Reducing Copper Trance Resistances, ideas?

Do you have a question? Post it now! No Registration Necessary

Translate This Thread From English to

Threaded View
Hi

We are running 25A in copper traces in a frequency inverter.

I have reduced the power dissipation of the traces by increasing the copper thickness from 70u to 105u and increased the widht of the traces

We are still experiencing to high temperatures from the trace dissipation

We could go to 6 layer PCB, or we could remove the soldermask to add tin to the copper traces on the bottom layer (from the solderwave process)

But, any other ways?

Perhaps someone has experience in adding a leadframe to the PCB to handle the low frequency currents?

Regards

Klaus

Re: Reducing Copper Trance Resistances, ideas?
On Wed, 12 Nov 2014 14:37:05 -0800 (PST), Klaus Kragelund

Quoted text here. Click to load it

You can use PCB solder-on busbars. Or buy boards with seriously thick
copper, $$$ from Bergquist etc.


--  

John Larkin         Highland Technology, Inc
picosecond timing   precision measurement  

We've slightly trimmed the long signature. Click to see the full one.
Re: Reducing Copper Trance Resistances, ideas?
On 11/12/2014 5:44 PM, John Larkin wrote:
Quoted text here. Click to load it
Or delete the solder mask over the high-current traces and wave-solder  
them to add thickness.  Solder has about 10%-20% the conductivity of  
copper, so you need quite a bit to make much of a difference, but every  
little helps.

Cheers

Phil Hobbs

--  
Dr Philip C D Hobbs
Principal Consultant
We've slightly trimmed the long signature. Click to see the full one.
Re: Reducing Copper Trance Resistances, ideas?
On Wed, 12 Nov 2014 19:46:56 -0500, Phil Hobbs

Quoted text here. Click to load it

Topside, solder paste and reflow.


--  

John Larkin         Highland Technology, Inc

jlarkin att highlandtechnology dott com
We've slightly trimmed the long signature. Click to see the full one.
Re: Reducing Copper Trance Resistances, ideas?
On Thursday, November 13, 2014 5:27:44 AM UTC+1, John Larkin wrote:
Quoted text here. Click to load it

Yes, that is also a good option

Thanks

Klaus

Re: Reducing Copper Trance Resistances, ideas?
On 11/12/2014 11:27 PM, John Larkin wrote:
Quoted text here. Click to load it
Assuming the traces are short.  Otherwise the stencil might fall apart.

Cheers

Phil Hobbs

--  
Dr Philip C D Hobbs
Principal Consultant
We've slightly trimmed the long signature. Click to see the full one.
Re: Reducing Copper Trance Resistances, ideas?
On Thu, 13 Nov 2014 09:01:35 -0500, Phil Hobbs

Quoted text here. Click to load it

You could do it in segments, or some appealing lozenge tiled pattern.

I wonder if there might be pick-and-place copper strips that you could
solder on top of traces.


--  

John Larkin         Highland Technology, Inc

jlarkin att highlandtechnology dott com
We've slightly trimmed the long signature. Click to see the full one.
Re: Reducing Copper Trance Resistances, ideas?
On Thursday, November 13, 2014 11:39:25 AM UTC-5, John Larkin wrote:
Quoted text here. Click to load it

That's a good product idea.

I like the bare-jumper technique.

 .----. .-----. .----.
    .----. .-----. .----.
 .----. .-----. .----.

My handy copper-trace spreadsheet says 3x16AWG is as good as 1" x 4oz
(25mm x 140um).

Cheers,
James

Re: Reducing Copper Trance Resistances, ideas?
On Thu, 13 Nov 2014 08:39:20 -0800, John Larkin

Quoted text here. Click to load it

I've seen some through-hole (vertical) bus bars (can't remember where
exactly). They could be custom made (either horizontal flat or
vertical with pins) using a chemical etching (subtractive) process.  

Lots of PCB makers are touting really thick copper- more than
6oz/ft^2- up to 120 or even 200oz, which would be several mm thick!  

Of course special design rules apply to the xtreme pcbs (and special
xtreme pricing, no doubt).  

