Posts Tagged ‘PCB’

15 October, 2010
Component Lead Forms

Before we go deeper into the various component families, we need to clarify the component lead forms of today’s component packaging technology and what is going to be eventually phased out and what is new and why.

The pin (component lead) pitch and the overall body height are continually shrinking. This is why the SSOP and TSOP land pattern names have to be dropped from the standard. S = Shrink for Fine Pitch and T = Thin for low profile height. If these 2 values are constantly changing then where is the line drawn? Whose part is Thin or Fine Pitch and by what measure? The Gull Wing lead has hit the wall at 0.4 mm pitch. Most assembly shops will try to convince you to swap that part out of your design for a larger pin pitch however, No-lead SON and QFN lead styles are being produced and manufactured at 0.4 mm pitch with no problems. The finer pitch parts have more I/O’s and a smaller footprint with a much lower profile than J-Lead or Gull Wing packages, so it’s obvious that the component industry is going to be no-lead or bottom only flat lead or side lead packages.

Let’s review the existing component lead forms in alphabetical order. The BGA or Ball Grid Array has been around since the 1980’s but the pin pitch started out with 1.5 mm and then quickly went to 1.27 mm (50 mils) for about 15 years. Then in the late 1990’s, the 1 mm pitch BGA was introduced and every couple years a smaller pin pitch was introduced. Today 0.4 mm pitch BGA’s are in every cell phone and 0.3 mm pitch BGA’s are the next generation.

There are 2 types of BGA Ball Leads –

  1. Collapsing – this is normally 0.65 mm pitch and higher, where the Land (pad) is smaller than the Ball size to allow the Ball to collapse around the sides of the Land. This requires a non-solder mask defined Land where the solder mask must be larger than the Land.
  2. Non-collapsing – this is normally 0.5 mm pitch and smaller, where the Land (pad) is larger than the ball to allow for via-in-pad technology and provide an adequate annular ring. The solder mask can be the same size as the Land. In some cases the Land for fine pitch BGA’s is solder mask defined where the solder mask encroaches slightly over the land. This provides protection for any trace routing between the lands but the most significant benefit is to help secure the Land to the PCB. During cell phone “drop testing”, the BGA solder joint normally holds better than the land to the Prepreg. i.e.: drop tests prove that the non-solder mask land will rip from the PCB before the solder joint breaks. So the solder mask defined land is secured better to the PCB for drop testing.

For more information about BGA’s, read my white paper “Metric Pitch BGA and Micro BGA Routing Solutions”.

Ball Lead

Ball Lead

Here is a picture that shows the non-collapsing BGA in the left and the collapsing BGA ball on the right.
Non-collapsing Ball vs: Collapsing Ball

Non-collapsing Ball vs: Collapsing Ball

While we’re on the subject of “Grid Array Lead Forms” let’s move on down the list of bottom only lead types. The next lead form in the “bottom only” category is the “Bump” lead. This is widely used in a package called “Land Grid Array” or LGA. The Land (pad) size can be the same as the Bump diameter and via-in-pad can be much more forgiving than BGA voids due to a dimple in the Land after the plug and plate process. This lead form is also highly lead-free compatible.

Bump Lead

Bump Lead

The next Grid Array lead form is the “Bottom Flat” and is also used in Land Grid Array (LGA) component packages. Linear Technologies is the leading provider of Bottom Flat Lead LGA packages. This lead form is also highly compatible with lead-free solder alloys as there is no reason for wetting (flow) properties in the solder.

We can also categorize the Pull-back Lead SON and QFN component packages with this solder joint goal as a slight periphery land is required to allow the solder to move from under the lead to the periphery to surround the protruding lead for a solid solder joint.

Bottom Flat Lead

Bottom Flat Lead

The next Grid Array component lead is the “Column”. Actel and Xilinx are the leading manufacturers for this lead style. You will not find any pin pitches smaller than 1 mm for the Column Lead. The Land must be slightly larger than the column to form a good solder joint.

Column Lead

Column Lead

Column Lead Solder Joint.

