Questions on stackup from Lesson 8 of "Schematic and PCB Design Course"

[Tom Yunghans]

Hi Robert,

In Lesson 8 you showed a list of standard vendor PCB material thicknesses you should choose from if you are building your own stackup. You also presented a proposed stackup from a PCB vendor. I have the following questions:

1. The PCB vendor specified a number of materials for the stackup which are not on your list of standard materials (e.g. there is no 60um or 80um prepreg or 0.1mm core on the standard list). Why is the vendor not specifying "standard" materials?

2. Why are some of the "expected thicknesses" on the vendor stackup greater than the nominal material thickness and some are less? (e.g. the expected thickness of the 100um prepreg is 114.7um while the expected thickness of the 180um prepreg is 147.8um).

3. According to the vendor stackup, if you wanted a 72 ohm differential impedance on the outside layer, you would need a 0.145mm etch and a 0.120mm space between the pair. However, if you placed differential pairs with 0.1mm etch and 0.1mm spacing, as was the case with the VOIPAC processor module, you might have trouble making that change without collisions with other objects. Should you be getting this feedback from the vendor on the stackup before you start laying any tracks?

4. Why aren't there impedances shown for layers 6 and 7 in the vendor stackup table?

Thank you, Tom

[robertferanec]

Hi Tom,

1) Some materials will enable you to make your tracks smaller or they are better for high quality high impedance tracks or make it possible to place GND plane closer to your signal layer ... all because of different properties of the materials e.g. Er. So, some manufacturers offer also other types of materials, so you can meet special requirements for you stackup.

2) When PCB is made, it is put into oven, heated up and pressed. Pressed Prepreg melts and it flows between tracks - that all can make real thickness smaller.

3) Ideally for differential pairs you may want to use the initial values like 0.1mm track / 0.2mm space / 0.1mm track (or even bigger if you have space). In reality that can make preliminary routing hard so I often use 0.1/0.1/0.1 but I am aware that I may need more space.

Yes, if you can get PCB feedback before starting layout that is great, in reality it can take some time and it can slow down you design process (you will not be routing until you do not have final answer from PCB manufacturer). So starting to route with some initial values and then adjusting the values is often very helpful.

4) There are no impedance controlled tracks routed, so I didn't ask them to calculate it.

Hope this helps.