RAMPS 1.4.2 fork: RD3D v1.0 (6 steppers, 24v, Due)

Quote
dc42
Too many through-hole parts and/or vias? Although the connectors for the Arduino and the stepsticks no doubt account for a lot of them.

yehyeh. RAMPS 1.4 has something like 300 holes, if i recall correctly. what RAMPS 1.4 _doesn't_ have is significant numbers of GND bridging / shielding VIAs. absolutely none along along the edge of the PCB, absolutely none joining the power planes together, and none joining the GND flood-fill together.

here's a picture of the drill-holes and component placement: the main component-additions compared to RAMPS 1.4.2 are the micro-sd, ICSP (SPI) and the 6th stepper, along with the extra pin-headers for configuring the 4 SPI-based steppers.



there's about 30 GND vias in the bottom left corner alone, 10 power vias around the fuse F1 output, 30 underneath the MOSFET power connector, 40 along the left-hand edge, 15 along the top edge... i couldn't get too many along the right-edge because of the 5V line going near-hard-up against the 18 pin LCD connector so i spaced a few out in the 2x18 connector instead... 10 around the MicroSD for ground shielding... 20 around the 8v power regulator... 15 to 20 surrounding the thermistors in order to shield that area... around 15 per stepper (times 6)...

basically none of these are unreasonable: they act either as power-provision, ground shielding or ground plane stitching. it was just still a bit of a shock. just opened up the RAMPS 1.4.1 board again and... there's absolutely no ground-plane stitching VIAs *at all*. which is even more of a shock. yes sure there's GND pins, particularly on the steppers and the power and arduino through-hole as well as the various AUX connectors but even so.

That's a lot of holes. Swiss cheese ain't got nothing on this board.

Quote
lkcl
... just opened up the RAMPS 1.4.1 board again and... there's absolutely no ground-plane stitching VIAs *at all*. which is even more of a shock. yes sure there's GND pins, particularly on the steppers and the power and arduino through-hole as well as the various AUX connectors but even so.

Common practice on 2-layer boards is to make the bottom layer ground plane as far as possible, and to put power and most of the interconnect on the top. So there is no ground plane on the top, and no stitching vias - except for thermal vias used to cool surface-mount components such as mosfets and soldered-in motor drivers.

Edited 1 time(s). Last edit at 10/12/2017 03:03AM by dc42.

---

Large delta printer [miscsolutions.wordpress.com], E3D tool changer, Robotdigg SCARA printer, Crane Quad and Ormerod

Disclosure: I design Duet electronics and work on RepRapFirmware, [duet3d.com].

Quote
dc42
Common practice on 2-layer boards is to make the bottom layer ground plane as far as possible, and to put power and most of the interconnect on the top. So there is no ground plane on the top, and no stitching vias - except for thermal vias used to cool surface-mount components such as mosfets and soldered-in motor drivers.

interesting - and useful good practice to know. i haven't done very much in the way of 2-layer (and i need to learn), so thank you.

looking at the two layers (this is RAMPS 1.4.1) i don't see any evidence of the bottom layer being treated as primarily a ground plane; it appears to be used for interconnect primarily in the diagonal direction SW to NE. the horizontal bits in the middle are where VMOT has dropped down to bottom layer so that tracks from *top* layer can cross top-edge to bottom-edge.

also, i'm not really sure why but it looks like "thermal" is switched on, on all copper pour. i think i'm right in saying that that means: right where it's necessary to pull 11+ amps from the power terminals the actual safe current-carrying capacity (a 10 degree rise assuming 1oz copper) is around... eight (four per layer). one of the fuse terminals (+12v not +12v2) the copper thermals are so thin on both sides it looks like the current carrying capacity is only around SIX amps. the top two MOSFETs only have power tracks on one side, with a safe (10C, 1oz copper) current-carrying capacity of FOUR amps...

slightly scared and concerned. i'd like to be wrong about this. i do realise the RD3D board's by no means perfect, it's definitely a compromise based on the limitations set (eagle, 2-layer, aiming for low-cost).

To achieve 18A bed current capacity on the Duets, we use 2oz copper and we duplicate the critical trace on the top and bottom of the board.

