# Impedance Matching: Distance H is to prepreg or to core ?

I have a doubt about something:

Considering a 4 layers PCB where the configuration is as follow: Toplayer / Prepreg / Ground Layer / Core / Power Layer / Prepreg/ Bottom Layer

Do I understand well that when performing impedance matching and width strip calculation on a micro strip on top layer (for an antenna strip for example), the calculation of W should be done using the dielectric constant of prepreg and H of prepreg being just below the top layer ?

When I ask our supplier what is the material used for prepreg and its related dielectric constant, they seems to be confused: one time they say FR4 and send the datasheet, another time they say 2116 but seems uncapable to give datasheet (hence I have no dielectric constan available and prepreg thickness calculation).

The height is the distance between the trace and the ground plane.

If you have a signal on the top layer, and a ground plane after the prepreg layer, it will be the thickness of the prepreg layer.

If the signal is on one side of the core, and ground plane on the other side of the core, then it would be the thickness of the core.

If you have a signal on one layer, and then the ground plane two layers away (e.g. Sig|prepreg|core|plane), then it will be the combined thickness of both.

As a side note, 2116 is an FR4 prepreg material. According to slide 6 of this presentation, it has a dielectric constant of roughly 3.6-3.8, although it seems to vary depending on the number of layers. For two layers, the next slide shows it goes up to about 3.9-4.3 which is about the same as an FR4 core.

I had a quick look, and several PCB companies I found use two layers of 2116 to build up the required thickness. So you can probably work on the theory of it being similar to the FR4 core. However in practice if impedance is that critical, you would make test pieces to measure and characterise the impedance.

• in case there are two layers of 2116, i suppose we just take the dielectric constant and add up the thickness. There is no special formula to apply to calculate dielectric equivalent of two 2116 being stack up. Commented Sep 14, 2016 at 3:54
• @chris they should tell you the thickness of the prepreg layer, in which case just use that value as they will specify the final thickness (if it is two sheets they will tell you the combined thickness) Commented Sep 14, 2016 at 3:56
• The thickness is ok, the problem is the dielectric constant. Commented Sep 14, 2016 at 5:07
• It does not matter how many layers, one, two or five are stacked up - this only defines the overall thickness. The dielectric constant is a property of material, and will be the same regardless of how many layers are used to make the specified H. Commented Sep 15, 2016 at 22:16
• @AliChen Theoretically, yes, but see the linked presentation from Wurth Elektronik. In the case of prepreg it may well make a difference as the Er depends on the glass/epoxy ratio. Putting one prepreg layer on a patterned copper layer could result in a different ratio (as epoxy is squeezed out to fill the gaps) when compared with the material attached to another layer of itself. The weave of the FR4 and how it lines up with two layers vs one may also cause a difference. Commented Sep 15, 2016 at 22:33

If your manufacturer cannot answer the question about dielectric constant of their material, or even when you get to the point of asking this (since it must be published in manufacturing specifications), you need to change your supplier. Normal supplier would publish all these parameters upfront, because designers need this input information to design proper traces.

More, a normal manufacturer would ask you to specify if the design needs controlled impedance or not. If yes, a normal manufacturer will correct your Gerbers - they will increase your trace width by a notch to compensate for their specific over-etch (which is their process-specific).

Still it is highly advisable to add transmission test coupons to your board, maybe several slightly different ones, and measure the resulting impedance, ether to correct the traces on next board spin, or use the impedance information to adjust driver impedance values if supported in silicon in use.

• this is exactly what I was thinking regarding manufacturer. Thank you for confirming. Commented Sep 16, 2016 at 9:51