Why can't I use a micro via

Question

I think I'm being dense!  I have a two layer board, and want to use a "micro-via", but the PCB properties/Copper Layers tab doesn't seem to allow this.
Why?  I want a rectangular spiral inductor on the board, and need a very small via in the centre to get to the back of the board without clashing with the track.
The inductor track is 3 mil, spacing 2 mil, area in the centre to place a via is about 8 mils by 8 mils.
How small will board vendors normally go for via hole and pad sizes?

Answer 1

Hi David,
Micro vias are used in conjunction with build-up layers and are generally blind or burried vias; they connect one or two (maximum) build-up layers to the copper top or bottom.  If you are unable to select this option in the PCB Properties, it is likely that you do not have any build-up layers on the top/bottom of board.  Here are some general steps to follow to place micro vias:
1. Under Options > PCB Properties, check the Micro Vias box found under the Vias Support group (note: you must have build-up layers on the top or bottom of your board.  You can change the number of single layer build-ups on the left)
2. In the Allowed Vias box, select the layers between which you would like to allow micro vias
(If you would like to allow micro vias between more than one layer (maximum of two), you can change the settings in the Pads/Vias tab under Maximum Layer Span.  Make sure to click Apply before you return to the PCB Properties tab)
3. After you have finished selecting the allowable layers, click OK and return to your design
4. Place a via (Place > Via)
5. In the dialog that pops up, select the layers between which you would like the via placed.  If you select a combination of layers that was enabled in the PCB Properties, Ultiboard will automatically know that you would like to place a micro via and will configure the hole size and annular ring based on this.  Now if you double-click on the via that was just placed, the heading of the properties dialog should say Micro Via Properties, which will show you that it you have configured it properly.
If you need a via that goes all the way through the board, I do not believe this fits the actual definition of a micro via.   You should really contact your board manufacturer to find out how small they are willing to go, but based on the IPC-2222 Sectional Design Standards for Rigid Organic Printed Boards, the minimum drilled hole sizes for plated-through hole vias should be at least 0.2 mm, but obviously larger as the thicknesse of the board increases.  And then you also have to take into account the annular ring of the via.
Message Edited by NatashaB on 02-04-2009 11:49 AM
Natasha Baker
R&D Engineer
National Instruments
Join the NI Circuit Design Community
Follow Multisim on Twitter!