70A Infineon BTN8980TA motor driver shield

Hi folks

I am a student at Columbia University. I have designed with the help of a freelancer and my limited knowledge some schematics for a shield for the arduino leonardo for a project that i am working on. I took a lot of advice from the freelancer and am not sure if this would work and therefore need some help so that i don’t waste any more money manufacturing it. I thought that the experts on the arduino forum would be the best to give me some advice.

The shield is designed to connect to 3 k-type thermocouples for temperature measurement, to control 3 x 24VDC, 50W purely resistive silicone heaters, to control a high current 24VDC, 120W worm gear motor, take power input from a 24VDC, 480W power supply and provide regulated 5V to the arduino. The schematics and PCB was designed in Eagle 6.

The AD8495 is used as ice point compensated thermocouple amplifier and the BTN8980TA from infineon is used as the motor driver. General purpose MOSFETS are used to driver the heaters.

I am not so sure if the schematics and the PCB is okay in terms of electronic engineering principles, circuit design best practices and as an arduino shield.

I will be highly grateful to anyone who could spare some time to give me some pointers and suggestions on this shield.

Thank you.

P.S: I am attaching in addition to the PCB and schematic files, the datasheets and motor curves. Also, I am very sorry for the low res images and for the pcb and schematics not being .sch or .brd.

The datasheet for the motor driver is http://www.infineon.com/dgdl/Infineon-BTN8980TA-DS-v01_00-en.pdf?fileId=db3a30433da668b6013da692a9c1003e&ack=t

schematics.pdf (36.5 KB)

pcb.pdf (73.9 KB)

pcb.pdf (73.9 KB)

schematics.pdf (36.5 KB)

Why would you trust free advice over the advice of the professional you paid for?

You did pay them? Or is that why the real files are missing?

Having never researched how to wire/measure a thermo couple or used that driver chip, and not really interested in researching them, I can only say it looks like they know what there doing electrically and iffy on the layout.

As to the PCB I'd say it depends on how your having that board made. With a proper solder mask it won't be to much of an issue unless your really sloppy at soldering, without a solder mask that will be a nightmare.

The board is quiet lose in via placements, the via's in some cases look closer to pads then they should be. You usually avoid putting via's underneath other components especially smt parts. If its made by a proper fab company and they say they can do it then it becomes a mute point in most cases cause there via's are nearly perfectly flat.

The spacing is really inconsistent, you have area's of nothing, but in some spots are mega jammed. Your using 2 layers, and although I really can't see what's on layer 2, it looks almost unused. But that's somewhat subjective to the electrical design.

The silk screen is a nightmare, the yellow part and the white center of the via's will not have any silk screen on them when finished. Your going to have a lot of chopped off labels. Not counting the plentiful number that aren't even going to be visible due to being under the components themselves. If your not doing silk screen then its a mute point, but then you could just delete them if that's the case.

See that L1 sitting alone in a sea of blue near the top of the pcb with no via's or traces. What is it going to do like that? Now that I'm looking, a few pads do seem to be just floating all by themselves, like Z1.

See the x8, x9, x10, you might want to remember that the USB is directly underneath it and is shield grounded. If they ever make contact even momentarily who knows what might happen. if you go ahead with that you'll definitely want to put something like electrical tape on the top of the USB plug.

If you have to pay money to get it made, I'd definitely do a full review of the electrical and make sure everything in the schematic is actually reflected on the pcb. Its quiet easy to have it look like a connection on the schematic when there is none if your not careful.

therefore need some help so that i don’t waste any more money manufacturing it

Have you made a prototype that actually works as desired?

Even without looking at the schematic its really obvious that something is wrong when you have a component connected to nothing.

L1 connects to Z1 & p-channel fet, L1 connects to U$1 pin 7. Based on the positioning I'd bet it was routed, something got changed and was never re-routed or not properly connected in schematic.

I'd tell you to learn how to use the software and more or less restart the routing process once you fix the schematic's missing connections. The software does most of the work if set up properly, its just a glorified connect the dots once you get to the routing part.

70A ? What is needing 70A?

Anyway the half-H-bridge circuit using the BTN8980 looks weird - what's the p-channel MOSFET for? Why is there no power supplied to the BTN8980?

MorganS:
Why would you trust free advice over the advice of the professional you paid for?

You did pay them? Or is that why the real files are missing?

I have paid him, but he is not an expert by his own admission. I thought that I would seek a second opinion, from people who know arduino before I went further. The real files he will give only after I give him feedback!

harddrive123:
The board is quiet lose in via placements, the via’s in some cases look closer to pads then they should be. You usually avoid putting via’s underneath other components especially smt parts. If its made by a proper fab company and they say they can do it then it becomes a mute point in most cases cause there via’s are nearly perfectly flat.

The spacing is really inconsistent, you have area’s of nothing, but in some spots are mega jammed. Your using 2 layers, and although I really can’t see what’s on layer 2, it looks almost unused. But that’s somewhat subjective to the electrical design.

See that L1 sitting alone in a sea of blue near the top of the pcb with no via’s or traces. What is it going to do like that? Now that I’m looking, a few pads do seem to be just floating all by themselves, like Z1.

See the x8, x9, x10, you might want to remember that the USB is directly underneath it and is shield grounded. If they ever make contact even momentarily who knows what might happen. if you go ahead with that you’ll definitely want to put something like electrical tape on the top of the USB plug.