Column Lead Solder Joint

Column Lead Solder Joint

The last SMT Grid Array is the newest lead form in the industry is the “Pillar Column”. Recently introduced by Actel, this component lead has much promise for an improved solder joint. But time will tell how long this one will last.

Pillar Column Lead

Pillar Column Lead

Here is a solder joint for the Pillar Column Lead. Nice connection!

Pillar Column Lead Solder Joint

Pillar Column Lead Solder Joint

The “Corner Concave” lead form is primarily used for the Oscillator component family. It’s perfect for Oscillators because it only has 4 leads that are necessary for the standard Oscillator requirements.

Corner Concave Lead

Corner Concave Lead

“Cylindrical End Cap” goes with the Metal Electrode Lead Face (MELF) component family for resistors and diodes. I still can’t figure out why the industry still produces round components, but engineers continue to design them into their schematics. I would like to know why?
Cylindrical End Cap Lead

Cylindrical End Cap Lead

“Flat Lead” components are coming on strong. These are the SODFL (Small Outline Diode Flat Lead) 2 leaded components and the SOTFL (Small Outline Transistor Flat Lead) packages that come in 3, 5, 6 and 8 lead components. Both of these component families are the direct replacement for the Gull Wing Lead SOD and SOT-23 packages.

Flat Lead

Flat Lead

“Flat No-lead” is used in the SON (Small Outline No-lead) with terminals on 2 sides and QFN (Quad Flat No-lead) with leads on 4 sides. The most common SON & QFN today is the “Edge” lead, where the component lead starts under the component and goes out to the component body edge. This solder joint goal requires a Toe, Heel and Side solder fillet where the toe joint is visible for inspection.

Flat No-lead Edge

Flat No-lead Edge

The other Flat No-lead is referred to as a “Pull-back” lead or “Bottom Only”. The solder joint goal is a periphery land around the terminal. Pull-back leads come in 2 lead shapes –

  • D-Shape or Bullet in some CAD tools
  • Rectangle

This lead style has the same solder joint goals as the Bottom Only LGA lead.

Bottom Only Lead

Bottom Only Lead

The “Flat Thermal” lead comes in a DPAK where the signal pins and Gull Wing and the thermal lead is Flat. The “Flat Thermal” lead is also used as the heat sink for SON, QFN, SOP and QFP packages. It is usually embedded in the plastic component body and therefore the solder joint goals are usually 1:1 scale for the maximum component lead size and Land size.

Flat Bottom Only Lead

Flat Bottom Only Lead

Every PCB designer is familiar with the Gull Wing lead, but it has 2 separate rule sets that are defined by the pin pitch –

  1. Less than 0.625 mm pitch
  2. Greater than 0.625 mm pitch

We need to note that 70% of the solder strength in the Gull Wing lead is in the “Heel” joint.

Gull Wing Lead

Gull Wing Lead

Gull Wing lead solder joint. A good solder joint has visible wetting under the component lead.
Gull Wing Solder Joint

Gull Wing Solder Joint

The “Inward Flat Ribbon L” is used for the Molded Body component family. This includes Polarized and Non-polarized Capacitors, Inductors, Resistors and LED’s. The most popular is the Tantalum Capacitor.

Inward Flat Ribbon L Lead

Inward Flat Ribbon L Lead

The “J-Lead” is one of the original SMT leads that became popular with the PLCC (Plastic Leaded Chip Carrier) and then the SOJ (Small Outline J-Lead). This lead form was very popular because the leads were stable and easy to manually solder. And the solder joint was easy to inspect. However, with the advent of High Speed technology, lead-free solder, low profile fine pitch component packages, this lead form will be one of the first SMT leads to become obsolete.

J-Lead

J-Lead

Here is a J-Lead solder joint.
J-Lead Solder Joint

J-Lead Solder Joint

The “Outward Flat Ribbon L” lead is used to reduce the footprint size of SOT and SOP components. It’s similar to a Gull Wing lead, but the lead bends downward immediately coming out of the component body and then is bent flat. The flat lead is very compatible to lead-free solder alloys and takes up less PCB real-estate. Since there is no heel and these components are so “low profile”, the land is usually trimmed at the nominal component body. If the land (pad) protrudes under the component body, it will end up with solder on the bottom of the component during reflow.

