topic Re: Setting up 4 layer PCB in EAGLE Forum

Setting up 4 layer PCB

diegoaSHQYX — Wed, 31 Jan 2018 17:54:20 GMT

I'm trying to setup a 4 layer PCB. The catch is I can't have any vias going from layer 1 to 4. So I need to be able to have vias between 1 and 2, 2 and 3, and 3 and 4.

I thought it would be like this: [2:(1*2)*(15*16):15]. But when I create a via, I only have the option of 1-2 and 15-16. How can I get 2-15 to be an option? Thanks.

Re: Setting up 4 layer PCB

jorge_garcia — Wed, 31 Jan 2018 22:12:44 GMT

Hi @diegoaSHQYX,

I hope you're doing well. Your setup is a little redundant using the parentheses you have duplicated the blind vias you defined on each end of the setup equation. What you are going for is:

[2:1*(2*15)*16:15]

Please let me know if there's anything else I can do for you.

Best Regards,

Re: Setting up 4 layer PCB

C.Nicks — Wed, 31 Jan 2018 22:18:54 GMT

You may want to check with the shop you're planning to have fab the boards to make sure they can make the drill stackup. Both blind and buried vias are cost drivers that can make boards very expensive.

Re: Setting up 4 layer PCB

diegoaSHQYX — Wed, 31 Jan 2018 22:40:23 GMT

Thanks @jorge_garcia. I see the via settings. However, on the manufacturing tab when I look at the PCB, I still see the vias going through the PCB when layers 1-2 have been selected.

Not sure if it matters, but I've imported 2 design blocks. 1 block I've added to layer 15-16. Those vias are correct. The other block is on layer 1-2, but I see the vias on layer 1-16 on the 'New' Manufacturing tab.

Re: Setting up 4 layer PCB

jorge_garcia — Thu, 01 Feb 2018 20:19:59 GMT

Hi @diegoaSHQYX,

I hope you're doing well, would you mind posting some screen shots of what you are seeing? What really concerns me is that you are seeing 1-16 vias can you show both the Preview tab and Drills tab of the manufacturing flyaway?

Let me know if there's anything else I can do for you.

Best Regards,

Re: Setting up 4 layer PCB

diegoaSHQYX — Fri, 02 Feb 2018 03:14:43 GMT

@jorge_garcia,

I hope this shows what I'm explaining. The PCB shows vias on layers 1-2. On the preview, I'm on the bottom side (15-16), yet I still see holes. The concentration of vias on the left-ish side of the preview are the same vias being shown on the PCB.

The same with the couple rows on the top of the preview. Those are on layers 2-15.

I also don't see a way on the preview to view the layers in between? Maybe this is being shown like this on purpose?

Re: Setting up 4 layer PCB

matt.berggren — Fri, 02 Feb 2018 04:09:02 GMT

Thanks for the question! I would also add to Cameron’s comments that this stack up can be an issue depending on the board house and layup. If the inner layer (between 2&3) is prepreg, this cant (generally) be drilled separately, which will mean you can’t do buried vías like this. If the top / bottom layers are impedance constrained, that can also be an issue because core thickness can be much thicker than thinner prepregs and and thus much harder to achieve reasonable trace widths. (And the use of prepreg is out when doing the top to layer 2 for blind vías.).

...Just a little food for thought. I’m sure you’re thinking about all of this (most people with the need for blind and buried vías have a solid understanding of the issues, so please don’t take offense) but worth a call to the board house if you haven’t already to confirm they can achieve what you’re after.

A nice article for Eurocircuits on layup and blind / buried vías here:

https://www.eurocircuits.com/blog/blind-and-buried-vias/

Best regards,

Matt - Autodesk

Re: Setting up 4 layer PCB

jorge_garcia — Fri, 02 Feb 2018 17:21:23 GMT

Hello @diegoaSHQYX,

I hope you're doing well. This is a current limitation of the manufacturing preview, it currently doesn't handle the inner layers well. We thought it better to release the first version of these features than to hold them back and wait for them to be perfect.

"Continuous improvement is better than delayed perfection" Mark Twain

Let me know if there's anything else I can do for you.

Best Regards,