Is it possible to remove some dielectric layers in some area of a PCB?

[ywxwszc]

I have designed a 4 layer RF PCB with coaxial connectors to be the input and output, and now want to remove the connectors and put the antennas directly on the board.

This is the layer definition of the 4 layer PCB:

And this is the layer definition of the antenna, which contains only the first 2 layers of the PCB:


So in the antenna area, now I need to remove the lower 2 metal and dielectric layers. It is easy to remove the metal, but is it possible to remove the dielectric layers? I have never seen such designs before, and haven't figure out a way to do it.

Looking for someone to tell me "yes, it's surely possible" and how.

 

[neena]

hi,

please mention the software you used ?

 

[ywxwszc]

hi,

please mention the software you used ?

Pads layout. It's possible?

 

[senilicus]

You should contact your pcb manufacturer for this. What you are actually asking is the fact that you want controlled depth milling. They can tell you about the possibilities.

 

[ywxwszc]

Thanks for neena and senilicus. I will contact the PCB manufacture.

By considering the gerber file, I don't think this is possible. PCB are manufactured according to gerber files in the end, and gerber files only contain the information for metal layers, silkscreen, paste mask, solder mask, and drill. There is no information about dielectric. It seems dielectric layers are defined by board outline only.

 

[FvM]

By considering the gerber file, I don't think this is possible. PCB are manufactured according to gerber files in the end, and gerber files only contain the information for metal layers, silkscreen, paste mask, solder mask, and drill.

This is a rather simplified idea of PCB manufacturing. It possibly applies to a pool manufacturer. PCBs are made according to the specifications and production data sent to the manufacturer or negotiated explicitely. Also your Rogers+FR4 hybrid PCB would need an additional text specification.

The more interesting question is about the technical limitations involved in the design. senilicus already mentioned miling. But it's rather uneffective to mill large areas, and you'll face problems to set the milling depth exactly. Another option is laminating partial (pre-cut) PCB parts to the final multilayer, sometimes used for flex-rigid PCBs. But you have to contact you PCB manufacturer, respectively ask some of them.

 

[ywxwszc]

Well, thanks for you all. FvM just reminds me to go for more learning;-)
I will contact the manufacture and post their answer here later.

 

[marce]

If the ground layer is going to be contigous under the antenna (forming the monopole reference plane) then any dielectric layers under that should have no affect on the antenna operation, just esure the area is free of copper and tracks. If the ground is not under the antenna (more common) you may be better looking at making the whole PCB thinner, using a thinner dielectric between the power and ground layers, or if possible tweek the length of the antenna to compensate for a thicker PCB.
What frequency band are you using out of interest.

 

[ywxwszc]

What frequency band are you using out of interest.

60 GHz. Thank you for the advice.

 

[marce]

:shock:Wow, thats some frequency, I've only player with little boys frequencies 2.5Ghz and once up in the 4GHz range:shock:

 

[ywxwszc]

Hi everyone, I've got good news for this problem. It is feasible.

Solution to this problem:
Use different board outline for the first two layers and the last two layers when you generate the gerber file.

Solutions to such kind of unusual problems:
Just as some professional players suggested in this thread, contact your PCB manufacturer, they are professional and always provide good service:-D

 

[nelsonys]

I think it's always a constraint for PCB designer in cost-controlled design. Therefore, it is not advisable to have very sophisticated design by requiring "extraordinary" shape, stackup, hybrid PCB (different materials, flex circuit with PCB) which will end up with extra costs in the budget for R&D

Isn't it a good suggestion by Marce that instead of looking for complex board fabrication, might as well tweak the trace width using the current board thickness. I do not know whether it would impose another design or calculation difficulties or at worst, limited board space due to widening of trace width.

 

[taisen]

This is possible. Using a Yag laser for controlling depth is another option besides milling. Milling is pretty accurate and can maintain a depth control of ~+/- .0015 mils. Using a Laser your depth control will be more accurate +/- 12um. The advantage of using a laser to do the milling (laser ablation) is that you can stop on the under lying metal (pad or trace) with out damaging it. I have done this for a customer and it works well for them. The metal thickness below the unwanted material was 9um (1/4 oz). If you have questions feel free to email me. The option of pre removing the material would be more cost effective and can be done as well.