PCB design and schematic for a half bridge power amplifier

In summary, the conversation discusses the design and circuit diagram for a half bridge power amplifier that operates at 24V and supplies around 3A current to an inductive load of 10mH. The bridge is controlled using a 20kHz PWM from a microcontroller and includes a current sensor for feedback. The design includes necessary decoupling capacitors and ground planes, with recommendations for improvements such as calculating dissipation on the FETs and improving mechanical stability. There is also a discussion on the start-up scenario and considerations for the microcontroller.
  • #1
thambiTeaInnumVarala
4
0
Hi,

I am making a half bridge power amplifier that operates at 24 V.
The bridge has to supply around 3A current to an inductive load (10mH)
The bridge will be controlled using 20kHz PWM from a microcontroller.
I have put a ACS712 current sensor in the load path to give feedaback to the microcontroller.
There is a IRF9Z24 P FET at the top and a IRFZ44 N FET at the bottom.
Both are driven by a single MC34125 Gate driver IC, which has a 12 V power supply.
The gate driver is connected to the microcontroller through a HCPL optocoupler.

I have maintained 80mil track width for the 3A paths, from a online track width calculator.
I have put necessary decoupling capacitors for the optocoupler and the gate driver ic.
There are 2 copper filled ground planes on top layer and bottom layer that I have not shown in the pcb schematic for visibility.

I have made a schematic and circuit diagram that i have linked here.

https://www.eevblog.com/forum/proje...mplifier/?action=dlattach;attach=679062;image

https://www.eevblog.com/forum/proje...mplifier/?action=dlattach;attach=679068;image

Pl suggest any modifications or pointers that will improve the circuit.
Thanks.
TIV
 
Engineering news on Phys.org
  • #2
A 10mH load has a reactance of 1240 Ohms at 20kHz, so the 24 volt supply will be unable to drive 3A into it. By Ohms Law, required voltage V=XI = 1240 x 3 = 3720 Volts.
 
  • #3
tech99 said:
A 10mH load has a reactance of 1240 Ohms at 20kHz, so the 24 volt supply will be unable to drive 3A into it. By Ohms Law, required voltage V=XI = 1240 x 3 = 3720 Volts.
Hi tech 99,

Thank you for the reply. 20khz is the frequency of the pwm signal to the mosfets from the micro controller. Operating frequency of the drive is about 100 hz, giving about 7 ohms reactance.

Thanks,
TIV
 
  • #4
thambiTeaInnumVarala said:
Hi tech 99,

Thank you for the reply. 20khz is the frequency of the pwm signal to the mosfets from the micro controller. Operating frequency of the drive is about 100 hz, giving about 7 ohms reactance.

Thanks,
TIV
Thanks, I did not notice the 220uF cap.
I notice that the ACS712 gives an AC output centred on 1/2 Vcc and assume you are aware of this.
 
  • #5
It also occurred to me that it might be worth checking that everything starts correctly at switch-on, especially as you have a micro controller involved.
 
  • #6
tech99 said:
It also occurred to me that it might be worth checking that everything starts correctly at switch-on, especially as you have a micro controller involved.
Thank you for the pointer. I will look at the start up scenario in detail and post back.
I will also condition the ACS current sensor output signal before giving the feed back to the mcu.
Thanks.
 
  • #7
Just some small remarks.

- Do you have any calculation about the expected dissipation on the FETs? 20kHz PWM mode with 3A current is not really a stressing matter for any decent FET but still, cooling might be needed and now is the right time to prepare for that. With moving only a few component you can make enough space for heatsinks up to ~10W in case cooling will be needed later on.

- The high current connector seems to be half-off of the PCB, but due the bigger plug with thicker wires this is the one which expected to have higher mechanical load. If it is not any special type or special mount of connector you might want to move it onto the PCB: that will give both the connector, both the holes better mechanical stability.

- You don't have any mounting holes.

- You have some acute angle problems around C4.

- It is better to have a bit wider copper for power lines even if the expected current does not means much requirement

- if you have two ground planes then tie them together regularly with some VIAs.

- avoid using too small VIAs. Makes them bigger, or use the component leads to switch between layers if possible. With some more work you don't need any VIA on this PCB at all (apart from the ones used to tie the GND planes).

These recommendations are admittedly a bit overkill since at 20kHz almost everything will work just fine. But the sooner you start to apply the general rules, the better: later on it takes a lot of work to get rid of the bad habits.
 
  • #8
Just for a lifetime consideration, unless their is an electrical reason not to, move C6 away from the heat of the FETs. (Right now it is in an oven between the FETs.)
 
  • Like
Likes Rive
  • #9
tech99 said:
It also occurred to me that it might be worth checking that everything starts correctly at switch-on, especially as you have a micro controller involved.
When the micro-controller switches on, there are 4 possible states for the two mosfets.

Both mosfets conducting : 3A flows. Actuators have been designed for this current.
PMOSFET OFF, N MOSFET ON: Actuator in free wheeling mode, current has to decrease gradually from 3 A.
MOSFET OFF, P MOSFET ON: Actuator in free wheeling mode, current has to decrease gradually from 3 A.
Both mosfets not conducting : No current flows.

All these 3 states occur in the operation of power amplifier and should not be a problem.
Thanks for the pointer.
TIV
 

1. What is a PCB design and schematic for a half bridge power amplifier?

A PCB design and schematic for a half bridge power amplifier is a layout and diagram that shows the electrical connections and components necessary to build a circuit that can amplify power. In a half bridge configuration, two switches are used to control the flow of current through the circuit, allowing for efficient power amplification.

2. What components are typically included in a PCB design and schematic for a half bridge power amplifier?

Common components found in a PCB design and schematic for a half bridge power amplifier include transistors, diodes, resistors, capacitors, and inductors. These components work together to control the flow of current and amplify power.

3. How does a half bridge power amplifier work?

In a half bridge power amplifier, two switches are used to alternate the flow of current through the circuit. When one switch is closed, current flows through the upper half of the bridge, and when the other switch is closed, current flows through the lower half of the bridge. This allows for efficient power amplification as the switches can control the flow of current to the output.

4. What are the advantages of using a half bridge power amplifier?

One advantage of a half bridge power amplifier is its efficiency. By using two switches to control the current flow, it can achieve higher power amplification with less energy loss. Additionally, a half bridge configuration is more cost-effective and compact compared to other amplifier designs.

5. What are some common applications of a half bridge power amplifier?

Half bridge power amplifiers are commonly used in audio amplifiers, motor controllers, and power supplies. They are also used in high-frequency switching circuits for applications such as LED lighting and wireless power transfer. Additionally, half bridge configurations are often used in inverters for converting DC power to AC power.

Similar threads

  • Electrical Engineering
Replies
23
Views
2K
  • Electrical Engineering
Replies
8
Views
3K
Replies
6
Views
4K
  • Electrical Engineering
Replies
5
Views
7K
  • Electrical Engineering
Replies
2
Views
2K
  • Electrical Engineering
Replies
4
Views
7K
  • Electrical Engineering
Replies
6
Views
3K
Replies
16
Views
10K
Replies
4
Views
2K
  • Electrical Engineering
Replies
2
Views
8K
Back
Top