Can prepreg layer be as thick as the core layer?

[treez]

Hello,

Is the only purpose of prepreg to act as a cheap separator for the copper layers of a PCB?

Is it true that we would ONLY use prepreg (and no core material) if the prepreg was a bit more sturdy and rigid?

So can we conclude that in any given PCB, no matter how many layers.....only ONE layer of rigid FR4 core is ever needed.?

....all other separators can be cheap prepreg?

Is it true that prepreg is cheaper than FR4 core material?

How do the layers (whether core or prepreg) of a PCB get glued together?.......what type of glue is used?......or is it the prepreg itself which provides the adhesion?

How soft is prepreg?.....is it simpy not possible to make, say, a single sided PCB on a layer of prepreg?

I've googled all the above, though google is not elaborating....the links seem to assume the asker already has trade knowledge of prepreg.

 

[Alan0354]

I am not a fab expert, but I don't think there is limitation on the thickness on the prepreg. You can use more than one prepreg. Far as I understand, prepreg is just a layer with no cladding. eg. If I do a 4 layer, you put the prepreg layer between two double clads. I can specify how thick I want the middle prepreg.

But as I said, I am on the engineering end, not the fab end. I don't think the thickness of each dielectric layer affect the cost much, mostly is the number of layers.

 

[treez]

Thanks Alan,

Youve smashed one of my misconceptions because i thought prepreg could have copper coating.

So for a four layer board, i must have two double sided clad boards, and put prepreg in between them?

For a four layer board, can i not have one central layer of FR4 (double sided copper) , with two copper coated prepreg layers on the top and bottom, each coated with copper?

...and by the way, does prepreg have low thermal conductivity?, because it would be excellent if it had, because you could have thermal vias going down to it, and use it to disperse heat ?......does this happen?

 

[Alan0354]

I am not comfortable in answering these fabrication question. I can only based on my experience with the Dupont flex circuit to comment these:

They only comes with double sided cladding, so it's just natural to put the layer with no copper in the middle. I don't know what kind of cladding and prepreg FR4 comes, it all depends on the available thickness.

I never heard people worry about the cost on different combination of cladding and prepreg, only on how many layers and different drill size and number of drill holes. We only worry about the Dupont flex circuit because their availability is not as broad and I had to play tricks to get certain dielectric thickness. But then again, I am the end user only, I specified the thickness and pay for it!!!

 

[FvM]

Prepreg has a specific function in multi-layer PCB. The full name is preimpregnated bonding layer, which should already answer part of your questions.

If you are interested to understand the possible ways to combine copper-clad laminates, prepreg layers and copper foils to multi-layer PCB, you should study the PCB stack-ups published by PCB manufacturers. For standard designs, there aren't much reasonable variations options, except for selecting different layer thickness. This is mainly interesting for impedance design, in some cases also for dielectrical strength.

German PCB manufacturer Ilfa has documented many multilayer construction types on their internet site. You'll notice that all listed 4-layer PCB are exclusively "single core" desgns, menas one copper-clad laminate is combined with prepregs and copper foils.

 

[treez]

Thanks FvM, that was a useful site with good diagrams.....though i could not see the explanation as to why sometimes they use three separate 0.06mm prepreg layers, and sometimes they use one 0.18mm prepreg layer.

As you say, impedance design is a factor, but this only applies for High frequency RF circuits.

So basically it looks to me that one should just use a thin-as-possible layer of prepreg with low fequency circuits?

.......for a 4 layer PCB, it would be best to just glue together two double sided FR4 cores.........however, the glue may not flow to all parts of the PCB, and so it looks to me that this is the reason they use prepreg, because it acts as an insulative separator for the various copper layers.

Also, i suspect that prepreg responds very well to glue, and so enables the copper layers to be glued "together", keeping the vias in line.

I wonder why a double sided PCB would not simply use a single layer of prepreg with copper either side of it.

I also wonder if prepreg comes in high thermal conductivity compounds?, which would help immensely in conducting heat away from SMT packages.


For a four layer PCB with through vias, it sounds incredibly complicated to ensure that the vias "line up" throughout the four layers.......i mean, the central FR4 core, and both outer prepreg layers need to be exactly lined up with respect to the vias, and this cannot be easy

 

[FvM]

You'll usually start to think about PCB stackups, and e.g. prepreg types, if you want to achieve something special. This isn't the case for most standard designs and I guess for your's neither. Nevertheless it's good to understand PCB fabrication basics even if you only refer to standard stackups offered by manufacturers.

The main difference between substrates and prepregs is that the resin filling of prepregs is "precured" epoxy, it's still malleable and starts to flow in the lamination press. Dielectric and thermal properties of both are similar, although not identical due to different glass-to-epoxy ratio.

In most cases, at least two prepreg layers are layed on top of each other to avoid possible pinholes that might endanger the dielectric strength. This is particularly important for higher voltage ratings and specified in some safety rules.

You are also right that adjusting the layer position isn't easy. Besides standard techniques known from other industries like register holes and pins, some manufacturers are using X-ray to check the exact position.

I hear several misunderstandings about PCB fabrication in your post, I can't comment all details in a short answer.

Some points should become obvious if you study the details of the galavanic process. You'll see, that the inner and outer copper layers are produced partly different. While inner copper layers are structured subtractive (etched), the outer layer process starts with additive copper deposit on top of a thin base copper layer, making both via metallization and the final weight of outer layer copper. It would be unsuitable to use a substrate with same copper thickness on both sides for inner and outer copper layers as well. Thus 4-layer boards are usually not made by bonding two double-sided substrates.