[danny71]

H500,

Thanks very much for the link. I will study it.

Dan

[yngndrw]

Can I have some feedback on this PCB design for the power section please ? (Attached)

It is a 2 layer PTH design - I tried to follow Mariss's design guidelines as much as possible.

I had to turn off thermal isolation on the MOSFET pads because the odd power plane shapes meant they were only connected by tiny traces.

PS: Shown on a 0.05" grid.

[H500]

It looks OK on first glance, but I don't consider myself an expert on laying out power electronics. The best thing is to try it and then we can compare results.
My board is quiet, but not completely silent. There's a soft hiss when the phase angle is at zero.

I'm using a single 3w chip resistor for each phase.

[yngndrw]

VPH asked me to upload the design files for the H-Bridge:
http://yngndrw.hostilezone.net/uploa...%20yngndrw.zip

Please note that it has not yet been tested.

The MOSFET section could possibly be made slightly smaller as it is and made even smaller with the use of some SMT components.

[Mariss Freimanis]

yngndrw,

Nice board layout. My purpose in life is to design and criticize (my own work as well) so I hope you take my comments in the helpful way they are intended:

A) Circuitry:

1) You should use a 33 to 100 Ohm resistor in series with your 1N4148 diodes to limit the boot-strap capacitor charge currents. Presently they are unlimited; a 100 Ohm resistor will keep the charging current pulse to a reasonable value (<100mA).

A single resistor in series with both diode anodes is fine for each H-bridge.

2) A little-known IR app-note addresses a potential start-up problem with the IR2104 half-bridge drivers. It says each MOSFET half-bridge output must be a zero volts on power-up or the IR2104 may destruct.

Place a 100K 1/4W resistor from each MOSFET output to GND. 4 resistors will be needed and they eliminate this potential catastrophe.

3) 0.1uF boot-strap capacitors are a little too small. What if you use a high-inductance motor and a low power supply voltage? The bridge output could conceivably have to be on for several milliseconds before switching and recharging the capacitors.

Figure on using 4.7uF / 16V ceramic multilayer capacitors.

4) Your current sense resistors look like they are the wire-wound type. That makes them inductive and any inductance in the MOSET source to ground path is potentially destructive.

Think about replacing them with non-inductive resistors and see if you can get 0.05 / 3W Ohm resistors instead of paralleled 0.1 Ohm as you now have.

5) IR2104 inputs. The IR2104 is a CMOS device. If it is intended to be unplugged from whatever drives its inputs, safety the inputs (including SD) with 4.7K resistors from input to GND.

6) Parallel your 100uF / 63V electrolytic with a 1uF / 100V multilayer ceramic capacitor (MLCC). Electrolytic capacitor impedance increases above a few hundred kHz to render the electrolytic cap is ineffective for bypass. The 1uF / 100V MLCC takes over bypass duties at the higher frequencies.

B) Board layout:

1) Learn to hate the color of FR4 green. It is the color of the printed circuit board where copper has been etched away. Always ask yourself "Wouldn't this circuit work better if the empty spaces were filled with copper?" The answer is usually "Yes, it would".

For instance, look at the red layer in the region where the 4 0.1 Ohm resistor GND leads are. Wouldn't the circuit work better if red layer copper connected them too as on the blue layer? How about the 'hot' end of those same resistors. Why etch away copper to leave that 'Y' looking like pattern? Make all of it a big island of copper.

Have your current sense voltage pick-off trace run up to the top of the hot side of your current sense resistor for a good Kelvin connection. Your GND side Kelvin connection is OK as it stands.

Mariss

[yngndrw]

Hi Mariss,

This kind of feedback is exactly what I was looking for, although I have a few questions about some of the points. I was having some issues with sourcing some of the components hence the 0.1Ohm 3W W/W resistors, but I will have another look at what I can get. (Will probably replace the current sense resistors with SMT resistors as the SMT versions should still be plenty big enough to hand solder easily.)

