DIY Economiser for OEM Contactors

[Pete9008]

Fairly sure both channels are different and not convinced either is quite right - my version had 4 resistors, you've added one to give the non-inverted input but still only have 4 TBH I always try to layout the schematic so that it flows, minimises crossed wires and tries to have positive at the top and gnd/neg at the bottom - I find it just makes it much easier to follow it and to spot errors.

On my kicad, which I think is a standard install, if you go to 'Add a symbol (A)' and then type BC857 in the search box it comes up with 4 items, the first one is in a SOT-23 package so looks like the one you want. The BC857 is a fairly generic part though, it just ties down the basic part type and footprint. Once it's in the schematic you can go into it and edit the value to exactly match the Digikey part so that the BOM comes out correctly (not exactly best practise but creating a new library part for every physical part becomes a nightmare and is a little unnecessary for this).

Just checked and there isn't a drv103 in the kicad library but the one you've created looks OK. Did you create the footprint or did you use one of the ones in the footprint library?

Edit - Think this is what you have for the lower channel:

And this is what you need:

Thinking about it it might also be worth adding a 10-100nF capacitor across Rpulldown2. Not too sure what the ESD protection on the DRV input pin is like and if the board is used without the transistor a cap will help it survive transients better.

[Zieg]

Ah damnit, you're right. My son isn't sleeping right now and thus I'm not either. Seems I'm affected more than I thought. I'm sorry to have wasted your time like that. I'll revisit it in a couple days and get it fixed up with that extra limiting resistor and capacitor. I'm pretty sure I understand how it's supposed to work now, at least.

And to answer your other questions, I did try putting 5v straight to the input pin and it did close and economize the contactor. Hopefully that means at least that driver isn't blown, because the stupid things are kind of expensive when you start going through them in pairs, haha. I also kind of hate the tantalum caps because they physically blow up when you solder them in backwards. Very difficult to tell polarity after you solder and desolder them once. But, that's what the datasheet calls for..

I'm not sure where that original box symbol came from but I believe it came up when I first added the transistor, so I just ran with it. Then I tried to swap it out for one that looks like the proper symbol and used "Transistor_BJT:BC857". The DRV103 footprint was downloaded from somewhere else, but I had to add the via in the middle. At the time I believed the one I was getting had a pad on the bottom for heat dissipation, but that turned out not to be the case. I just left the via in case anyone did have one with that feature.

[Pete9008]

No problem, know what it's like to lose sleep and how much it affects things, not nice. Also no problem with my time, I'm recovering from a health issue at the moment - well enough to get bored but still without the energy to do anything physically or mentally strenuous so PCB type stuff is ideal. Happy to provide as little or as much help as is useful.

Regarding the power dissipation I tend to be a little conservative on power ratings, I know the max operating temp for these is 125C but I don't like letting anything get above 70-80C to maximise life (and prefer to keep it down to 60C to minimise the chance of burning myself while testing!). Using an 80C limit, 40C ambient and the device without the power pad (thermal resistance of 150C/W) means that the continuous current would be limited to around 0.75A. A 100C limit would get you around 0.9A. If that isn't enough then it might be worth considering moving to the power pad device, and adding a small plane area, to get nearer to 1A continuous at 80C (although they appear to be out of stock at the moment).

I know what you mean about the tants, I have a bit of a love hate relationship with them. Compared to electrolytics they have a much better life and better high frequency performance but they do have a habit of self destructing if put on backwards. Some types also have a habit of self destructing if they are on a low impedance supply with a fast rising edge, essentially the current surge as they charge is enough to physically damage them. Fortunately ceramics have come a long way in recent years, you can get a 10uF 50V ceramic in a 1206 package now for quite reasonable money. They are also better than tants for decoupling. I'd be tempted to switch a couple of these in parallel on each device (say Digikey 1276-6736-1-ND).

[Zieg]

Ah, I hope the rest of your recovery is as speedy and easy as possible! Any help you're willing/able to provide is highly appreciated. I'm sure many others here appreciate it too! I had given up hope of ever making it work on my own...

I don't think the power pad will be needed. At least, not according to my math. Hopefully my own use case will be pretty standard, which is a LEV200 contactor. The coil in that is about 10 ohms. If I assume 14.5VDC from the DC/DC converter and a 20% PWM duty cycle, I'm looking at about 2.9v through that 10 ohm coil, resulting in .29 amps (I = V/R). If I take the contactors from my pacifica battery, they have a coil resistance of just 3.1 ohms, so probably best to configure the DRV for a 10% PWM (1.45 volts) resulting in .47 amps.

