Saturn PCB Toolkit vs aisler.net impedance calculation

[TomS_]

Hi all,

Over the years Ive heard so many people sing praises for the Saturn PCB Toolkit, so I decided to download it and try it out to confirm some design parameters for a PCB that I am working on.

I am targeting a 4 layer board from aisler.net, who provides some trace width/spacing for their board for 90ohm differential pairs (my board will have USB 2.0 diff pairs on it).

I laid out my traces according to what the manufacturer supplied on their website, and later in the process I decided to chuck the same figures into Saturn PCB Toolkit just to verify they were correct.

The problem: Saturn PCB Toolkit gives me an impedance of around 81ohm with the same trace width/spacing.

Aislers web page with their stackup and impedance calculations: https://community.aisler.net/t/4-layer-1-6mm-enig-design-rules/3733#p-6035-stackup-16

Attached is a screenshot of Saturn PCB Toolkit showing the results I get. Other than entering in the width, spacing and height, and tweaking Er to match what the manufacturer specifies, I really don't know what the rest of the fields are in this tool. A little bit of experimentation didnt seem to change anything really, so .. 

Can anyone help me understand why there is such a vast difference between the two? Is Saturn PCB Toolkit wrong? Have I entered the wrong figures? Is the PCB manufacturers website wrong? KiCad's built in calculator gave me pretty much bang on 90ohm for the same basic calculation...

81ohm would be on the lower limit of the USB 2.0 spec which allows +/- 10% tolerance for impedance. And as someone else pointed out, USB 2.0 often runs over 0.1" pin headers and ribbon cables that arent close to impedance controlled, so it would seem like maybe a just-in-spec diff pair on a PCB would "just work anyway", but it would be nice to have the impedance as close to ideal as possible.

I have asked the question to Aisler directly, but I'm still waiting for their response after a few days now, so trying my luck here.

Thanks!

[nctnico]

IME the problem is that the 'rule of thumb' formulas as used by these tools don't work well with thin dielectrics. Field solver based programs give better results.

[thm_w]

As you said, either one will work fine. If Aisler is producing it, I would use their calculation.

https://www.reddit.com/r/Altium/comments/1h8pe6o/big_difference_between_jlc_and_altium_impedance/
https://electronics.stackexchange.com/questions/669162/unexpected-low-characteristic-impedance-using-the-jlcpcb-impedance-calculator

[TomS_]

I (finally) got a response back from the PCB manufacturer, albeit only a week after I received my PCBs (made to their specs), assembled and tested (and it works, although I have no means to verify it). 

Their reply indicates they used a field solver, and the Saturn PCB Toolkit didnt account for the soldermask.

So at the end of the day, Saturn PCB Toolkit is not the silver bullet I thought it to be, and it is best to get your answers from the manufacturer.

[Gerhard_dk4xp]

JLCpcb's calculator seems to be right on spot. I checked their
el-cheapo 4 layer process against a TDR.
Without controlled impedance option for the board.

<     https://www.flickr.com/photos/137684711@N07/53780597885/in/datetaken/      >

and some pics to the left/right. I think I have published that ~here already.

Cheers, Gerhard

[asmi]

So at the end of the day, Saturn PCB Toolkit is not the silver bullet I thought it to be, and it is best to get your answers from the manufacturer.

That is always the best idea as manufacturer knows their process the best. "Talk to your manufacturer" (C) Zack Peterson of Altium

[free_electron]

Ask the manufacturer.

The problem is they apply their own secret sauce. Buttercoating , planarisation, pressout, glass weave, resin content, glass type . it all throws a spanner in the works.

You need to know your materials and what they will be like AFTER PROCESSING. Don't go by the material datasheet. Those numbers are BEFORE processing.
Depending on the number of lamination cycles and the buttercoat/planarisation the end thicknesses can be 10 to 15% different from spec.

The manufacturer knows what the end results are because they insert test-coupons in the panels they run. They do cross-cuts to measure actual layer thicknesses as part of their process control. They also measure the coupon structures. so they can give you real numbers. They will typically propose you a stackup that they frequently run in their shop and know well. If you really must have something customized then all bets are off and you need to run a test stack.

Last word of advice : be very careful with dK numbers... The factories typically measure those at 10GHz. dK is NOT a constant over frequency and for many applications you need to get the numbers at different frequencies.

Other issues are etchback. The crosscut of a trace is a trapezoid. The factories will compensate your gerber for etchback. You can get those numbers. If you use Altium you can enter that in the controlled impedance settings. Altium uses the Symbeor engine and that thing is spot on