Searching \ for '[OT] routing 0.250 traces to pins on 0.100 centers' in subject line. ()
Make payments with PayPal - it's fast, free and secure! Help us get a faster server
FAQ page: www.piclist.com/techref/index.htm?key=routing+0250+traces
Search entire site for: 'routing 0.250 traces to pins on 0.100 centers'.

Exact match. Not showing close matches.
PICList Thread
'[OT] routing 0.250 traces to pins on 0.100 centers'
2000\04\04@132748 by Eisermann, Phil [Ridg/CO]

flavicon
face
Sorry for yet another off topic question, but:

I need to route some 0.250 traces to a FET. The
FET's pins are 0.100 inches apart. I've offset the
pins so they aren't in a straight line, but rather
staggered. There still isn't enough room between
the pins for a trace this wide. I should mention
that this is a 5-pin FET (SenseFET/HEXSense
from International Rectifier).

Does anyone have an accepted method of doing
this? I have two possible solutions: (1) drilling two
"phantom holes" next to the real hole in a triangle
pattern and (2) creating a triangle shaped plane
that touches the pin in question.

Any help is greatly appreciated.

Phil Eisermann
H:(440) 284-3787 (spam_OUTmazerTakeThisOuTspamix.netcom.com)
O:(440) 329-4680 (.....peisermaKILLspamspam@spam@ridgid.com)

2000\04\04@134446 by peter_teng

flavicon
face
Phil,

       One more suggestion, how about leave out the solder mask on the thinner
traces? This creates a thicker metal connection on the trace, and helps to
carry higher current.

best regards,
Peter Teng



{Original Message removed}

2000\04\04@140604 by Wagner Lipnharski

flavicon
face
In cases like that, one suggestion is to NOT solder the FET directly to
the board, but using extension lead wires instead. It also helps to
avoid the thermal mechanical movement between the FET, heatsync and
loosen solder by movement. Use one to two inches long wires to connect
the FET to the Board, so you can spread the traces as far as you need.

If you really need to solder the FET directly to the board, you can also
bend the FET 5 pins one forward one backward, and route the traces
accordingly.  Lots of power chips use this technique from factory.  If
this particular FET doesn't have the leads in this shape (straight
leads), probably the manufacturer don't think you need to use a trace
wider than 80 or 85 mils, at least close to the device.

Wagner.

"Eisermann, Phil [Ridg/CO]" wrote:
{Quote hidden}

2000\04\04@161324 by Roland Andrag

flavicon
face
Phill, besides what Wagner and others have said, you should able to come in
from three sides.  i.e. if the pins are in a vertical line, bring trace to
top pin running north-south, bottom pin south north and middle pin east
west.  That allows you say 150 mills to the centre pin if you make the pads
rectangular (with/without round corners), and 250 mills to outer pins.
Which pin is the gate - that one should not require a thick track anyhow.

Also you could use a 2 or 3 oz board to increase the current handling
capability.
For 200 mill tracks, 1 oz board: 6 A
2 oz: 11 A
3 oz: 14 A.

I am of course assuming that you want the tracks wide for current carrying
capability. They also help in conducting heat away of course.  For this
reason they become hard to solder when very wide.

Roland


{Original Message removed}

2000\04\04@171607 by Eisermann, Phil [Ridg/CO]

flavicon
face
Thanks to everyone for their suggestions. Based on an off-list
suggestion, I will neck-down the traces right at the pin.

I liked the suggestion of going at the trace from three sides.
Unfortunately, the power pins are in the middle (of course
they are!). Plus running 0.250 traces from one source
takes up a lot of space!

FWIW, the 0.250 width was a bare minimum that would work,
based on 50C heat rise, 1oz copper weight, and on the fact that I
planned to put traces on both top and bottom sides. I can add
more of a margin/lower the heat rise by going to higher copper
weight.


Phil Eisermann
H:(440) 284-3787 (EraseMEmazerspam_OUTspamTakeThisOuTix.netcom.com)
O:(440) 329-4680 (peisermaspamspam_OUTridgid.com)

2000\04\05@011320 by Dwayne Reid

flavicon
face
<x-flowed>At 05:12 PM 4/4/00 -0400, Eisermann, Phil [Ridg/CO] wrote:
>Thanks to everyone for their suggestions. Based on an off-list
>suggestion, I will neck-down the traces right at the pin.
>
>FWIW, the 0.250 width was a bare minimum that would work,
>based on 50C heat rise, 1oz copper weight, and on the fact that I
>planned to put traces on both top and bottom sides. I can add
>more of a margin/lower the heat rise by going to higher copper
>weight.

Check with your board supplier.  When I order 1 oz copper, they send me 1.5
oz (double sided boards).  Something about them starting off with 0.5 oz
stock, then plating until they get 1 oz within the holes.  The net result
is 1 oz hole walls, 1.5 oz tracks.

I now count on this for some of my triac boards.

dwayne



Dwayne Reid   <@spam@dwaynerKILLspamspamplanet.eon.net>
Trinity Electronics Systems Ltd    Edmonton, AB, CANADA
(780) 489-3199 voice          (780) 487-6397 fax

Celebrating 16 years of Engineering Innovation (1984 - 2000)

* * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Do NOT send unsolicited commercial email to this email address.
This message neither grants consent to receive unsolicited
commercial email nor is intended to solicit commercial email.

</x-flowed>

2000\04\08@161325 by Arthur Brown

flavicon
face
how about laying wire onto 0.1 tracks or two-sided track to FET.
Art
----- Original Message -----
From: Eisermann, Phil [Ridg/CO] <KILLspampeisermaKILLspamspamRIDGID.COM>
To: <RemoveMEPICLISTTakeThisOuTspamMITVMA.MIT.EDU>
Sent: Tuesday, April 04, 2000 6:22 PM
Subject: [OT] routing 0.250 traces to pins on 0.100 centers?


{Quote hidden}

More... (looser matching)
- Last day of these posts
- In 2000 , 2001 only
- Today
- New search...