Prevent Power/GND connections from Connecting Directly to Flood Planes


#1

Is there a way to have Components power and Gnd connections not be connected directly to their respective filled planes via thermal relief.
I seem to think it would be best to run a trace from 0V and 5V from the Component to the bypass cap first and then let it tie into the Filled Plane. This would also help when hand soldering from a thermal relief standpoint. Even with the Thermal Relief, it is more difficult to solder the Power and GND connections when they are directly tied to the Plane.
Is changing net names required to make this happen? Then you would have to connect two different Net Names to each other which wouldnt seem to work out.
I could define a Keepout Zone around my traces to keep them from connecting to planes automatically but that seems tedious as well.
Any thoughts?

Edit: Using v 4.0.7.


#2

Maybe Defining Keepout Zones is the best way to go…


#3

[quote=“gremlin, post:1, topic:8475”]
Is there a way to have Components power and Gnd connections not be connected directly to their respective filled planes via thermal relief.
[/quote]Thermal relief is a zone setting unless I misunderstand your question?


#4

It appears that your first problem is that you don’t have an adequate soldering iron. I’ve done several boards now, and I’ve sent some of them to a friend of mine, and neither of us have had issues with soldering to both through-hole and SMD pads with thermal reliefs.

The second issue may be that your thermal relief settings in the zone settings are set to wide.


#5

That is a possible solution: define a keep-out zone surrounding the trace from your power pin to the bypass capacitor. The zone’s “Properties” can be defined to exclude ONLY the copper pour, while permitting pads and traces.

That statement is true as far as it goes, but there’s more to it.

The zone’s “Properties” allow you to define several types of default connections from the zone to copper features of the zone’s net.

  • “Solid” - this causes the fill to completely cover the copper feature - no gaps.

  • “Thermal Relief” - creates a gap between the zone and ALL pads touching the zone. The width of the gap is set by the “Antipad Clearance” parameter in the zone’s Properties, and the connecting spokes have a width defined by “Spoke Width”.

  • “THT Thermal” - this creates thermal relief gaps (as above) between the zone and Through-Hole Pads ONLY. The SMD pads have a “Solid” connection to the zone. (Probably based on the assumption that SMD components will be reflow soldered, where thermal relief isn’t necessary, while thru-hole components will be hand soldered.)

  • “None” - All pads, even pads in the zone’s net, are isolated from the zone by the “Antipad Clearance” value. Traces, however, are covered by the fill.

Here’s where a little more information makes things interesting.

The parameters related to connections between pads and zones can be set on a pad-by-pad basis.

The individual pad parameters can be set when the footprint is created, or after the footprint has been placed on a board. The pad parameters over-ride the zone defaults.

So that suggests a solution to the problem described by @gremlin. Recall, he has a power pin connected to a bypass capacitor, and both pads are enclosed by a zone connected to the power net. He wants to fill the zone, but leave the trace from the power pin to the capacitor pad unconnected from the zone. Here’s the plan:

  • Make sure the capacitor pad is physically close to the power pin. (If they aren’t, it’s probably not worth worrying about the copper fill flooding over the connecting trace.)

  • Edit the power pin’s “Properties”. Set the Zone Connection type to “None”, and make the “Thermal relief gap” value equal to half the distance to the bypass capacitor’s pad. (There’s a more exact formula for the “Thermal relief gap” value, but for now just trust me.)

  • Edit the “Properties” of the bypass capacitor’s pad. Set its type to “Thermal Relief”, and make the “Thermal relief gap” value equal to half the distance to the power pin’s pad.

  • Run a trace between the power pin and the bypass capacitor by the most direct route.

  • Fill the zone.

Did it work?

Dale


#6

I’m with @gremlin on this one. Even with thermal relief, a pad connected to a copper pour is more difficult to solder than a pad with only traces connected to it. Certainly not as difficult as trying to solder a pad connected directly to the copper pour, but still difficult. My personal trick is to use TWO soldering irons simultaneously. My cube-mate laughs, but it gets the job done.

Dale


#7

@dchisholm
One word, “Metcal”.
Second two words, “Many dollars”.

