EEVblog Electronics Community Forum
Electronics => Projects, Designs, and Technical Stuff => Topic started by: satyamfifa on January 29, 2018, 01:30:32 pm
-
Hey All,
I am trying to design a BLDC motor controller with 3 phase inverter, the controller in total must be able to handle 60 Ampere on continuous current, I don't want to use parallel MOSFET therefore I have decided to use only 6 MOSFETs (IPT007N06N) (HSOF package) each capable of handling continuous current on 300 Ampere and with RDSon of 750 microhms max. For the gate driver I have decided to use TI DRV8323S. My question is mainly regarding the design of PCB and trace routing as 60 A or even traces for 20 A are going to be quite wide, also connecting then to MOSFET was there MOSFETs have tiny footprint compared to the required trace width. Anything from suggestion to design tips will be quire helpful.
Regards,
Sparsh
-
It's fine for the traces to slim down to the size of the MOSFET at the last moment (i.e., 45 degree angles fanning out from the MOSFET). It's not like any reduction in a trace's width (within reason) is going to vaporise; the wider parts of the heatsink are going to provide heatsinking for the narrower parts.
You're going to be dissipating a few watts in that package, so you need to pay extra close attention to heatsinking the device.
You can opt for 2oz copper to let you get away with thinner traces, although:
- it's more expensive
- clearance restrictions go up so you can't use fine pitch components
- I'm guessing you can't halve the width of the traces because then you'd be dissipating the same power in a piece of copper with less surface area.
-
Usually this kind of layout is done using 90um or 120um copper (opposed to standard 35um). Check with your PCB supplier and EMS service for available options and design rules. Usually the minimum clearance increases with thickness of copper, and at some point you don't want to place small and fine pitch SMD packages there anymore. Running 60Amps or more through such a trace is common in power electronics. You should look up some copper thickness vs. trace width vs. maximum current / maximum temperature rise tables, I can't tell the numbers by heart.
-
Usually this kind of layout is done using 90um or 120um copper (opposed to standard 35um). Check with your PCB supplier and EMS service for available options and design rules. Usually the minimum clearance increases with thickness of copper, and at some point you don't want to place small and fine pitch SMD packages there anymore. Running 60Amps or more through such a trace is common in power electronics. You should look up some copper thickness vs. trace width vs. maximum current / maximum temperature rise tables, I can't tell the numbers by heart.
Seconding what these two have said.
Your clearances have to increase as your copper layers increase in thickness. One way to get around this is to put your control circuitry onto a secondary board and either mount it as a castelated PCB or using a set of sockets. You can also look at beefing your tracks up by using dual layer tracks with via stitching (and 0 ohm resistors to jump things) or by bonding copper wires onto the tracks post production (either through solder or spot welding. Wurth offered this at one point)
If your volumes end up high enough, there is a company in Germany that does special layer designs. They can do non-standard track thicknesses and weird layer arrangements. Unfortunately I've lost they details. :(
-
No paralleling? You better be switching that poor thing quite slowly...
With an incredibly low load impedance (fractional ohms), stray inductance becomes ever more critical.
Inductance arises from transmission line structures on the PCB -- typically with traces overlapping, and loaded with transistor capacitance, the characteristic impedance of these is in the 10s to low 100s ohms. Matching load impedance to characteristic impedance gives the best compromise between peak voltage and current during switching, for the least switching loss.
You must have dV/dt, or peak V clamp, snubbers on those transistors. Trouble is, with an impedance this low, you probably can't even get those physically close enough to do the job required.
Which leaves you with the last option, burning extra switching loss by slowing down the transistors.
At least the DRV8323 has adjustable slew rate, so that's cool. You must start at low supply voltage and low current, and increase the supply and load while monitoring peak drain voltage with a fast oscilloscope (>= 100MHz). If it starts to peak, reduce gate drive current setting.
To manage switching loss, the switching frequency must be kept low, probably under 10kHz. (Hope you like motor whine?..)
If you require better performance, then you require paralleled transistors, with individual snubbers (and probably external gate drivers -- or multiple DRV's if they can be ganged together).
Tim
-
Have a look at speed controllers for brushless motors used on RC models. 60A is not uncommon for a medium sized electric RC airplane.
-
Hey Tim,
Thank's a lot for your response.