---

Large delta printer [miscsolutions.wordpress.com], E3D tool changer, Robotdigg SCARA printer, Crane Quad and Ormerod

Disclosure: I design Duet electronics and work on RepRapFirmware, [duet3d.com].

... here is the PCB-design of one of my "high-current"-drivers with +V and GND on the top/bottom layers - tested it with pulsing currents of up to 40 Amperes (limited by the PS) ... have to test for max. "safe" DC-current too:



Edited 1 time(s). Last edit at 10/12/2017 01:14PM by VDX.

---

Viktor
--------
Aufruf zum Projekt "Müll-freie Meere" - [reprap.org] -- Deutsche Facebook-Gruppe - [www.facebook.com]

Call for the project "garbage-free seas" - [reprap.org]

Quote
dc42
To achieve 18A bed current capacity on the Duets, we use 2oz copper and we duplicate the critical trace on the top and bottom of the board.

18 amps, that's a staggering amount. at 24 volt that's 430 watts. so you support Printbed MK2/3 using the 1.4 ohm connection normally reserved for 12v only. (24 * 24 / 1.4 ohm = 411 Watts) i might just be able to get 360 if i'm lucky.. 100W's no problem. yes the RAMPS 1.4 boards double-up the traces: it's just that they forgot to switch off the thermal connection.

dc42: i take it you switched off thermal connections to the power, the MOSFET power pins, and the bed connector, right?

Quote
VDX
... here is the PCB-design of one of my "high-current"-drivers with +V and GND on the top/bottom layers - tested it with pulsing currents of up to 40 Amperes (limited by the PS) ... have to test for max. "safe" DC-current too:

very cool (or... very hot... VDX ) how big's that board? (what area, cm^2)? how wide's the main power line at the start? i can see it's dropping down in staggered increments, but it's only on one layer... exceeeeept... to that first MOSFET, is that right?

btw just because i can, i put together a dual TMC2660 expansion board yesterday, started from the Trinamic 2660 v3 Reference design (and checked with the DuetWifi schematics... ) it's a 5.5 x 7.5 PCB so 41.25 cm^2 - i *believe* that's within acceptable thermal tolerance, i read somewhere they recommend 20 cm^2 per IC. thanks to eagle being a hand-editable XML file-format i managed to work out that you can still *view* the file, you can still generate gerbers.... so i first committed to a git repo, then *hand-edited* the PCB file, creating or moving tracks / polygons first on BOTTOM layer, then using "git diff" to locate them, cut/paste a copy and edited its layer. laborious but it worked.

git repo (and files) are here: [hands.com]

i kept it simple: i removed the "reference clock" - i know what it's for, it's so that the steppers can properly synchronise precise movement. i'm assuming that SPI-driving or STEP/DIR is quick enough for 3D printing. i also removed the 0603 NTC thermistor: yes i could have left it on and run it to the (one) spare pin left.... i might still do that.

also given that the steppers can be hot-disabled (MOSFETs off) using the SPI interface i put the EN(N) pins onto a jumper. i'l have to read the datasheet again, as it's just occurred to me that they might be "default open enabled pulled low" and i haven't got a pull-up resistor in there. the BAMS team (awesome design concept) might have made a mistake with their TMC2660 blades, they wired the SPI CSN *and* ENN together. that would only work if it's possible to communicate with multiple slaves over SPI at once... i don't think it is.

oh - i also need to add SPI CSN pull-up resistors, just to be safe. otherwise i'd have to do the trick of turning the CSN line into an output and setting it high from the Arduino/Due. any suggestions on values to use?

thoughts appreciated on naming / etc. here as i would like this to be a "generic" board rather than something that's specific to RD3D. it's a general-putpose header, 14-pin DIL, i specifically put only the two steppers on it because that covers X and Y. Z i figured is not a problem using A4988s. extruders... not so sure.. but i don't think people are pushing extruders NEMA17s beyond 2A right now, are they??





Edited 1 time(s). Last edit at 10/12/2017 08:58PM by lkcl.

SPI is too slow for commanding stepping on a 3D printer. So you still need the step and dir pins. The ENN pin can be common to all drivers, as it is on the Duet.

---

Large delta printer [miscsolutions.wordpress.com], E3D tool changer, Robotdigg SCARA printer, Crane Quad and Ormerod

Disclosure: I design Duet electronics and work on RepRapFirmware, [duet3d.com].