I'm going to try to set up a Github for this, will post the link shortly.

Edit: Completely new to this too, but I believe I have this set up correctly now: (edit: forget the github, see Pete's attachment below)

[Pete9008]

You're probably right on the power pad not being needed but it doesn't do any harm to include it and it does allow the operating range to be extended in future if needed.

I'll probably have a look at it this evening if that's ok? Is there anything that shouldn't change? Are the dimensions just as small as possible (do you want to stick with 1206 or are 0805 or 0603 an option?). Are the mounting hole positions fixed? Can the connector pinout change at all to ease routing?

Github is great for sharing the design but not sure it works well for kicad collaborations (unlike software there's no easy way to merge changes other than copy the whole new file across). I'll just post a zip of any changes here and then it's up to you whether to use it or not.

[Zieg]

Okay fair enough. The only thing about the power pad is that it prevents someone from running a trace under the chip, but I suppose it shouldn't be necessary to do that anyway.

Dims are just small as reasonably possible, and yeah pinout can change for sure.

For component sizing, I went with 1206 because I thought I'd have a reasonable chance of hand soldering stuff where needed. So far I have been using solder paste and flowing it in my kitchen oven, then hand soldering things when I need to make changes. If anyone knows of a place that can do the pick/place/soldering for small runs then smaller components are fine, but I don't think my hand is steady enough to place an 0805 size component reliably.

[Pete9008]

Revised files attached, please feel free to keep or ignore any or all of the changes. I think everything discussed is included but please check it all thoroughly.

Quite enjoy doing boards like that!

PWMEconomizerTest_r3.zip

(102.94 KiB) Downloaded 66 times

Edit - Just realised that the entire current was flowing though a single via on the gnd pin of the drv - not ideal. Just added a second track and via and updated the zip.

Edit2 - 30th May - ZIP file updated to correct swapped reference designators mentioned in later posts.

[Zieg]

Holy crap! That is AMAZING! Thank you so much for doing that. I can't believe how nice and clean that looks. I'm going to order a run of three PCBs right now.

[Pete9008]

No problem, glad to help and enjoyed doing it. Just hope it works!

Also realised that I mislabelled four of the resistors. Rin on each channel was supposed to be the non-inverting input while Rinv was supposed to be the inverting - I seem to have managed to get them the wrong way round. Shouldn't affect operation at all, just a little irritating, but might be worth fixing before getting anything made? (just change the names over in the schematic, update PCB from schematic (but make sure that re-link footprints based on reference designators is NOT checked) and then run the PCB design rules check to make sure it's all still OK)

[Zieg]

Ah, I did order it last night already, maybe it's worth just updating it in the zip you posted?

I'm also going to put together an updated BOM from Digikey and call out each item by its new name on the schematic. Then I can also suggest some different configurations depending on the desired PWM frequency and whether the signal is inverted. So glad this thread popped up and that Pete took notice and saved the day. What a great community!



Posting the info below now because it was easy to compile while building my own order, but feel free to wait for me to get my test PCBs and be the guinea pig to make sure everything works as intended....

Okay here's the cart I have put together. $31 CAD - not bad! https://www.digikey.ca/short/h20v7vrc

I do like ordering a couple extras of the resistors and caps and such, but the quantities here are the minimum to build one board (which runs two contactors).

This is set up for the following:
20% duty cycle
110ms of full power output before starting the PWM
25kHz PWM frequency (lower might make the coils 'sing')
Negative input signal (such as running off an OpenInverter board)

Depending on your contactors, you may need to vary some or all of those values. The DRV103 datasheet has tables to let you figure out what value to change the Rpwm, Cdly and Rfrq components. https://www.ti.com/general/docs/supppro ... n%2Fdrv103

Lastly, if you are using a positive signal, you can omit the transistor, Rpu, Rinv and Rlim, and instead populate Rin. The value for that resistor will depend on the voltage of the positive signal you are feeding it, but I believe if it's over 5v you will want to calculate the value based on supplying only 0.12mA to the input pin?

You'll also need some solder paste, a way to flow it (I use my oven), and a pair of plastic tweezers are really helpful for placing components. A magnifying glass and a good soldering iron are great for checking/fixing all the connections after it's out of the oven. You'll want to carefully manage your caffeine levels to get the steadiest hand possible while placing these things.

[Pete9008]

Ah, I did order it last night already, maybe it's worth just updating it in the zip you posted?

Sorry about that File updated with the corrected reference designators above.

You'll also need some solder paste, a way to flow it (I use my oven), and a pair of plastic tweezers are really helpful for placing components. A magnifying glass and a good soldering iron are great for checking/fixing all the connections after it's out of the oven. You'll want to carefully manage your caffeine levels to get the steadiest hand possible while placing these things.

