Bug report - buried via annual ring incorrect in outer layer.

[Anonymous]

Hello,

We are making multi-layer PCB in eagle ver. 7.2. We defined 6 layer PCB with buried vias between 2-5 layers. This via should have

diameter 0.5mm on its outer layers (those are 2,5 layers) and 0.3mm on its inner layers (those are 3,4 layer). In properties of via Eagle

shows outer and inner diameter correctly, but all diameters are set as 0.3mm. It seems that Eagle takes outer layer as always 1 and 6.

This is true only for vias 1-6. Burried via diameters should be treated differently. Start and end of that via should be treated as outer, and

rest as inner diameters. 

This bug is still present in ver. 8.4.

I look forward to hearing from you.

Best regars,

Mateusz Spychała

[Anonymous]

Hello,

We are making multi-layer PCB in eagle ver. 7.2. We defined 6 layer PCB with buried vias between 2-5 layers. This via should have

diameter 0.5mm on its outer layers (those are 2,5 layers) and 0.3mm on its inner layers (those are 3,4 layer). In properties of via Eagle

shows outer and inner diameter correctly, but all diameters are set as 0.3mm. It seems that Eagle takes outer layer as always 1 and 6.

This is true only for vias 1-6. Burried via diameters should be treated differently. Start and end of that via should be treated as outer, and

rest as inner diameters. 

This bug is still present in ver. 8.4.

I look forward to hearing from you.

Best regars,

Mateusz Spychała

[jorge_garcia]

Hello Mateusz,

I hope you're doing well. I think you have defined your layers incorrectly and that's possibly why the diameters don't appear properly. Layers should be defined from the outside surfaces towards the center. So for a six layer board it should be:

(1*(2*3*14*15)*16)

This includes the buried vias from layer 2 to 15. I can get away with using all * because the core and prepreg information doesn't currently make it into the gerbers. EAGLE treats layers 1 Top and 16 Bottom special which allows EAGLE to see them as the outer layers. If you don't want to move things around too much the following setup equation would work.

(1*(2*3*4*5)*16).

Try it and let me know if the differences are now respected. The other thing you need to do to be able to verify that the diameters are correct is change the layer colors of the pads and vias layers to be the same as your background. This will render the vias on each layer individually(it'll make sense once you see it).

Let me know if I have misunderstood something.

Best Regards,

[jorge_garcia]

Hello Mateusz,

I hope you're doing well. I think you have defined your layers incorrectly and that's possibly why the diameters don't appear properly. Layers should be defined from the outside surfaces towards the center. So for a six layer board it should be:

(1*(2*3*14*15)*16)

This includes the buried vias from layer 2 to 15. I can get away with using all * because the core and prepreg information doesn't currently make it into the gerbers. EAGLE treats layers 1 Top and 16 Bottom special which allows EAGLE to see them as the outer layers. If you don't want to move things around too much the following setup equation would work.

(1*(2*3*4*5)*16).

Try it and let me know if the differences are now respected. The other thing you need to do to be able to verify that the diameters are correct is change the layer colors of the pads and vias layers to be the same as your background. This will render the vias on each layer individually(it'll make sense once you see it).

Let me know if I have misunderstood something.

Best Regards,

[Anonymous]

Hello Jorge,

Thank you for your help. I'm afraid that we defined layers correctly. Our settings are:

[3:(1+(2+(3*4)+5)+16):4]

That means we can create following types of VIAS.

1. Through hole

2. Micro via layer 1-2

3. Micro via layer 2-3

4. Micro via layer 4-5

5. Micro via layer 5-16

6. Buried via layer 3-4

7. Buried via layer 2-5.

There is no problem with vias types 1-5. Problem we have with VIA types 6 and 7. 

E. g. for buried via (layers 2-5) there are 4 annual rigs generated.

On layers 2,3,4,5. And all of them are treated as inner layers annual ring (small one). 

Problem is that, layers 2 and 5 for this type of buried via should be treated as outer

layer, because in manufacturing process this via is drilled when there is no layers 1 and 6 put together. 

Manufacturer demands that this buried via should have bigger annual ring. 

I hope this time I made is clear. 

Best regards,

Mateusz Spychała 

[Anonymous]

Hello Jorge,

Thank you for your help. I'm afraid that we defined layers correctly. Our settings are:

[3:(1+(2+(3*4)+5)+16):4]

That means we can create following types of VIAS.

