KiCad - TO-220-5 package

TO-220-5 package

Printed From: PCB Libraries Forum
Category: Libraries
Forum Name: KiCad
Forum Description:
URL: https://www.PCBLibraries.com/forum/forum_posts.asp?TID=2432
Printed Date: 25 Nov 2024 at 3:23am

Topic: TO-220-5 package

Posted By: LarryJoy
Subject: TO-220-5 package
Date 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

Replies:

Posted By: tgrodnicki
Date 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.

Posted By: LarryJoy
Date 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

Posted By: tgrodnicki
Date 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.