It's also quite possible to do it by hand with just a fine tipped soldering iron. The technique I use is to put a little bit of solder on one pad, hold the component in the tweezers while reheating the soldered pad and manoeuvrer the component into place (might take a little adjusting to get just right), solder up the other pad/s and then reflow the first one (either with a little flux or a tiny bit more solder). Only really suitable for smaller boards as it is slower and also takes a little practise but I've managed down to 0402 components using this approach in the past (didn't like doing it though!). The results aren't quite as good as reflowing in an oven but they can be pretty close. I agree on the coffee too!

[Zieg]

All good! I just updated the Digikey BOM to reflect that too.

Hm, at some point if I find myself doing more of this, it might be cool to convert an old 3d printer to a ghetto pick and place machine, haha.

[Zieg]

It works! It works!

Got the PCBs in a couple days ago, finally managed to get one soldered and tested tonight. Initially I forgot about the change to the in/inv naming convention and had to move that resistor (shown in the wrong spot in the photo). But after that, I plugged it in and both channels are working exactly as expected. Thanks so much Pete!


For anyone wondering, this was all done with low temp solder paste and flowed in my convection oven preheated at 350F while watching it like a hawk. When I saw all the solder flow, I took it out. Don't, uh, look at C2/C4. They are meant to be connected there anyway...

[arber333]

It works! It works!

Got the PCBs in a couple days ago, finally managed to get one soldered and tested tonight. Initially I forgot about the change to the in/inv naming convention and had to move that resistor (shown in the wrong spot in the photo). But after that, I plugged it in and both channels are working exactly as expected. Thanks so much Pete!


For anyone wondering, this was all done with low temp solder paste and flowed in my convection oven preheated at 350F while watching it like a hawk. When I saw all the solder flow, I took it out. Don't, uh, look at C2/C4. They are meant to be connected there anyway...


pwm econo.jpg

Hey! Nice job!
Can you send me one board for two contactors?
PM me.

EDIT: I am sorry are you from CA? I thought you are from UK...

[Zieg]

Yeah I'm in Canada. Should be everything you need in this thread if you did want to order the parts though. I don't know if I'd trust myself to make up a batch of these for other people by myself, but maybe I could find a cheap low volume assembler if enough people wanted one?

[PaulUdrea]

Hello Zieg,
I would be interested to buy 2 or 3 economisers if you have available. I am in Canada as well, Toronto area. Alternatively, if you need some as well, maybe we can order a batch through JLCPCB. I don't mind having more than 3.
Nice work, thanks to you and Pete for the efforts.
Cheers,
Paul

[Zieg]

Pete did all the hard work! I just selected components. I don't have any made up right now aside from the one that's currently in my (unfinished) car. If you don't feel like trying to solder it yourself I say try JLC. I'd be curious to see what they charge for it anyway. Hopefully not much more than the digikey bom + oshpark pcb print.

[PaulUdrea]

I should be able to solder the components, but my thought was, if we have to order the PCBs, we might as well let JLC place them. I've ordered in the past some boards from JLC and the price was good, considering the amount of work needed for soldering by hand. JLC will need the file (spreadsheet) for locating the components, can't remember the name, cpl or something like this. Do you have it? I've never used KiCAD so I don't know if it can be generated with KiCAD.

[uhi22]

For KiCAD there is a Plugin which creates exactly what jlc needs (Gerber, bom, placement), it is really convenient.

[jrbe]

Search the KiCad plugin manager for JLC. It's something like JLC PCB toolkit. Just click install.

https://github.com/bennymeg/JLC-Plugin-for-KiCad for more info on it , what it can do and how to do it. It's extremely helpful and has solutions for what everyone struggles with using JLC.

[PaulUdrea]

Great, thank you uhi and jrbe. I'll give it a go.

[uhi22]

Sorry I'm confused, where did you find the Kicad files? Are they on github? Or anywhere else? Would like to have a look into.

[PaulUdrea]

Yes, on github, Zieg saved them there. The link is on this thread, see Zieg's post from 28th of May

[PaulUdrea]

KiCAD generated the gerber files, but I can't attach them to my post. I'll message Johu.
On KiCAD there is a feature called Inspect, I run it and it came with some warnings. I've never used KiCAD so, I've left everything as is. Next, I'll try to get a quote from JLC and let you know the price.

[Zieg]

I don't think that github has the latest version. I should probably delete that link. I believe the latest one is in the ZIP file Pete has attached to his post about 15 posts up from this one.