I am currently working on a board design where I have placed the Mosfet gate resistor inside it’s courtyard. Apart from the DRC error it shows, which I believe I can ignore, I would really like to know if I will be facing any issue wrt SMT assembly service for the PCB. The package of the Mosfet & resistor are DPAK and 0603 respectively.
Will this cause any problem for the pick & place device or during reflow soldering ? The PCB copper thickness will most likely be kept at 2oz.
Any suggestion or advice will highly be appreciated. Please let me know if any other details are required.
The PnP machine would have to place the resistor first and then risk knocking it aside when placing the mosfet.
Reflow of the resistor then gets dodgy as the mosfet blocks the IR heating
It might be possible, but discuss with the assembler first.
Rework gets very challenging
I would shy away from such a design unless it’s absolutely necessary. While it looks “neat” in the screenshot you posted, it is at least in this case absolutely not necessary.
Now the question is… what are you building? I few hobby boards or a full production board for a commercial product.
In a commercial setting, had a designer working for me proposed this I would say “no”. Go fix it.
IMHO
My thoughts would be mfg and in circuit board testing issues, soldering method limitations or requirements. Perhaps it can be done by some assembly houses but not others.
Or stated another way… if the designer wishes to deviate from know production process they better have a D…N good reason.
Board testing issues
That resistor is the gate resistor for your Mosfet. Its value can vary widely and the board will still function. However if it is too low the EMC signature may be pushed out of specification. If too high, added thermal load and possibly delaying turn-off where in a bridge can generate very high fault currents.
Thanks everyone for the wonderful insights that you guys have provided. I think the most logical step now would be to place the gate resistor somewhere else. This board is meant for mass production, thus ill have to be a little more careful w.r.t component placement.
One of my company’s customers tends to lay out their boards such that the smaller passive parts (like the gate resistors here) wind up on the bottom of the board.
If the OP is open to doing a double-sided board, then it would be a trivial matter to flip the gate resistors to the back side.
Hi Meterman2026,
I agree with your point of placing the gate resistor on the Bottom layer, however there will be a heatsink over there which is going to cover the entire board. I am not really sure how effective it’s going to be, but it’s a requirement.
Won’t you have issues with the via’s in that area then?
You appear to be pushing components very close to the board edge (that 2512 to the left). You should have more than enough room to place the gate resistor at the board edge
Hi Naib,
I agree that I can place the resistor on the bottom edge, however there’s a copper track/pour which is connecting one of the pads of the 2512 shunt to the source of the mosfet. The gate resistor’s would break this pour.
Placing this pour on the bottom side distorts the current return path, which I would like to avoid.
Yes the Via’s will be Tented, which will provide some kind of insulation between the copper and heatsink. Also the heatsink will be having some kind of sticky silicon rubber type of thermally conductive material.
I didn’t want to make assumption about the TIM they plan to use. To give you an idea I now only use Graphite sheet (far superior) but this is electrically conductive.
The silicon pads that the OP now mentions they will use will be electrically insulative so they are good ( I wouldn’t dare go near them )
)