1. Through hole

2. Micro via layer 1-2

3. Micro via layer 2-3

4. Micro via layer 4-5

5. Micro via layer 5-16

6. Buried via layer 3-4

7. Buried via layer 2-5.

There is no problem with vias types 1-5. Problem we have with VIA types 6 and 7. 

E. g. for buried via (layers 2-5) there are 4 annual rigs generated.

On layers 2,3,4,5. And all of them are treated as inner layers annual ring (small one). 

Problem is that, layers 2 and 5 for this type of buried via should be treated as outer

layer, because in manufacturing process this via is drilled when there is no layers 1 and 6 put together. 

Manufacturer demands that this buried via should have bigger annual ring. 

I hope this time I made is clear. 

Best regards,

Mateusz Spychała 

[hanakp_BUT]

I believe I've run into this bug, and it's still present in 8.6.3. The problem is that Eagle doesn't properly generate the minimum Annular ring width for buried vias. I've attached a simple example. I set up DRC according to the pictures below - as you can see, both through and buried vias should have minimum 0,3 mm annular ring width. But when you actually create the vias with Route, the buried vias are visibly thinner. However, it's not so simple. If you analyze my example closely, you will notice "Drill Size" DRC errors in the vias - they have 0,4 mm drill, but I set 0,6 mm minimum drill in DRC. When you use Change-Drill and increase the buried via diameter to 0,6 mm or greater, the annular ring suddenly jumps to a correct width. The same happens if you decrease the Minimum Drill value in DRC to 0,4 mm or lower. So, it seems the underlying problem is deeper than Route command.

[hanakp_BUT]

I believe I've run into this bug, and it's still present in 8.6.3. The problem is that Eagle doesn't properly generate the minimum Annular ring width for buried vias. I've attached a simple example. I set up DRC according to the pictures below - as you can see, both through and buried vias should have minimum 0,3 mm annular ring width. But when you actually create the vias with Route, the buried vias are visibly thinner. However, it's not so simple. If you analyze my example closely, you will notice "Drill Size" DRC errors in the vias - they have 0,4 mm drill, but I set 0,6 mm minimum drill in DRC. When you use Change-Drill and increase the buried via diameter to 0,6 mm or greater, the annular ring suddenly jumps to a correct width. The same happens if you decrease the Minimum Drill value in DRC to 0,4 mm or lower. So, it seems the underlying problem is deeper than Route command.

[hudriwudri]

"It's not a bug, it's a feature!"

Or rather, there is a bug, but with out-of-spec micro vias and not with buried vias.

In DRC->Sizes, you have set the min drill for normal vias to 0.6mm, and min micro via to 9.9mm (good). But because your 0.4mm via drill is smaller than both of these values, the DRC error appears (correctly). And Eagle still takes the 2-15 via as a micro via (questionably) and applies the anular ring of micro vias to it. As soon as you increase the drill size to 0.6 or bigger, it is taken as a normal via (without error) with your specified anular ring sizes. The other two vias are not candidates for micro vias, thus they always have the anular ring of normal vias.

Solution/workaround: Set anular ring sizes for micro vias the same as normal vias.

[hudriwudri]

"It's not a bug, it's a feature!"

Or rather, there is a bug, but with out-of-spec micro vias and not with buried vias.

In DRC->Sizes, you have set the min drill for normal vias to 0.6mm, and min micro via to 9.9mm (good). But because your 0.4mm via drill is smaller than both of these values, the DRC error appears (correctly). And Eagle still takes the 2-15 via as a micro via (questionably) and applies the anular ring of micro vias to it. As soon as you increase the drill size to 0.6 or bigger, it is taken as a normal via (without error) with your specified anular ring sizes. The other two vias are not candidates for micro vias, thus they always have the anular ring of normal vias.

Solution/workaround: Set anular ring sizes for micro vias the same as normal vias.

[hanakp_BUT]

Well, in that case, it means that Eagle (also?) incorrectly detects Microvias. Because according to the help text in the Annular Ring menu, it should detect only blind vias as Microvias, not buried vias as in my example.