The Outward L lead also has 2 separate rule sets that are defined by the pin pitch –

  1. Less than 0.625 mm pitch
  2. Greater than 0.625 mm pitch
Outward L Lead

Outward L Lead

The first component lead was the Plated Through-hole (PTH) and it’s still used today for almost every type of discrete component and connector. The through-hole components are mostly used for today’s power supply boards and proto-type boards that require hand soldering and rework.

Plated Though-hole Lead

Plated Though-hole Lead

The “Rectangular End Cap” is used for discrete resistors, capacitors and inductors. This lead type is by far the most popular due to the component count. An average PCB has 80 – 90% of the total part quantity using the Rectangular End Cap lead form. These components are easy to manually solder and easy to rework if necessary. However, the new DFN (Dual Flat No-lead) component with Bottom Only terminations is better for lead-free solder and part placement density.

Rectangular End Cap Lead

Rectangular End Cap Lead

Here is a rectangular end cap solder joint.

Rectangular End Cap Solder Joint

Rectangular End Cap Solder Joint

The “Side Lead” comes in 3 different lead styles –

  • Concave
  • Convex
  • Flat

The Side Lead is on the outside perimeter of the component body and normally runs from the bottom to the top of the component. It is used widely for Chip Array’s and LCC (Leadless Chip Carriers) and has 2 different sets of solder joint goals depending on the lead pitch –

  • Pitch is less than or equal to 1 mm
  • Pitch is greater than 1 mm

Here is the Concave “Side Lead” –

Concave Lead

Concave Lead

Here is the Flat “Side Lead” –

Side Flat Lead

Side Flat Lead

Here is the Convex “Side Lead” –

Side Convex Lead

Side Convex Lead

The last component lead form in the list is the “Under Body Outward L”. This lead form is used for Aluminum Electrolytic Capacitors and 2-pin SMT Crystals. This lead form has 2 different solder joint goals that are based on the component height. Once the component height exceeds 10 mm, the solder joint goals have to be more robust.

Under Body Outward L Lead

Under Body Outward L Lead

Now that we covered all the component lead forms, we can dive into the various component families and relate their lead forms back to this post. It’s going to be interesting to find out what new component lead will be invented by a component manufacturer in the years to come, but when they do, the IPC-7351 land pattern committee will be there to develop the optimized solder joint goal chart.

Next week I’m planning on posting “The Anatomy of a Land Pattern” and all the various elements that a quality land pattern must have in order to qualify for PCB design perfection. Here is a sample picture of the details we’ll cover –

Anatomy of a Land Pattern

Anatomy of a Land Pattern

, ,

8 October, 2010

SOT (Small Outline Transistor) Components

The SOT23 is the most popular of this component family. It has 3, 5, 6 and 8 pin variations and 3 popular pin pitches.

  • 0.50 mm Pitch
  • 0.65 mm Pitch
  • 0.95 mm Pitch 
  • Note: All pictures are shown in the “Nominal Environment” land pattern.

    Figure 19 illustrates 0.5 mm pitch SOT23 3-pin and 8-pin examples.

    FIGURE 19

    FIGURE 19

    0.5 mm pitch SOT23 fanout examples. Figure 20 illustrates 4 different 0.5mm pitch 3-pin SOT23 land pattern via fanout techniques. The SOT23 parts are placed on a 0.5 mm grid system and all the vias snap to a 1 mm grid.

    • There are two 0.1 mm trace/space technology on all layers.
    • Via land size is 0.5 mm, hole size is 0.25 mm and plane anti-pad is 0.7mm
    FIGURE 20

    FIGURE 20

    0.5 mm pitch SOT23 fanout examples. Figure 21 illustrates 4 different 0.5mm pitch 8 pin SOT23 land pattern via fanout techniques. The SOT23 parts are placed on a 0.5 mm grid system and all the vias snap to a 1 mm grid. This allows two 0.1 mm trace/space technology on all layers.

