Propeller based Bot board

[kurte]

Since I ported the Phoenix code to run on a propeller based system, I have been playing around with trying to design a propeller based bot board. I am a complete novice at designing circuit boards. Currently I am using a program called diptrace to help design the board. They have a freeware version of this that can handle up to 300 pins. I think I slightly exceeded this. I am now registered as doing this for not a profit so they allow the program to handle up to 500 pins…

My current design is sort-of a cross between a Bot Board 2, a propeller robot controller board (gadgetgangster.com/find-a-projec … ectnum=257" onclick="window.open(this.href);return false;)

In particular I am using a Propeller chip (PX832A-Q44), FTDI Dhip (FT232RL). 2 TI TXB0108PW chips and 1 TI TXB0104PW to do bidirectional voltage translations on 20 of the IO pins. Also a 24LC512 EEPROM, which allows for the program to be stored in the lower 32K and the user to be able to store stuff in the upper 32K.

Here is my current schematic:

Likewise here is my current layout:

As I mentioned above, I have never tried to design a board so there are probably lots of things that I overlooked or could be improved on and would appreciate any help you can give. Some of these components I had to guess at, so I know there will probably need some tweaking. Things like which buttons are used. I think I am pretty close to the ones that are on the BB2, likewise the speaker I believe I have the right one…

Some questions or issues that I wonder about include:
a) Power supply. I am I thinking along the line of LM2937-5.0 and could use the same type for the 3.3. But since the input voltage for the 5V needs to be near 6V, we don’t need an LDO type here. Suggestions? Alternative is to do a power supply like they have on the Parallax Propeller Robot Control Board. They use an IC LT3501 plus other stuff to give them the two voltages (regulated 3 amp)… Also need to double check to see if I have the right size power connectors here… Likewise size of components/connections/clearances… Likewise not sure of how many and necessary locations for capacitors. I know that each IC needs a .01… But should there be large ones hung off of VS and VL? Or should the large ones be off of the +5V or +3.3V or all of the above?

b) the preferred line widths and the like, both for normal signal wires as well as power buses. I believe most of my signal wires are .01. My VS is something like .2 and the VL is something like .15…

c) IO lines and voltages both for power and signal. What I have now is:
P0-P15 - IO is always 5V through conversions of 2 TXB0108PW chips. The power lines can be VS or +5V switchable on 4 pins like BB2

P16-P19 - IO can be 5V or 3.3V (I think). Also Power can be VS, 5V, or 3.3V. I thought it would be nice to be able to hook up things like XBees without having to go through multiple voltages. What I did was to feed VccB of the TXB0104PW chip with either 5V or 3.3 V depending on the one jumper that also feeds into the Non-VS side of the second jumper for those 4 IO pins… Not sure if that makes sense?

P20-P23 - For PS2. 3.3v through 220 resistors. Power is 3.3v (like actual PS2). I put in two sets of 3.3V connectors in case you wish to hook up another 3.3V device, like I2C…

P24 - Speaker - Hopefully I have everything in here…

P25-P27 - Buttons/LEDs

P28-P29 - I2C - Used for EEPROM. But I also have connectors for SCL/SDA so user can add on. Not sure if I should put in some resistors like 220s to protect IC… I have pull-ups on both SCL and SDA. May not need one on SDA unless we want to support multiple masters.

P30-P31 - USB using FT232RL… - Not sure if I should try to add/remove stuff here to allow VL to run off of USB…

D) esthetic’s - Once I know that we are reasonably close, need to make pass and do things like line up components… Also are there rules/preferences by the board manufactures on where things should or should not be put…

E) Conversion to whatever formats of documents that are needed…

That is all for now.

Thoughts?
Kurt

[miked-6]

Kurt,

The board looks good, and I think it maps the BB2 functionality to the Propeller nicely. A few comments off the top of my head.

The original buzzer for the BB2 was CUI part number CEM-1206S (Digikey 102-1155-ND). The buttons were E-Switch part number TL1107AF130W (Digikey EG2510-ND). Anything that matches these footprints should do.

If you are planning to use screw terminal blocks for VS and VL, watch for clearance. It looks like C4 might be a bit close to VL. In retrospect I recommend not using the 0.1" terminal blocks, but switching to a slightly larger one such as the Digikey 277-1860-ND. And use a 4-position block rather than a pair of 2-position ones, even if you stick with 0.1" blocks. Much better mechanical stability.

The 2937 family of regulators is great, but as you say you don’t need LDO for the 3.3V supply. Using a non-LDO you can get by with a less expensive output capacitor and probably a less expensive IC. Each regulator needs a large output cap. The LDO regulators are sensitive to the characteristics of this cap, and give specifics in the data sheet. Otherwise, one cap per IC is pretty standard. Keep them as close as possible to the supply pins.

I would consider 0.01 the minimum width for any trace on the board. That way just about any board house should be able to build it without trouble. Power and ground traces should be as wide as you can make them. It looks like you are using copper fill to make ground and power planes. That is good.

The BB2 shares I/O lines between buttons and LEDs because there just isn’t enough I/O to do otherwise. If you have enough I/O on the Prop, I would split those out. (The schematic is not high enough resolution for me to make out the chip labels, so I can’t see if there are unused I/O.)

I would use the pullup on SCL and SDA both. I think the I2C spec from Philips had series resistors for protection. Maybe not as big as 220 Ohm though. 100 Ohm sticks in my mind. It’s been a while since I read it.

Diptrace should do automatic Design Rules Check. I know Eagle does that, and comes with some standard design rules files (and board houses might provide design rules as well–I got 10mil and 8mil desgin rules for Eagle from Olimex.com).

Each board house will have its own rules. I have dealt with Olimex several times. They have a minimum silk screen width, a limited set of drill sizes, etc.

I don’t know how to generate the files from Diptrace, but these packages make it easy. I have played with Diptrace and know they have a good tutorial, so it should be able to get you going. The board house will say specifically which files they need and how to bundle them. Typically Gerber files top copper, bottom copper, top silk screen, top resist, and bottom resist. And Excellon drill files to specify hole sizes and locations.

One final thing about the aesthetics of the schematic. I recommend never rotating ground symbols at all, and never rotating transistors 180 degrees (though it is often OK to mirror a transistor left-to-right). Wherever possible, current should flow top-to-bottom and left-to-right in the schematic for ease of reading. Sometimes it is difficult (or impossible) to do this in the free versions of schematic capture programs due to limitations in number or size of pages. But if possible, re-organize to avoid confusing rotations.

Good luck.

Mike

[kurte]

Thanks Mike,

I will take a pass through making the suggestions you mentioned.

Yes Diptrace does have the design rule checking and the like and I fixed all of the problems it found…

If you still have Diptrace installed anywhere, I could upload the design file, which would make it easier to look at it.

Thanks again!

Kurt

[miked-6]

Kurt,

I do still have Diptrace (the 500 pin version) installed and would be interested in taking a look at the design up close.

One more thing I noticed when I looked at the datasheet for the TXB0108 this morning. The drive strength on that chip is quite low. It has a 4k source impedance, so it can only drive a little over 1mA at 5V. Not enough to light an LED very brightly, but probably enough for signaling (i.e. driving a servo). Just something to be aware of.

Mike

[kurte]

Thanks, here are the current ones…

I need to get a lib file up here with the TXB0108… I added it earlier to the TI one but that makes the file to large to post. So I will try to extract it to secondary lib file…

Kurt

EDIT: I extracted the two components from the TI and created a new library which I new have included
Dip Trace Design.zip (58.2 KB)

[kurte]

Thanks again, I have been playing around some with the schematics and layout and I have fixed a few of the things (I think).

I think I have the correct speaker, I used the markings off of a current BB2(KC1206). Likewise I think I have the right switches, they ones you mentioned appear to match the ones I found earlier up on mouser.

I updated to use the screw terminals you mentioned. I know others have had problems with the current ones so that makes a lot of sense.

I found some errors in the capacitors associated with the voltage regulators. Suggestion on what voltage regulator to use for 3.3v? Also do you have suggestions on what types of capacitors to use with the power supply?

Yep I copied the LED and buttons like you had. Also not sure if that is the best but It seamed like a reasonable compromise. I wanted the 20 IO lines for normal IOS, I know that Jim would probably want PS2 support so I thought running 4 IO lines that were not converted to 5v for this would be a good idea. 2 IO lines are needed for USB/UART plus 2 lines needed at least part time for EEPROM, which left 4 IOs left. So I used one for the speaker and the other 3 for the buttons and LEDs.