A1) R1 and R4 (33 Ohm) are already in series with the 1N4148 diodes - Are you suggesting that they should be 100 Ohm instead or have I placed them incorrectly ?

A6) There is already a 1uF capacitor (C5) in parallel with the electrolytic but I didn't pay much attention to the type - I will be sure to get the right type when I write a BOM. Is the distance of the red trace between these (The negative trace.) acceptable for this ?

B1) My concern here was to make the distance between the pads (And hence the resistance) approximately the same, so that the parallel resistors would see the same current. With this in mind, is it still better to just flood the whole area ? I will try and switch to SMT current-sense resistors anyway which should make the whole section much ore compact anyway. (If I have to use parallel SMT resistors, should I have them side-by-side or stack them ?)

Thanks for the feedback, it's very helpful.

[yngndrw]

New version:

http://yngndrw.hostilezone.net/uploa...%20yngndrw.zip

Bill Of Materials: (Farnell didn't have 4.7uF 16V ceramic capacitors, so to save the cost of getting 50V ones, I added an eBay link for one of the items)
https://docs.google.com/spreadsheet/...lE&output=html

The MOSFETs are to be mounted on the bottom, which is why the large capacitor goes over where they are.

I couldn't find 0.05Ohm 3W resistors, so it's still using 2x 0.1Ohm resistors - They are SMD resistors though.

The resistor parts are single-sided due to them being SMD components and the tracks needing to run under there to the MOSFETs.

I've added lots of extra copper in other parts and made all of the other changes Mariss suggested.

[lucas]

A few more comments if I may (from own experience):

- the 100µ Elco is a standard 85° one, you will need a low ESR type or it will get hot (and die prematurely) from the high switching currents from the mosfets.

- There are no decoupling cap's or elco on the +12V as far a I can see? The IR driver chips are switching a substantial current to drive the mosfets gates, I used one elco and 4 100nF's on each IR chip.

- For how much current/phase did you design the PCB? I don't think you need 3W sense resistors. I used a 500mW 0.05ohm for 4A per phase.
If that 4Amp was continous: P= (4*0.05)*4= 800mW but it's pulsed and the 500mW is sufficient for 4A. Farnell partnumber: 110-7371, 1W version: 110-7401.

One question I am still struggling with: which parts should be considered as "power" and thus be connected to the power ground and where does the signal ground starts. I opted to include the IR2104's in the power section, you connect them to signal ground.
I really don't know wich is best but my gutt feeling tell's me that a pulsed 100mA @ 12V signal is more power than signal. What do the expert's think? Anyone?

Last but not least: Nice design, I tried a similar one, seperate power pcb with the Fet's on the bottom but didn't like the loss in PCB real estate and also the conflict between power and signal mentioned above, you now have the current sense signals routed to another PCB, these are very low level (a few millivolts in microstepping) and as I wouldn't risk problems here I abandoned the dual PCB design.
But it has it's advantages, I still think that a good AVR can do the job also and be more flexible to add option's.

Hope this helps,
Luc.

[yngndrw]

Thanks for the feedback.

I will change the capacitors as you mentioned shortly. I'll also switch to 1W resistors as there was a 0.5Ohm version in that size. I wanted physically larger resistors for the soldering size as well as the rating.

I didn't really have a specific current figure I designed it for, so I was just going to see what it could handle when I make one.

I might also use a radial capacitor for the main one to save on the length of the board a bit.

I was designing it to fall within these sizes: (The smallest being the cheapest)
5cm x 5cm
5cm x 10cm
10cm x 10cm

I managed to shrink the power section from my last design, but I then added labels to the connectors so it ended up being within the 10cm x 10cm price band unfortunately.

Regarding the grounding, in this design you effectively have three ground planes:
1) Power, where the MOSFETs are
2) Driver, where the IR2104's are
3) Logic, on a separate PCB which is driving this one.