    FIGURE 21

    FIGURE 21

    Figure 22 illustrates 0.65 mm pitch SOT23 3, 5, 6 and 8-pin examples.

    FIGURE 22

    FIGURE 22

    0.65 mm pitch SOT23 fanout examples. Figure 23 illustrates 5 different 0.65mm pitch 3, 5, 6 and 8 pin SOT23 land pattern via fanout techniques. The SOT23 parts are placed on a 0.5 mm grid system and all the vias snap to a 1 mm grid. This allows two 0.1 mm trace/space technology on all layers with 0.5 mm via land.

    FIGURE 23

    FIGURE 23

    Figure 24 illustrates 0.95 mm pitch SOT23 3, 5, 6 and 8-pin examples.

    Figure 24

    Figure 24

    0.95 mm pitch SOT23 fanout examples. Figure 25 illustrates 5 different 0.95mm pitch 3, 5, 6 and 8 pin SOT23 land pattern via fanout techniques. The SOT23 parts are placed on a 0.5 mm grid system and all the vias snap to a 1 mm grid. This allows two 0.1 mm trace/space technology on all layers.

    Figure 25

    Figure 25

    The SOT223 is the next most popular component family. It has 4, 5 and 6 pin variations and 3 popular pin pitches.

    • 1.27 mm Pitch
    • 1.50 mm Pitch
    • 2.30 mm Pitch

    Figure 26 shows the 6-pin 1.27 mm pitch SOT223 land pattern.

    FIGURE 26

    FIGURE 26

    Figure 27 shows the 6-pin 1.27 mm pitch SOT223 land pattern via fanout using a power via with a 1 mm land and a 0.5 mm hole snapped to a 1 mm grid. The signal trace/space rules are 0.1 mm.

    FIGURE 27

    FIGURE 27

    Figure 28 shows the 5-pin 1.5 mm pitch SOT223 land pattern.

    FIGURE 28

    FIGURE 28

    Figure 29 shows the 5-pin 1.5 mm pitch SOT223 land pattern via fanout using a power via with a 1 mm land and a 0.5 mm hole snapped to a 1 mm grid. The trace/space rules are 0.1 mm.

    FIGURE 29

    FIGURE 29

    Figure 30 shows the 4-pin 2.3 mm pitch SOT223 land pattern.

    FIGURE 30

    FIGURE 30

    Figure 31 shows the 4-pin 1.5 mm pitch SOT223 land pattern via fanout using a power via with a 1 mm land and a 0.5 mm hole snapped to a 1 mm grid. The trace/space rules are 0.1 mm but the routing grid is 0.05 mm.

    FIGURE 31

    FIGURE 31

    The SOT143 is the next most popular component family. It has 4 pins with a larger Pin 1. The pin pitch is 1.9 mm. See Figure 32.

    FIGURE 32

    FIGURE 32

    Figure 33 shows the 4-pin 1.9 mm pitch SOT143 land pattern via fanout using a via with a 0.5 mm land and a 0.25 mm hole snapped to a 1 mm grid. The trace/space rules are 0.1 mm and the routing grid is 0.1 mm.

    FIGURE 33

    FIGURE 33

    The SOT343 is the next most popular component family. It has 4 pins with a larger Pin 1. See Figure 34.

    FIGURE 34

    FIGURE 34

     

    Figure 35 shows the 4-pin 1.3 mm pitch SOT343 land pattern via fanout using a via with a 0.5 mm land and a 0.25 mm hole snapped to a 1 mm grid. The trace/space rules are 0.1 mm and the routing grid is 0.1 mm. The via fanout direction depends on which layer you need more routing channels.

    FIGURE 35

    FIGURE 35

    The SOT component family uses a Gull Wing component lead. All Gull Wing leaded components have four different sets of land pattern rules. These examples are for the “Nominal Environment”.

