Altium Layer Stackup For Transmission Lines

[PsychedelicBreakfast]

I'm a bit puzzled by Altium's layer stackup. I emailed my PCB fab. (Gold Phoenix) about substrate height, copper height and the dielectric constant and I was told the following:

   

1.6mm 1oz
Top---------------------------------- 1oz

               PP  7628(0.17mm)

     L2---------------------------------- 1oz

             core  1.2mm

     L3---------------------------------- 1oz

              PP  7628(0.17mm)

Bottom--------------------------------1oz

       1.61mm+/-10%

So I set the top and bottom layer to 1.6mm and the prepregs to 0.17mm and the core to 1.2mm, as shown in the picture below:



But when I try to setup a width rule based on characteristic impedence, I get negative values for the width(!). What am I doing wrong?

[free_electron]

you got something else wrong ...
6.69+6.69+47.2 don't add up to 189 ...

so you got your copper thickness wrong...

[gxti]

The copper thickness doesn't show up directly in that dialog, you have to double-click on each copper layer and verify that it is set to 1 oz (1.4 mils, 0.036mm)

[PsychedelicBreakfast]

Copper thickness as stated in the email is 1.6mm. I set that too, for both bottom and top layer. So 62.9 * 2 mil + 47.244 + 6.693*2 =  186.43. If you add in the gnd and vcc plane thickness, it adds upto 189. The email didn't state anything about the thickness of the gnd/vcc plane (and Gold Phoenix isn't being helpful now) so I left it as default.

[free_electron]

1.6mm copper on the outer layers ? what kind of board is this ?
1.6 mm they mean the total board thickness.
that outer layer copper  is 1oz . i do't kno any pacb house that uses such thick copper on the outer layers... that'll be an trmendously expensive board..

[PsychedelicBreakfast]

1.6mm copper on the outer layers ? what kind of board is this ?
1.6 mm they mean the total board thickness.
that outer layer copper  is 1oz . i do't kno any pacb house that uses such thick copper on the outer layers... that'll be an trmendously expensive board..

You're right. When I set 1.4 mil as the thickness for all the layers, the width came out as about 10 mil for 50 Ohm Zo. I was confused by their figures because they quoted 1.6mm twice, once near the top layer and once near the bottom layer.

Sorry about all the confusion! I appreciate the help.

[free_electron]

you got negative numbers becasue the aspect ratio changed... the trace would have been thicker than it was wide ... and that upsets the calcs...