Quote
dc42
SPI is too slow for commanding stepping on a 3D printer.

really? iinteresting... that's a big surprise. mind you.... 25mhz serial speeds... commands take 20, 24-bits to send... 1M-commands per second, not including processing time (setup i.e. latency). i saw how RRF does the Step/Dir by pushing the same 32-bits to all the timers, but only enabling the pin-ports that are actually needed, in such a way that it could be done in parallel @ 80mhz / 120mhz... so yeah that makes sense.

i think trinamic has been trying to solve the synchronisation issue by having a separate (global) clock. so, you send the commands, they arrive at different times, but the clock pulse goes "tick" and stuff happens synchronously.

Quote

So you still need the step and dir pins. The ENN pin can be common to all drivers, as it is on the Duet.

ahh of course. duh. well... *thinks*... the ENN in this case can be software-driven, it's not massively critical (unlike step/dir) and then the spare/last remaining (14th) pin can be reserved for an ADC (on-board thermistor). if nothing else... well... the M1EN and M2EN i have on separate 2.54mm pin-headers... hmm.... in theeorryyy... i could move those to where the 14-pin AUX header is, make it a sort-of 18-pin... hmmm...

ok so i noticed that RAMPS says it can do between 12 and 35v, so i checked the ratings on everything: the MC7808 can do 35v, the STP55s and the IRLB3034s can do 60v, but the PMV40UN can only do 30. soooOoo.... i tried looking around to see if i could find a suitable similar SOT23-3 MOSFET-N with a higher max voltage, and found the Si2356ds:

[www.digikey.com]
[www.vishay.com]

it looks to me like it's a drop-in replacement, 40V, reacts RDS(on) @ 2.5v (not as good as the PMV40U which starts to switch on somewhere around 2v), drain current up to 4.3A, does it look like a reasonable drop-in replacement?

ok so yeh i lined up the 2 "EN" headers to make the 2x7 effectively into a 2x9, which means that anyone wishing to use this board with hardware-controlled enable can do so.

dc42, what's the layer stack like on the DuetNG? 4 layer? did you follow (precisely) the TMC2660 Reference Design? i'm curious to know if you stuck with the big power planes for the motor out(s) on Layer 2 only, rather than having them on Layer 3 for the B-side connections and Layer 2 for A-side. in the Reference Design the B-side connections are just 3mm-side tracks on Layer 3, whereas the A-side they're 3mm tracks... *and* a big power-plane, with the B-side big power planes... totally disconnected except by the 5 vias punched through the board on each motor NET. all a bit... weird.

[edit: found the PCB file, taking a look....]



Edited 1 time(s). Last edit at 10/13/2017 12:37PM by lkcl.

You can find the KiCad files for the Duets in the T3P3 github repository. We use the top and bottom layers for heatsinking, connected by thermal vias. The top and bottom layers are 20z copper, whereas the inner layers are thinner (I think 0.5oz is standard).

---

Large delta printer [miscsolutions.wordpress.com], E3D tool changer, Robotdigg SCARA printer, Crane Quad and Ormerod

Disclosure: I design Duet electronics and work on RepRapFirmware, [duet3d.com].

Quote
dc42
You can find the KiCad files for the Duets in the T3P3 github repository. We use the top and bottom layers for heatsinking, connected by thermal vias. The top and bottom layers are 20z copper, whereas the inner layers are thinner (I think 0.5oz is standard).

gottem, thanks for the heads-up. hmm, that's a hell of a lot of vias no thermal problems there.

ok so i figured i'd make an attempt to do this as a 2-layer board, making it quite large: not just for heat dissipation but also as a chance to spread things out. so it's 70x85mm or 60cm^2 where if i recall correctly each TMC2660 needs 20cm^2 in free air.

the VM power plane completely surrounds the motor connector on TOP, with the motor tracks spreading out in a V that allows a GND area to exist between them. the same outer edge of that V - on BOTTOM - is connected to the (inner) rectangle on TOP, and also from several sides: that allows plenty of connectivity to the TMC2660's Motor VSS which surprisingly is only two pins. hmm, just checking that: the double pin-width of the big motor, GND and VM tracks is only 1mm... which at 1oz copper would mean only 2.4 amp current-carrying capacity. that's... not really good enough - let's fix that:



ok so each motor NET has 2x 1mm (double-pin) sets of terminals, for a maximum current-carrying capacity of 4.8 amps - overkill. GND and VM on the other hand are a bit dicey. what i've done is split that diagonal corner 45 degrees between VM and GND so that they can get a 1.5mm width (3.6A) worth of copper each to them, and use the fact that QFN pins at the ends of each row will have solder crawling up not just the front of the pin but *also up the side*.

