Exact match. Not showing close matches.
'[EE] Re: Tips for hand routing boards?'
forwarding with tag added
On Wed, Feb 8, 2012, at 03:59 PM, Marc Nicholas wrote:
> Hi all,
> Does anyone have any "tricks of the trade" for hand routing boards?
> Specifically, hand routing from reasonably high density TQFP/QFN parts
> and 64-pin) in 6 to 8-mil to other lower density components (think hub
> I'm getting beyond the stage where Eagle's autorouter does a good job...
> Appreciated in advance.
-- http://www.fastmail.fm - IMAP accessible web-mail
|Ahhh a question worthy of books of advice. I'm sure others will pitch in, here's my 2c.
If you haven't already, change the design rules to allow 16mil drill vias, rather than the default. DRC -> Sizes Tab -> minimum Drill set to 16, and I think the Restring Tab -> vias -> I have the min set to 8mil outer and inner, % to 25, and Max to 20mil.
Humm. Place all parts before doing any routing at all. Decoupling caps especially.
If you can do 8/8 and 16mil drills, this means you can use nearly any boardhouse's typical cheap manufacturing.
Ground pour on top and bottom. I don't do the +3.3V (or whatever) power pour ever, even on 4-layer. I always route power so I know what is going where. Ground I don't route, but am mindful of trying to keep the pour successful. Use lots of vias to ground, they're cheap and make things easier.
I have a separate USB keypad with programmable keys (designed for gaming) configured to switch between 9 different tools in eagle when doing layout, so move/ripup/ratsnest/route is real fast to switch between. Left hand on keypad, right hand on mouse, with mousewheel of course and click of mousewheel ("middle" mouse button) and drag is pan. Very very handy. Essential.
You can use the autorouter to "check your work" ... if it is having big problems with routing, you probably will too. Move parts, watch airwires, try to avoid long airwires that cross others, etc. etc.
For placing parts, I usually use a grid of 10mil. For routing, 5mil.
It is pretty Zen. I hand route everything, the autorouter is just for getting an idea of difficulty, tho I'm still on eagle 4.x and I hear it has been improved. 4-layer 2000 net pcbs, yes, by hand. It does take awhile, but with good parts placement, it almost "routes itself", mostly.
Bob Blick wrote:
Jesse Lackey wrote:
> I have a separate USB keypad with programmable keys (designed for
> gaming) configured to switch between 9 different tools in eagle when
> doing layout, so move/ripup/ratsnest/route is real fast to switch
> between. Left hand on keypad, right hand on mouse, with mousewheel of
> course and click of mousewheel ("middle" mouse button) and drag is pan.
> Very very handy. Essential.
It sounds cool! Can you click an image and post it somewhere so that we can have a dekko? How about a YouTube video demoing it?!
Thank you very much for the feedback, Jesse!!!
|Excellent tips Jesse. I hand route everything as well.
Placement is the key - start with the main component (usually a
microcontroller). Place it more or less in the center, then move and
rotate each supporting component around and watch the airwires - you
will find both a location and an orientation that makes routing
between the two easiest. Keep doing this for all additional
components and pretty soon you'll produce the best placement for all
Then pour your ground plane and route all your ground wires. I also
hand route all the power wires.
After that I usually start on one edge of the board, top or bottom,
and work my way up/down until all my airwires are traces. Then go get
a cup of coffee and a cookie, and come back 20 minutes later and look
at the big picture. At that point you'll see some trace routing that
you can optimize.
Lately I've found myself going back to the schematic throughout the
routing process to change the routing - usually of buffers or
inverters - to make physical routing easier. For instance, if you've
got 6 inputs and 6 outputs on a chip you'll pick the most direct
routing in the schematic but when you place the part you might find
that the traces have to go over/under whereas if you go over/under in
the schematic the traces will go parallel.
A Youtube video is a great idea. I might actually followup on that.
caveat I don't do high speed or RF.
On Thu, Feb 9, 2012 at 5:37 AM, Marc Nicholas <gmail.com> wrote: geekything
> Thank you very much for the feedback, Jesse!!!
On Thu, Feb 9, 2012 at 1:19 PM, doug metzler <gmail.com> wrote: doug.metzler
> Excellent tips Jesse. I hand route everything as well.
I use a 3d connexion space pilot with Altium. Many buttons, and the
knob thing is really nice for 3d views.
Place your unmoveable components, then the others, high priority to
bypassing and high frequency paths.
Place crystals and their caps as close as possible to the chip, and
return the crystal caps directly, and only to the nearest ground pin
on the chip that is using the crystal. From that point flood an
isolated island on the other side of the board.
Select bypass caps according to the frequencies of interest, not 0.1uF for all.
I diverge from the conventional wisdom in that I don't use planes to
return power, I route explicit paths that mirror as closely as
possible the sourcing path. The power and ground route to the bypass
cap, and then to the chip. Never "T" into a bypass, rather make it a
"V" with the cap at the point of the "V". FORCE the current to travel
to the cap, don't give it any other options.
The result of all this is a board that is two layer only, spends
usually $0.00 on emi supression, and passes radiated and conducted
emissions by being so quiet that it is almost completely unobservable
in a GTEM.