I am certainly no expert in high current MOSFET design. From what I understand from your post is that there is stray inductance on the PCB, which will cause voltage spikes when the MOSFET tuns off causing the MOSFET to go into avalanche. I also understand that due to low impedance of MOSFETs the snubbers have to be physically close to MOSFET "for some reason that I don't understand", also that parallel MOSFETs are used to increase the capacitance to counteract the stray inductance, hope I am on the line so far. I don't think it's possible to drive parallel MOSFETs with DRV8323 or gang them together.
Here are some possible solution that I have so far:
1. Design the PCB in a way to add capacitance between traces, maybe used to a metal bar?
2. Use MOSFETs that can take high avalanche power, such as Infineon's StrongFET.
3. If nothing else works the slow switching speed, as you suggested.
Do you think any of these solution will work? If yes could you please point me towards the design resources?
Kind Regards,
Sparsh
-
The only thing you need to know about transmission lines here is this: an ideal transmission line is defined by its length and its impedance.
The LF equivalent is inductance and capacitance, and both are proportional to length.
The inductance of free space is 1.26 nH/mm. In a practical circuit, this will be lower (because of geometry factors: basically, the closer together two plates are, the more squeezed the magnetic field between them is, and therefore lower inductance). How much lower? If you know the characteristic impedance, it's simply the ratio to 377 ohms (the impedance of free space).
Likewise, the capacitance goes up by the same factor, but also by the dielectric constant.
You can usually ignore capacitance in a switching circuit, because the circuit is much lower impedance. You're worried about the energy stored in the stray inductance. Example: a very wide trace (say 2.5cm, on a 1.6mm board) is merely the low 10s of ohms. Good luck routing that between TO-220 parts! Yet the circuit might be 1 ohm or less (e.g., 24V and >24A).
So, keep things short. It's not enough to make things "as short as possible", because that ignores the length scale inherent in the circuit. It's also easy to fool yourself thinking that's always the right thing to do (which it isn't -- it's old advice). Indeed, it might be impossible to route a circuit with low enough strays, given some component placement. That doesn't mean the circuit itself is impossible, but it may need adjustment to behave.
A row of TO-220's spaced 2.5cm apart, connected with copper pours on top and bottom layers, will have about 17nH between transistors (10 of which is in the transistor body and leads, where you have no control over it beyond inserting it to full depth). 17nH gives a modest 10V overshoot at (10V) / (17nH) = dI/dt or ~600 A/us, which would get you 60A in 100ns. Going faster reduces your safety factor between supply voltage and transistor avalanche.
As for 1, 2 and 3:
1. This is two things. Metal bars are good -- wider facing area, and thinner gap, between two conductors, means less stray inductance.
It also increases capacitance, but not by enough to matter. Again, Zo isn't going to be /that/ low.
Don't go out of your way to add capacitance. Even if you load it down to the correct (sub-1 ohm) impedance, you still have the reactive energy to deal with, except now you have a whole lot of extra capacitive energy to deal with, too. The capacitance exchanges peak voltage for peak current, which changes when the switching loss is dissipated (turn-on rather than turn-off). There are some ways to deal with this, still (ZVS switching comes to mind), but that's not a general method (if you need regenerative braking, you won't have ZVS under all conditions). Anyway, you can't stack capacitance up the transistor legs and bond wires, so you're still left with strays.
2. Helps, but even with higher avalanche ratings I wouldn't trust a design that relies on avalanche on a repetitive basis.
Tim
-
Hey Tim,
Thank you very much for you response, you mentioned TO-220 package and I understand that it's a industry standard package and it doesn't has good characteristics for high current application, the MOSFETs I am considering have DirectFET large can or HSOF package do you the are better for the low impedance / high capacitance and routing????
Thanks in advance
Kind Regards,
Sparsh
-
Ah, that helps. No-lead SMTs can be in the few-nH range. If you can splurge for a multilayer board, even better!
Tim
-
I’ve wanted to try DirectFETs for a while. If you solder them down flat (I suggest you fork out for a paste stencil) you should be able to put a thermal pad and heat sink straight on top :-)
However, DirectFETs seem to be a single-source component. Infineon (who purchased IR a few years ago) is quite a reliable company, but occasionally experiences long lead times...
-
You'll be wanting to read this:
http://scolton.blogspot.co.uk/p/motor-controllers.html (http://scolton.blogspot.co.uk/p/motor-controllers.html)
-
60A at the power supply or at the motor phase? That's quite different.