Thank you so very much for pointing out these mistakes. I will look into it. I am also attaching some of the other pcb files for layer 2.

zoomkat:
Have you made a prototype that actually works as desired?

I don’t have a prototype that works, I meant that I don’t want to get something wrong manufactured.

MarkT:
70A ? What is needing 70A?

Anyway the half-H-bridge circuit using the BTN8980 looks weird - what’s the p-channel
MOSFET for? Why is there no power supplied to the BTN8980?

The motor we were using earlier had a stall current of 48A. The half bridge is the same as suggested in the infineon application note. the p-channel is for reverse polarity protection and power is supplied via X3-1 and X3-2 direct from the power supply.

Freelancer-shield3.pdf (42.3 KB)

Freelancer-shield4.pdf (37 KB)

Freelancer-shield5.pdf (32.7 KB)

I don't have a prototype that works

Perhaps you should get a motor driver like below and study how it is made and works, then adapt that to your project.

http://www.ebay.com/itm/390908373242?_trksid=p2060778.m2749.l2649&ssPageName=STRK%3AMEBIDX%3AIT

BTW, one of the biggest things that can screw you over is having the wrong part number/foot print.

There can be a lot of parts with similar names in the libraries, the only real difference is usually the pad size and spacing. Pick the wrong one and it won't be solderable or extremely difficult.

There is a learning curve to this stuff but you should probably be the one that's making the mistakes.

laykf: The motor we were using earlier had a stall current of 48A. The half bridge is the same as suggested in the infineon application note. the p-channel is for reverse polarity protection and power is supplied via X3-1 and X3-2 direct from the power supply.

Ah yes, got it - you should have a supply symbol on every supply then it would be clear. C23 can probably go after the reverse protection (it must if its polarised - 47uF is likely to be electrolytic?).

Check the current ratings for the connectors so they don't overheat on stall currents, ditto the PCB trace sizes.

Hi, I'm sorry but apart from one very little schematic, where are the ones that the rest of the forum is talking about, I know some are using the PCB layout, but where is the FULL Schematic that we can use as reference.

Tom...... :)

Every time I look at that board I see more problems.

You have even more serious VIA issues then I thought.

As one example the via near the top left of C1 silk, is touching a trace on the bottom layer.

There is another via set which is near U2 silk, that literally eats half a pad and is directly under an smt part. Even if the via and the pad are the same connection you never ever do that. combined with the fact that its under a part with almost no clearance between the via and the other pad, if you don't solder that perfectly it will short and you'll never ever find it when you go back looking for where the short is.

Plus the other part of that set what is up and to the right, is literally sitting on a different trace, and freakishly close to another pad.

Take that whole routing + via's and chuck it. Move the parts further away from each other and do it from scratch. Plus increase the polyground clearences/tolerances, there is no reason everything needs to be so close together. Objectively if you know how to use the software, shouldn't take more then 1-2h at most.

Your in electronics? Didn't they make you take a class yet that introduces you to PCB design software and teach you the basic's of schematic and pcb layouts?

zoomkat:
Perhaps you should get a motor driver like below and study how it is made and works, then adapt that to your project.

http://www.ebay.com/itm/390908373242?_trksid=p2060778.m2749.l2649&ssPageName=STRK%3AMEBIDX%3AIT

Yes, I just purchased one of those. thanks for the suggestion!

MarkT:
Ah yes, got it - you should have a supply symbol on every supply then it would be
clear. C23 can probably go after the reverse protection (it must if its polarised - 47uF
is likely to be electrolytic?).

Check the current ratings for the connectors so they don’t overheat on stall currents,
ditto the PCB trace sizes.

Thanks for that, I am working on it.

TomGeorge:
Hi, I’m sorry but apart from one very little schematic, where are the ones that the rest of the forum is talking about, I know some are using the PCB layout, but where is the FULL Schematic that we can use as reference.

Tom… :slight_smile:

I have attached a schematics.pdf file that has the detailed schematics.Is that what you are referring to?

harddrive123:
Every time I look at that board I see more problems.

You have even more serious VIA issues then I thought.

As one example the via near the top left of C1 silk, is touching a trace on the bottom layer.

There is another via set which is near U2 silk, that literally eats half a pad and is directly under an smt part.
Even if the via and the pad are the same connection you never ever do that. combined with the fact that its under a part with almost no clearance between the via and the other pad, if you don’t solder that perfectly it will short and you’ll never ever find it when you go back looking for where the short is.

Plus the other part of that set what is up and to the right, is literally sitting on a different trace, and freakishly close to another pad.

Take that whole routing + via’s and chuck it. Move the parts further away from each other and do it from scratch. Plus increase the polyground clearences/tolerances, there is no reason everything needs to be so close together. Objectively if you know how to use the software, shouldn’t take more then 1-2h at most.

Your in electronics? Didn’t they make you take a class yet that introduces you to PCB design software and teach you the basic’s of schematic and pcb layouts?

Thank you so much for your help, much appreciated, I would have been very lost if it was not for your input. I am not an electronics student but a mechanical engineering student. This is a side project I am working on. Thanks again. I hope to work on the mistakes you and the others on the forum have pointed out and will post them shortly.

Have you run ERC and DRC on the Eagle design?

Hi everyone

Thanks again for your feedback and suggestions on my project. I have incorporated quite a few of them, please let me know how I am doing and if there are some more corrections to make. Thanks!

MarkT:
Have you run ERC and DRC on the Eagle design?

I ran the ERC.

Thanks everyone! Much appreciated.

pcb_v1.pdf (207 KB)