so the risky bit is crossing-over of the VCC (3.3/5v) IO line and the step and dir lines over the top of the motor outputs. that's really the only bit that has me concerned about doing this as a 2-layer board. so i've made sure that VCC and the STEP/DIR lines go over the motor outputs at right-angles (as far as possible), and run over the top of GND copper only otherwise, with plenty of GND vias joining the places where these tracks cross through.

i might see if i can get some GND separation between STEP and DIR (including some vias) but it takes up about... 0.9 mm to do that (track-to-track is 0.3 and track width is 0.3) - that would eat into the VM power trace width... unleess.... i do the VM power plane diagonally leading away from the TMC2660 top-right corner... yeah i think i can do it.

anyway, it's kinda fascinating and hair-raising at the same time. but, at the end of this if it works there will be a dual stepper board that people can connect to any 3D printing board with an extension header: it's powered separately, so you'd just run a pair of DC input wires to it and work out a wiring loom for the 14 (or now 18) pin header.

yep managed it. diagonal out with VM, plane width of around... 2mm so definitely a 4+ amp carrying capacity, that then allowed STEP and DIR to come out diagonally, staggered and separated by a GND area with VIAs each, linked to the GND flood-fill crossing on the other side at right-angles. there's only one VIA in the corner of those big (1206) capacitors - C10 - but i can live with that. the motor output traces are 2mm wide which is enormous (and a huge gap to have to cross), hence the concern about EMI jumping from the motor output to STEP / DIR.



it's not possible (or... more like "not sensible") to cross back underneath the TMC2660. that would interfere with the size of the motor output planes, which are deliberately very large and deliberately underneath the TMC2660. it would not only be necessary to put in the STEP / DIR pins but also some GND separation as well: that's around... 1.2mm in total and that's far too much to cut off those power planes.

i sort-of understand why STEP and DIR are on this side of the IC, it's because the gate controller circuitry for the MOSFET H-Bridge will be on that side. why Trinamic didn't route the tracks to the opposite side of the IC using the PCB that the bare die sits on, i really don't know.

the only other idea i can think of which would improve things would be to split the 2mm motor outputs into two separate 1mm traces, running a GND track between them onto which more VIAs could be tacked. that would make a 45 degree criss-cross pattern where there would be only a 1mm gap for STEP / DIR to span each time. honestly though? i don't know if it would be effective, or necessary, or worth it, or... what? i mean, these ICs are supposed to be outputting clean sine-waves, that's their whole advantage. anyone any thoughts on that?

Edited 1 time(s). Last edit at 10/14/2017 06:19AM by lkcl.

ok so i decided i didn't like the idea of crossing over the STEP/DIR and VCC lines, and it occurred to me: if the motor connector is isolated in an island surrounded by GND and VM, why not do the same thing for STEP/DIR/VCC? so i did: i put them onto a separate header per TMC2660, requiring separate flying leads. it's an expansion board, so it's possible to get away with that.

also i took the opportunity to replace all 0603 components with 0805, so that the whole board can be hand-assembled. the TMC2660 is a QFP not a QFN, which i didn't realise before, so that's possible if a little fiddly (0.5mm pitch pins). with this board being 2-layer it begins to put it into the realm of home/diy electronics which is nice.



