via size (PCB) and impedance control

[xzswq21]

Hello
I'm designing a 4-Layer PCB. when I place a via in the Altium Designer, the via size has two options:
Hole Size: 0.3mm
Diameter: 1mm

but when I want to check the inductance and the current, the formulas are in term of the Diameter and the Height and the via platting thickness!

could please help me to understand this puzzle?!

is it right? via platting thickness=Diameter-Hole Size??

I'm using the below PCB toolkit software:
http://www.saturnpcb.com/pcb_toolkit.htm

Best Regards

[Philfreeze]

The via height is basically the thickness of your FR4 board (plus a bit more because of the platting process).
The diameter of the via is the diameter of the copper part of your via.
The hole size is the diameter of the hole in your via or to be more accurate, the drill bit they will use to drill this hole.
After they drill the hole they then plate the holes (so that one side is electrically connected with the other side) which adds a small amount of material to the inside of the hole, effectively making the hole smaller.

The manufacturer cares about the actual copper diameter (included in the gerber files) and the drill bit he has to use (included in an NC-Drill or similar file). Some manufacturers are able to make via with a hole size smaller than the platting thickness but usually I would not recommend it as it can lead to a higher resistance between the two layers (not enough copper in there).

If you set the hole size in Altium Designer to 0.1mm, the diameter to 0.3mm and the board is platted with 35um (1.4mil / 1oz) copper you will end up with the following:
a copper pad with a diameter of 0.3mm inside which is a platted hole where the platting has a thickness of 0.035mm and the finished hole has a diameter of 0.03mm (0.1mm - 0.035mm*2).
Though platting inside vias is usually not as precise in small vias as it is in big vias so the actual diameter might vary a bit.



Disclaimer: I am by no means an expert, which is why I will not recommend any via sizes.

[chrisl]

There are many variables to determine the most optimum settings.

However, most fab houses will not complain if you use 12 mil drill with 22 mil pad size VIAs and 6 mil trace width/ 6 mil spacing for you design.
More detailed info is required if you want more optimum setting...  i.e. stackup, the pitch of the devices.. etc.

[Rerouter]

Unless your using a special process via plating thickness is generally half your board copper thickness, e.g. a 1 Oz board begins as a 0.5 Oz board, they then put it through some chemical baths so the copper can plate to the via hole walls, then plate the entire thing with another 0.5 Oz of copper, making a 1 Oz board with 0.5 Oz via thickness

Because Via's are plated on in an electroplating bath your minimum hole size is determined by the board thickness, you generally don't want your holes smaller than 1/8th of the boards thickness, as the plating solution will struggle to make it down to the center of the hole, where this happens you can have the plating plug on one or both sides and leave a void in the center of the hole.

1/4th board thickness is for high reliability stuff, the chance of a hole voiding with that aspect ratio is almost 0,

because they are formed by a plating process, there thickness is not uniform, in general they will be thicker towards the edges, and thinner towards the middle. a 1/4 hole will be highly uniform, a 1/8 much less so,

If you do want to impedance control your via's focus more on how far you pull back your ground planes from the pads, and place return path vias spaced correctly to define it,

[xzswq21]

Unless your using a special process via plating thickness is generally half your board copper thickness, e.g. a 1 Oz board begins as a 0.5 Oz board, they then put it through some chemical baths so the copper can plate to the via hole walls, then plate the entire thing with another 0.5 Oz of copper, making a 1 Oz board with 0.5 Oz via thickness

Because Via's are plated on in an electroplating bath your minimum hole size is determined by the board thickness, you generally don't want your holes smaller than 1/8th of the boards thickness, as the plating solution will struggle to make it down to the center of the hole, where this happens you can have the plating plug on one or both sides and leave a void in the center of the hole.

1/4th board thickness is for high reliability stuff, the chance of a hole voiding with that aspect ratio is almost 0,

because they are formed by a plating process, there thickness is not uniform, in general they will be thicker towards the edges, and thinner towards the middle. a 1/4 hole will be highly uniform, a 1/8 much less so,

If you do want to impedance control your via's focus more on how far you pull back your ground planes from the pads, and place return path vias spaced correctly to define it,

Dear
I want to have impedance control.
there are two ground traces around the signal trace and a ground plane under the signal trace.
the thickness of the Board is 1.575mm so I should use 2.95mm trace for the signal trace.
Which size of via should I use to have 50 ohm impedance?
in my design I want to use via as follow: 0.3mm hole size and 0.6mm diameter.

[Maarten Baert]

Dear
I want to have impedance control.
there are two ground traces around the signal trace and a ground plane under the signal trace.
the thickness of the Board is 1.575mm so I should use 2.95mm trace for the signal trace.
Which size of via should I use to have 50 ohm impedance?
in my design I want to use via as follow: 0.3mm hole size and 0.6mm diameter.

Can you post a screenshot of what you are actually trying to do? Because this doesn't make a lot of sense. If you have a 4-layer board, the distance from the track to the ground plane should be much less than 1.575mm, so I suspect that you are not calculating the impedance correctly. Depending on the type of buildup (ask your manufacturer) the thickness will probably be somewhere in the range of 0.25mm to 0.5mm. So your trace should be about 0.5mm to 1mm wide if it was a regular microstrip. If you also have ground traces on either side, that's called a 'coplanar waveguide with ground', which requires an even smaller track width.

Via size is not the only thing that will determine the impedance, there are many factors to consider:
- Hole diameter (higher diameter = lower inductance, lower impedance)
- Pad diameter (higher diameter = higher capacitance, lower impedance)
- Spacing between via and the hole in your ground plane (higher spacing = lower capacitance, higher impedance)
- Board thickness (higher thickness = higher inductance (via) and lower capacitance (pads), higher impedance)

Via plating thickness is pretty much irrelevant. You could even fill the via completely with copper, it's not like there's going to be any significant electromagnetic field on the inside of the via.

If you really want to accurately calculate which dimensions you need to use to maintain an impedance of 50 ohm, you will have to model the entire thing in a 3D electromagnetic simulator like CST or HFSS. In practice very few people bother with this, because:
- For most applications, the mismatch caused by a via isn't significant.
- For those applications where it is significant, you generally try to avoid vias in RF signals entirely.

What kind of frequency are we talking about here? These things usually only become relevant if you are really dealing with RF signals in the GHz range.

[Rerouter]

Sorry, took a while to find this thread again,

To maintain 50 ohms, with your current via size, you would want a 0.3mm hole, a 0.6mm pad, and a ground plane opening diameter of 1.08mm (clearance)

This is all stuff available on the free "saturn pcb toolkit", you would then want to space 3 or so ground via's around this via so that there pads line up with the edge of the clearance, this will provide a path for the return current to pass.