IPC-7095C-2013.pdf - 第63页

One side T ype a T wo sides T ype b T ented V ia (T ype I Via) A via with a dry ﬁlm mask material applied bridging over the via wherein no additional materials are in the hole. It may be applied to one side. (T ype I-a) …

damage the via wall resulting in open vias. However,

applying the via caps after the surface ﬁnish has been

applied can degrade some surface ﬁnishes (e.g., OSP,

ImAg, ImSn) due to the thermal exposure that is necessary

to cure the via cap material. Both of these issues must be

taken into account when making a decision to ﬂood or cap

vias. Most PCB suppliers ﬂood or cap vias before the sur-

face ﬁnish is applied.

There are presently eight different methods of via plugging/

capping identiﬁed in IPC standardization. These are shown

in Figure 5-12. It is important to realize that the choice of

tented, plugged and ﬁlled vias for via protection can have

direct impacts on the subsequent assembly processes.

Table 5-4 provides the pros and cons of tenting, plugging

and ﬁlling vias. The choice among the options presented

will depend on the capabilities of both the fabricators and

the assemblers. To avoid complication during assembly, it

is imperative that all involved in the manufacturing process

understand the trade-offs among the options.

5.5 Thermal Spreader Structure Incorporation (e.g.,

Metal Core Boards)

When structural, thermal, or electri-

cal requirements dictate, a conductive constraining core or

metal core can be inserted into the layer structure. It is rec-

ommended that the board circuitry layer conﬁguration is

made symmetrical about the the core as the center. It is

possible to create structures that are asymmetrical (i.e.,

having a different number of layers to either side of the

core); however, plated-through holes going through the

entire stack may be less reliable due to the differences in

expansion on either side of the metal or constraining core

(see Figure 5-13).

One reason for asymmetrical design is the separation of

electrical functions from mechanical or thermal functions,

but this advantage might be offset by board distortion or

warping during soldering operations (or during thermal

cycling in the intended operating environment) due to dif-

ferences in the thermal expansion of materials.

Some compensation can be achieved by having additional

copper planes added to the back of the interconnection

product. The extra copper plane may increase the expan-

sion coefficient slightly and make soldering more difficult

due to the need to put more energy into the board to assure

proper solder joint formation; however, a positive effect is

that it enhances thermal conductivity.

5.5.1 Lamination Sequences As previously noted, more

desirable constructions are those where circuit layers are

symmetrical about the core chosen to serve at the center of

the board. By so doing, individual multilayer circuits can

be produced separately, each with their own laminating

sequence. For example, a four layer board might be manu-

factured having vias through the entire four layers and this

can be duplicated for use on either side of the core.

To achieve mechanical constraint within a chosen and use-

ful range, the total thickness of the core in the multilayer

should be approximately 25% of the board’s total thick-

ness. Constraining core board is more often used because

the core layers may be imaged, etched, and connected to

the plated-through hole. The thicker center core must be

machined. Better thermal cycle survival has been shown in

some studies for structures having two constraining cores

in the board rather than one.

Another conﬁguration is to have a special constraining core

board made by bonding a multilayer board to each side of

a thick metal core after each of the boards has been com-

pleted. The composite board is then sequentially drilled,

plated, and etched to form plated-through hole connections

between the two boards. Coupons should be provided to

test the integrity of the composite structure.

5.5.2 Heat Transfer Pathway Metal core boards add sig-

niﬁcantly to the thermal mass of the assembly. This may

force the preheating soldering process to be operated at

abnormally high limits. These designs should be thor-

oughly evaluated under production conditions prior to

release. Laminate ruptures and discoloration and grainier

textured solder are typical effects that have been observed.

The heat transfer path between components and the planes

are usually accomplished through either direct contact with

the plane or through thermal vias positioned under the

component and connected to the thermal core or plane in

its position.

Table 5-3 Via Filling/Encroachment to Surface Finish Process Evaluation

Surface Finish Tenting Flooding Capping Plugging Encroaching

HASL Okay Okay Okay Okay Okay

OSP Okay Not Recommended Okay Okay Okay

ENIG Okay Okay Okay Okay Okay

ImAg Okay Not Recommended Okay Okay Okay

ImSn Okay Not Recommended Okay Okay Okay

IPC-7095C January 2013

Provided by IHS under license with IPC

Not for Resale

No reproduction or networking permitted without license from IHS

--`,,```,,,,````-`-`,,`,,`,`,,`---

One side Type a Two sides Type b

Tented Via (Type I Via)

A via with a dry ﬁlm mask material applied

bridging over the via wherein no additional

materials are in the hole. It may be applied

to one side.