RF immunity on our products only needs to be 3V/M, but the last one I
tested in extremis was running as a bare board (no enclosure of any
kind) in the GTEM at a field > 192V/M. The field measurement
instrument started giving erratic readings above that point, so we
couldn't trust it for higher readings. We were putting >50W into the
Hi - sorry no pics but there isn't much to see. The keyboard is this:
but has been obsolete for awhile. It is pretty good physically, have had lots of headaches with the drivers.
I suggest getting any kind of secondary keypad that allows the keys to be programmed. What I did was assign various alt+Key to different tools (like alt+I is copy, alt+J is Name, alt+K is label, etc. for schematic) and then program the keypad so that various keys output the alt+whatever. I don't use it much in schematic entry, but for routing it is a major timesaver.
Mohit (Lists) wrote:
> Jesse Lackey wrote:
>> I have a separate USB keypad with programmable keys (designed for
>> gaming) configured to switch between 9 different tools in eagle when
>> doing layout, so move/ripup/ratsnest/route is real fast to switch
>> between. Left hand on keypad, right hand on mouse, with mousewheel of
>> course and click of mousewheel ("middle" mouse button) and drag is pan.
>> Very very handy. Essential.
> It sounds cool! Can you click an image and post it somewhere so that we
> can have a dekko? How about a YouTube video demoing it?!
Hi - thanks for the description. This is very interesting. Do you put power and ground parallel to each other on the same pcb side, or have them follow each other on opposite sides of the pcb? It sounds like they run parallel with your description of connecting the decouple cap then the chip.
Do you have a pic showing this? I want to make sure I understand the "T" vs. the "V".
I'm doing a bluetooth LE design in the coming weeks, and if I can make it on a 2-layer (vs. 4-layer reference design) it would be a big win. I realize there's a lot more to successful RF than power routing and decoupling caps, but it would certainly help.
David VanHorn wrote:
|On Fri, Feb 10, 2012 at 1:54 AM, Jesse Lackey <celestialaudio.com> wrote: jsl-ml
> Hi - thanks for the description. This is very interesting. Do you put
> power and ground parallel to each other on the same pcb side, or have
> them follow each other on opposite sides of the pcb? It sounds like
> they run parallel with your description of connecting the decouple cap
> then the chip.
You can do that, and I have on occasion, but that pretty much limits
you to the edges of the board since on two layers you can't route
anything across that on either layer. It's more about having parallel
paths with as small a loop area as practical.
> Do you have a pic showing this? I want to make sure I understand the
> "T" vs. the "V".
Not easily. If you think of the capacitor footprint, then each pad
would have two traces connecting it, one pair goes to the chip and the
other pair goes to the source. There are (expensive) caps that
implement this with a four pad design, called "X2Y" caps. I haven't
needed them yet.
> I'm doing a bluetooth LE design in the coming weeks, and if I can make
> it on a 2-layer (vs. 4-layer reference design) it would be a big win. I
> realize there's a lot more to successful RF than power routing and
> decoupling caps, but it would certainly help.
I am doing 2.4 G on FR4 double sided. Be aware, the antenna dims are
critical to 0.1mm and tuning varies with any dielectric material up to
about 0.5" away from the antenna, and the exact shape of your ground
plane. Whether the antenna is on the PCB or not, a mistuned antenna
may cause your third harmonic to be drastically higher than it should
be. We've seen 30dB reduction in third harmonics by using a
particular filter balun from Johansen, and by keeping the antenna well
matched. A significant mismatch may also drastically reduce your
transmit power, depending on whether or not the folds back its output
power on mismatch.
We took our original antenna design to Don DeGroot in Longmont CO,
with samples of the plastics for the enclosure. He used a VNA to
measure the antenna in and out of the enclosure, and his own rig to
measure the plastics dielectic constant, then redesigned the antenna
for the proper tuning in the case. Well worth the cost!
If you're in trouble with RF, and he can't help you... You are really hosed!
Hi David, super good tips, thank you again for writing this up.
Am envious you're in Altium-land ... I just don't do enough EE design work to warrant the jump from Eagle. The Altium demos are awesome, it is so clearly way way ahead of Eagle, but alas. I spend too much time dealing with firmware and not strictly EE design. :)
David VanHorn wrote:
On Fri, Feb 10, 2012 at 2:28 PM, Jesse Lackey <celestialaudio.com> wrote: jsl-ml
> Hi David, super good tips, thank you again for writing this up.
> Am envious you're in Altium-land ... I just don't do enough EE design
> work to warrant the jump from Eagle. The Altium demos are awesome, it
> is so clearly way way ahead of Eagle, but alas. I spend too much time
> dealing with firmware and not strictly EE design. :)
It wasn't an easy sell, but we do a lot of odd shaped boards in odd
shaped enclosures, and it works very nicely with SolidWorks, which
allows us to "see" the board in the enclosure and prevent expensive
board spins. I'd say it has paid for itself in that alone.
I wish they'd do a "Student version" somehow, but it is also a large
learning curve and we've found that sometimes it will do something we
need but the support people don't know that it does. We end up
discovering it much later by accident.
More... (looser matching)
- Last day of these posts
- In 2012
, 2013 only
- New search...