# PCB traces: oz to mil (thickness) conversion (for stripline)

According to http://referencedesigner.com/cal/cal_02.php, the conversion between "oz" and "mil" (thickness) for a PCB trace is 1.37. Also, according to zcalc.exe (http://www.fedevel.com/welldoneblog/wp-content/uploads/2011/08/Zcalc.zip) 4.8mil correspond to 3.5 oz.

Now I get the following table from my foundry:

weight (cu)  thickness (mil)
0.25         0.30
0.375        0.45
0.5          0.6
1            1.2
2            2.4
3            3.6
4            4.8


These numbers are off by quite a bit.

1. How can this difference be explained?

Now I want to calculate the thicknes of my stripline (e.g. with the calculator referenced above).

1. But which number should I use/trust from the table for my calculations? For example, for 4oz copper ... should I use 4.8mil should I use 4x1.37=5.48mil?

(I would tend to 4.8mil because the input to the stripline equations is thickness but I do not understand the discrepancy)

• Ask the foundry, are they really giving you thinner copper than you spec'ed or what? – The Photon Feb 24 '18 at 3:36
• Also, why are you doing stripline in 4 oz copper? That's a really strange requirement, and likely to be a cost adder. – The Photon Feb 24 '18 at 3:43
• You probably want your ground plane thickness to match th power plane thickness, so use this 4 oz layer for ground, and put signal on a different, lighter copper layer. – The Photon Feb 24 '18 at 4:21

As another answer says, "1 oz" copper is 35 microns thick or 1.4 mils.

You can ask your vendor if they're actually giving you thinner copper than you spec'ed. Or you can just give them the spec in microns or even in mils. But first check the datasheet for the laminate material from the laminate vendor. If they actually provide 1.2 mil copper thickness, the board fab isn't going to be able to change that.

As for the stripline calculation, the characteristic impedance is only weakly dependent on the copper thickness. Try calculating the Z0 with the correct thickness for your spec, and with the number given by your vendor and if the error in Z0 is less than 5% don't worry about it. For example, I just did an example in Saturn's PCB tool and changing from 4 oz copper to 3 oz changed the Z0 from 50 to 53 ohms.

There are lots of other things like under and over-etching, etch profile, substrate Dk variation, etc., that can cause similar errors and aren't under your control. If really tight impedance control is required, include a test trace in your design and be prepared to check its Z0 on a network analyzer or TDR.

I would tend to 4.8mil because the input to the stripline equations is thickness

Stripline in 4 oz copper is a very unusual requirement. I could imagine in this case the etch profile (the fact that after etching the cross section tends to be trapezoidal rather than rectangular) could cause some additional Z0 errors.

• The actual reason for 4oz copper was that at the other side of the PCB (symmetry) I have a power plane which I want to have as thick as possible. Furthermore, the thicker the TL, the lower the loss! But I do understand your point. Maybe you can add what a "good" copper thickness for a 50 ohm stripline is? – divB Feb 24 '18 at 4:29
• Also, my striplines are currently 10mil and I adjust the dielectric to 40mil to get 50 Ohm. I could increase the width of the trace (for same loss) but this not only makes routing harder but also requires thicker dielectric. And again, due to symmetry I want the dielectric on the other side to be as thin as possible for the power/ground planes. Is there anything wrong with that? – divB Feb 24 '18 at 4:29
• Obviously I don't know all your requirements, but for power handling, stripline or microstrip widths in the 100-250 mil range are not uncommon. Of course that doesn't fly in a high-density design. – The Photon Feb 24 '18 at 5:13

1 ounce/foot square of copper foil (the standard) is 1.4 mils, or 35 microns.