    1.       Pin pitch less than 0.625mm (side goal is -0.02 mm) considered “fine pitch”

    2.       Pin pitch greater than 0.625 mm (side goal is 0.03 mm)

    3.       Outward Flat Ribbon with pin pitch less than 0.625mm (heel goal is 0.15 mm and side goal is -0.02 mm)

    4.       Outward Flat Ribbon with pin pitch greater than 0.625mm (heel goal is 0.15 mm and side goal is 0.03 mm)

    The formula that calculates the difference between Gull Wing and Outward Flat Ribbon (Mini Gull Wing) is shown in Figure 36.

    FIGURE 36

    FIGURE 36

    We already discussed Chip and Molded Body assembly outlines and Ref Des. It’s important to note that the Lands (Pads) do not get added to the assembly drawing layer for small parts. The 2 most important things on the assembly drawing are the Ref Des and Component Outline. If the part is too small and the Lands interfere with the Ref Des, then do not add the Top Assembly Lands to the padstack. However, if the Lands do not interfere with the Ref Des then we should add the Top Assembly Lands to the padstack.

    Here are some of the various assembly outlines for the 0.95 mm pitch SOT23 component family. See Figure 37 for the 3, 5 & 6 pin versions of the Assembly Outline, Ref Des, Polarity Marker for pin 1 location and Lands (Pads). Note that the polarity marker shape in a triangle in the corner because the component is too small for the standard circle polarity marker.

    FIGURE 37

    FIGURE 37

    Here are some of the various assembly outlines for the SOT223 component family. See Figure 38 for the 4, 5 & 6 pin versions of the Assembly Outline, Ref Des, Polarity Marker for pin 1 location and Lands (Pads).

    FIGURE 38

    FIGURE 38

    Here are some of the assembly outlines for the SOT143 component family. See Figure 39 for the standard and reverse pin versions of the Assembly Outline, Ref Des, Polarity Marker for pin 1 location and Lands (Pads). Note that the polarity marker shape in a triangle in the corner because the component is too small for the standard circle polarity marker.

    FIGURE 39

    FIGURE 39

    Here are some of the various silkscreen outlines for the SOT component families. See Figure 40 for the SOT23, SOT223 and SOT143 versions of the Silkscreen Outline, Polarity Marker and 0.5 mm Post Assembly Inspection Dot for pin 1 location and Lands (Pads). Note that the SOT23 and SOT143 do not have a polarity marker inside the silkscreen outline because the component is too small. The Post Assembly Inspection Dot will be the Polarity Marker.

    FIGURE 40

    FIGURE 40

  • 0.50 mm Pitch
  • 0.65 mm Pitch
  • 0.95 mm Pitch
  • , ,

    1 October, 2010

    Molded Body Components

    The next most popular component family on a PCB design layout is the Molded Body Tantalum Capacitor (CAPM). The CAPM components have an “L-Bend” component lead form. Most Molded Body Tantalum Capacitors are metric by default including their standard EIA names –

    • 3216 – 3.2 mm X 1.6 mm
    • 6032 – 6.0 mm X 3.2 mm
    • 7243 – 7.2 mm X 4.3 mm
    • 7343 – 7.3 mm X 4.3 mm

    The common component families that use the Molded Body package are -

    • Non-polarized Capacitors
    • Polarized Capacitors
    • Diodes
    • Resistors
    • Inductors
    • Fuses
    • LED’s

    See Figure 15 for the 6032 component and land pattern dimensions. I broke 1 rule to create this land pattern. Instead of a 1.0 mm Land Placement Round-off I used a 2.0 mm Land Placement Round-off to snap the land centers on a 0.5 mm grid from the center of the land pattern. When the land pattern is placed on a 0.5 mm grid, the land centers fall on a 0.5 mm grid. This improves the via fanout seen in Figure 17.

    FIGURE 15

    FIGURE 15

    Figure 16 illustrates the silkscreen and placement courtyard rules and sizes. The illustration shows the component leads on top of the land for graphic representation.