But this raises another question - if the Microvias even should be limited only to blind vias. Because contemporary high-density PCBs are routinely manufactured with stacked micro vias:

https://epp-europe.industrie.de/technology/products/blind-buried-vias-stacked-microvias-with-laser-d...

I guess it depends on what Eagle programmers aimed to do...

[hanakp_BUT]

Well, in that case, it means that Eagle (also?) incorrectly detects Microvias. Because according to the help text in the Annular Ring menu, it should detect only blind vias as Microvias, not buried vias as in my example.

But this raises another question - if the Microvias even should be limited only to blind vias. Because contemporary high-density PCBs are routinely manufactured with stacked micro vias:

https://epp-europe.industrie.de/technology/products/blind-buried-vias-stacked-microvias-with-laser-d...

I guess it depends on what Eagle programmers aimed to do...

[rachaelATWH4]

---

@hanakp_BUT wrote:

But this raises another question - if the Microvias even should be limited only to blind vias. Because contemporary high-density PCBs are routinely manufactured with stacked micro vias:

https://epp-europe.industrie.de/technology/products/blind-buried-vias-stacked-microvias-with-laser-d...

I guess it depends on what Eagle programmers aimed to do...

---

They aren't currently limited to blind vias and I don't think they should be. I've got boards where I am doing stacked microvias and it works correctly as is. If the microvias were limited to blind only I couldn't have done my boards. I suspect its a case that the documentation needs updating rather than EAGLE being changed in this respect.

Best Regards,

Rachael

[rachaelATWH4]

---

@hanakp_BUT wrote:

But this raises another question - if the Microvias even should be limited only to blind vias. Because contemporary high-density PCBs are routinely manufactured with stacked micro vias:

https://epp-europe.industrie.de/technology/products/blind-buried-vias-stacked-microvias-with-laser-d...

I guess it depends on what Eagle programmers aimed to do...

---

They aren't currently limited to blind vias and I don't think they should be. I've got boards where I am doing stacked microvias and it works correctly as is. If the microvias were limited to blind only I couldn't have done my boards. I suspect its a case that the documentation needs updating rather than EAGLE being changed in this respect.

Best Regards,

Rachael

[Anonymous]

Hello,

I've checked all proposed solutions and ideas and couldn't find solution. 

We have defined layers as follows:

[2:[3:(1+[3:(2+(3*4)+5):4]+16):4]:5]

In my opinion outer annual rings should be there:

 

But in Eagle they are there:

Is this behavior correct?

Best regards,

Mateusz Spychała

[Anonymous]

Hello,

I've checked all proposed solutions and ideas and couldn't find solution. 

We have defined layers as follows:

[2:[3:(1+[3:(2+(3*4)+5):4]+16):4]:5]

In my opinion outer annual rings should be there:

 

But in Eagle they are there:

Is this behavior correct?

Best regards,

Mateusz Spychała

[jorge_garcia · Accepted solution]

Hi Mateusz,

Looking at the picture I now realize that I had misunderstood what you were saying, but the picture makes it fully clear. As far as EAGLE is concerned Outer layers means 1 and 16, inner layers means anything else. So the behavior EAGLE is showing is as designed.

The problem here is that you are expecting out layers to equal the limits of your different via configurations and it just doesn't work that way. I've never run into a board house that needed wider annular rings on the inner layers, did they ask for this? What's the use case?

Best Regards,

[jorge_garcia · Accepted solution]

Hi Mateusz,

Looking at the picture I now realize that I had misunderstood what you were saying, but the picture makes it fully clear. As far as EAGLE is concerned Outer layers means 1 and 16, inner layers means anything else. So the behavior EAGLE is showing is as designed.

The problem here is that you are expecting out layers to equal the limits of your different via configurations and it just doesn't work that way. I've never run into a board house that needed wider annular rings on the inner layers, did they ask for this? What's the use case?

Best Regards,

[Anonymous]

Hello,

We sent our design to manufacturer and they have accepted it, so it seems that this behavior is acceptable. I don't know why they

initially sad us to make bigger "outer" rings in inner layer. 

Thank you for your help. 

Best regards,

Mateusz Spychała

[Anonymous]

Hello,

We sent our design to manufacturer and they have accepted it, so it seems that this behavior is acceptable. I don't know why they

initially sad us to make bigger "outer" rings in inner layer. 

Thank you for your help. 

Best regards,

Mateusz Spychała