Best regards,  
--Spehro Pefhany  



Re: Reducing Copper Trance Resistances, ideas?
On Thursday, November 13, 2014 5:39:25 PM UTC+1, John Larkin wrote:
Quoted text here. Click to load it
Nice idea :-)

Re: Reducing Copper Trance Resistances, ideas?
Den torsdag den 13. november 2014 20.49.50 UTC+1 skrev snipped-for-privacy@gmail.com:
Quoted text here. Click to load it

that's why I suggested the smd shunts/jumpers from Harwin, they come in rolls and are made for pick-n-place, but they are a bit small if you need +200mm

We occasionally get special solder-on shielding cans made, there is a bit of NRE because they need to make tools for the bending. But I think a flat shape  
would be much cheaper since they are made by etching similar to PCBs

If guess those who make stencils could do the same, though I think they mostly use stainless steel


So strips made in the shape of the traces reflowed on top of the traces?

-Lasse

Re: Reducing Copper Trance Resistances, ideas?
On Thursday, November 13, 2014 1:46:58 AM UTC+1, Phil Hobbs wrote:
Quoted text here. Click to load it
Yes, I saw a link (EEblog), which stated typically a 50% reduction of the resistance, but ofcourse that depends on what production equipment is used (but it's free)

Thanks

Klaus

Re: Reducing Copper Trance Resistances, ideas?

Quoted text here. Click to load it

Depending on the production environment/scale you can solder big fat  
copper wires to them (or silver if you really have scratch and want the  
last little bit of conductivity.) You could even use strip stock bent-up  
on edge to get more surface area for cooling and/or skin effect. This  
does require at least one truly skilled worker.

Alternatively, delete the traces and put in a jumper [I come from the  
crude but effective school of thought, and have done this on a  
(low-volume) production board.] If you for some reason HAVE to keep this  
as a "in-board" solution, a very wide internal power layer or layers  
might be another approach (ie, dedicate a whole layer to moving this  
current around, or two if the geometry demands that, just like an  
internal power plane.)

--  
Cats, coffee, chocolate...vices to live by
Please don't feed the trolls. Killfile and ignore them so they will go away.

Re: Reducing Copper Trance Resistances, ideas?
On Thursday, November 13, 2014 5:31:44 PM UTC+1, Ecnerwal wrote:
Quoted text here. Click to load it

We are using 30mm wide traces in average, duplicated in 4 layers for routing the 3 phases, maximizing the trace thickness

Cheers

Klaus

Re: Reducing Copper Trance Resistances, ideas?
On 11/13/2014 2:42 PM, snipped-for-privacy@gmail.com wrote:
Quoted text here. Click to load it

That is a hugely wide trace.  How little power loss are you trying to  
achieve?  I assume your problem is that this is a parasitic loss rather  
than the temperature rise of the PCB?  Using an online calculator I find  
that the temperature rise of a single surface layer of 3 oz copper  

the resistance is just 1 mohm the voltage drop is 27 mW and the power  
dissipated is 678 mW.  Which of these is a problem?

It is not clear to me if you are saying that each of the three phases is  
carried on 30 mm wide traces on all four layers or that you have four  
layers to route the three phases up to a single 30 mm wide trace for  
each.  If you combine four layers of traces, all 30 mm wide for a single  
phase, that would cut the voltage drop and power by a factor of four.

If you are running four layers of copper for each phase, I can't imagine  
much more you can do in the PCB.  I think you need to either add jumper  
wires or the bus bar stiffeners some are pointing you to.  If you can  
find space to add runs of 14 gauge wire, each two jumpers will have the  
same resistance as one of your 30 mm wide traces approx.  So 8 jumpers  
of 14 gauge wire will give you about half the resistance you currently  
have.

Is this a volume production item where wire jumpers are not such a good  
idea?

BTW, in reviewing your posts you start off saying you have increased the  
copper thickness from 70 to 105 um, but you later say you are limited to  
2 oz copper thickness which is 70 um.  Which is it?