    FIGURE 16

    FIGURE 16

    Figure 17 illustrates the via fanout for a 6032 Tantalum Capacitor. If you are going to use the same size via to maintain trace/space compatibility with the rest of the PCB layout I recommend at least two vias. The placement of these vias is critical in accomplish reduced impedance and increased capacitance. It’s important that the vias be placed as close as possible to the capacitor terminal leads. In Figure 17, the 2 vias coming out the side are 0.15 mm away from the terminal lead. The vias coming out the ends on the land pattern are 0.75 mm away from the terminal leads. That’s 5 times farther away than the vias coming out the sides however some EE engineers will request all 4 vias. Since all the traces and vias are snapped to a 0.5 mm grid, this makes copy/paste much easier to manually fanout all of the 6032 Molded Body Capacitors. The dot grid display is 1 mm and the land pattern is placed on a 0.5 mm grid. All the vias in this illustration fall on a 1 mm snap grid.

    FIGURE 17

    FIGURE 17

    See Figure 18 for the 7343 Molded Body Tantalum Capacitor I recommend a larger via size with a 1 mm land size, 0.55 mm hole size and 1.3 mm plane anti-pad. This via can carry more current and you only need two (but the EE will ask for a 3rd one). The illustration in Figure 16 snaps all the vias to a 1 mm grid system. These vias are twice the size of the previous vias but all the same trace/space rules apply. The display grid is 1 mm.

    Because the land pattern, traces and the vias are on a 1 mm snap grid, this improves the copy/paste feature for manual fanout of all of the 7343 Molded Body components in your PCB layout.

    FIGURE 18

    FIGURE 18

     

    , ,

    22 September, 2010
    Chip Components Smaller Than 1608 (EIA 0603)

    Before you read this blog ‘Part 2″, read Part 1 White Paper of this series – “PCB Design Perfection Starts in the CAD Library” for the introduction information. Download it here – http://www.mentor.com/products/pcb-system-design/techpubs/download?id=60454

    Parts 3, 4, 5 etc. will be posted here over the next couple weeks. I’m really looking forward to your feedback on this subject. I believe that everyone who follows these basic rules will increase productivity levels in their PCB design layouts.

    See Figure 6 for the dimensions of a standard 1005 (EIA 0402) component superimposed with its related land pattern. In this case, I decided to break 2 rules –

    1.       Land size round-off 0.05 mm

    2.       Land snap grid round-off 1.0 mm

    The land center to land center spacing is 1.0 mm which is perfect for 1.0 mm space via fanout and the placement courtyard width is 1.0 mm which is perfect for placing parts 1.0 mm from center to center.

    When placing the 1005 in the PCB layout use a 0.1mm grid to optimize the part placement and via fanout.

    FIGURE 6

    FIGURE 6

    The 1005 (EIA 0402) was made for 1mm pitch BGA fanout. In Figure 7 you can see 2 different fanout options and one is superior to the other. The fanout coming out the top has all the key features. The vias are 0.25 mm closer to the capacitor component terminals than the typical right/left fanout which decreases impedance and increases capacitance. Also, the top fanout vias snap to a 1 mm grid because the 1005 land pattern was snapped to a 0.1 mm grid system. The 0.5 mm via land (pad) diameter with 0.25 mm hole size and 0.7 mm plane anti-pad is perfect for 0.1mm trace/space technology. See Figure 4. The trace width for the power fanout is 0.3 mm.

    FIGURE 7

    FIGURE 7

     
    See Figure 8 for the dimensions of a standard 0603 (EIA 0201) component superimposed with its related land pattern. In this case, I decided to break 2 rules –

    1.       Land size round-off 0.05 mm

    2.       Land snap grid round-off 1.0 mm

    3.       Use the “Least” environment due to component miniaturization

    For chip components smaller than 1 mm X 0.5 mm I use the IPC-7351B Least Environment to prevent tombstoning. When 2 pin micro-miniature parts have too much solder volume tombstoning can occur in the reflow oven. The land size for the 0603 should be slightly more than 2 times the terminal lead size.

