Why is DFM needed in PCB production?
- Some times there are errors from the PCB designer or when converting PCB files from one format to another, our engineer may be able to find out the errors when checking them;
- The material or technology used in the PCB design may not be available for PCB manufacturers;
- We can optimize the stack-up, material or other aspects to make PCB more robust or cost-effectively, etc.
What DFM do we do in Viasion:
Here at Viasion, our skilled engineers will check all your files carefully, including Gerber files and other notes. Please refer to the following main points we are going to check.
Get a free quote now!
Material
Sometimes, we had to change material for some reasons, such as the long lead time of the specified material type or thickness or the selected material type being no longer active. Then we will advise a suitable substitution and ask the customer to check and approve.
Meanwhile, to lower cost and meet high base material utilization, we will choose suitable array style and size using our unique software, usually, min.85% for the single or double-sided board and min.75% for the multi-layer board.
Drill
1. Tolerance
2. