Laugh At It If You Must, Critique It If You Must, But I Think It'll Do The Trick :)

idbruce

Hello Everyone

Over the last several days, I have been combining the schematic of the EVAL6208N and the typical application schematic for the L6208N stepper driver IC, and I have a very good idea just how I want the board laid out. I know this is no big deal for some of you, but for me, it was a bit time consuming. Although I am not 100% certain, I do believe this design for a stepper driver should be good enough for my first trial. And yes I know, I jumped some numbers in the part naming, but I will fix that when I get a very accurate list of the actual part numbers. If you see any blatant errors, please let me know.

Bruce

EDIT: ERROR FOUND!!! Please refer to Post #6.

ElectricAye

One of the problems I had when tinkering with the L6208 is getting the heat sink pins' solder to properly bond with the ground plane/heat sink in the PDIP version. Although the solder joint looked good, the fact the ground plane sucked away so much heat often caused unseen faults in the bond, and because the bonds were not as good as they needed to be, the chip turned into a spark plug. I had to preheat the ground plane with a heat gun before soldering those pins. Just something to look out for if you use the ground plane for a heat sink.

idbruce

@ElectricAye

the chip turned into a spark plug

LOL You got a chuckle out of me.

I definitely plan to use the ground plane as a heat sink, so I surely appreciate the tip, and I will have to do some research on a good remedy for the problem that you describe. The EVAL6208N claims to be able to withstand 2.86A and it uses nothing more than the ground plane for the heatsink, so I believe I can accomplish the same by following the EVAL6208N grounding layout. I used fans on some other driver boards I made and it caused me a lot of extra work. I also intend to try and achieve that 2.86A benchmark, and if I release some magic smoke, I guess I will know better next time. Seriously, thanks for the tip.

Bruce

Mark_T

The two VREFs need to be kept separate if you want microstepping - they can provide the quadrature signal (K.abs(cos(theta)), K.abs(sin(theta)) ) for arbitrary phase angle theta and drive level K

[edit: you need to use NORMAL MODE for microstepping this way, both phases driven]

idbruce

@Mark_T

Yea I know, but I decided to just do half and full steps this time around, just to get me feet wet with this chip and test the amperage rating of the board without fans or a heatsink. If all goes well, I might try a microstepping board or perhaps try and progress to the L6480H. Anyhow thanks for the corcern, I appreciate it.

Bruce

idbruce

Just in case someone uses this schematic as a starting point for their own L6208N schematic, I found an error. Referring to My_L6208N_Sch.jpg attached above, the SENSEA trace coming from pin #3 of the L6208N needs to go to the opposite side of the resistor network. As it stands right now, SENSEA is going straight to GND.

Bruce

idbruce

With the exception of routing the signal grounds, altering some trace widths, and making my planes, I believe I am getting it pretty close to where I want it to be. Hopefully by tomorrow sometime, I might be able to start making my photomasks.

Circuitsoft

If I were you, I'd try to route everything except ground on the top, and make a plane on the bottom. Add a few bottom traces here and there if necessary for jumpers, but for the most part, try to keep the bottom as an uninterrupted plane.

idbruce

@Circuitsoft

Fifty percent of this board is modeled after the EVAL6208N evaluation board, so alot of my layout was dependent upon that schematic and layout of that board. If you look at the attached images, you will see that the main ground plane is on the top layer and that there are alot of traces on the bottom layer. I would imagine that the chip is placed in direct contact with the top layer for heat dissipation purposes.

Bruce

idbruce

To Those That May Be Interested

In order to assist with the visualization of the similarities between my board and the EVAL6208N, I have attached two more images which only show the component layers for both boards.

Bruce

idbruce

To Those That May Be Interested

Before getting too carried away with my current project, I decided to review the necessary components, values, and initial layout. The desire to create a PCB design around the L6208N actually started several years ago. In fact as previously mentioned, I already designed one board around this chip, but I was very unhappy with results. One of the problems that I had way back then was finding a suitable substitute for the sensing resistors. With the substitution resistors that I am currently using, this choice of resistors has increased the board length by an unnecessary amount 3/8 - 1/2". Considering that my biggest concern is the size of the board, which is currently 3.35 X 2.75", I believe I will revisit the issue of the components and values for the sensing resistors. If I can find more suitable replacements for the sensing resistors, this should result in a board size of approximately 2.75 X 2.75", however I will have to alter the design and rearrange the layout a little to compensate for these changes.

Bruce

Circuitsoft

What sense resistors/resistor range are you looking for? Oftentimes, current sense resistors are actually easier to find in surface mount than through-hole, and if it's an 0805 or 1206, it'll still be plenty easy to solder.

idbruce

Circuitsoft

I will be looking for (6) 1 Ohm, 0.4Watt, metallic film resistors per board. If I can find them, I should be able to modify my current design with minimum hassle, and shrink the board considerably. I have not looked for them in approximately 3-4 years, but I should be able to find something compatible. If necessary, I could perhaps increase the power rating to 1/2W, which would make my search easier, but I would have to review the datasheet to see if that combination will work properly.

