PCB Libraries Forum Homepage
Forum Home Forum Home > Libraries > Footprints / Land Patterns > KiCad
  New Posts New Posts RSS Feed - TO-220-5 package
  FAQ FAQ  Forum Search   Events   Register Register  Login Login

TO-220-5 package

 Post Reply Post Reply
Author
Message
LarryJoy View Drop Down
Active User
Active User


Joined: 08 Jul 2018
Status: Offline
Points: 25
Post Options Post Options   Thanks (0) Thanks(0)   Quote LarryJoy Quote  Post ReplyReply Direct Link To This Post 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
Back to Top
tgrodnicki View Drop Down
Active User
Active User


Joined: 30 Sep 2014
Status: Offline
Points: 41
Post Options Post Options   Thanks (1) Thanks(1)   Quote tgrodnicki Quote  Post ReplyReply Direct Link To This Post 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.

Back to Top
LarryJoy View Drop Down
Active User
Active User


Joined: 08 Jul 2018
Status: Offline
Points: 25
Post Options Post Options   Thanks (0) Thanks(0)   Quote LarryJoy Quote  Post ReplyReply Direct Link To This Post 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
Back to Top
tgrodnicki View Drop Down
Active User
Active User


Joined: 30 Sep 2014
Status: Offline
Points: 41
Post Options Post Options   Thanks (0) Thanks(0)   Quote tgrodnicki Quote  Post ReplyReply Direct Link To This Post 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.

Back to Top
 Post Reply Post Reply

Forum Jump Forum Permissions View Drop Down



This page was generated in 0.125 seconds.