Homebrew PCBs

Hi

I am designing and building a pwm motor controller.

I am desigining it to run a DC motor with a maximum current of 8 amps and 12 Volts DC supply.

I am using surface mount components and using home etched PCB's.

I am now at the stage of designing the PCB layout. I have been investigating the current caryying capacity of the copper clad board and the track widths needed.

I have found an equation that calculates the minimum track width but this depends on the maximum temperature rise that I allow.

What is a suitable temperature rise?


I will most liley be using FR4 board, with a copper thickness of (1oz) 34uM. 
For example if I allow a rise in temperature pf 20 degress C the width is 3.4mm or 136.7 mil
10 degress the track width is 5.22mm or 208 mil.

I will be using mosfet and diodes in this circuit all of wich will have heat sinks. The connection from the board to the motor will be via a cable connected to the pcb by terminal blocks.

I presume it is best practice to have the track between the mosfet and the terminal block as short as possible? Is there any good practice measures I should be aware of here, can the fets and diodes be too close to the terminals or can i come straight from the mosfet pins to the pcb terminals then leaving the board?


Thank you.

I would think you could allow a temperature rise at least as much as the
operating-temp rating of your mosfets. That might be as high as 125 degrees
C., but that's pretty damn hot! In practice, I use my calibrated fingers to
test component, wire, and pcb trace temperatures: if I can't keep my finger
on them indefinately, they're too hot!

Here's a few other considerations.

1. A trace narrow enough to heat significantly above ambient temperature is
one with voltage-dropping resistance. You probably don't want much of that.

2. Unless you are trying to shoehorn your controller onto a small pcb, you
might as well make the traces as wide as you can within the area of the
board. In other words, you can work out the design from the other end: how
big can your pcb be and therefore how wide can your traces be?

3. If you use a double-sided board, you can run heavy-current-carrying
traces on one side, and signal traces on the other, or some combination of
the two, thereby doubling you pcb surface area.

Best,

Todd
------------------------------------------------------------------------------------
K7TFC / Medford, Oregon, USA / CN82ni / UTC-8
------------------------------------------------------------------------------------
QRP (CW & SSB) / EmComm / SOTA / Homebrew / Design


On Wed, Feb 20, 2013 at 2:53 PM, scubadogct <scubadogct@gmail.com> wrote:

> **
>
>
> Hi
>
> I am designing and building a pwm motor controller.
>
> I am desigining it to run a DC motor with a maximum current of 8 amps and
> 12 Volts DC supply.
>
> I am using surface mount components and using home etched PCB's.
>
> I am now at the stage of designing the PCB layout. I have been
> investigating the current caryying capacity of the copper clad board and
> the track widths needed.
>
> I have found an equation that calculates the minimum track width but this
> depends on the maximum temperature rise that I allow.
>
> What is a suitable temperature rise?
>
> I will most liley be using FR4 board, with a copper thickness of (1oz)
> 34uM.
> For example if I allow a rise in temperature pf 20 degress C the width is
> 3.4mm or 136.7 mil
> 10 degress the track width is 5.22mm or 208 mil.
>
> I will be using mosfet and diodes in this circuit all of wich will have
> heat sinks. The connection from the board to the motor will be via a cable
> connected to the pcb by terminal blocks.
>
> I presume it is best practice to have the track between the mosfet and the
> terminal block as short as possible? Is there any good practice measures I
> should be aware of here, can the fets and diodes be too close to the
> terminals or can i come straight from the mosfet pins to the pcb terminals
> then leaving the board?
>
> Thank you.
>
>  
>


[Non-text portions of this message have been removed]

On Thu, Feb 21, 2013 at 10:57 AM, Todd F. Carney <k7tfc@...> wrote:
>
> 3. If you use a double-sided board, you can run heavy-current-carrying
> traces on one side, and signal traces on the other, or some combination of
> the two, thereby doubling you pcb surface area.

Some of my customers leave the soldermask off their high-current
traces: The HASL solder will carry some more current.

Mitch.

If you can design the board for a 10 degree C rise, that would be great, but you probably can live with 20 degrees C. I would keep the leads fairly short and mount the FET's as close to the terminals as practical, given that you may want to have a heat sink for the FET's.I would also add a few ceramic capacitors between DC power and ground as close to the FET as possible. It is probably a good idea to use a 0.1 uF in parallel with a 1.0 uF to take care of fast current spikes and limit noise. Be sure to use one pair for each FET. The reason for this is that all conductors have some resistance and more importantly a significant amount of inductance. When a fast pulse of current occurs the inductance allows the voltage to drop due to the quickly changing current, and the capacitors tend to keep the voltage more constant.

The subject of trace width to handle current is often overlooked. For example in the last two years I had a Bosch dishwasher that failed to heat the water, and a refrigerator that failed to turn on a compressor motor, both due to traces overheating to the point that sometimes a solder connection melted causing failure. Both were repaired by adding a 14 AWG copper wire to parallel the narrow trace. If you search online, there are hundreds of people who had similar failures with the Bosch dishwashers. Bosch even changed a relay to a higher current rating trying to fix it, but did not replace the wimpy circuit board.





[Non-text portions of this message have been removed]