Changing normal vias to b lind or burred vias

Karl Lautman wrote:

I'm developing my first 4-layer board in v4.16.  My plan is to prototype it

with Osh Park before doing a pilot run with the final vendor.  For

aesthetic reasons (this is for a piece of functional sculpture), I'd like

the final version to use blind and, possibly, buried vias (so one side of

the PCB will be "unblemished"), but Osh only supports normal ones that go

all the way through.  It's not clear to me from the Eagle docs

 

1.  How to specify which type of via is created when routing on an internal

layer, or

 

2.  How to change a normal via to a blind or buried one later. 

 

Any tips on either or both of these issues appreciated.  I'm wondering how

big a chore it's going to be to go back and change all the normal vias for

the production version.

first you need to configure the stackup in tools/DRC/Layers

than you can use "change layer" or the info dialog to modify the vias

after the fact, and the middle mouse contect menu during routing.

--

Lorenz

On 23.09.2016 01:04, Karl Lautman wrote:

I'm developing my first 4-layer board in v4.16.  My plan is to prototype it

with Osh Park before doing a pilot run with the final vendor.  For

aesthetic reasons (this is for a piece of functional sculpture), I'd like

the final version to use blind and, possibly, buried vias (so one side of

the PCB will be "unblemished"), but Osh only supports normal ones that go

all the way through.  It's not clear to me from the Eagle docs

1.  How to specify which type of via is created when routing on an internal

layer, or

 

2.  How to change a normal via to a blind or buried one later.

 

Any tips on either or both of these issues appreciated.  I'm wondering how

big a chore it's going to be to go back and change all the normal vias for

the production version.

Blind vias are vias you dont see, cause they are internal only, in your

case between layer 2 and 3. They normally need microvias between L1-2

and in your case, maybe between L3-4 too.

I'm not sure if I understand you, but if you want it to be "free of

holes", there are easier and cheaper ways than using blind vias.

1-If there is nothing on the board but hole mounted components, you can

just add two outer layers of nothing. A 6 layer board may be cheaper

than what you are trying to do. You will also get some artistic freedom

to draw art on the outer layers

2-Just fill the vias with solder.

3-Stop filled holes, make the diameter as small as possible, and

under DRC->Masks, set the "Limit" parameter larger than your via drill

parameter to make eagle remove stop mask over them. Also talk to your

manufacturer to make sure they can fill them. The end result will not be

as flat as when using 2 or blind+microvias, but sufficient to keep

dirt/humidity out.

4-Copper filled vias. You need to find a manufacturer that can do that

and actually talk to them about it. If your design has PAD's, you need

to make your own CAM file to output VIAs in a separate file, so they

don't fill your PADs too.

Lorenz:  If I start routing a trace on the top layer and then center-click

to move it to the 2nd layer, will that via be a blind via or regular via?

If blind, how do I make it regular, and vice-versa?  As far as I can tell,

changing layers only works on traces; corresponding vias get changed

automatically, but you can't change them directly.

Morten:  I want to end up with one side containing only solder mask:  no

holes (filled or otherwise) or even traces beneath the mask.  The other

side of the board will contain all the circuitry in surface mount packages,

connected via traces on this side and the two inner layers (both of which

will be signal layers). 

1.  What do 6 layers get me that I can't get with 4?

2.  These would still be visible where they penetrated the mask.

3.  Won't this cause the mask to cover everything, including pads I need to

solder to?

4.  Same problem as 2.

--

Web access to CadSoft support forums at www.eaglecentral.ca.  Where the CadSoft EAGLE community meets.

On 23/09/2016 11:04 a.m., Karl Lautman wrote:

I'm developing my first 4-layer board in v4.16.  My plan is to prototype it

with Osh Park before doing a pilot run with the final vendor.  For

aesthetic reasons (this is for a piece of functional sculpture), I'd like

the final version to use blind and, possibly, buried vias (so one side of

the PCB will be "unblemished"), but Osh only supports normal ones that go

all the way through.  It's not clear to me from the Eagle docs

 

1.  How to specify which type of via is created when routing on an internal

layer, or

 

2.  How to change a normal via to a blind or buried one later.

 

Any tips on either or both of these issues appreciated.  I'm wondering how

big a chore it's going to be to go back and change all the normal vias for

the production version.

 

Thanks.

 

Hi

You may not need to do much with the design.

Your prototype is a two sided core. If the board house attaches another

core to it with pre-preg, hey presto, you have what you need. In this

stack-up you are using layers 1 and 2 and nothing on 15 and 16.

So you only need to change all vias to a depth of 1-2

HTH

Warren

Warren:  That's a good idea.  I'll ask the board house if they can do that,

though I'd still like to know how to control blind/buried/regular vias.

Karl

--

Web access to CadSoft support forums at www.eaglecentral.ca.  Where the CadSoft EAGLE community meets.

On second thought, I don't think that will work, Warren.  There actually

ARE some vias (pads, actually) that I need to go all the way through, it's

just that they'll be covered by some components (display modules) that

connect to them on the "unblemished" side so you won't see them.  This side

has these modules and nothing else.  Forgot about that. 

--

Web access to CadSoft support forums at www.eaglecentral.ca.  Where the CadSoft EAGLE community meets.

On 24/09/2016 8:28 a.m., Karl Lautman wrote:

On second thought, I don't think that will work, Warren.  There actually

ARE some vias (pads, actually) that I need to go all the way through, it's

just that they'll be covered by some components (display modules) that

connect to them on the "unblemished" side so you won't see them.  This side

has these modules and nothing else.  Forgot about that.

 

As always

You will only receive applicable suggestions if the OP takes the time to

provides accurate descriptions in the first instance.

Good Luck

Warren

Am 23.09.2016 um 19:21 schrieb Karl Lautman:

If blind, how do I make it regular, and vice-versa?  As far as I can tell,

CHANGE VIA, if I'm not misunderstanding you.

Rene

Rene:

Got it.  Had my Setup wrong on Layers.  Thanks.

--

Web access to CadSoft support forums at www.eaglecentral.ca.  Where the CadSoft EAGLE community meets.