MOSFET gate PCB design question

[HighHopes]

thanks, just PM me with the link is fine. i'm always after more knowledge.

normally ferrite beads are to filter very high frequency noise.. but place between driver and mosfet in series.. my guess is that it is used to provide a slight damping on the edge rate of the gate drive current .. or .. somehow is there to change the resonant frequency to avoid oscillaitions between gates of a parallel mosfet topology.

i would say that the mosfet is designed to take very high rate of current (i.e. 15V pulse applied through a resistor to the mosfet gate pin) with no need to limit the di/dt by using an inductor. the rate is limited by the RC time constant of the gate resistor and mosfet internal gate capacitance. anyway, the mosfet is designed to take it, is tested & validated by the manufacdturer as such. maybe for RF application its different, but we're talking about a motor drive application.

for oscillations between gates .. like ONE gate resistor supplying current to 6 parallel mosfets for example.. yes it is possible that between the gate pins of reach parallel mosfet there could be an osciating voltage which would be very bad. this is why most power mosfets actually have 1ohm INTERNAL gate resistance built in just incase someone decides to put 15V direct to the pin with little to no external gate resistance. for me, i would not solve this problem by adding a ferrite bead. actually, if you look at zombiess' cadilack design you'll see 0805 size 0.5 Ohm resistors on each gate which is there to dampen (not avoid) the oscillations.

Should those be placed as close as possible to the gate pin on the MOSFET or is it more important to route the gate path away from the high current paths (source-drain)?

you could argue both. gate resistor must be close too the gate pin to minimize loop area & copper traces which have 10nH inductance per inch (or something like that). vias have a lot of inductance so you should try to avoid this. when you route the copper trace from driver IC to mosfet gate pin the return path (mosfet source pin back to driver) should be routed on a different layer directly underneath the supply trace .. not beside it.

also you have to keep the gate pin & resistor away from the drain pin as you say because the drain pin has DC bus voltage on it while your gate resistor and ICs are only rated for a fraction of the voltage.. so keep far way! thankfully, in an effort to minimize loop area between driver IC and mosfet gate pin you will find that it works out in your favour to avoid close proximity of the drain pin. you tightly control the traces, their location, the componenets.. all in small area, no wild traces going willy/nilly where ever near drain pins.. no.

 

[zombiess]

I guess you meant "gate to source"?...

Ugh, totally screwed that one up. I've corrected now. Not sure WTF was going through my head when I typed that. I've got at least a dozen different schematics I've drawn all with gate - source resistors in place LOL. Derp.

 

[Honk]

Honk, yes, it's the FDMS86500DC I'm planning on using. The Dual Cool devices have slightly better specs than the non-Dual Cool FDMS86500L devices.

Did you know there's a new boy in town? The extremely low RDSon FDMS86550 @ 60V, 100A, 1.4mR typ, but slightly higher Ciss at 8235pF.
Not Dual Cool but just easy to keep cool anyway by a top heatsink. I wouldn't be surprised to see a DC version of this fet soon showing up. 8)
As long as an application doesn't stress the fet more than a third of its current rating it will be favorable to use due to the lower RDSon.

I don't know what you mean by using high speed switching as power limit, can you explain or point me to some reading?

I'm afraid I didn't explain this very well, I was tired late yesterday evening.
What I meant was the duty cycle control of the fets On-Time in order to control speed or current limit of the motor. See page 12 and 18 at this PDF
Usually it's the On-Time of the lower set of fets that is being chopped by fixed frequency and variable duty cycle. Normal frequency is 16-25KHz for most applications.
This "power chopping" adds heating by the Fets rise and fall times x Used frequency x Current level. This is additional losses besides the resistive I2R.

 

[Futterama]

Personally I never use parallel schottkys, instead I closely match the H-bridge for perfection without any cross conduction.
That's so much better and efficient.

I don't understand what you mean by match the H-bridge without cross conduction. Please explain

Myself I prefer using size 0402 1R as gate resistor and it fuses really well if needed.
Size 0402 works beautifully and has really protected my prototype designs at several occasions.

I don't think I have ever soldered anything smaller than 0805, so 0402 will be fun to try

Two application notes that mention the ferrite bead:
APT-0402 Eliminating Parasitic Oscillation between Parallel MOSFETs
AN-9005 Driving and Layout Design for Fast Switching Super-Junction MOSFETs

I don't see how I could keep the current loop small (what is small anyway?) with these SMD devices. I could really use to see a good design where this loop area is small. But to keep it small, you suggest the gate driver should be placed on the same PCB as the MOSFETs? I think this would require an even larger loop since the driver has to be out of the way of the physical large high current paths. Also, the driver would have to be placed between the high side and low side MOSFETs so the loop is equally small to both of them.
I will have to get creative then.

