Stepper Driver 1.2 (Single Sided)

I'm currently in the process of building my first reprap machine and was looking for a nice single sided, through-the-hole stepper driver board. Since i couldn't find any i decided to re-layout the 1.2 driver to be single sided. I have not done this before so i would like someone to take a look at it to check if it's ok the way i did it. Any advice, critics, ideas, ... appreciated.

Stepper1.2SingleSidedv0.1.pdf

Note:
- Red outline is edge of board (9x7 cm)
- Max and Min headers have a different pinout (5v center pin) / no RJ-45 connectors

thx in advance

There are designs using the newer microstepping Pololu 1201 boards that would be better instead of the old half-stepping ones. Check in [www.thingiverse.com]. Here's one that's single-sided:
http://www.thingiverse.com/thing:4526

Edited 1 time(s). Last edit at 04/09/2011 09:19AM by brnrd.

thanks for the link.
i read it but the problem is the Allegro chip on the Pololu used.
first it's smd which i'm not confident enough to solder myself and second it's very hard to get here (and expensive on top of that).
the part for the 1.2 board cost about 6-8€ total. since i'm on a tight budget and half-stepping is all i need why spend more money on it then needed ? don't get me wrong if i'd have the money i'd spend it no questions asked.

The machine is very noisy using half stepping.

---

[www.hydraraptor.blogspot.com]

well, if you know a stepper driver using microstepping being through-the-hole solderable, completely without smd parts, for not more than 6-8 € a piece then i'm all for it. i haven't found any but i doubt i have seen it all. so if you know any i'll gladly take a look at it.

up until then for as long as half stepping won't have a huge impact on printed part quality it'll do.

but to get back on topic. it's not about halfstepping or microstepping ... it's all about whether or not the layout i did is correct and/or safe for use (meaning spacing and such). since it's the first time i layout a circuit-board with more than about 100mA running through, i'm a bit nervous and don't want to kill myself trying or fry the parts on the board for that matter.

so i appreciate your input on loudness and such but i'm really interested in input regarding improvments to the layout

Yes there is at least one through hole microstepping driver that has been mentioned in these forums but I can't remember the part number.

The ground takes a very indirect route to the chip with some thin tracks and the HF decoupling should be close to the chip rather than the power connector. You might get some instability.

---

[www.hydraraptor.blogspot.com]

The Pololu 1201 is a A4983 Stepper Motor Driver Carrier is through hole and is usually used with a socket so it's easy to replace. In the US, they are $13 each so it's in to your price range. It's easy to interface to the MB since you're just basically connecting them to the right output of the microcontroller. There are even designs in this forum that includes them with the ATMega in one board. I still think this is the better route.

I don't think you need to worry about killing yourself since you're only working with 12 V.

I find smd components being easier to solder with my iron and clips than trough-hole components. I think most ppls find smd easier too. Besides, smd generally are better at noise and etc. Also i think you plan to use 5V from the atx, which is smps and i think it probably has more noise in it than the usual 7805 voltage regulator.

Single sided is not optimal. At toner transfer or photo, double sided is same work with more benefit, dunno about milling boards tbh. If you plan to make the board yourself, why not making double sided, for example with back plane being ground. The other pins will get isolated a little by the polygon isolation, but this would free up the gnd routes on the top and maybe make a more compact layout. Not sure for this chip if this should be a clean star gnd though or w/e else, datasheet or some app notes should have some mentions regarding gnd.

Edit:
Try TB6560, torugh hole, microstep, newer stuff, lower external components count. Its overkill in terms of current, but at first glance it looks like a better choice (at least to me). Lots of schematics and boards on the net, single sided most of them. One attached as example, i would like to give credit to whomever made it just tbh i had it on my pc and dont remember from where. Havent tried it myself so cant say more. Good Luck!

Edited 2 time(s). Last edit at 04/09/2011 11:00PM by NoobMan.

nophead Wrote:
-----------------------------------------------------
> The ground takes a very indirect route to the chip
> with some thin tracks and the HF decoupling should
> be close to the chip rather than the power
> connector. You might get some instability.

Well that was one of my concerns. ground is at a very bad place to be connected with a thicker trace but i will try ... maybe i'll somehow manage to get it to there.


