TO-220-5 package

Message Topic Search Topic Options Post Reply Create New Topic Printable Version Translate Topic

   I am trying to make a land pattern/footprint for a Micrel (now Microchip) MIC29152WT LDO adjustable voltage regulator in a TO-220 5 in line leaded package using 2019.01 version of Library Expert Pro. At first I tried the horizontal mount configuration because I want to bend the leads and use the copper on the PCB as a heat sink. All five pads overlap and thus all five leads are shorted together. Also the body outline just doesn't seem right. I tried the vertical mount configuration and the pads for the leads all overlap.

This is Mouser P/N 998-MIC29152WT and Mouser is now using SamacSys for all their symbols, footprints, and 3D renditions. No need to enter package dimensions as the information is on a part by part basis and if SamacSys doesn't have the information already, submit the part number to them and they will develop the information and get back to you in 24 h or less, mostly less. And all of this is at no charge (as in "free").
--Regards, Larry

Author	Message Topic Search Topic Options Post Reply Create New Topic Printable Version Translate Topic
LarryJoy Members Profile Send Private Message Find Members Posts Add to Buddy List Active User Joined: 08 Jul 2018 Status: Offline Points: 31	Post Options Post Reply Quote LarryJoy Report Post Thanks(0) Quote Reply Topic: TO-220-5 package Posted: 24 Jan 2019 at 10:25am
	I am trying to make a land pattern/footprint for a Micrel (now Microchip) MIC29152WT LDO adjustable voltage regulator in a TO-220 5 in line leaded package using 2019.01 version of Library Expert Pro. At first I tried the horizontal mount configuration because I want to bend the leads and use the copper on the PCB as a heat sink. All five pads overlap and thus all five leads are shorted together. Also the body outline just doesn't seem right. I tried the vertical mount configuration and the pads for the leads all overlap. This is Mouser P/N 998-MIC29152WT and Mouser is now using SamacSys for all their symbols, footprints, and 3D renditions. No need to enter package dimensions as the information is on a part by part basis and if SamacSys doesn't have the information already, submit the part number to them and they will develop the information and get back to you in 24 h or less, mostly less. And all of this is at no charge (as in "free"). --Regards, Larry



tgrodnicki Members Profile Send Private Message Find Members Posts Add to Buddy List Advanced User Joined: 30 Sep 2014 Status: Offline Points: 104	Post Options Post Reply Quote tgrodnicki Report Post Thanks(1) Quote Reply Posted: 27 Jan 2019 at 11:40pm
	I suppose you created footprint with all pads in line. With 0.067” pitch and 0.0325” x 0.017” pins this leads to overlapping pads. You should enter appropriate “D” and “D1” dimensions, to place pads in staggered mode.

LarryJoy Members Profile Send Private Message Find Members Posts Add to Buddy List Active User Joined: 08 Jul 2018 Status: Offline Points: 31	Post Options Post Reply Quote LarryJoy Report Post Thanks(0) Quote Reply Posted: 01 Feb 2019 at 1:15pm
	tgrodnicki, Thanks for your reply. Yes, the SamacSys people came up with the same solution of staggered pins. However, when I looked up the footprints that KiCad has for a generic TO-220-5 package they kept the terminals/pins in a single row and used oval pads with flat sides. Thus the pads are probably smaller than what the IPC standards suggest but leaves the terminals untouched as far as having to bend them. I will have to study the dimensions and go from there. --Larry

tgrodnicki Members Profile Send Private Message Find Members Posts Add to Buddy List Advanced User Joined: 30 Sep 2014 Status: Offline Points: 104	Post Options Post Reply Quote tgrodnicki Report Post Thanks(0) Quote Reply Posted: 02 Feb 2019 at 3:39pm
	KiCad generic footprint "TO-220-5_Vertical" has pads with 1.1 mm hole. MIC29152WT has 0.040"x0.22" (max) leads. PCB Library Expert suggest for such dimensions hole size of 0.052" (1.32 mm). To satisfy manufacturer's minimum annular ring of about 0.004" the pad should have 0.060" (1.524mm) lesser dimension. This leaves only 7 mils (~0.18 mm) clearance between pads - a small value if the regulator input voltage is in range of 50 volts.