Go Down

Topic: Advise for circuit, and pcb layout (Read 15931 times) previous topic - next topic

TomGeorge

#45
Mar 02, 2014, 01:19 am Last Edit: Mar 02, 2014, 01:34 am by TomGeorge Reason: 1
Hi, because the board has no flat sides it is awkward to get your output terminals and switching BTN7971N to be as close to each other and an edge, this would minimize the length of power tracks and optomise their width.

So go with what you can, you may have to build up solder on the thinner tracks.
Connector choice, check the spec of the plug/socket you are going to use, with 5A flowing you need a combination that is enclosed, not like the ones you have, and lock securely.
The ones you have on your board can move around, even though they are locked in. This can cause connection problems, heat build up and damage to the PCB material.

Tom........ :)
Everything runs on smoke, let the smoke out, it stops running....

graynomad

Quote
will a 1.8mm trace be able to handle 5 Amps

The theoretical min trace width for 5A is 1.38mm, so you should be ok but it also depends on the length of the run. That said it just seems a bit light on to me, but then I over-engineer everything. If you have room I would up the width.

Looking at the schematic, I assumed that opto had a logic output because of the way it was drawn, but I just looked at the datasheet and it actually has an open-collector output. I don't think it will effect you in this case but that's bad practice to show something that doesn't exist.

What values are the resistors on the outputs of the optos, I assume 350R because you have 351 next to them but in other places you use a different format, ie 10k. If they are really 350R where do you plan to get a 350R resistor? AFAIK the nearest you can get is 352R and that's an E192 value (ie very precise). Surely a 330R will do the same here.

I have to say that the schematic is still very badly drawn, and this



Is just mind-numbing. I'm collecting material for a "worst schematic practices I've seen" article and may include this. :)

The PCB on the other hand seems quite well laid out at first glance. A couple of things though.



Clean this sort of thing up, it's a real mess and the sort of thing the auto-router would do, no human could run traces like that. If you are using the AR then clean up after it. BTW all ARs are crap, I don't know anybody that uses them.

Also right-angle corners are generally frowned upon because acute internal angles on a trace can form acid traps that eat out the trace a little more than the average. With a course board like this it won't matter but it's good to get into the habit of using 45-degree corner. But in some cases using 45-degree corners would reduce the trace length considerably, never a bad thing for high-current runs.

Some traces look very close



But that may just be an aliasing issue with the lo-res graphic. Have you set you design rules according to the fab house you will use and does the board pass DRC?



This is a bit odd, especially for what I assume is a high-current trace, why not pin through and go direct to the chip?

One way to spot this sort of dumb trace placement is to turn all layers off except the top copper. This removes the context of components and silk screen confusion and you can clearly see what the copper is doing. When you see something that looks a bit odd turn the other layers back on and see if it really has to be like that.

Then repeat with all other copper layers.

______
Rob
Rob Gray aka the GRAYnomad www.robgray.com

Jak24


Quote
will a 1.8mm trace be able to handle 5 Amps

The theoretical min trace width for 5A is 1.38mm, so you should be ok but it also depends on the length of the run. That said it just seems a bit light on to me, but then I over-engineer everything. If you have room I would up the width.


Well 5 Amp is the stall current so , hopefully that won't be to much of a problem.



Looking at the schematic, I assumed that opto had a logic output because of the way it was drawn, but I just looked at the datasheet and it actually has an open-collector output. I don't think it will effect you in this case but that's bad practice to show something that doesn't exist.

What values are the resistors on the outputs of the optos, I assume 350R because you have 351 next to them but in other places you use a different format, ie 10k. If they are really 350R where do you plan to get a 350R resistor? AFAIK the nearest you can get is 352R and that's an E192 value (ie very precise). Surely a 330R will do the same here.


Yes, I got 348ohm resistors, hope it'll do the trick , the reason I wrote 351, was because that is what they wrote in the original schematic.
No idea why, :D


I have to say that the schematic is still very badly drawn, and this



Is just mind-numbing. I'm collecting material for a "worst schematic practices I've seen" article and may include this. :)

The PCB on the other hand seems quite well laid out at first glance. A couple of things though.



Clean this sort of thing up, it's a real mess and the sort of thing the auto-router would do, no human could run traces like that. If you are using the AR then clean up after it. BTW all ARs are crap, I don't know anybody that uses them.

Also right-angle corners are generally frowned upon because acute internal angles on a trace can form acid traps that eat out the trace a little more than the average. With a course board like this it won't matter but it's good to get into the habit of using 45-degree corner. But in some cases using 45-degree corners would reduce the trace length considerably, never a bad thing for high-current runs.

Some traces look very close



But that may just be an aliasing issue with the lo-res graphic. Have you set you design rules according to the fab house you will use and does the board pass DRC?
______
Rob


Sorry for the schematic, attached a new one, hope it's satisfactory.
and yes it was a lo-res error, I attached I higher res image.
I will try and fix and runs, the reason why I don' pin through, is I want to be able to use the pins on the arduino there.
But I will try and redo those.
Thanks for all the tips btw,
Otherwise, am I pretty much good to go ahead and other?
Thanks Again.

Edit: Yes the clearances were set according to fab house design rules.

MarvinMartian

My input for what it's worth..

I'd turn off the component values on the PCB layer before sending it off - or spend some time tidying everything up so there's no overlapping text! Have a look at the 'smash' command - this lets you position the text independently of the component placement.

Just because the fab house has a minimum clearance, it doesn't mean you should always use it - there's lots of instances where it looks like min clearance is used when a much safer clearance would be perfectly possible (especially traces passing vias)

There's a school that says right angles in traces are bad, I certainly avoid them but that's mostly for asthetics - but there also seems to be a lot of unnecessary corners in many of the traces. As was mentioned earlier, turn off all layers except one copper layer at a time and look for any deviations in a straight route that are not absolutely required.

if you shifted JP1 down by 0.05" you could elimiate a lot of those corners.


matheusgrit


Good afternoon!
I'm using BTN7971B based on datasheet . I found problems at the time of the tests. When I tested the full bridge circuit ( using 2 ICs ) of these warmed the fuamaƧa out bridge. When tested the half-bridge , it did not work, and the circuit opened ( the engine does not stop spinning ) . I wonder if your project worked perfectly. Thank you for your help , my job is to complete my graduation.

Go Up