The main reason to have this entire board separate to the logic is so that it can be used for anything.


Edit: Then again thinking about the trace width I think it will be okay with 10A, in which case that is 5W @ 0.05Ohms, so the 6W of sense resistors is required. I'm not sure if it is wise to expect 10A capacity out of this board, though. (Will be 1oz copper.)

[H500]

yngndrw, you can solder wires to the pcb to increase the current capacity. But noise might become an issue if you approach 10 amps.

[lucas]

I didn't really have a specific current figure I designed it for, so I was just going to see what it could handle when I make one.

That"s just what I did, those chinese PCB's are real cheap and a burned one is no disaster if you can recuperate the components.
I now have a machine running reliably at 4Amp with 3 drives, the next one will need higher current and supply, so I will build one to suit what I need and test the hell of out it.

Regarding the grounding, in this design you effectively have three ground planes:
1) Power, where the MOSFETs are
2) Driver, where the IR2104's are
3) Logic, on a separate PCB which is driving this one.

Ok, this looks like a good solution, but:
I don't have Eagle and can't see where your logic ground goes, all seperate ground signals should be "star" connected to the Kelvin ground (as Mariss call's it), thus the logic ground may not pass via the driver ground.

Then again thinking about the trace width I think it will be okay with 10A, in which case that is 5W @ 0.05Ohms, so the 6W of sense resistors is required.

That calculated 5W is for a continous 10A current, but the current is pulsed. Let's assume a dutycycle of 50% (5Amp average), then the power drops to 1.25W..
My first protoype did also have big size resistors, but then I noticed the very small ones on a G540, I'm no expert and thus like a peek at how the pro's do it...
Made some measurements and calculations and so I used the 0.5W ones (still bigger than the 540 ones).
I would suggest: go ahead with what you feel comfortable with and when the whole thing works then measure, analyse, think... and adapt the design accordingly.

[yngndrw]

Thanks.

I've been looking at some of the components and noticed that some of the ones I've selected are US stock only which means an extra £16 on the order price - I'll change these when I change the capacitor.

I will also switch to 1W resistors as I think there was a 0.05Ohm version in Farnell, if I remember correctly.

As for the ground, the Kelvin connection is done at the negative 100uF capacitor pad - Essentially it is the blue trace which connects the large ground copper pour with a ground plane that covers the entire driver section. The red plane in the driver section is a 12V power plane.

Because of these planes, it should be very easy to add the decoupling capacitors you mentioned. I might even put them under the driver IC sockets to get them nice and close.

[Helmute2000]

Hi,

why not using in that case an IRF540Z? These components have a RDS(on) = 26.5mΩ. This would be avoid more unnecessary waste heat.

Also the Total Gate Charge is nearly 42nC. The IRF 540N has a Total Gate Charge fom 71nC.

Your layout would be better and better, but I#m wondering whay you are not using IR2104S your board could be shrinked substantially. Please be aware, that you need a power supply, from an input voltage about 20 ... 100V you need output voltage from 1,8V for the CPLD, 3,3V for IR2104S and optocouplers and last but not least 12V or 15V for the drivers.

My suggestion is that you plan a double board solution. The driver board with the power supply and the control board with optocouplers and other logic IC's. That would be a nice architecture and I'd like to build also some of these boards. Please consider also a current setting switching part. Also a possibility to select the micro steps 1/1, 1/ 1/2, 1 / 1/4, 1/ 1/5, 1/ 1/8 1/ 1/10 ...

Br,
Helmut

[yngndrw]

Helmut,

The reason for not picking the IRF540Z was cost. £30 is already quite high for a h-bridge.

I picked the 8pin DIP package for the driver so that everything (Apart from the current sense resistors) was through hole for easy soldering - It also allows for IC sockets as they are quite expensive ICs.

I was considering adding a 12V switching power supply to it, but didn't want to add 3.3V and 1.8V regulators due to wanting the design to be as generic as possible.

