Go Down

Topic: BTN7970 Motor Driver (Read 16809 times) previous topic - next topic

dc42

Well, that might work OK, but it's not how I would lay it out. I would put the power and motor connector behind the ICs, allowing you to route the output terminals direct to the pads and use really short positive supply traces. I'd keep all these traces on the top surface Then I'd put the capacitor right in front of the ICs, or possibly between them. Then I'd put the resistors in front of the ICs, using traces on the back of the board if necessary to cross the power lines to the ICs, and finally the signal connector right at the front. The aim being:

- Keep the power and motor traces thick, short, and away from the input resistors and wiring
- Use short traces only on the reverse side, and only for signal connections
Formal verification of safety-critical software, software development, and electronic design and prototyping. See http://www.eschertech.com. Please do not ask for unpaid help via PM, use the forum.

drewdavis

I would like to start by saying thank you! I have learned quite a bit about PCB making because of you. Hopefully this will be my last attempt at making this PCB...

dc42

That'e getting better IMO, however the trace between IC2 power and C1 should be wider. Also, try to route the power and motor lines without using the bottom side, so that you won't be passing large currents through vias. Assuming your screw terminals are insulated underneath (the ones I have used are), you can route some of the power or motor wires around the sides of and underneath the terminal block, to avoid the crossovers.

The traces that really need to be short are the ones between the positive supply pin of each IC and C1. I would go for one capacitor per IC, so that you can keep these really short.

Also you could have larger copper pads around the tabs, for better heat sinking.
Formal verification of safety-critical software, software development, and electronic design and prototyping. See http://www.eschertech.com. Please do not ask for unpaid help via PM, use the forum.

drewdavis

I was able to do everything except keep the power from having to go through a via. I was just not able to think of a design that would work. I did add a few more vias so hopefully that will help. Also, the motor is only 12v, and i'm guessing around 5 amps. (no data sheet)


Do you think this one will work?


Thanks!

dc42

That's probably OK, however I don't see why you can't route traces underneath the screw terminals, assuming the terminal block is insulated underneath apart from where you solder it in (the ones I use are). Specifically, from terminal 4 (the leftmost one) you could route the trace up, then right, going underneath terminals 3, 2 and 1. From underneath terminal 1 it can continue to go right, then down to join up with IC1 and C2. A branch can also come down between terminals 1 and 2 to join up with IC2 and C1. It would be even simpler if you swapped the functions of terminals 1/2 with 3/4, because then the power would be on the correct side for the ICs anyway.
Formal verification of safety-critical software, software development, and electronic design and prototyping. See http://www.eschertech.com. Please do not ask for unpaid help via PM, use the forum.

drewdavis

I get it now! How is this…

dc42

That looks good. C1 and C2 should connect direct to the ground plane, instead of through a short trace and a via. The right-hand end of R4 looks like it's not connected - I think the ground plane may be overlapping the trace you have from it. Similarly for some of the other traces on the reverse side. I would also shorten the longer traces on the reverse side - run the traces on the top side except where you actually need to perform a crossover, so as to avoid disrupting the ground plane more than necessary.
Formal verification of safety-critical software, software development, and electronic design and prototyping. See http://www.eschertech.com. Please do not ask for unpaid help via PM, use the forum.

drewdavis

I was able to make all the changes except connecting the capacitors directly to ground. How do I do that?

Thank you so much for all of your wonderful help!

dc42

1. Remove the ground plane.

2. Route all the ground wires completely on the underside. So, where you have ground traces on the top side, tell Eagle to move them to the underside. It may be easiest to rats-nest the ground net and then turn the connections into traces on the underside.

3. Make any other changes you need to other traces on the underside.

4. Create the ground plane.
Formal verification of safety-critical software, software development, and electronic design and prototyping. See http://www.eschertech.com. Please do not ask for unpaid help via PM, use the forum.

drewdavis

I believe that it is finished!

dc42

That looks basically sound to me, although it could be tided up. Are you sure you have left enough room for C1 and C2 - what value are they? You should probably use at least 470uF each (preferably 1000uF), which will have circular outlines and may be too big to fit in that space.
Formal verification of safety-critical software, software development, and electronic design and prototyping. See http://www.eschertech.com. Please do not ask for unpaid help via PM, use the forum.

drewdavis

This is what I bought…

http://www.ebay.com/itm/290940423904?ssPageName=STRK:MEWNX:IT&_trksid=p3984.m1439.l2649

If they work I think I will leave the PCB as-is because I would be afraid I would mess something up in my effort to make it look neater.

Thank you so much for all the help you have given me! Hopefully everything I have learned in this forum will help me when I go to get a degree in Electrical Engineering next year.

dc42

Those caps are 470nF. If you look at the example on the datasheet, they have 470nF caps right at the chip, and a 470uF a bit further away. I suggest you add a 470uF or preferably 1000uF capacitor, as well as keeping the capacitors you already have. Otherwise, you will get large PWM currents in the power supply wires, which are likely to cause interference. It doesn't need to be as close to the chips as the 470nF capacitors, so I suggest you put it near the terminal block.
Formal verification of safety-critical software, software development, and electronic design and prototyping. See http://www.eschertech.com. Please do not ask for unpaid help via PM, use the forum.

drewdavis


dc42

Looks good! I presume you have checked that you have a big enough space for it and the correct lead spacing. I don't think I can add any more, other than to repeat that I have not checked the signal wiring.

Don't forget to do a DRC (design rules check) in Eagle.
Formal verification of safety-critical software, software development, and electronic design and prototyping. See http://www.eschertech.com. Please do not ask for unpaid help via PM, use the forum.

Go Up