Need to pay very special attention to the layout due to the already mentioned parasitic inductance. Use a "laminated" structure and short traces as much as possible. Some of the critical parts are the connection between bottom and top FETs, the inductance in the supply decoupling caps loop, the driver connection to the FETs. In general it is already "too much power" for snubbers to be used, never seen them at maybe 20A and above (they will also heat up); control the voltage spikes with a careful layout and adjusted switching time (here's a starting point for you if you're lost: 0.5 - 1us).
You can beef up traces with solder or solder with tick wires.
Don't believe the amps at the FETs datasheets, read it carefully; you'll not be able to keep the die at 25ºC :). And sometimes the value is for the die, the packages have lower limits.
-
Also the Rds goes up with temperature. I typically look at a MOSFET spec, then double the stated Rds and halve the ‘maximum’ current
-
The consensus solution in manufacturing for electric bikes , 1 horse power range , was to push the voltage up for BLDC motors. 60 amps at 12 volts is 15 amps at 60 volts. This is more power mosfet friendly in the area of 100 volts 20 amps 10 m ohm on. Those ones are cheaper and mass produced in case a given supplier dries up. I have seen them get away with 18 gauge wire for a 3 phase BLDC motor. Maybe snoop around some electric bike controllers and see if you like it.
-
...Anything from suggestion to design tips will be quire helpful.
this esc might be good design inspiration:
http://vedder.se/2014/01/a-custom-bldc-motor-controller/ (http://vedder.se/2014/01/a-custom-bldc-motor-controller/)
I think there are many more open designs out there for radio-controlled and robotics or cnc applications.
-
I have been looking at the Design of this Direct Drive ESC:
http://scolton.blogspot.nl/p/motor-controllers.html (http://scolton.blogspot.nl/p/motor-controllers.html)
I see that traces are no where more that 17 mm think on a single layer and the ESC is rated for 200 A, can someone please explain how is it possible, when any trace width calculator would suggest that it has to be at least much more that 80 mm |O
(http://4.bp.blogspot.com/-MlVb7lEA0Ws/TgFEVmNAqbI/AAAAAAAABDE/xAFoaxIoVVc/s1600/dd43.jpg)
(https://i.imgur.com/EBVjAZ7.png)
(https://i.imgur.com/yWa7cam.png)
(https://i.imgur.com/D8D319A.png)
-
Trace width calculations are only meaningful for long traces, L > 10*W say.
If the whole board is sandwiched between thermal pads and heat sinks, the current density can be an order of magnitude higher.
Tim
-
Hey Tim,
Thanks a lot, I suspected the same.
Kind regards,
Sparsh
-
The beginner mistake is to think that the trace width calculators are telling an universal truth, and then to make room for the "wide traces needed", you end up increasing distances to make those traces fit. This is a very fundamental mistake to make.
Instead, increase the integration level and miniatyrize everything. Then you don't even have something you could call "traces". You just have component pads connect to each other almost directly, using fills as wide as the pads. Both inductance and resistance is minimized. Now, if you insist on adding wide "traces" here, you can only join it to the component pad at the pad width, anyway. So, you are just adding some extra resistance by adding the "wide trace" - instead, just join the next component there directly!
If you look at some 1000A (continuous) capable IGBT modules, for example, you are surprised to see how freaking thin those bond wires are! According to any wire width table, those would be only good to maybe 50A max. The key is the short length - the absolute amount of power loss (heat generated) is small, and it is directly conducted to whatever that wire connects to; it doesn't need to rely to the (small) surface area of that wire to cool!
-
Yup.
Some tweaks to that:
- Wide pads, traces, pours, etc., around nearby pairs of pads, don't decrease the electrical resistance much. This is correct.
- However, thermal resistance is decreased, by spreading the heat out, into more board or convection area. So it can be a win, even if the resistance isn't being decreased substantially in the process. :)
- Bonus points for studding the connection with vias, to spread the heat more rapidly through the board layers (FR-4 is a terrible conductor thru-plane, but in-plane it's okay). Any heat you can distribute towards other metal layers is a big bonus.
It's difficult to estimate just how much heat can be carried on component leads. It depends on lead length, how much heat is coming from the connecting traces, how much dissipation the package can handle, case temperature...
On the upside, if you're using a thermal-pack construction (say, PCB sandwiched between heatsinks, with gooey Gap-Pad filling basically every crevice), you can get huge dissipation capacity from the PCB, traces, even pads and leads if they're exposed. Those DirectFETs are probably pretty good on this (solder-bump dies have good thermal conductivity through the silicon die to the back side heatsink), and a low profile build allows everything else (traces, chip resistors, capacitors and so on) to be cooled just as well.