Edited 1 time(s). Last edit at 10/16/2017 11:18PM by lkcl.

wha-hey! the 10th october board revision arrived - the one with the corrections and so on. this is on the table at the factory, my friend mike is waiting for the component vendor to put the (small) parts list together. the vendor's taking his time because there's very little profit in it for him. so, mike's being smart and has also given him a big order from another customer at the same time.

i know i've mentioned it before, but i have to admit i'm sort-of... a mixture of alarmed, and amazed, and... i don't know what, really, it's hard to describe - the number of GND and Power stitching VIAs in this board. mike said that when he took the photo it actually hurt his eyes putting it under the light: the sizes of the pads and so on meant a massive amount of reflected light...

still, this is all about keeping costs down but getting good functionality at the same time. that absolutely means 2-layer, big VIAs (the ones in this board are 23mil drill sizes), large tracks and clearances... 12mil - 12mil although i may have messed that up a bit, i'll have to double-check..... yyeah going to have to put up with an 8mil clearance on this board as there are tracks that have to go in between the 2.54mm pins. all the tracks are actually 12mil minimum, just with 8mil clearance. it might be possible to use 10/10 instead, i'll investigate that.

anyway, i estimate i should have these by the end of the week and can start assembling one of them.

There's quite a bit going on there... more soldering! I might have to order a full soldering station soon, that looks like fun.

I'm actually reworking an HDMI switching board that have failing caps on them tonight for my home theater. good times.

Quote
obelisk79
There's quite a bit going on there... more soldering! I might have to order a full soldering station soon, that looks like fun.

hey i'm happy to send you a PCB and a set's worth of components if it takes your fancy. v1 took me 2 days to do / debug. ok... 3 hours to solder, then 1.75 days to debug...

btw my friend mike found me a soldering station, called "Yihua 8786D" - they're actually on ebay and there's even youtube videos (bizarrre....) - i have to say it's pretty good.

Quote


I'm actually reworking an HDMI switching board that have failing caps on them tonight for my home theater. good times.

lloovely... we have a kindle here, and i've got micro-hdmi cables: bit concerned about them, we have to plug/re-plug 4 to 6 times before it doesn't get mad eye-burning brain-melting epilepsy-inducing fuzz / flicker.

Edited 1 time(s). Last edit at 10/17/2017 12:42PM by lkcl.

ok so i did the DRC review, and i can get away with 10mil track-to-track and 10mil trace widths, but not 10 mil track-to-pad/throughhole. the reason is: the 2.54mm through-hole connectors have really large surrounds. i've nearrlly managed to get to 10mil for via clearances (0.25mm not 0.254mm)... honestly though whilst it would be really nice to get down to 12mil/12mil so that this board could hit really *really* cheap one-off production on eurocircuits, it's not a huge priority.

anyway: i don't want to make too many drastic changes until i've assembled and tested the ones arriving in a few days.

Perhaps you should switch from Eagle to KiCad? Then you would be able to make the board larger or 4-layer, which would make the routing easier.

---

Large delta printer [miscsolutions.wordpress.com], E3D tool changer, Robotdigg SCARA printer, Crane Quad and Ormerod

Disclosure: I design Duet electronics and work on RepRapFirmware, [duet3d.com].

Quote
lkcl
hey i'm happy to send you a PCB and a set's worth of components if it takes your fancy. v1 took me 2 days to do / debug. ok... 3 hours to solder, then 1.75 days to debug...

btw my friend mike found me a soldering station, called "Yihua 8786D" - they're actually on ebay and there's even youtube videos (bizarrre....) - i have to say it's pretty good.

I'd love to take a stab at v2 (since v1 still had issues), if you pm me your info I can pay you for the expense of the materials/shipping. Also, thanks for the recommendation on the soldering station.

Quote
lkcl
ok so i did the DRC review, and i can get away with 10mil track-to-track and 10mil trace widths, but not 10 mil track-to-pad/throughhole. the reason is: the 2.54mm through-hole connectors have really large surrounds. i've nearrlly managed to get to 10mil for via clearances (0.25mm not 0.254mm)... honestly though whilst it would be really nice to get down to 12mil/12mil so that this board could hit really *really* cheap one-off production on eurocircuits, it's not a huge priority.

anyway: i don't want to make too many drastic changes until i've assembled and tested the ones arriving in a few days.

How many iterations of RD3D do you have ordered already? Oy!