NoobMan Wrote:
-------------------------------------------------------
> Also i think you plan to use 5V from the atx, which is smps and i think it probably has more noise in it than the usual 7805 voltage regulator.

Yes, i thought about that one too. I wanted to feed the board from my arduino board with 5 volts but since it's been this way in the original scematics i thougt it would be ok. well maybe i'll redo it.

> Try TB6560

yeah seen it. sadly it's unavailable to me. tried to find it but found no source with a decent price. same goes to the other chips from toshiba.

edit:
Done with the changes

Stepper1.2SingleSidedv.2.pdf

- ground line straightened
- moved the (12V line) capacitors a little closer to the l298 (don't want to block the space for the heat sink)
- 5v now coming from the 2x3 header (powered by the arduino) next to the power connector

the sad thing:
- i had to build in a wire to feed the ground connection to the l298 (i hope this will be better than the other approach with the signal routed through pin 7 and 9

any more input appreciated

Edited 1 time(s). Last edit at 04/10/2011 08:24AM by Khan.

It is important that the ground of the sense resistors is close to the ground (i.e at the same potential) as the ground to the L297. It should really be a star point or a plane. I wouldn't build this sort of circuit single sided for that reason.

Probably better to place R2 and R1 where R4 and R3 are and make the star point where the bottom of your wire link is, with a second link for R2's ground. C1 should be as close as possible to that point. C2 can be further away, near the connector. The ground for the left hand part of the circuit should also meet at the star point rather than the power connector. The diodes are OK going direct like they do.

If possible C4 and C3 should also ground at the star point. I would move them closer to R1 and R2.

You should also add decoupling on the 5V rail close to the VCC pin of the L297.

What you should bear in mind is that tracks have resistance and inductance so you want to keep the tracks between things that need to be the same voltage as short as possible. It doesn't matter how long the track from the power connector is because it is just an extension of the wire but the tracks between the ground of R1, R2, C3, C4 and the L297 should be as short as possible and meet at one point.

Edited 3 time(s). Last edit at 04/10/2011 11:45AM by nophead.

---

[www.hydraraptor.blogspot.com]

A more concise way to describe it is that it is the L297 that is measuring the voltage across the sense resistors, so the star point should be near its ground pin, not at the power connector.

---

[www.hydraraptor.blogspot.com]

Changes done.

I think it's as close as it'll ever get (unless i solder it at the other side of the board)
although the wires are kind of bugging me

Stepper1.2SingleSidedv.3.pdf

any more suggestions appreciated

That is a lot better but I would make it a proper star point. I.e. all grounds emanate from one point and no shared traces. In particular I would take the bottom end of wire 2 to the bottom end of wire 1 and make that the star point.

---

[www.hydraraptor.blogspot.com]

If I remember it correctly there is a Singe sided PCB design in one of data sheets... for the L297 or L298.

---

Bodge It [reprap.org]
=======================================

---

BIQ Sanguinololu SD LCD board	BIQ Stepcon	BIQ Opto Endstop
BIQ Heater Block PCB	BIQ Extruder Peek clamp replacement	BIQ Huxley Seedling
BIQ Sanguinololu mounting	BIQ standalone Sanguinololu or Ramps mounting	Print It Stick It Cut it

My rep strap: [repstrapbertha.blogspot.com]

Buy the bits from B&Q pipestrap [diyrepstrap.blogspot.com]
How to Build a Darwin without any Rep Rap Parts [repstrapdarwin.blogspot.com]
Web Site [www.takeaway3dtech.com]

thanks for all the input.
i think i'll stick to the last layout although i might add a second solder point to r1 and r2 since i might need to wire 2 resistors in parallel to get 0.5 ohm 2 watt as mentioned here Stepper Motor Driver 1.2 Wiki

Do not be tempted to use wire wound resistors for the L298 as inductance will affect the curent measured this is mentioned in the same DATA sheet that the SS PCB layout is on.