    FIGURE 8

    FIGURE 8

    One of the techniques that can be used to prevent tombstoning for the 0603 (EIA 0201) is to thin the paste stencil from 0.15 mm to a smaller value for every occurrence of this component in the paste mask stencil. See Figure 9. The responsibility of the stencil thickness thinning process is placed on the assembly shop and the stencil manufacturer (not the PCB designer). Assembly shops use various solder alloys that require unique stencil creation.

    FIGURE 9

    FIGURE 9

    See Figure 10 for the dimensions of a standard 0603 (EIA 0201) component superimposed with its related land pattern. If you normally use the “Most” environment, my recommendation for the 0603 (EIA 0201) land pattern is to use the “Nominal” environment. The IPC nominal land size for the 0603 is about 3 times the size of the terminal lead. For this 0603 micro-miniature component, stay away from the “Most” environment as the solder volume is more than 4 times greater than the terminal lead footprint.

    FIGURE 10

    FIGURE 10

     The 1005 (EIA 0402) & 0603 (EIA 0201) chip components are very compatible with 1 mm pitch BGA. In Figure 11 there are 2 uses for the 1005 and one in-between the vias and one via-in-pad method. Because the 1005 land centers are on 1 mm pitch, the capacitor land (pad) falls directly centered on the via. Via-in-Pad technology will increase PCB cost because these vias need to be plated, filled and surface finish on the capacitor pad. The 0603 fall in-between the vias for the 0.1 mm trace/space technology DRC. This solution will not increase PCB fabrication cost. The dot grid display is 0.05 mm.

    FIGURE 11

    FIGURE 11

    IPC does not have a “standard” on drafting items such as silkscreen and assembly outlines and polarity markings yet.  There are several types of silkscreen outlines and polarity markings that are used for Non-polarized Chip parts, Polarized Capacitors, Diodes and LED’s.

    For a standard Non-polarized chip there are 2 options. See Figure 12 for both options. One is a line that separates the 2 lands. The default size is 0.2 mm and the default silkscreen the land gap is 0.25 mm. The CAD librarian can change both the line width and the gap to achieve placing a line between two lands that only have a 0.3 mm Gap by simply changing the line width and gap rules to 0.1 mm.

    FIGURE 12

    FIGURE 12

    See Figure 13 for the silkscreen outline for the Chip Diode. The Chip Diode also has a Post Assembly Inspection Dot so you can visually verify if the assembly inserted the Diode or LED in the correct rotation. The Polarized Chip Capacitor would have the same exact silkscreen outline but without the 0.6 mm bar.

    FIGURE 13

    FIGURE 13

    The Assembly Drawing Outlines and Polarity Markings are totally different than the Silkscreen Outlines and Polarity Markings. The first most obvious difference is that the outline shape is 1:1 scale of the component body. This outline can be either the “Nominal” or “Maximum” component body size. Another difference is the Reference Designator is centered inside the component outline and is never moved or relocated. The reference designator default size is 1.5 mm height with a 10% line width.

    The Reference Designator and Assembly Outline only change rules for micro-miniature parts. The Assembly Outline will grow as large as the placement courtyard in order to fit the Reference Designator inside the Assembly Outline. When the component gets smaller, the Reference Designator will decrease from the default 1.5 mm height to a sliding scale of values until it fits inside the assembly outline. The reference designator scaling width is always 10% of the height. The various reference designator heights for micro-miniature components are –

    ·         0.15 mm

    ·         0.125 mm

    ·         0.1 mm

    ·         0.075 mm

    ·         0.05 mm (this is the smallest human readable text height)

    See Figure 14 for the non-polarized and polarized capacitor, diode and resistor assembly outlines and Reference designators. Notice the absence of land pads. From all Chip and Molded Body components, the Land is removed from the SMT padstack to insure that the reference designators are unobstructed. Also, for CAD tools that have this feature, Right Reading Orthogonal is always recommended so when the component is rotated, the reference designator is always flipped to right reading orientation.

    FIGURE 14

    FIGURE 14

     
    Read Part 3 “Molded Body Components” coming up next.
     

    , ,

    @MentorPCB tweets

    Follow MentorPCB