PCB Clearance recommendation for 3 ounce copper

Hi,

Can any one please advice me on the clearance that I have to follow for the below PCB layer stack up.


File Name
Copper weight
TOP H TOP_COPPER.GER 3 Ounce
POWER1 V POWER1.GER 3 Ounce
GROUND1 H GROUND1.GER 1 Ounce
SIGNAL1 V SIGNAL1.GER 1 Ounce
SIGNAL2 H SIGNAL2.GER 1 Ounce
GROUND2 V GROUND2.GER 1 Ounce
POWER2 H POWER2.GER 3 Ounce
BOTTOM V BOTTOM_COPPER.GER 3 Ounce

Is this a proper copper weight for this stack up.

Will this result in any manufacturing or assembly issues ?

Clearance has very little to do with copper thickness, assuming you are talking about voltage creepage. It depends more on voltage and environment (altitude, for example).

It looks like a very strange stackup to me. You've got 3 oz power plane but only one ounce ground plane. Doesn't the same current flow in both planes?

Not sure what you are asking about a "proper copper weight"; it depends on your design. But, for a definitive answer, contact your board house.

We could be referencing 2 types of clearance here, high voltage and basic clearances for normal routing signal lines etc. Here copper weight plays a part, when you etch a board you etch inwards as well as down so manufacturers apply etch compensation to your artworks:

The etch factor is also proportional to the thickness of the copper or copper weight being removed. The more copper being etched through the larger the etch factor.

Click to expand...

So the thicker the copper, the more etch compensation added and thus the larger the standard track to track spacing's etc. manufacturers publish their capabilities which should state the minimum features and spacing's for a particular copper weight.
**broken link removed**

Spacing for creepage and clearance do not change with regards to base PCB weight.
I have done similar stack ups including up to 4oz.

I have 32 power tracks carrying 5A for 20mS. The thickness of the track is reduced to 2.5mm for 3ounce copper and I have routed it on top,bottom,power1 and power 2.

I have a common ground DGND for the power tracks GROUND1 and GROUND 2.

For 2.5mm track width I would like to know the track clearance and will the track clearance differs with respect to the copper thickness of the PCB because of etching. ?

- - - Updated - - -

Hi Marce,


Can I please know the stack up I have got above is correct . I dont want to increase the copper thickness as we have for some connectors to be soldered on to the board.

Should I have to use same copper thickness for ground plane with respect to the power plane ?

Read my reply I have answered most of your points.....regarding copper weight and spacing.
For voltage related spacing refer to the relevant regulations and documents, here is some basic info:
http://www.creepage.com/

I do not know the design so can only give (and will only give) hints and guidance.
I have used a similar stackup with 4 oz copper, same layers just thicker copper, I used the same weight for my GND as the power layers. So it can be done check with your manufacturer.

marce said:

We could be referencing 2 types of clearance here, high voltage and basic clearances for normal routing signal lines etc. Here copper weight plays a part, when you etch a board you etch inwards as well as down so manufacturers apply etch compensation to your artworks:

So the thicker the copper, the more etch compensation added and thus the larger the standard track to track spacing's etc. manufacturers publish their capabilities which should state the minimum features and spacing's for a particular copper weight.
**broken link removed**

Spacing for creepage and clearance do not change with regards to base PCB weight.
I have done similar stack ups including up to 4oz.

Click to expand...

I believe the etch factor is something the PCB manufacturer has to worry about, not the PCB designer. The etch factor is just the amount of 'oversize' the manufacturer has to add to get the right trace width when it's done etching. The effect on the actual trace only limits the minimum width. Referring to your reference document, the minimum trace width difference between 1 oz and 3 oz copper is only .002" (.007" vs .005"); that's not much, especially considering that the OP intends to have large currents and, thus, large trace widths; otherwise, why would he be using 3 oz to begin with? In other words, if the OP needs a .005" trace, why is he using 3 oz copper?

The stackup listed in post #1 can be only build sequentially due to the arrangement of inner 3 oz layers. It would be better (less costly) to use 3 oz for the ground layers, too.

barry said:

I believe the etch factor is something the PCB manufacturer has to worry about, not the PCB designer. The etch factor is just the amount of 'oversize' the manufacturer has to add to get the right trace width when it's done etching. The effect on the actual trace only limits the minimum width. Referring to your reference document, the minimum trace width difference between 1 oz and 3 oz copper is only .002" (.007" vs .005"); that's not much, especially considering that the OP intends to have large currents and, thus, large trace widths; otherwise, why would he be using 3 oz to begin with? In other words, if the OP needs a .005" trace, why is he using 3 oz copper?

Click to expand...

The PCB designer has to be aware of etch factor otherwise you can cause the manufacturer problems and as a consequence problems with your design. If you are a competent PCB designer then you have to understand how your boards are made and assembled, you cannot say it is a problem for the manufacturer, it is the designer who designs the boards and they should understand what they are doing.
You can also have control electronics on such a board and often this is the case.
I already find more and more are coming into PCB design with little or no understanding of the PCB manufacturing process or the assembly process, this knowledge is just as important as understanding at least basic circuitry, signal integrity, current carrying abilities etc. etc. The view that anyone can throw together a PCB and the dumbing down of PCB design is not helped by this.

When etch factor is added the shape and size of negative geometries change on your design, this could limit the amount of etchant that could get in these areas.
instead of pulling me up maybe you should be supporting my drive to improve both the education and knowledge base of PCB designers and help improve the global view of PCB design in general.