1
\$\begingroup\$

I am using IXYH16N170CV1 IGBT's mounted at the edge of a PCB. The legs will be long and bent back to reach the heatsink shown in the image.

This device is rated for 1700 V and 16 A. My nominal voltage will be about 600 VDC and 11 A with a max of 1400 V.

The pitch spacing between the pins is 5.45 mm and the distance from the edge of the pins is about 4 mm at the narrow part and 3 mm at the thicker bit closer to the body of the device.

The distance between the 2 copper pours on Q1 is 2.5 mm. According to the distance calculator (image below) for 1400 V this is not enough.

Can these devices be connected to PCBs at this pitch and voltage rating?

Also, is there any implications for having the legs very long? Are arcs more likely?

Thanks.

enter image description here

enter image description here

\$\endgroup\$
7
  • \$\begingroup\$ Classic issue! What CTI does your PCB have? Even if you space out the PCB pads like @Elmesito suggests, please be aware that the body of the transistor itself will be the weak spot due to CTI 400 and short distance from drain to source. \$\endgroup\$
    – winny
    Commented Feb 21, 2019 at 10:12
  • \$\begingroup\$ Its FR4 so CTI 175 which is (correct me if I am wrong) material group 3 and for 1400V would give distance of 12.5. So for the transistor of CTI400 material group 3 at that voltage would require 9mm but pin pitch is 5mm. Can you clarify that? \$\endgroup\$
    – MXG123
    Commented Feb 21, 2019 at 11:18
  • \$\begingroup\$ CTI 175 is material group III. CTI 400 is material group II. See here: en.wikipedia.org/wiki/Comparative_Tracking_Index What's your pollution degree? \$\endgroup\$
    – winny
    Commented Feb 21, 2019 at 12:12
  • \$\begingroup\$ Pollution Degree 2 here in workshop but may go to pollution degree 3 if in dirty test room \$\endgroup\$
    – MXG123
    Commented Feb 21, 2019 at 12:21
  • \$\begingroup\$ Test room isn’t an issue. What’s the end product usage area? Indoors? Will there be welding/grinding/casting or anything similar going on there? \$\endgroup\$
    – winny
    Commented Feb 21, 2019 at 12:23

1 Answer 1

Reset to default
5
\$\begingroup\$

I have designed a few boards like this in the past, and the first thing that I would do, if possible, was to stagger the middle pin inwards into the PCB, in order to increase the clearance to the outer pins. This is not always possible, so the next step is to cut slots between the pads.

This article explains quite well the issue of creepage

One thing that I find concerning is the mounting hole so close to the IGBTs, have you taken the isolation from that into consideration?

\$\endgroup\$
1
  • 2
    \$\begingroup\$ +1 for mentioning creepage slots. That is definitely something that should be added, even if the nominal distance was enough. \$\endgroup\$
    – DerStrom8
    Commented Feb 21, 2019 at 11:57

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

Not the answer you're looking for? Browse other questions tagged or ask your own question.