Quote
dc42
Perhaps you should switch from Eagle to KiCad? Then you would be able to make the board larger or 4-layer, which would make the routing easier.

i appreciate the suggestion: bit of a long story, quite a lot of background - bear in mind that i've attempted to use kicad a number of times, the last time was an effort to make a libre 6-layer board with a 440-pin 0.6mm BGA with four 78-pin DDR3x8 ICs.

me and kicad (and the kicad developers) have a long history going back over six or seven years now. on that libre board, kicad managed to destroy several days worth of work and consistently and repeatedly corrupted libraries that also took several weeks to write and debug, due to not one but *several* inherent design / useability flaw along-side serious bugs. when i raised the issues with the kicad developers, going to the trouble of providing them with comprehensive explanations of the issues involved, they made a half-hearted effort to fix one (and only one) of them, and dismissed the rest *despite* several other users agreeing that the design / useability flaws were actually rather important to fix.

from this i learned that kicad is about a decade away from being useful and safe to use, and i was so angry at the developers that i will not use it - not because they dismissed me alone but because they dismissed *several* people's valuable input. i do realise it's libre software: i do realise none of us are paying them. that having been said: when their attitude changes and they are prepared to acknowledge important design flaws and useability issues, i'll reconsider using the software that they're writing.

bottom line is: they don't understand what software libre is about: they've violated the inherent contract between user and developer: if i use the software that they've developed then that means that i endorse and accept their behaviour. i can't do that... so instead i have simply... stopped using the software that they've developed.

about eagle: on the tmc2660 dual stepper board i managed to work out how to use it to create and edit 4-layer boards: it's quite simple, you edit on TOP or BOTTOM... then you identify the tracks / polygons in the file (changing them to another layer and using git diff is a good way) and.... you edit the layer number in the XML file, hit save on the text editor, hit "load" on the file in eagle and you're done. it requires that you be happy to make proper use of git to keep the changes being made, but i am used to that so it's fine.

the primary reason to keep this board to 2-layer and also to keep its size down is: cost and "acceptability". even if i was happy to use kicad, i would still do it as 2-layer. by "acceptability" i mean that if it gets any bigger, chances are high that users will not "accept" it. bear in mind, it's an upgrade to RAMPS, and is 25% wider than RAMPS already (i moved the steppers).

the only other way, which i am giving some thought to, is to split it into two. one split for steppers and endstops, the other MOSFETs and thermistors. the primary reason i haven't done that is: again, the sizes get bigger, and also, how do you connect them? the arduino/due is actually quite a neat u-shape providing good stable connectivity to whatever is plugged into it.

one possibility on that would be to use the left half of the arduino connectors for MOSFETs (D8 to D13 plus the VIN/3.3v/GND header), and the right-hand set for steppers and endstops. however the only real advantage of doing so would be, i feel, if the separate boards (the theoretical MOSFET board, the theoretical stepper board) could also be used as expansion boards *as well*. in the case of the MOSFET boards, that would work if it was possible to plug in a low-cost MCU which could then communicate via I2C, UART or SPI, to the main Due board. i would suggest a dedicated I2C PWM/GPIO IC there but the cost of those ICs is often $1 when you can just as easily get hold of a 20-pin STM32F030 for $0.30 which has a built-in RC circuit for running without a crystal, so it makes no sense to use a dedicated I2C chip!

the stepper boards on the other hand, i'm mindful of what you said about it being absolutely necessary to use STEP/DIR control. EN is not so important, it can be global. save some pins.

overall though.... $3.50 market selling price in Huaqiang Road for RAMPS 1.4... damn that has me floored. anything that i'm putting together for this board has to go through the "filter" of "is it going to significantly increase the cost?" - multiple connectors (for modules), 4-layer boards, all these ideas: beyond a certain threshold set by that price, i'm really reluctant to prioritise them over other considerations.

Quote
lkcl

Quote
VDX
... here is the PCB-design of one of my "high-current"-drivers with +V and GND on the top/bottom layers - tested it with pulsing currents of up to 40 Amperes (limited by the PS) ... have to test for max. "safe" DC-current too:

very cool (or... very hot... VDX ) how big's that board? (what area, cm^2)? how wide's the main power line at the start? i can see it's dropping down in staggered increments, but it's only on one layer... exceeeeept... to that first MOSFET, is that right?

... this board is 160x24mm "big" (or better "small") -- the coolers will be much bigger

Here's an image of the three populated boards - the one in the back is complete with coolers and base-plate:

---

Viktor
--------
Aufruf zum Projekt "Müll-freie Meere" - [reprap.org] -- Deutsche Facebook-Gruppe - [www.facebook.com]

Call for the project "garbage-free seas" - [reprap.org]

Quote
VDX

... this board is 160x24mm "big" (or better "small") -- the coolers will be much bigger

Here's an image of the three populated boards - the one in the back is complete with coolers and base-plate:

neat. hey, you use a microscope to help with soldering, that's a good idea. i left my silly-looking headwear in storage in the US when travelling to taiwan.