I left the pull-up on the SCL and SDA. I have also added the resistors to the IO lines. I currently defined them as 100s.

I think the transistors are back in the normal configuration. I will work on rearranging the schematic to make it easier to read.

That is all for now
Kurt

EDIT: Since I don’t think Mike or Robot Dude have been up here since this post, I am in the process of updating the capacitors. I am guessing that the ones that are used on both the BB2 and SSC-32 are close to this one from Digikey: 478-3899-2-ND (CAP TANTALUM 22UF 16V 10% SMD). I will update the two power ones to be close to this one. I am not seeing the package case (2312) in the current stuff in the diptrace library, so I will either use the 2213 that is defined which is probably close enough or may copy it and modify to the appropriate, will update documents probably later today…

Edit2: I updated the images again. I have now also added resistors to SCL/SDA. Also found a major issue where the IO lines were missing from RX/TX from the USB to P30/P31. I fixed it, but it took awhile to get the IO lines routed…

Edit3: I did some cleanup of some signal line routing that I did not like…
Dip Trace Design.zip (61.9 KB)

[robotdude]

This is looking nice.

I will let Mike know you have made updates. Thanks!

[kurte]

Thanks, I did some minor editing of the etches today, but at times wonder if we should do something to add AtoD support to the board. I know that several people have used the MCP3208 chip. In fact Parallax sells them: parallax.com/Store/Microcont … fault.aspx

These chips use an SPI interface and the current spin modules for this require 3 IO pins to be defined. Could currently use the 3 IO pins I am using for Leds/buttons. If so could either remove the buttons/LEDS which would save room, or could multi-task them onto some other pins like the ones I have for PS2. Maybe have it jumpered.

Also not sure where to add extra pins for the AtoD. Would it be sufficient to have them as solitary pins and not art of 3 pin servo type connections?

Just some more to think about…

Kurt

[robotdude]

I forgot to ask Mike to check in. Because the Prop has several unique human interface items, I am ok with losing the pushbuttons and LED’s. Would like to retain the PS2 controller. Does the board have the connector for whatever it uses for the keyboard, video, etc?

[kurte]

So far I have not done anything about adding things like mouse/keyboard. Many of the boards don’t do it… What is your thoughts on Analog?

Kurt

[robotdude]

Yes analog is desirable. I would give up the buttons and LEDs to achieve analog inputs. Would anything more than a connector be required for the user interfaces? I need to look it up to see what it takes. Sorry no time.

[kurte]

I have not used the UI parts much on my Prop boards. But if you look at the Wulfden board that you can purchase the UI parts as daughter boards. The daughter boards are mainly the connectors as well as some discrete components (resistors and capacitors…), but the real issue is the IO Requirements. That is both boards basically use up IO pins 16-27, especially if you go VGA. That is:
VGA P16-P23
Mouse P24-25
Keyboard P26-P27

If only Composite Video: P20-23
Simple Audio: P19
Mouse/Keyboard…

With P28-29 needed at a minimum at startup for I2C to load the program from EEPROM and P30-P31 needed for serial communications. This only leaves the lower 16 IO lines to use for digital IOs and if we use SPI interface for Analog that would reduce it more. Optionally Analog could be added with I2C interface, I did see a few chips that did this, but probably higher cost.

The question is, if we go this route, would we want this dedicated, or would we want some way to jumper in this type of configuration?

Thoughts?
Kurt

[robotdude]

I thought they were all on a simple bus or something. This sounds like a bad idea. As Roseanne Rosanadana would say… Nevermind…

[kurte]

Hi Jim and Mike,

I have been playing around today adding in analog lines using an MCP3208 chip as this appears to be one that is used reasonably often on the parallax site. I have added an 8 pin connector for the Analog signals, but have not added extra ground or power lines. May be able to that if you think this important. I have used the IO lines that I was previously using for the buttons/leds to control the analog chip. I so far have kept the buttons and leds, and have doubled these up on the 4 IO lines that were setup for PS2 support. I have not added jumpers yet to disable this, may find room if you think we need it. I am not 100% sure if I need some other support chips or signals for this chip or not. I did put one decoupling capacitor near it…

I have not cleaned up the schematic yet, should probably break it up to multiple pages.

