D3.

Things around and above U3 look a little tight.

-Mike

[andylippitt]

I'm not expert here, but I've found that when soldering a wire to a board, it's nice to have the physical strength of going through a hole. With the pot, I don't think this is as big a deal, but it would be nice to have that strength (and perhaps vibration resistance) on the external leads.

[ginge]

I have created an eagle version of the ""V2.0 Mike edition"". I suggest we at least use this as a starting point for future work, as it has nicest layout so far.

These layouts are very close to the original design, although I had to use replacement components for the inductors.

I have uploaded the new layouts to CVS, and also updated my page.
You may want to change the URL of my designs on the main wiki to the new cleaner page title:-
http://www.headfuzz.co.uk/?q=openservopcb

Some of the traces are too close. I have just done a test etch, and it needs tidying up a little.

I am maintaining both the edge connector version, and the 2x4 pin header version for the moment. It's at least useful to me.

Here it is



Again, by no means perfect, but certainly a start

Barry

[RifRaf]

Mike it appears on your parts layout that R2 from reset is taken to ground rather than vcc, am i just mistaken cause the schematic appears to conflict

[mpthompson]

RifRaf in my design R2 is connected to +5v, but it appears differently in Barry's reimplementation in Eagle. It can be seen a little more clearly in the diagram below:

http://www.openservo.com/moin.cgi/PartsPlacement2?action=AttachFile&do=get&target=parts_placement_2.pdf

-Mike

PS. RifRaf, do you have regular name we can call you by ?