Regards,
Dan
The Tab Up variant puts the tab (metal backside) of the package up, if is placed on the top of the PCB. In your picture, the “Tab up” version is used, combined with putting the footprint on the bottom of the PCB.
It’s easier to see with TO220, which is assymetrical and the tab is longer, and it’s 3D model is included in KiCad. Left is the TO0247-3-Horizontal_TabUp and right is the TO220-3-Horzintal_TabUp.
If I wanted to duplicate the MOSFET installation as seen in the picture I included I would use to ‘Tab Down’?
Regards,
Dan
And a bit of *&^%$#@! because this forum software has a silly character idiocy.
In the picture I provided the metal back of the MOSFET is facing the heatsink and insulated from touching the heatsink with a Keratherm (pink) insulator. This is the method I want to duplicate.
Regards,
Dan
If you installed the FET on the top of the board (like the other components in the photo) it would be horizontal, metal tab down and leads bent down.
Because you are installing from the underside of the board, it is still horizontal, tab down, but you bend the leads in the opposite direction (point the leads up).
???
The “Tab Down” footprint has the tab facing the PCB, and is therefore not suitable for mounting on an external heatsink.
No, you still use the “Tab Up” footprint, but you flip the footprint itself to the back side of the PCB.
This is quite clear and logic to me. I really don’t understand how this can lead to confusion.
And as I already mentioned, it is also easy to put some TO220 footprints on a PCB, and then view it in the 3D viewer. The TO220 footprint is handy because it’s 3D model is part of KiCad.
Tab up footprint mounted on the underside of the board = tab down footprint mounted on the underside with the leads bent upwards.
I was trying to show an alternative way of observing the mounting as the OP still seemed unconvinced and confused, unlike either you or I 
EDIT: The other joy of designing the PCB with the tab down image (which is also the way the horizontal footprint is drawn), BUT reversing the bend of the leads so they point upwards then mounting underneath means the pads do not need to be reversed in the PCB design.
Thanks for your patience JMK!
Hi @Tour50, you are using the wrong footprint.
If you use the “tab up” footprint, then solder it on the underside of the board ( like your first photo) pad 1 will need to be on the RHS and pin 3 on the LHS.
If you use the “tab down” footprint (as if you were soldering to the top of the board) pad 1 will be on the RHS and pad 3 on the LHS which is what you need for assembly as your original photo. You will be assembling with the tab down against the heatsink with the leads turned up into the PCB from the bottom.
Paul is also right, to add to your confusion. The problem with using the the “tab up” footprint is when you mount the FET from underneath. You need to REVERSE the pins, so, instead of creating a special footprint with reversed pins for your tab up footprint, use the tab down footprint which has the pads reversed already.
Do you understand the problem now, or are you completely lost? 
Another way of looking at the problem:
First: Tab up means heatsink side up. Tab down is heatsink side down.
Now, the screenshot of your PCB is the view “looking down on the board” from above. You wish to attach your FET underneath, so, flip the board to get the underside view by View > Flip Board View.
Now place your “Tab up” FET in its correct position.
Next, flip the board back to the top down view and you will see pin 1 is on the RHS.
So either place the “Tab up” Fet on the flipped (underside) of the board or place the “Tab down” FET on the top side of the board… exactly the same result, but opposite to what you have posted for your PCB.
I really dislike this option. It’s against standards. If the Fet is on the back of the pcb. Then also put the footprint is on the back. Abusing a footprint just because the pins accidentally line up is bad practice.
With the “Tab Up” footprint, the Fet is on the same side as the footprint itself, and it’s just 100% standard and as intended. It does put the silkscreen text also on the back, but you have to insert the footprint from the back anyway so that is a good thing. Silkscreen text is also easy to modify if you wish so.
Whatever method you choose, make sure to triple check the pinout before you start ordering the PCB’s.
Kicad shows the pad for pin 1 as rectangular.
Pin 1 of an IRF 270 is the Gate.
The heatsink for an IRF 270 needs to be attached to the bottom (tab side) of the case (green arrow).
There is still a problem with your footprint selection or placement.
From what I can see, there also seems to be a problem with your circuit design or schematic or PCB.
The Source and Gate are not generally connected together with a large wattage resistor then disappear off board as a single path.
I was unable to see where the gate should be on the PCB, but when you do things like this there is indeed an opportunity to connect the mosfet pins mirrored, and then your circuit won’t work.
You are correct about the MOSFETs wiring. But in this particular case it’s being used as a CCS
(constant current source) and it is correct. It will be generating a lot of heat so I have to connect it
to a heatsink and then to a board on the same heatsink which will be supported by nylon standoffs.
Regards,
Dan
Thanks for the schematic, this makes life easy
The footprint is still incorrect.
Your FET needs to be attached to the heatsink. It is located UNDER the PCB, so the leads need to be bent UPWARDS (see the TO 247 drawing I posted).
Your PCB layout shows the Source will be soldered to the rectangular pin, which in turn goes directly to the + side of the capacitor and the pin named Drain on J4. This is NOT what you want according to your schematic.
You want the Source attached to the 1Ω resistor only, and the Gate connected to the Drain pin of J4.