The idea was to have a H-Bridge which could be used for anything. (AVRs, FPGAs, CPLDs, etc) This is why it is just the H-Bridge section and not the control board with microstepping and current selection components. I personally planned to just breadboard the control side of it.

I've not yet had the time to implement the changes from lucas' feedback but will get the changes done soon.

[Helmute2000]

Hi,

thx for your reply. That is a great idea! I would start such the same project in the past but I didn't find time. I'm really intersted in your progress.

I saw hier in a German price list the following prices for
IRF 540 0,48€
IRF 540N 0,40€
IRF 540Z 0,38€

So I didn't understand your answer, could you proof this again? Is it possible for you to design the layout in that way that we could use only or maybe both SMD parts? If not I'll find the time to design that beside you, if you will accept this.

I'd like also the idea to build up a breadboard to analyse the results from this product. I heard here in a lot of threads that the noise level of the current measurements in the comparator is a big issue.

I'm missing the schematic file for your last design, could you please be so kind to send your eagle schematic too?

Thanks a lot!

Br,
Helmut

[yngndrw]

From Farnell, the 540N is £0.95: IRF540NPBF - INTERNATIONAL RECTIFIER - MOSFET, N, 100V, 33A, TO-220 | Farnell United Kingdom

The 540Z is £1.53: AUIRF540Z - INTERNATIONAL RECTIFIER - MOSFET,N CH,100V,36A,TO220AB | Farnell United Kingdom

These prices are excluding Tax.

I think I will find a new supplier for the parts. As I mentioned a couple of posts back, some of the parts have a "US Stock fee" as well so I already wanted to change a few parts.

Regarding doing an SMD version - As it depends on the parts that you can get locally, you're probably best just doing your own SMD version using a local German supplier. That way you can get parts which are more convenient, cheaper and can spec. it exactly how you want.

[Helmute2000]

If you take the IRF 540Z, you do not need more heat sink, then you can also use other types of construction and the components are soldered directly onto the board without a heat sink, it does not have to be equal to a H bridge with 100V and 10A. What do you think?

Perhaps it is completely without heat sink with d²Pak, or from a TO262?

The performance of the H Bridge would result then about 100V and 5A. That's not bad. When you design the bridge for maximum 50V, there are some very interesting vendors with a MOSFET RDSon of 0.009 ohms. That avoid the heatsink completely.

Would be a better future fit, all world is crying to cool technology.

I have in mind such a H Bridge, where there is no appreciable heat is observed. So to speak, a "Cool Runner H Bridge".

[Mariss Freimanis]

There's more to picking a candidate MOSFET than Rds ON, gate charge and price.

As a designer, one of my main MOSFET specifications is single-pulse energy tolerance and the device's SOA curve. The IRF540Z is clearly more fragile than the IRF540N.

The IRF540Z is rated at 120mJ. The IRF540N is rated at 700mJ.

The IRF540Z SOA curve shows 300mA @ 100V for 1ms. The IRF540N SOA curve shows 4A @ 100V for 1ms.

To me, the IRF540Z part will blow with far less provocation than the IRF540N part. This matters a lot if you are designing motor drives.

Mariss

[yngndrw]

Even with the higher Rds(on), I don't think that the heat generated would be an issue even with a simple / small heatsink - Looking at the G250 shows how little heatsinking is required thanks to using all N-channel MOSFETs.

I never would have expected a MOSFET with a lower Rds(on) to be more fragile and I wouldn't have ever thought to check that.

Thank you both.

[Helmute2000]

Hi Mariss,

that is a really good point. I never thougth that the MOSFETS are so different. What do you think, for my idea with a very cool drive when using a IRF 1405 (55V 5mOhm).

This Device has a SOA curve 20A @ 55V 1100mJ.

Do you expect with that devoce also problems, despite the low voltage from 55V?

Br,
Helmut