Impedance controlled trace

Hello i trying to route a WiFi chip (CC3200) with an antenna connector.
i using saturn pcb calculator and i decide to go with coplanar waveguide.

In my research on the internet i found that there's many different layer-stackups from manufacturer to manufacturer
and my problem is i don't know what values to use in my calculator.

Is there something standar (4-layer) which used to to manufacturing?

Thanks!

You should be able to email your manufacturer regarding layer stackups or even just mention the controlled impedance and tolerance in the manufacturing notes and have them adjust thicknesses as needed.

If you want to continue the calculator route could you give us an idea what parameters you're struggling with?

There won't necessarily be a standard since the impedance will change with trace and layer thickness, dielectric material, number of layers and all sorts of other things that can vary between manufacturers.

I sent an email to one manufacturer and he inform me that there's no standar stack.

I want impedance control (50 ohm) in just one trace!
The trace of WiFi antenna which goes out from chip to antenna female ufl connector.

The length of that trace would not exceed the 7mm!

I trying to place the connector closer to the chip as possible to avoid the results of impedance mismatching which may be occurs from
manufacturing

For a trace so small you may not even need to worry yourself with controlled impedance but if you want to play it safe I would stick with the Saturn calculator. I just downloaded it myself and it seems very helpful. Which parameters in the Conductor Impedance tab are confusing you? Maybe we can help you figure out what stackup you'll need.

Thank you very much!
I haven't any problem with Saturn Calculator. It is very helpful and simple.
My problem is that i don't know the dielectric thickness. The other parameters is very familiar to me.

And i don't know where i can found the dielectric thickness information.
I asked one manufacturer and he gave me a "standar prototype stack" which he using it but he inform me
that there's no guarantee of using it.


I decide to proceed with this information
http://eurocircuits.com/images/stori...-4-2010-v2.pdf

Usually dielectric thickness is something you're able to specify to the manufacturer if you're using a high end service. If those diagrams are from your manufacturer I would go with them like you said. Even if there are slight variations in the actual product you can use Saturn to see how it would effect your final impedance.

For example changing the conductor height by 2 mil (pretty significant) it only changes your trace impedance less than an ohm with the other default settings.

Thanks for that one
was unaware of that prog


cheers
Dave

Presume you are asking about industry standard 1.55 mm 4-layer PCB stackup. Most manufacturers have a standard stackup for pool manufacturing of prototypes, typical 700 μm up to 1000 μm core and 200 μm to 380 μm prepreg combination for the outer dielectric, mostly in the 350 - 380 μm range. If you design your transmission lines for the latter range, you can choose between many pool services.

Impedance controlled is a different thing than systematically designed impedance, it involves test structures and adjustment of process parameters after impedance measurements. It's rarely needed for general purpose RF design which have a wider tolerance for transmission line impedances, so I guess you are not talking about actual impedance control.



Quite a few constraints can't be avoided if the talk about designed impedances makes sense at all. The cheapest pool manufacturers may be sorted out then, but there should be still many that at least do rely on a standard prototype stackup.