Welcome to EDAboard.com

Welcome to our site! EDAboard.com is an international Electronic Discussion Forum focused on EDA software, circuits, schematics, books, theory, papers, asic, pld, 8051, DSP, Network, RF, Analog Design, PCB, Service Manuals... and a whole lot more! To participate you need to register. Registration is free. Click here to register now.

Register Log in

Via-In-Pad or Via-Next-To-Pad - which is best?

Status
Not open for further replies.

reshaping

Newbie level 1
Joined
Jan 16, 2003
Messages
0
Helped
0
Reputation
0
Reaction score
0
Trophy points
1,280
Activity points
140
Which has the minuimum inductance for a decoupling cap:

1. Blind via-in-pad with via diameter of 0.15mm finished,
extending from layers 1 to 5 in a 6-layer board, OR

2. Tracking to an immediately-adjacent 0.7mm pad, 0.3mm
finished blind via,extending from layers 1 to 5 in a 6-layer
board?
 

zgx

Member level 1
Joined
Feb 25, 2002
Messages
38
Helped
1
Reputation
2
Reaction score
0
Trophy points
1,286
Activity points
162
the inductance is related to the track width and length, vias diameter and depth. the good method is using EDA software to design.
 

loki

Junior Member level 3
Joined
Jan 12, 2002
Messages
27
Helped
0
Reputation
2
Reaction score
0
Trophy points
1,281
Activity points
276
suggestion

You'll generally get better results using the microvia in pad method. Blind vias seem like an expensive option. Don't really know what manufacturers can handle blind microvias.

You may be better off adding a couple of additional ground planes for the additional cost of the microvias and blind vias.

General notes to try to ween you away from blind vias.
Is you're design above 500 MHz, whats are the fastest signal rise times your design is looking at? Are you having problems in the 50 -200 MHz range for EMI?
Use the smallest package size cap (low ESL) since the most inductance is going to be from the cap teminals.
Good multiple solid signal return planes with thin laminate between them and the signal planes will help contain the high frequency return signals!
Try to determine the return paths of your signals and avoid plane jumping of critical high speed signals.
 

Beepster

Advanced Member level 4
Joined
Jul 21, 2001
Messages
118
Helped
8
Reputation
16
Reaction score
2
Trophy points
1,298
Location
unknown
Activity points
787
Anything bigger than a microvia will suck all the solder off the pad and down the hole.

Filled vias (where the vias are plated solid -no hole is left) are very expensive. Don't do it !
 

homan

Junior Member level 1
Joined
May 31, 2001
Messages
16
Helped
0
Reputation
0
Reaction score
0
Trophy points
1,281
Activity points
43
good info. web page.
 

brmadhukar

Advanced Member level 3
Joined
Jun 21, 2002
Messages
840
Helped
42
Reputation
84
Reaction score
11
Trophy points
1,298
Location
India
Activity points
6,783
Hi,
The frequency is important. Assuming a hi frequency, the placement of bypass capacitors becomes important. For analog ICs the bypass capacitors need not as close to the pin as for digital IC or pins. dI/dt matters. For HF the pin capacitance also matters.
 

prouddad_1

Newbie level 4
Joined
Mar 5, 2003
Messages
6
Helped
0
Reputation
0
Reaction score
0
Trophy points
1,281
Activity points
80
Important consideration when using via in pad.

An important thing to consider when putting a via in pad:

If this is a first time design with no bugs discovered, there is very little you can do to fix or modify the board if the via is located in the pad. If you can afford the space I would recommend putting the via offpad incase rework is needed to debug the board. Once the design is stable via on pad is fine provided the via is small due to the reason mention earlier.
Large via will suck solder into the via compromising pin contact to pad.
 

Hero

Full Member level 2
Joined
Mar 6, 2002
Messages
145
Helped
4
Reputation
8
Reaction score
2
Trophy points
1,298
Activity points
1,608
Hi,

Don't forget cost, fabrication and testing problems. Standard via is cheaper than microvia. If you need low cost not too high density board you can use standard via instead microvias.

You need to consider soldering process and potentional problems before use microvia. If you have mixed SMT and PTH components in that case you need to use wave soldering process. In this case you will probably have problems with microvias.

If you use microvias you will have more problems with PCB testing because you cannot always put test points on microvias.

If you really don't need microvias don't use them.

In general for bypass capacitor use X7R capacitors, low ESR tantals with power planes and SMT instead DIP packages. This reducing allover serial inductance.

Also take care of choosen logical family or technology to reduce ground bounce. If you don't need high-speed design use slower families or slow slew rate drivers.


Regards
 

Phil woz ere

Full Member level 2
Joined
Feb 12, 2002
Messages
130
Helped
6
Reputation
12
Reaction score
3
Trophy points
1,298
Location
UK
Activity points
968
Via in pad will cause manufacturing problems.
1: Larger holes wick the solder away from the pad.
2: Cause thermal differences between pads.
3: Possiblilty of getting black pad effect from the plating/cleaning process.

Also ot should be noted that blind or buried holes are more expensive to produce and the depth they can travel through the board is limited normally to the next layer down in the stack.

If you can, always pull the via hole away from the solder pad.

Phil 8)
 

Status
Not open for further replies.
Toggle Sidebar

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Top