How to route and solder TO-263AB packages?

Question

Am working on making a PCB and i was using RFP30N06LE MOSFET on my breadboard circuit, now that am making a PCB i want to use the other variation RF1S30N06LESM of the same component. which as you can see the datasheet does not say much on the pads, spacing, etc.

This is my first time working on such packaging so please excuse my lack of knowledge. my questions are:

1. Does TO-263AB packages have a fixed standard sizes, pads, etc.? I checked out other datasheets for other components and it seems that TO-263AB packages have standard measurements.
2. The drain pad in TO-263AB packages is quite a large pad, when routing it do i need to make a large trace for it?
3. Is there any special "configurations" or things i need to put in mind while working with TO-263AB packages?

Thank you and again i have never worked with TO-263AB packages and i cant seem to find much information on working with it.

Answer 1

1. Yes the sizes are standard. Any major manufacturer will use JEDEC standard dimensions. There can be minor variations within the limits from manufacturer to manufacturer because their tooling will vary.

2. Aside from making the traces leading away from all the pads heavy enough (width and thickness) for the current, the most important thing is to ensure you have low enough thermal resistance for your application. Most of the heat dissipated by the part needs to be conducted out from the tab. This is not a simple calculation- it depends a lot on the type of PCB, whether you incorporate thermal vias under the tab and so on. This TI application note has a lot of information- far too much for an answer here. Keep in mind that datasheet \$R_{θJA}\$ numbers are based on assumptions for the PCB pattern and construction that may not match what you come up with. Usually they're in some other document than the datasheet, if you can find them at all.

3. The solder paste stencil "hole" for the tab is so large that it requires a grid pattern of support but the stencil manufacturer should do that for you automatically even if you just create a rectangle of paste.
4. As far as the exact pattern, IPC has guidelines as to the pad dimensions but the full standards are not free. If you find a suggested PCB pattern on a datasheet that fits, it's probably good enough. Some EDA packages such as Altium will help you create a new IPC-compliant pattern based on the exact package dimensions and tolerances.

Below is a rough guide for coupling to the PCB (only, not to the ambient), from this app note. Note that it's assuming 2oz copper.

Answer 2

1: yes also known as D²Pak, DDPak and TO263-3

2: the pad needs to be large to stick the part down, the trace only needs to be enough to carry the current you need, you can also place extra copper to act as a heatsink.

3: all I can think of is don't place any tall parts where the stub of centre lead would hit them.

Answer 3

The TO-263AB is a standard package.

Diodes Incorporated provides a datasheet with the dimensions you need to make a footprint.

Other companies might provide footprint data as well.

Here's what Diodes Incorporated recommends:

The drain tab is big because that't where the transistor has to get rid of heat. If you are going to use it to switch high currents, you'll want to extend the drain pad to a large copper area. The given dimensions are what you need to solder to. You can make the drain pad larger to radiate heat away, but make sure to leave the recommended pad area free to solder too.

I can't help you in figuring out how much area you need to keep the transistor from overheating. I don't know enough about it, and you haven't mentioned how much current it will have to pass.