Bruce

idbruce

Oh... And they need a tolerance of 1%.

idbruce

Yep... That is indeed a difficult find

Circuitsoft

Search Mouser for SR732BTTE1R00F or SR732ETTD1R00F

idbruce

Circuitsoft

I would have to redesign my whole board to compensate for surface mount resistors and I am not prepared to do that. I think I will stick with my current design of the board and use these resistors or similar resistors of the same series:

http://www.mouser.com/ProductDetail/KOA-Speer/MF1-4DCT52R1R00F/?qs=sGAEpiMZZMu61qfTUdNhG%2fDQawzJ6c7PIvQ2H%252bMxjBM%3d

I misquoted the maximum rating for the EVAL6208N at 2.86A, when the documentation of AN1764 in fact says 2.64A. However considering the documention of AN1451 provided in Sec.2.5 and the component listing of the sensing resistors in Sec. 4.2, I see the maximum amperage of the EVAL6208N to actually be more in the realm of 1.5A per phase. Once again "however", I believe the board might be able to push this amperage rating past 1.5A with the use of a 2oz. copper board, the ground planes they recommend, and by changing the values of the sensing resistors. On the other hand, I just may melt the copper from the board or turn the chip into ash

Bruce

idbruce

To Those That May Be Interested

I rearranged quite a few things, and with the exception of drawing my various planes and rearranging a few part names, I believe this baby is ready for production. The board will measure 2.70" Wide X 3.00" Long. Oh, and I am shooting for 2.5A per phase.

Bruce

EDIT: I just realized that I forgot to add a power LED. Oh well, that is pretty much just show anyhow.

Circuitsoft

You have tiny traces going from the chip to the sense resistors. Also, the lines from the main input filter cap to the L6208 are pretty thin.

On the half/full jumper, why do you have two? Put a large pullup on it, and have the jumper pull it low. That way, you won't have an illegal condition if somebody either forgets the jumper or puts two on. Same with the fast/slow decay switch.

idbruce

@Circuitsoft

You have tiny traces going from the chip to the sense resistors. Also, the lines from the main input filter cap to the L6208 are pretty thin.

As mentioned, a large portion of this board is modeled after the EVAL6208N. If you refer to Post #9, which shows the top and bottom layers for that board, you will see that the whole sensing area is comprised of three planes, which will rectify the thin traces going from the chip to the sensing resistors. Additionally, the positive and the negative of the main filter capacitor is also attached to two major planes, which would also rectify those thin traces.

On the half/full jumper, why do you have two? Put a large pullup on it, and have the jumper pull it low. That way, you won't have an illegal condition if somebody either forgets the jumper or puts two on. Same with the fast/slow decay switch.

Thanks for pointing that out to me, because that is a serious potential problem. By placing two jumpers or a single jumper across the wrong two terminals, a direct short would exist.

Thanks for the advice.

Bruce

idbruce

Hello Everyone

I do believe I need a little help.

As can be seen on my board in Post # 18, JP2 is goes to one side of R3 and the other side of R3 goes to PIN 12 (HALF/FULL) of the L6208N. Additionally R3 has a resistance of 10K Ohms. The default for the drive is FULL step mode, with a jumper positioned on JP2 so that GND is going to R3. In HALF step mode, a jumper would be positioned on JP2 so that 5V is going to R3, instead of GND going to R3. In the original schematic and on the EVAL6208N evaluation board, STMicroelectronics had the exact same circuitry, except they used a two position switch to make and break contact between GND and 5V. However as Circuitsoft so kindly pointed out in Post #19, a direct short could occur if someone placed a jumper in the wrong position. Now we all know this would never happen to me , but nonetheless it is a potential problem, which can and should be eliminated pretty easily (I think, although I have not done a thorugh examination of the current board real estate). Anyhow here is a quote from Post #19, in which he identifies the potential problem:

On the half/full jumper, why do you have two? Put a large pullup on it, and have the jumper pull it low. That way, you won't have an illegal condition if somebody either forgets the jumper or puts two on. Same with the fast/slow decay switch.

By examining the board layout in Post #18, you will see exactly what he is talking about, and as he mentions, there are two identical problem areas, but they should both have the same solution. Even though he definitely has the right idea, I want to switch his solution around a little to provide the default settings without jumpers, as it applies to the EVAL6208N evaluation board schematic. In order to do this, although not 100% certain, I believe that I would need to use a pull down instead of a pull up. I base this upon the datasheet which says:

Step Mode Selector. HIGH logic level sets HALF STEP Mode. LOW logic level sets FULL STEP Mode. If not used, it has to be connected to GND or +5V.

Decay Mode Selector. HIGH logic level sets SLOW DECAY Mode. LOW logic level sets FAST DECAY Mode. If not used, it has to be connected to GND or +5V.

The attached image below depicts the proposed solution, however I am uncertain how to obtain the proper values for R3 and R_UNKNOWN. Considering the original value of R3 (10K), how would I determine the new value of R3 and the value for R_UNKNOWN?

Thanks in advance.

Bruce

idbruce

Refering to my previous post, here is a portion of another board designed by another individual. On his board, he put a two pin header in between the resistor and PIN 12 which connects to GND with a jumper installed, and without the jumper installed, the resistor for PIN 12 has 5V going to it. In this case, I believe the default for his board is HALF step mode without the jumper. Is this method also acceptable? Please refer to the attached image.

Circuitsoft

That should be fine. They're CMOS inputs, so even a 10k resistor will have no trouble pulling them up or down. The problem with leaving them open is that, with the high-impedance CMOS input, they will float and could cause the input circuits to draw a lot of current.

Circuitsoft

idbruce wrote: »

In this case, I believe the default for his board is HALF step mode without the jumper. Is this method also acceptable? Please refer to the attached image.

That's exactly the circuit I was trying to describe.

idbruce

@Circuitsoft

That's exactly the circuit I was trying to describe.

Well that's good, because I opted to go that route for the sake of simplicity. While I was at it, I took the time to reroute a couple of other traces and straighten out my part names.

For those that may be interested, I have attached three more images to show the current state of everything. Please note that you may copy my work and layout for personal use, but commercial use is out of bounds.

Bruce

idbruce

To Those That May Be Interested

I just got finished with the copper pours/planes (whatever you want to call them) for the bottom layer. I have attached an image of my bottom layer and the bottom layer of the original EVAL6208N evaluation board, so that you can compare them and notice some of the similarities.

Bruce