I moved most everything around in the board and started over on routing things to get this to fit as you can see:

Warning I need to make another pass through and cleanup how things are labeled and the like. But first hopefully get close to the functionality.

I included he diptrace document files in case you wish to look them…

Let me know what you think.

Kurt
Propeller with Analog.zip (104 KB)

[kurte]

Hi Guys, I played a little more with this. I made it that all of the anlog pins had 3 pin connectors, with the voltage set to the VRef pin. Also added +3V/Gnd pins for each of the PS2 pins to make it like the rest… Pretty crowded now. What do you think? Probably won’t do anything else until I hear something…

Kurt
Propeller with Analog.zip (108 KB)

[robotdude]

Wow, if it can be built it could be very nice!

I have often considered allowing a 3" x 3" board, but retaining the same mounting holes. Should keep the connectors in the same place they are now for clearance issues. Will ask Mike for his opinion. Do you think we should try to make one yet? Thanks! Jim

[kurte]

Thanks Jim,

I think it would be fun to make one soon if it is buildable, but probably need to go through and update the resistor values, possibly need more decoupling capacitors… Some cleanup on what shows up on the mask… Having that extra width would help things for sure, but it would be interesting to see how it would fit in the different platforms, like the inside the phoenix or inside the T-Hex… For things like the Brat that would not be much of an issue.

It would be very good to get Mike’s opinion here as I have never done this before… Things like, is it OK to have traces under the USB connector or will that create issues. Likewise clearance issues. Probably should move R19 slightly to make more room for speaker…
Kurt

[miked-6]

Kurt,

Jim pinged me last week to remind me to check this out, but I was swamped. I’ll download the latest files and comment. It’s looking really good so far.

Mike

[miked-6]

Kurt,

I checked the I2C doc from NXP for the recommended series and pullup resistors. It looks like 220 Ohms would work quite will with 10k pullups. You might want to consider dropping the pullup to 4.7k for offboard connections, to handle high line capacitance. Even with a 4.7k pullup and 3.3V supply, a 220 Ohm series resistance should work. (Here is the NXP spec: nxp.com/acrobat_download2/li … 340011.pdf)

R9,10,11 at 4.7k are way too large. For 3.3V supply, 220 Ohm would probably be good.

I think the 220 Ohm series resistors may be too large to use with the 1K pullups on the PS2 connector. But you can always populate different values if necessary to get it to work reliably.

It looks as though you haven’t placed or wired the A/D converter (U10) yet. That will be tight. I noticed that you have connected DIN and DOUT of the A/D together. From the datasheet it looks like the MPC3208 should be able to handle that. Does the Prop library work in this configuration? (I am not very knowledgeable on the Prop.)

The regulators you chose seem reasonable. I am surprised that the datasheet doesn’t have design recommendations for the input/output caps. I would be inclined to use a 0.33uF ceramic cap on the input and a 10uF or greater tantalum on the output. The tantalum voltage should be at least double the regulator output voltage.

I’ll try to append further comments tomorrow.

Mike

[kurte]

Thanks Mike,

I have made the changes to the resistors you mentioned. (4.7K for pull-ups and 220 ohm for the ones feeding the leds (I meant to do that one earlier )

The Analog chip and wiring was on the latest one. If you look at the last printout of the board I posted it is toward the upper right of the board, just below the Analog IO pins and above the FTDI chip… (It is definitely tight…), since that printout I moved R19 slightly as I thought it was too close to the speaker. Yes the Propeller spin file mentions wiring the IN/Out to each other, in particular:

[code]PUB start(dpin, cpin, spin, mode) : okay

‘’ Start driver - starts a cog
‘’ returns false if no cog available
‘’ may be called again to change settings
‘’
‘’ dpin = pin connected to both DIN and DOUT on MCP3208
‘’ cpin = pin connected to CLK on MCP3208
‘’ spin = pin connected to CS on MCP3208
‘’ mode = channel enables in bits 0…7, diff mode enables in bits 8…15
[/code]

I believe the data sheet called for the voltage regulators called for .1uf input and 10uf. Looking at both the BB2 and SSC-32, on the tantalum side you called out for the 22uf at 10v but the parts were 16v, so I tried to match. As for the input side, I believe the SSC-32 had it as a .1uf, so I stuck with that, but not sure what is actually on the board (my eyes can not read that small ) Should I up them to .33uf just to be sure?

Thanks again!
Kurt