 

[Honk]

I don't understand what you mean by match the H-bridge without cross conduction. Please explain

Google is your friend....
More friendship....
Simply put, the top and bottom fets should never conduct simultaneously. In a ordinary three phase BLDC controller with trapezoidal waveform it's not a problem
But within a high frequency sinusoidal three phase controller both upper and lower mosfets is switching on/off continuously at high frequency while
adjusting the duty cycle to form a sinusoidal wave from square waves. The proportional output equals a sinus wave, and that is what the motor sees.
To make it efficient you need to make sure the fets never cross conduct as this will cause high spike currents and unwanted heating.
At idle motor all three mosfet bridges operates at 50% duty cycle continuously and the output is zero as the duty cycle difference is zero.
Due to the motor being feed by 50% square waves on all phases when idle it's important to use a high frequency to block idle currents through the phase inductance.

I don't see how I could keep the current loop small (what is small anyway?) with these SMD devices.

Place the drivers at bottom side of the PCB below the mosfets. Use a 4-layer board with 210um copper to handle the currents.
Solder copper bars to strengthen the current path. Go from bottom side drivers to top layer by a small via hole just next to each gate under the mosfet.

 

[Futterama]

Why do I need 4 layers? What is the middle 2 layers for? I can see the point in 1 middle layer, acting as an EMI shield...

I was planning on making the PCBs myself, using 105µm PCBs (the thickest I could find), and then add some current "reinforcement" using 0.8mm bare copper wire soldered on top of the copper layer. I have always made my own PCBs, this is part of the fun process for me.

I was also planning to have MOSFETs on both sides of the bus bar, to keep the total controller size small enough to fit the 70x70mm heatsink. I was then thinking that I could place the ferrite bead and gate resistor on the other side of the MOSFET PCB, to keep them close to the gate pin, but I would have the problem of missing a shield plane between MOSFET plane and gate components plane unless I use 2 PCBs "glued" together to form a 3 layer PCB. This approach would add to the bus bar thickness, and I started thinking about skin effect and I guess my mind wandered off into "holy crap"-state.

 

[Honk]

A 4-layer board is not necessary but gives very good results. From my experience there is no 3-layer board. The choice is 2, 4, 6 layers and so on unless you make your own
I usually make my own 2-layer boards and via holes, but for my big 250A ESC project I have decided to buy some high quality boards.
It does make a difference when it come to design flexibility and easy routing, like placing small vias below a Power56 case.
The 210um copper thickness improves board low resistivity besides using copper bars. I prefer PCBCart with high quality and good prices.

 

[Futterama]

I have been working a bit more on my design, and I just could not see how I could make a small gate loop when the MOSFETs are placed with a busbar between them, but this was because I was planning on using the FAN7190_F085 which is a high & low side driver. But I can just use separate high and low side driver ICs. Fairchild has some really powerful (9A) low side drivers which also features undervoltage lockout like the FAN3122T. Their 4A high side drivers does not have much explanation in the datasheet, and I cannot see how the bootstrap capacitor is charged, so maybe I could use the originally planned FAN7190_F085 as high side driver and the use the devices low side driver to drive a small MOSFET for charging the bootstrap capacitor.

Which MOSFETs are usually switched during PWM, the high side or the low side? Or is "load balancing" used so sometimes it's the high side and sometimes it's the low side, to spread out the switching losses between high and low side switches?

 

[zombiess]

Boot strap can be as simple as a cap and a diode on the gate supply side.

Figure 1 in the FAN7190_F085 spec sheet shows it.

A more interesting method I've seen is from the IXYS AN-401 app note Figure 15 which uses the high side PWM input to switch a FET to charge a cap, never seen that setup before. IXYS has some very good app notes, much better than most of the IR ones I have read. I've been looking at the IR2114 is a fully featured chip with LOTS of really nice features to protect the FETs. This PDF even has a decent PCB layout in it that talks about the loops and ground plane.
http://www.irf.com/product-info/datasheets/data/ir2114ss.pdf

It's only a 3A driver, but that can easily be boosted to >10A with 2 transistors and a 10uF XR7 cap if needed.

Are you still set on the SMD FETs? Remember that stray inductance and heat are the enemy, but if you have packaging constraints that have to be met then it is what it is.

If you are doing unipolar PWM then I don't think it shouldn't matter if you PWM the high or low side, I've seen controllers do it both ways, not sure if one way is better than the other.