Speaking of bondwires -- if you're looking at an ampacity calculation for bare wire, in still air, you'll get a considerably more conservative number. Bondwires floating in gorilla snot (or whatever the rubbery stuff is they fill IGBT modules with ;D ), or encapsulated in epoxy or potting, can dissipate much more heat!
Tim
-
What do you think so far a very basic design?? I am planning on soldering metal bars, and planning on getting a 70 micrometer copper board (end 90 micrometer), still have not thought about capacitors or snubbers
(https://i.imgur.com/kAMcl2t.png)
(https://i.imgur.com/YRWdjBq.png)
maybe I need to move those shunt resistors away from the can drain, I don't want them to short
-
The chosen MOSFET is very slow - I use this exact one but only for routing high-current DC, not switching.
I would imagine your switching frequency to be uselessly low or have dramatic switching losses. The fancy Rds(on) spec is only interesting if you can get the Vgs above a reasonable threshold the majority of the time. This MOSFET will spend a lot of time in its linear region and facing a giant pile of current.
-
I currently thinking on going with IRF7749L2TRPBF with turn on delay time on 17 ns and turn of delay time of 78 ns, is that slow?? Competitively I don't find it slow with similar MOSFETs
-
That device has a Qg (Gate Charge) of about 200nC which is useful in estimating how long it will take to fully turn on. That charge with a 2A gate driver will take about 100ns - which is no joke at the currents you are dealing with. The turn on delay (I believe) is the time it takes for the Vgs to reach Vgs(th) - the threshold where it begins to conduct. What is more important is how long it takes to fully charge and the resistance of the device approaches Rds(on)
My latest design is using Qg - 37nC and 5A drives to get a manageable switch loss at 250Khz - roughly 8ns to fully charge the gate at about 20A drain current. Switching losses can dominate the total losses with slow devices - so the faster the better up to the point where you get slapped with the challenges of high dv/dt and di/dt.
Parallel MOSFETs with independent drivers or at least very high current drivers is not a bad idea.
EDIT: It looks like your chosen gate driver can only do 1A which is small for a 200nC gate charge.
-
I've seen the use of solid copper rods soldered onto the pads in some SMPS designs that required higher current rails.
They looked like 2mm diameter copper rods and were soldered directly onto the copper traces, the entire length of the trace (which was straight).
-
Hey Thanks for your reply,
I according to my Gate-Driver datasheet calculation I should be able to drive a MOSFET with Qg = 333nC with IVCP of 15mA at 45kHz PWM switching frequency, does higher switching frequency offer any significant advantage?
The whole point of using DRV8323 is to able to do Field Oriented Control with less hassle, that is to make a board which is compatible to TI-InstaSPIN, unfortunately I have not seen a single example of a TI driver supporting instaspin with parallel MOSFETs, and best example I was was a 50 A E-bike with TI-InstaSPIN again with no parallel MOSFETs, currently I don't see reason why it may not be doable as long as stray inductance is kept under a certain limit.
-
Are you familiar with switching losses in power converters?
It is a big a thick topic - but for what you are doing, important.
-
Nope I don't, although at this moment I wish I did, I thought switching losses low rise and fall time can be compensated with lower PWM frequency
-
Switching losses happen during the transition from off-on and on-off. When the MOSFET is off - it dissipates no power. When it is on it generally dissipates very little power. During the time it takes to get from one state to the other is very lossy and a lot of power is dissipated - essentially this is when the MOSFET is behaving like a resistor.
The PWM frequency determines how many of these switching cycles you go through per unit of time - you simply multiply the losses from each switch cycle by the number of cycles to get the total loss. Therefore, lower frequency PWM will lower losses at the expense of needing larger inductors and capacitors. Once you slow the PWM down to the audible range - you will hear it squealing or whining and the inductors and capacitors will be really big.
In very general terms - the goal is to charge and discharge the gate as fast as possible. The rise time of the gate is determined by the gate charge the current available to fill it up. If your design is very low inductance - (meaning a really good PCB layout) - you can charge the gate very fast and minimize the resistive switching losses. If you have a considerable amount of parasitic inductance in the devices and PCB you will start to see overshoots and ringing that can cause other problems. It is common to put a resistor on the gate trace to have control over the charge time to compensate for the PCB.