From Blogger Pictures

---

Bodge It [reprap.org]
=======================================

---

BIQ Sanguinololu SD LCD board	BIQ Stepcon	BIQ Opto Endstop
BIQ Heater Block PCB	BIQ Extruder Peek clamp replacement	BIQ Huxley Seedling
BIQ Sanguinololu mounting	BIQ standalone Sanguinololu or Ramps mounting	Print It Stick It Cut it

My rep strap: [repstrapbertha.blogspot.com]

Buy the bits from B&Q pipestrap [diyrepstrap.blogspot.com]
How to Build a Darwin without any Rep Rap Parts [repstrapdarwin.blogspot.com]
Web Site [www.takeaway3dtech.com]

I think he could use those resistors, I have seen wirewound resistors like that used, paralelled with one facing the other, presumably this reverses the coils one to the other (as long are the same product/manufacturer) so this way it minimizes inductance. Might be a good tip on that wiki page saying to make their signs mirroring to each other. Even if its not the best solution, but it should work.

- Edited that wiki page with that tip.

Edited 1 time(s). Last edit at 04/12/2011 09:48PM by NoobMan.

Quote

presumably this reverses the coils

I don't think so! A clockwise spiral is still clockwise which ever end you look from. Even if they were counter wound they would need to be on the same axis to cancel out.

---

[www.hydraraptor.blogspot.com]

.. huh, true, i had a misconception about it then. I stand corrected.

I will remember direction doesnt matter and inductance is only halved by paralleling.

However, as i do scavenge what i can for parts, i have met many boards that have the wirewound resistors like that. Picturing a high rf amp that i ripped for its huge radiators to use in a psu. That board has 4 pairs of resistors just like that on one side, and 4 on the other side, all facing each other. Also I have met other pairs also like that on other pieces. I tend to think its not a coincidence they are all facing each other. Is there anything else about it then, or any reason for that?

And btw, i remembered i didnt thanked you for straightening me lately, so again thanks for straightening me for the ..... 12346541645 'th time or something like that.

Quote

Is there anything else about it then, or any reason for that?

I don't know, perhaps it's a common myth, or perhaps there is a valid reason. You can get special low inductance wire would resistors that reverse the turns half way I believe, but for these powers you can get metal film or carbon comp. Since the sense lines include an RC filter it might not make that much difference, but the data sheet recommends not using wire wound, so why take the risk?

---

[www.hydraraptor.blogspot.com]

Data sheet link

The single sided board I included shows they useed 4 resistors in parallel.

There is a popular CNC board design where there is an attempt to compensate for the affect of using wirewound resistors here. I would still avoid using this design.

---

Bodge It [reprap.org]
=======================================

---

BIQ Sanguinololu SD LCD board	BIQ Stepcon	BIQ Opto Endstop
BIQ Heater Block PCB	BIQ Extruder Peek clamp replacement	BIQ Huxley Seedling
BIQ Sanguinololu mounting	BIQ standalone Sanguinololu or Ramps mounting	Print It Stick It Cut it

My rep strap: [repstrapbertha.blogspot.com]

Buy the bits from B&Q pipestrap [diyrepstrap.blogspot.com]
How to Build a Darwin without any Rep Rap Parts [repstrapdarwin.blogspot.com]
Web Site [www.takeaway3dtech.com]

Mouser has it for $3.36 in qty 10. Is that not a decent enough price? Does shipping to your local kill the deal?

@Khan any chance you could upload that final version of your single sided board ? I'm kind of in the same situation as you ....

If it's just about having a single sided solution, Gen7 electronics might be worth a look.

---

Generation 7 Electronics	Teacup Firmware	RepRap DIY

Yes Gen7 is relativly easy to etch by toner transfer I have etched a few ...

From Blogger Pictures

I think I uploaded a PDF file that made this PCB in the Gen7 forum a while back... it has the plug in Screw terminal connectors as used on most CNC controlers and on the Ultimaker PCBs

---

Bodge It [reprap.org]
=======================================

---

BIQ Sanguinololu SD LCD board	BIQ Stepcon	BIQ Opto Endstop
BIQ Heater Block PCB	BIQ Extruder Peek clamp replacement	BIQ Huxley Seedling
BIQ Sanguinololu mounting	BIQ standalone Sanguinololu or Ramps mounting	Print It Stick It Cut it

My rep strap: [repstrapbertha.blogspot.com]

Buy the bits from B&Q pipestrap [diyrepstrap.blogspot.com]
How to Build a Darwin without any Rep Rap Parts [repstrapdarwin.blogspot.com]
Web Site [www.takeaway3dtech.com]

PDFs for etching Gen7 PCBs are in the "release documents" section on Github. They support screw terminals.

---

Generation 7 Electronics	Teacup Firmware	RepRap DIY