And, to be practical, I’ve been soldering for a very long time; I might even wager that I can solder to QA J-standards with just a Bic lighter and a paper clip!


#8

I know the brand only by its (excellent) reputation.

At my current job it took a fight and some executive intervention just to replace Radio Shack non-temp-controlled irons with Hakko FX-888’s.

If you ever pass through St Louis, I’ll let you demonstrate the BIC lighter technique!

Dale


#9

Some of the Hakko units are also quality instruments; and used in commercial applications.

But we have seen that the tip temperature calibration seems a little bit on the low side for anything over small detail work.

I know this may come across as irksome, but with the one iron we have, upping the temp to 730 indicated seemed to make it feel more like using a Metcal.

And this is with lead and 2%silver solder. Lead Free solder is going to require yet another bump in temperature.

We are also using non-corrosive flux; which is some really sticky stuff if one wants to handle the board after hand soldering.

Thermal connections to filled zones have not presented any notable difference in soldering performance using the default settings in KiCad.


#10

I’ve done quite a few things with the Bravo India Charlie Model Two Thousand that I should not have done; but it got the work completed!

I’ve not really actually tried it… but I’m not certain that I would not be able to actually do it. Thus the reason for the wager.

Now your comments are likely going to have me go the local Maker Space to see if I can really pull it off!!!


#11

I probably shouldn’t even have mentioned that about soldering. I probably just muddied the waters and made it not as clear as what I was actually trying to achieve. We really don’t have any trouble soldering. We’ve built about 150 boards and I have about 4 different people that may do some of the hand soldering. I had just noticed that the power connection was where a couple of them had the ugliest joints. Overall, not a problem though.
I was just really trying to figure out the best way to trace through the Bypass Caps before tying to the Plane if that makes sense.
@dchisholm, Thanks for the info. Ill have to mess around with individual pad properties but for now the Keepout zones seem to be achieving what I am looking for.

Also, While this thread is getting a little attention… Anyone know of a US based PCB fab where I can get about 5 boards made with a 1-2 day turn without costing an arm and a leg… I use ALLPCB out of China but of course that takes 5-7 days to get boards and I’m in a bind on time. I looked at Advanced Circuits (4pcb.com) and I was shocked at high cost…
I was expecting 10-20 times more expensive than China but it was 50-60 times…


#12

I’ll try setting the tip temp to 730F. I was running the Hakko FX-888 at 700F, and it often struggled to make visually good joints on pads with thermal relief to a zone, especially through-hole pads. I was afraid that 700F would damage components, so when I started using two irons on pads connected to zones, I backed it down to 650F.

Dale


#13

Offhand I don’t know of any board fabricators in North America that meet your criteria. My current employer uses Imagineering; I don’t know what their promised turnaround time is, but boards land on my worktable 7 - 10 days after I hand off a file set to Purchasing. Imagineering has a U.S. headquarters address (Chicago region, if I recall correctly) but I think their manufacturing is done in India.

I know that cost rises exponentially as turnaround time decreases, and 1 - 2 days is probably pushing the limits of what is practical for a full-featured board. I have seen ads for “naked boards” (no silkscreen; no soldermask) that could probably be done in one day, but never investigated them.

If I truly had to work with a short fuse like that, I’d look into creating an in-house capability to fabricate boards, either chemical etching or surface milling of the copper foil. That should cut the turnaround time down to a few hours. Milling is attractive because, in theory, the machine that does the milling can also do the drilling. Be prepared to take a hit on precision - I suspect that 10/10 design rules are about as good as you can do with inexpensive in-house methods. And I don’t know if silkscreen and soldermask are even practical for in-house fabrication.

Dale


#14

If you haven’t already you could check out Sunstone Circuits.


#15

How old are your Hakko tips?

I’m not super up to date on the Hakko product line, but I thought the new, t18-d16 tip, used some newer metallurgy.

We are using the new Hakko tip, afaik, and still need the extra 30 degrees F to make it “feel” the same as the similar Metcal tip rated at 700F. Once an operator gets used to a certain “feel” every day, they don’t tend to like it being different, and having to re-learn.