High current connector options for PCB 4

[SolarTrap]

Hi All,

I am looking for an alternative to these cable lugs
On my current PCB design I am using 10 of these in a row (rating of 30V DC with max 50A)

Unfortunately these lugs makes if very hard to design an enclosure and I came across the 'Powerpole PP75' connectors from Anderson Power.

Has anyone experience using them? I am in particular interested in the usage of the 'BusBar' type (rightmost pair):

Can they be directly screwed into the PCB?

Markus

 

[VEBill]

Those type of bus bars are also sometimes described as PCB or Board Stiffeners. Or more precisely, I have seen some being described as both.

 

[mcgyvr]

mcgyvr; Are you saying you use various swagged/soldered standoffs (very short I imagine) then screw down essentially just flat copper with holes drilled to match the standoff placement? In other words home-fabbed busbar?

Yes we have done that for certain products and never had a problem with it. In the past we would actually solder the tin plated standoff to the pcb pad after swaging to ensure it wouldn't loosen but after some extensive testing (lots of thermal cycling,etc...) we determined that really wasn't needed.
We typically use that connection just to tie the bus bar to the board from maybe an input connector or something like that.
We aren't using the bus bar to improve the current rating of the trace (but it obviously does help some as its a great heatsink).. Its more of just a way to transition from bus bar to PCB.. And the only reason we use the standoffs vs directly bolting the bar to the PCB is because of other pins/protrusions in that area so we don't have a flat plane to bolt to.

 

[itsmoked]

Most interesting mcgyvr, thanks for that!

I had no idea so many of us run mammoth currents on our circuit boards. You folks are fearless.

I've seen hottub control boards with big traces. Comcokid is doing inverters. Scotty mentioned UPSs.

What other kinds of products are needing these big trace currents?

Keith Cress
kcress -

http://www.flaminsystems.com

 

[mcgyvr]

I'm DC power distribution.
I've never run into a problem where the "trace heating" is the problem. Its obviously always the other "heat generating" devices on the board that give me the worst headaches..
Not to mention our products are placed in high ambients (65-70deg C) and couple that with people always wanting higher density and lower cost..And all our products rely on natural convection only.. I've gotten pretty creative/out of the norm lately..

With most of the world reducing power requirements.. we go the opposite way.

 

[Comcokid]

As promised, here is a list of heavy copper PCB vendors I have. The list is about 2 years old. The key words for a Google search is "PCB" and "extreme copper".

http://www.upe-inc.com

(up to 200 oz)

http://www.asapcb.com

(up to 10 oz)

http://www.epectec.com/pcb/extreme-copper/

(up to 40 oz)

http://www.bestpcbs.com/products/heavy-copper-pcb.htm

(up to 200 oz)

http://www.saturnelectronics.com

(up to 20 oz)

http://www.methode.com

They did list up to 200 oz, but I couldn't find a recent link at their website. However, they do have connectors for up to 200 amps that might be suitable for the OP question.

Some of these vendors example PCBs capable of carrying up to 1000 amps.

 

[SolarTrap]

@mcgyvr: 'thermal reliefs to aid in soldering,etc... As well as thermal vias to help spread the heat' -- I looked this up in wikipedia but I am not really clear how it looks like. Do you have a good picture? Also, are your high current boards all UL certified?

@MacGyverS2000: I need UL approval for my board, so solder buildup is a no-go, right? What are the UL certifies looking for when they inspect a board in terms of routing and copper thickness?

@Comcokid: Thanks for the list of links - I might have to get quotes from them now. The lugs I am showing are sold here:

http://lugsdirect.com/PCBsolderable-lugs.htm

 

[MacGyverS2000]

For UL, you will need to meet the requirements for track spacing (to prevent arc-over) and track thickness (to carry the current level desired within a specified level of heat rise).

Here is an example of thermal relief on a pad:
[image

http://pcb.geda-project.org/pcb-20060422/thermal.png

]

I've never tried doing such a thing with heavy copper, but the overall premise is the same. Note: Thermal relief defeats the purpose of heavy copper if the pad you're relieving will be carrying heavy current... you can't do the latter if you're including the former.






Dan - Owner

http://www.Hi-TecDesigns.com

 

[MacGyverS2000]

I copied the above image from Google... and I just noticed the pad/via without thermal relief really should be completely surrounded/touching the plane (red touching gray) to make sense of what we're discussing. Otherwise, it's just a regular via.



Dan - Owner

http://www.Hi-TecDesigns.com

 

[mcgyvr]

http://www.synqor.com/documents/appnotes/appnt_thermal_relief_study.pdf

A "thermal via" is just a regular "via" but its intended purpose is to help transfer heat to the other plane and not intended (but it does) to pass electrical signals (if using double sided boards,etc.. where the copper plane on the other side is in the same net as the top side)

 

[MacGyverS2000]

Wait, I thought we were talking about thermal relief vias, not thermal vias. Two different animals with different goals.

Dan - Owner

http://www.Hi-TecDesigns.com

 

[IRstuff]

mcgvr mentions both in his posting, which is probably where the confusion comes from.

Note that with thick copper, thermal reliefs will still suck a lot of heat away from a soldering iron, so a really hot one is probably needed to get a good joint

TTFN
faq731-376

Need help writing a question or understanding a reply? forum1529

Of course I can. I can do anything. I can do absolutely anything. I'm an expert!

 

[mcgyvr]

The trick with thermal reliefs is finding the "spoke width" that works best for each application.. Not too thin to where it can't carry the required currents without negative effects and not too thick to where its sucking the heat away too fast as IRstuff mentioned..

 

[Comcokid]

Earlier in this post I mentioned I use a double sided 10oz board with SMT. This board also has some thru-hole radial electrolytics. For electrolytics that have a lead making plane connection both under the part and on the solder side, I use a thermal relief on the plane under the part. On the solder side I have found it most effective skip the thermal relief, and to put a rectangular mask opening the width of the solder tip being used to solder. The rectangular mask opening is 0.2" x 0.1" so a Metcal STTC-117 tip (0.2" wide) can solder the part.

Extreme copper PCBs require extreme soldering irons, like Metcal. The thermal relief under the part makes it possible to melt the solder under the part from the solder side. You really have to think carefully about the heat flow for assembly and rework. If you don't, you can easily create an un-solderable and un-reworkable PCB.