(Type I-a) or both sides (Type I-b) of the via

structure (IPC-4761, Figure 5-1).

Tented and Covered Via (Type II Via)

A Type I via with a secondary covering of mask

material applied over the tented via. The material

may be applied to one side (Type II-a) or both

sides (Type II-b) of the via structure (IPC-4761,

Figure 5-2).

Plugged Via (Type III Via)

A via with material applied allowing partial

penetration into the via. The plug material

may be applied from either one side (Type III-a)

or both sides (Type III-b) of the via structure

(IPC-4761, Figure 5-3).

Plugged and Covered Via (Type IV Via)

A Type III via with a secondary covering of

material applied over the via. The plug and

secondary covering material may be applied

from either one side (Type IV-a) or both sides

(Type IV-b) of the via structure (IPC-4761,

Figure 5-4).

Filled Via (Type V Via)

A via with material applied into the via targeting

a full penetration and encapsulation of the hole

(IPC-4761, Figure 5-5).

Filled and Covered Via (Type VI Via)

A Type V via with a secondary covering of

material (liquid or dry ﬁlm soldermask) applied

over the via. The covering material may be

applied from either one side (Type VI-a) or

both sides (Type VI-b) of the via structure

(IPC-4761, Figure 5-6).

Filled and Capped Via (Type VII Via)

A Type V via with a secondary metallized

coating covering the via. The metallization

is on both sides (IPC-4761, Figure 5-7).

Partially Filled Via

The illustrations show a via ﬁlled with

nonconductive epoxy and then plated

over with copper. This is commonly

used for via in pad applications

(IPC-4761, Figure 5-8).

Figure 5-12 Via Plug Methods

January 2013 IPC-7095C

Provided by IHS under license with IPC

Not for Resale

No reproduction or networking permitted without license from IHS

--`,,```,,,,````-`-`,,`,,`,`,,`---

6 PRINTED CIRCUIT ASSEMBLY DESIGN CONSIDER-

ATION

6.1 Component Placement and Clearances

It is recom-

mended that sufficient clearance (3 mm to 5 mm) be pro-

vided around BGAs to facilitate rework. The high-end

clearances are recommended, especially for CBGA when

using a step stencil to deposit solder paste and using hot air

for rework. However, if using diode laser systems for

rework the spacing can be reduced to 0.5 mm to 1.0 mm

since laser rework does not impact adjacent components.

6.1.1 Pick and Place Requirements An advantage of

BGA packages over other advanced, high-pin count pack-

ages (ﬁne pitch, TAB, PGA, etc.) is the ability to be placed

using existing surface mount placement equipment. BGAs

are more forgiving in the pick-and-place process because

they self-align.

6.1.2 Repair/Rework Requirements Repair/rework of

BGA components is a major driver for component spacing

requirements. A typical BGA rework method requires ﬁve

steps:

1) heating the solder joints to reﬂow temperatures for

package removal;

2) removal and clean-up of solder on the BGA land pat-

tern;

3) application of new solder paste or ﬂux;

4) placement of the new BGA package;

5) heating the solder joints to reﬂow temperatures for

assembly of the BGA component to the circuit board.

A keepout area may be needed for each of these steps.

Rework equipment manufacturers can provide speciﬁc

details regarding necessary keepout areas. General rules are

outlined below.

Table 5-4 Via Fill Options

Top Bottom Top & Bottom No Plug

Pros

Increase rework robustness Yes Yes Yes No

Reduce secondary reﬂow risk at wave Yes Yes Yes No

Prevent solder drain Yes Yes Yes No

Cons

Secondary Fab process Yes Yes Yes No

Component side height proﬁle restriction

less than 50 µm

above solder mask

less than 50 µm

above solder mask

Flux contaminant concern

Yes – (if exposed to

wave solder directly)

No No No

Plug integrity concern

Yes (tented, plugged)

No (ﬁlled)

Yes (tented,

plugged)

No (ﬁlled)

Yes (tented, plugged)

No (ﬁlled)

IPC-7095c-5-13

Figure 5-13 Metal Core Board Construction Examples

IPC-7095C January 2013

Provided by IHS under license with IPC

Not for Resale

No reproduction or networking permitted without license from IHS

--`,,```,,,,````-`-`,,`,,`,`,,`---