FEDEVEL
Platform forum

Raza Parvi , 07-31-2019, 12:33 AM

Hello @robertferanec , I have recently downloaded the OpenRex Altium design and trying to learn from this project. In order to get to know how impedance is calculated, I put every details given in the mechanical file into three different software namely Saturn PCB Design Inc, Polar Si9000 PCB transmission and Altium's built-in impedance calculator. The calculated impedance , say for 100 ohm, are different in each software. Would you please guide me which software should I use when calculating impedance. If you see any mistake somewhere during these calculation please mention it. Screenshots are hereby attached.

robertferanec , 07-31-2019, 08:17 AM

Software will only give you approximate values - PCB manufacturer needs to send you the values which you should follow.

When they manufacture PCB some values may change e.g. prepreg can squeeze and only the PCB manufacturer knows how they need to adjust the stackup to get the impedance values they are targeting - means even if you put values what you get from PCB manufacturer into a calculator, you may not get the exact numbers what will be achieved after manufacturing.

I attached the original file for OpenRex, hope this helps.

Raza Parvi , 08-01-2019, 04:54 AM

Thanks Robert for your quick reply.

So that means, after placement and before start routing, we need to contact the manufacture in the first place. Upon receiving the layer stack-up information that conforms the required impedance, one should start routing and finalize the board. In that case, the designer does not need to bother about the Impedance calculations as is done by manufacturer right.Or, we can calculate a close value first and later change it a bit according to manufacturer stackup?

robertferanec , 08-02-2019, 07:23 AM

Usually I use wider tracks for whole layout e.g. 0.1mm and by the end of layout when I have all the info I will adjust the track width to meet the spec (I make the tracks smaller e.g 0.08mm for 50OHM). Of course, you need to be sure, that the final track width will be smaller as the width which you used initially.

This approach has couple of advantages e.g. the track width can be easily adjusted between different PCB manufacturers and stackups as there is always enough space between tracks (one PCB manufacturer may use 0.09 for 50OHMS, other can use 0.08mm and there is no problem). Also, when I make width of the track smaller, this will increase clearance (gap / space) between tracks and it helps to improve crosstalk results.

For differential pairs I often initially use 0.1 / 0.1 / 0.1mm (track / space / track) but after impedance adjustment this usually needs a little bit of more space.

Of course, these are just approximate numbers you need to use your own number - depends how expensive your PCB is going to be (e.g. for cheaper PCB you may want to route by 0.3mm or 0.2mm and go down to 0.15mm).