I tend to design converters with the highest switching speed I can while hitting the other design targets - efficiency, size, etc... For high current, parallel FETs or interleaved converters deliver high-efficiency and high current while still being small.
-
https://www.eevblog.com/forum/projects/lost-trying-to-calculate-switching-time-of-power-mosfet/ (https://www.eevblog.com/forum/projects/lost-trying-to-calculate-switching-time-of-power-mosfet/)
-
Hey All,
Thanks for the replies, I think I have finally made up my mind about what I am going to do:
1) Use DirectFET MOSFET's to keep the stray inductance as low as possible as the main issue with no parallel MOSFET is that, and try not destroy MOSFETs by putting them through avalanche.
2) Go go for low Rds(on) MOSFET instead of fast switcihng MOSFET (which takes me right back to IRF7749/AUIRF7749), as swtiching characteristics are unpredicatble anyways, use a PWM frequecny of about 45kHz to minizime the switching losses and keep the MOSFET in conducation region.
3) High switching speed isn't desirable anyways again to avoid high avalanche peaks as suggested my Tim in his previous posts, therefor 1A source of DRV8323 should be enough.
4) Place large capacitors as close to MOSFETs as possible for the low PWM frequency. Again something I saw in Direct Drive ESC example.
5) Design PCB with shortest trace length, provide ample amount of area for heat dissipation.
6) Try to cover as much area of PCB with heatsink as possible, again as suggested by Tim.
7) I am gonna use double sided track both top and bottom (90 micrometer each) to dissipate heat and low stray inductance and resistance.
So who knows it might be a win. Please let me know what you all think.
Kind Regards,
Sparsh
-
I don't see a point going much over 16 - 18KHz (if you don't like to ear it) switching frequency, unless your motor's phase has some really low inductance. Higher switching frequency -> higher losses. Inductive switching dissipation can be estimated by FPWM * (Tsw(ON) + Tsw(OFF)) * Vds * Id * 0.5
-
I don't see a point going much over 16 - 18KHz (if you don't like to ear it) switching frequency, unless your motor's phase has some really low inductance. Higher switching frequency -> higher losses. Inductive switching dissipation can be estimated by FPWM * (Tsw(ON) + Tsw(OFF)) * Vds * Id * 0.5
The overall size of the solution is the dominant reason. Ripple current can also be drastically reduced with higher switching speed.
It is a giant pile of parameters that have to balance to best meet the needs of the final product. Size, cost, noise, transient performance, ripple currents, thermal budget, etc,etc.... Kind of like spinning a dozen plates while walking a tightrope.
-
How will the size of the solution be reduced with increased switching frequency?
-
The inductors and capacitors grow.
-
In a DC-DC converter yes, but a motor controller is a little different. The inductor has fixed size and is outside the board (the motor). The bulky capacitors can't be reduced that directly, because the power wiring doesn't change, and there's the risk of resonance. On the other hand, higher dissipation -> bulkier heatsinking.
I would say use the lowest switching frequency possible that keeps your motor current ripple at an acceptable level.
-
In a DC-DC converter yes, but a motor controller is a little different. The inductor has fixed size and is outside the board (the motor). The bulky capacitors can't be reduced that directly, because the power wiring doesn't change, and there's the risk of resonance. On the other hand, higher dissipation -> bulkier heatsinking.
I would say use the lowest switching frequency possible that keeps your motor current ripple at an acceptable level.
You are right - I totally forgot this project is a motor drive. :-//
-
Assuming you have short and/or shielded cables leading to the motor, of course -- otherwise with EMI filtering, it basically constitutes a rather powerful class D audio amplifier, and you might as well push up the frequency!
Tim
-
For motor control, you'll be running your d/q axis current control function locked into the fundamental PWM loop. Because you'll want to change the phase voltage modulation at every opportunity. If you run too fast, you won't be able to fit your control code into the time available and hence you now will have several PWM cycles with the same modulation, which defeats a lot of the purpose of running faster!
For pretty much all practical motors, using centre aligned pwm, with it's intrinsic frequency doubling, means that the ripple currents will already be very small at most sensible fundamental pwm frequencies (8 to 20 khz). Of course, if you are driving some sort of ultra-trick, ultra low inductance high speed eMachine then sure, start ramping the frequencies up.
And of course, honorable mention here to EMC compliance? IS it required, to what level? The faster you switch, the bigger head-ache it becomes. Or if you switch slowly, then your deadtime becomes a larger proportion of your modulation index.