Difference between Altium and Saturn PCB Toolkit Impedance Calculation?

[Blue_Alien]

Hello, I am trying to figure out why Altium and the Saturn PCB Design Toolkit disagree on the impedance of a trace.

In Altium, with 1oz copper on the top and plane layers, and 0.127mm of prepreg between them, Er 4.58, it says a 50ohm trace is 0.151mm wide.

In Saturn PCB Toolkit with these same parameters, it calculates the impedance of a 0.151mm wide trace to be 56.99ohms.

I can't find the equation that Saturn is using. It just says that it uses a complex formula, not the simplified formula. The results track Sonnet 3D solver.

[T3sl4co1l]

If you think that's not good enough, you have your choice of three here:
http://www.chemandy.com/calculators/calculator-index.htm
Wadell's gives 57.86, Hartley gives 63.84 and IPC gives 56.31 ohms.

Saturn may well be more accurate.  But none of it really matters as you have to tell the PCB manufacturer what you want, and it's up to them to get it within the stated tolerance. Which is usually something like 10% if you're really picky, and 20% otherwise.

Tim

[czorgormez]

probably altium is adding er 3.5 solder resist coating in calculations. use polar si 8000 or si 9000 for better results.  contact your pcb manufacturer for impedance controlled lines for best result.  because your real prepregs never be a perfect eR 4.58.

[37electrons]

They give different results indeed. Let us know how you've got this issue solved in the end.

I've noticed an error in you data however (which, in fact, makes the difference even greater):
Saturn PCB allows you to set base copper thickness and plating thickness independently. So, according to your picture, when you set base copper weight as 35um AND plating thickness 35um then you essentially calculate impedance for 2oz copper (not for 1oz as you do in Altium). The app shows you this at the bottom: "Total Copper Thickness: 70um".
So in Saturn app it should be set either as '35um base copper + bare PCB' or '18um + 18um' - both variants will mean 1oz copper (finished thickness), however, since internal layers are not plated, they would also mean 1oz internal plane or 0.5oz internal plane correspondingly. See the 'General Settings' section here https://www.saturnpcb.com/toolkit_help.htm for explanation of those options.

Cheers!

[technotronix]

I think the impedance is more accurate in sature PCB. Here I found more details on why sature PCB is more accurate. https://www.saturnpcb.com/toolkit_help.htm

[SPCBD]

Hello, the answer is in the screenshot. The PCB Toolkit uses a complex formula, I've spent quite a bit of time on it.
The formula in the Altium screenshot is the simplified IPC formula but they are also adding in the soldermask.
Your top copper weight is different too.
Regards
Ken

[37electrons]

The PCB Toolkit uses a complex formula, I've spent quite a bit of time on it.
The formula in the Altium screenshot is the simplified IPC formula but they are also adding in the soldermask.

The beauty of  this forum is that you can get an answer firsthand 

From the Altium "Formula Editor" screenshot I cannot see any soldermask-related values used in the formula (although they are provided to AD on the "Layer Stack Manager" screenshot).

Do original IPC formulas allow to take soldermask into account at all? If so, how big is its contribution? (My guess is it must be minor if any).
Would be also interesting to know if Altium uses the Soldermask Dielectric Constant & Thickness anywhere in calculations at all (except the total PCB thickness, obviously).

[Blue_Alien]

Thanks for the replies everyone. I realized after I posted that I had the plating settings off. In the end, I went with the width from the Saturn calculator.