--  

Rick

Re: Reducing Copper Trance Resistances, ideas?
On Thursday, November 13, 2014 4:24:36 PM UTC-5, rickman wrote:
Quoted text here. Click to load it
r
ry
e
up
is
uting the 3 phases, maximizing the trace thickness
Quoted text here. Click to load it
  
Quoted text here. Click to load it
  
Quoted text here. Click to load it

  
Quoted text here. Click to load it

I get similar results. I calculate that a single 70um x 30mm x 200mm trace
(2 oz.) has a resistance of 1.8 milliohms, and dissipates 1.1W @ 25A d.c.

Cheers,
James Arthur

Re: Reducing Copper Trance Resistances, ideas?
On Thursday, November 13, 2014 11:29:47 PM UTC+1, snipped-for-privacy@yahoo.com wrot
e:
Quoted text here. Click to load it
der
f
very
the
t-up
Quoted text here. Click to load it
s
e
this
routing the 3 phases, maximizing the trace thickness
Quoted text here. Click to load it
  
Quoted text here. Click to load it
  
Quoted text here. Click to load it
d  
Quoted text here. Click to load it

th  
Quoted text here. Click to load it
  
Quoted text here. Click to load it
e
I have total trace lenght of about 300cm. In some places the widht is less  
than 20mm

Cheers

Klaus

Re: Reducing Copper Trance Resistances, ideas?
On Thursday, November 13, 2014 10:24:36 PM UTC+1, rickman wrote:
Quoted text here. Click to load it
r
ry
e
up
is
uting the 3 phases, maximizing the trace thickness
Quoted text here. Click to load it
  
Quoted text here. Click to load it
  
Quoted text here. Click to load it

  
Quoted text here. Click to load it
  
Quoted text here. Click to load it
  
Quoted text here. Click to load it
  
Quoted text here. Click to load it
  
Quoted text here. Click to load it
  
Quoted text here. Click to load it

We have a total of about 40mohm trace resistance accross the entire PCB, wi
th about 25A rms currents, which translates to approx. 20W loss. Some addit
ional resistance is due to connectors, but that is out of my hands

I am running about 20mm wide trace on 3 layers. Each layer has 25A current  
from a phase.  

[snip]

Quoted text here. Click to load it

  
Quoted text here. Click to load it
  
Quoted text here. Click to load it

It is a combination of 70u on outer layers (to allow for fine pitch devices
) and 105u on inner layers (total of 4 layers). So a mix of 2 and 3 Oz.

I think the jumpers may be a good idea. Need to find something cheap for th
at. On the other side, increasing to 6 layers avoids the use of leaded asse
mbly, which can be the same price as the cost of 2 extra layer  

Regards

Klaus

Re: Reducing Copper Trance Resistances, ideas?
On Thursday, November 13, 2014 5:30:23 PM UTC-5, Klaus Kragelund wrote:
Quoted text here. Click to load it
<snip>
Quoted text here. Click to load it

With all three phases mostly on top of each other?  
If there's top room then I like the bus bars.
put three is parallel one reaching down to each phase.
yeah you lose copper for the hole to the inner layers.
plastic barrier strips between bus bars if you need them.

George H.

Re: Reducing Copper Trance Resistances, ideas?
On 11/13/2014 5:30 PM, Klaus Kragelund wrote:
Quoted text here. Click to load it

Quoted text here. Click to load it

Something is rotten in Denmark.  According tp a trace calculator the  
resistance of the 20 mm wide, 105 um thick inner layer traces should be  
4.41 mohm and dissipate 1.05 Watts each.  The outer layer trace should  
be 2.47 mohms and power is 1.55 Watts.  I don't see how you can get 20  
Watts on the PCB.  Of course the connector resistance will be more than  
this depending on how many contacts you use and how well they work.


Quoted text here. Click to load it

You can't get much cheaper than wire.  14 gauge is inexpensive and 2.5  
mohm.  Or you can go with one run of 10 ga per phase and get 1 mohm over  
300 mm.

I guess one dumb question would be why are you running this current  
through the board rather than on a wire?  I assume this is essential to  
the function of the board?

Is the problem the heat on the board or the loss of voltage across the  
connections?

Before you worry any more about the PCB traces, I think you need to find  
out why a 4 mohm trace is showing up as 40 mohms.  That is your problem.

--  

Rick

Site Timeline