Quote
obelisk79
I'd love to take a stab at v2 (since v1 still had issues), if you pm me your info I can pay you for the expense of the materials/shipping. Also, thanks for the recommendation on the soldering station.

sure, i can do that. smallest components are 0805. if you're interested, help on editing the wiki with photos to advise people on which components to do first much appreciated, if you put certain components on first they get in the way later, and i have no idea what to advise people for the electrolytic capacitors if they only have a soldering iron for example. i chose to tin the ends then use the heatgun to heat it until the entire capacitor was up to temp and it dropped down onto the board.

Quote

How many iterations of RD3D do you have ordered already? Oy!

two sets of 10 that's all!

the MOSFETs.... remember they arrive from the markets in little zip-loc plastic bags, i'll send you some extras. if they all don't work you'll easily be able to get them on digikey/farnell/etc.

[s.taobao.com]

oh my god. USD $0.50 to $1 for A4988 steppers. USD $1 for a CNC "shield" that takes 4 stepper boards. USD $12 for a full RAMPS 1.4 kit. this is insane.

that may explain why there have been a few users recently trying to build repraps using cnc shields...

.... but this also explains why fewer and fewer competent developers are willing to present their own developments to the community... it sometimes takes only a few weeks until a clone from China appears at a fraction of the cost price....

---

Viktor
--------
Aufruf zum Projekt "Müll-freie Meere" - [reprap.org] -- Deutsche Facebook-Gruppe - [www.facebook.com]

Call for the project "garbage-free seas" - [reprap.org]

Quote
VDX
.... but this also explains why fewer and fewer competent developers are willing to present their own developments to the community... it sometimes takes only a few weeks until a clone from China appears at a fraction of the cost price....

great! design it... pretend you're going to make it yourself... get it cloned then buy and import it [at a fraction of the price...] stock it to the ceiling and sell it to unsuspecting westerners yay! save yourself a fortune in manufacturing costs and the hassle of having to bother communicating with china factories *and* with western prices. i don't see a downside... ok ok it's a good idea to do some QA, but _apart_ from that...

i can see reprap.me are already doing this: the blue connector on this [www.reprap.me] tells me that they're importing that board from china, and likely making 50% on it. likewise [www.reprap.me] but here if the taobao costs are anything to go by they might be making a 100%+ markup, depending on import costs.

recognising the reality of what's happening - china cloning - well, i feel that we can either let ourselves be "victims", pretending it's not happening and hiding all development, letting ourselves be quotes exploited quotes and letting the open reprap community be effectively and completely and utterly destroyed... or we can be *aware* that cloning takes place, and take *advantage* of that to save on production and development costs.

now, i did see what happened with RAMPS-FD: seeedstudio took an early prototype, shoved it into production and, when they were warned that it was faulty and causing problems for users and they refused to pull it, bobc terminated all development and put up a massive warning on the page. seeedstudio's reputation is now in the shitter as a result. if they do that too many times, such that the online forums here become completely overwhelmed with reports of seeedstudio's f***-ups, it won't be that long before they'll have to shut up shop.

yes we *really do* have the collective power - indirectly - to influence manufacturers. look at what happened to HTC when they started criminally infringing copyright (GPL violations), and more to the point look what happened when they pissed off the XDA-developers forum key strategic developers with some of their "new" product lines. they produced products that annoyed the XDA developers forum leads so badly that the forum was absolutely stuffed full of complaints. and what happened? their products tanked. why? because the first thing that users do when researching a new product to buy is: get online. type in the keyword aaaand what comes up on the top page? XDA-developers forum. oh look, lots of complaints - i won't buy *that* then!

in exactly the same way, this forum (and the reprap.org wiki) - as one of the longest-running and thus the highest google pagerank - has an enormous influence on the manufacturers as it's where people come to find out about what to buy. yes unfortunately it means some people have to get ripped off, but that's just... reality. they should have gone into the purchase eyes-open and done the research in advance. that's their lesson to learn and we can't take that away from them.