 

[bigmoose]

Zomb, I had not yet seen the IXYS app note that you mentioned. It is excellent! Everything in one place, great application schematics. Thanks for that reference.

http://www.ixysic.com/home/pdfs.nsf/www/AN-401.pdf/$file/AN-401.pdf

 

[zombiess]

Zomb, I had not yet seen the IXYS app note that you mentioned. It is excellent! Everything in one place, great application schematics. Thanks for that reference.

http://www.ixysic.com/home/pdfs.nsf/www/AN-401.pdf/$file/AN-401.pdf

Of all the app notes I have read from different manufactueres, IXYS seems to have some of the best ones. Some of the newest IR ones are getting good too, to the point of including working PCB layouts with smaller loops and ground plane layouts.

Learning this driver design stuff is very challenging. If a school offered a course on this they would probably have to spend around a year teaching many of the intricacies to new engineers. Even with all the hand holding I have had with this, I still choke on PCB layout and spend 1-2 weeks worth of working hours just to do a driver IC.

I'm finally at a point I understand a large percentage of what I'm doing and can prove most component selection mathematically and explain function, but I'd say i'm only about 60%.

 

[Futterama]

zombiess, the FAN7190_F085 charges the bootstrap capacitor when the low side MOSFET is ON or through the load if that is connected to GND.

I don't see how Fairchilds high side drivers charge the bootstrap capacitor, but they don't mention motor drives directly as an application for the drivers. Like this one: FAN7371

Regarding the circuit for increasing the gate drive current using transistors, will this also be possible for the high side when using bootstrapping?

Yes, I'm still hooked on the SMD devices. The controller I'm building is for a RC motor for largescale RC cars. I have added hall sensors to the motor since sensored motors are superior in smaller scale cars, but for some reason I have not yet seen a sensored motor for largescale cars. The hall sensors will also make it easier for me to do the commutation since I don't have to worry about measuring the BEMF, I just have to look at the hall sensor states.
The RC controllers for largescale cars that I have seen are very very small. I have 2 of them from different manufacturers, they don't work anymore, the MOSFETs are burned but the cooling was also very poorly designed. I will post some information and pictures of them in a minute.
Anyway, the controller will need to fit inside the car along with all the batteries and the motor and the cooling fans for the motor. So a small controller will be easier to find the right place for. Also, the car is used for competition, so the controller should not be too heavy as a lighter car will be faster around the track (offroad).

Unipolar PWM, that is something I have not heard before so I don't know if that is what I'm doing :?

If I have a 4.5A high side bootstrapped gate driver, and a 9A low side gate driver, I would assume that using the low side driver for the PWM switching would be most effective since this can switch faster due to the increased gate current capability over the high side driver. So when I need to energize a phase, I would simply switch ON the correct high side MOSFETs, and let them be on for the whole phase period (requires a "big" bootstrap capacitor and the motor would have a limited minimum speed), and then modulate the phase current using PWM on the low side MOSFETs. Is this an incorrect assumption?

Thanks for the link to the IXYS application note, I will have to look that over.

 

[Futterama]

Some pictures of the RC controllers I have. I got these from friends, I haven't been using them myself.

The first one is a Castle Creations Mamba XL2. It is not the current version according to my friend from who I got this, since these will fry, I got 2 of these.
The brain board attaches to the power board using some kind of connector, the boards are very easily seperated.
Look at the heatsink, few fins and only 59g. (2.08 ounces) of aluminium. It was fitted with a 40mm fan and had contact to the PCB using thermal adhesive, like heat conducting (I hope) double sided tape.
The MOSFETs are 48pcs Infinion BSC019N04NSG.
The MOSFET drivers are 3pcs International Rectifier IRS21867S.

Link: http://www.castlecreations.com/products/mamba_xl2.html


View attachment 8





The other one is a SkyRC TORO EX 200A ESC.
I got this from another friend. I was there when it malfunctioned. He was running it on 8S LiPo using a SkyRC motor. It started smoking and he didn't even run it very long, just a few seconds or so. The brain board is still alive, but the power board is fried. On of the laid down electrolytic capacitors have a melted pin and the MOSFETs are cracked and there is bits of melted solder around the board. The contruction looks alot like the Mamba, same connector between boards, same kind of heatsink ect. It was mounted with two 40mm fans and the heatsink is a bit larger, 76g. (2.68 ounces) of aluminium.
The MOSFETs are 60pcs NXP PSMN2R6-40YS.
The MOSFET drivers are 3pcs Intersil ISL6700.

Link: http://www.skyrc.com/index.php?route=product/product&path=18_36_84&product_id=161

View attachment 3
View attachment 2

 

[rafeh1]

Honk, if I can use a ferrite bead rated for 200mA, it will have a DC resistance of 1Ω. Would this allow me to use the ferrite bead internal resistance as the gate resistor? It would also have a higher impedance at 100MHz which I guess would remove even more of the oscillations.

Bigmoose, the problem is I cannot demonstrate high frequency issues without a better scope, and I just don't have the cash for a better scope right now, thats why I recently got the 12MHz I have now. Since the price of the bead is something like $1 for 50pcs, I would just add them as a precaution.

Futterama
I have 1 ghz digital scope sitting around from my consulting days. where are you located. Im in socal let me know if u r close u can borrow mine.

 

[Futterama]

I'm from Denmark, northern Europe 8)

 

[Honk]

And I'm from Sweden, county Skåne.
Even further north of Europe but pretty close to Denmark..... 8) 8)

 

[Futterama]

Hello Sweden!

 

[Futterama]

Ok, I'm back on this project after a few days with a cold and watching old Star Trek movies.

To keep the gate loop short, I would have put the gate driver directly below the MOSFET near the gate pin. But the gate drive circuit would be 13mm long and this would create a bigger distance between the busbars and make the "PCB trace reinforcements" longer (with higher resistive losses), make the overall footprint larger and also make the distance between VDD and GND larger, resulting in longer traces for the capacitors (ceramic and electrolytic) that goes between VDD and GND.

So I came up with another idea. I made this quick illustration of a cross section of the PCB and busbars for the new idea. The gate drive PCB would be at an 90 degree angle to the MOSFET PCB. The gate loop would only be something like 1-2mm longer this way, with only the bend on the copper wire adding to the distance.

What do you think about that?
Do I still need to add some shield/ground planes to cancel the magnetic field from the high current paths, if yes, then where?

 

[Honk]

Hmmm, it's kind of difficult to determine exactly how it's designed by the picture.
Myself, I wouldn't worry to much about a few mm here or there in the gate driver circuit.
Easy access and proper VCC-VDD decoupling by at least 1uF ceramic of each gate driver is my recommendation.

 

[Futterama]

I finished the high side gate drive board layout yesterday, so I can print it on paper and show in 3D how it is designed. I can also post the schematic and board layout from Eagle.

Honk, what would you decouple with 1µF ceramic caps? From VBAT (42V) to GND? From gate driver IC VDD (15V) to GND?

I think I also saw some capacitors on the phase outputs in a circuit once. Any comments on that part?

 

[Honk]

I would decouple gate driver IC VDD (15V) to GND!!! Always does that. If not instability may occur.
This is important as the gate driver consumes a short puls of high current when driving the gate.
The cap shall sit as close as possible to the gate driver IC pins. If placed further away then use fat tracks.

It is also good to decouple the main "three phase mosfets" using good heavy duty ceramics.
Size 1210: http://www.digikey.com/product-detail/en/UMK325BJ106MM-T/587-2225-1-ND/2002923
Size 2220: http://www.digikey.com/product-detail/en/C2220X106K5RACTU/399-5531-1-ND/2002744

 

[Futterama]

Oh yes, the high side gate drive IC and helper MOSFET needs to charge the bootstrap capacitor which will probably be 4.7µF. And the low side gate drive IC will of course also need a big capacitor close by. I have placed these capacitors right next to the IC, you'll see later when I post my board layout.

 

[HighHopes]

you should use helper transistors not mosets (when needing a boost). if you use helper transistors then the large decoupling capacitors go across the power rails of the transistors not the gate drive IC. the gate drive IC can also have decoupling caps but very small 1uF and 0.1uF in parallel is enough. this description applies to booster transistor topology only. the booster transistors need to be close to the power mosfet to minimize loop area.

the decoupling cap on the boost transistor (or gate drive IC when no boost transistors in use) should be a calculated value. when the power mosfet receives its initial peak current pulse, the boost transistor voltage can not dip by more than 5%. C = i*dv/dt , now you can calculate your decoupling "C" for a known gate resistor and power mosfet, dV is whatever 5% of your rail voltage is probably 0.05*15V, dt is the time it takes for mosfet to reach platu voltage . there is a bit more to it than that, but we start to leave casual discussion and enter detail design.

agreed about using ceramic caps. most definately not electrolytic.

 

[Futterama]

The helper MOSFET I mentioned is only there to charge the bootstrap capacitor for the high side MOSFET since I will be using a seperate low side driver IC and then the high side driver will be missing the low side MOSFET to charge the bootstrap capacitor. Nothing boost here, it is the gate driver IC that drives the gates.

Don't mind the missing traces for power on the driver board, it is not 100% complete yet.

 

[rafeh1]

use arduino as controller.
then use arduino bluetooth to stream live data to ur cell phone. nano Arduinos r avail for under 10

http://www.ebay.com/itm/Brand-New-Tosduino-Nano-Board-100-Arduino-compatible-/321155530084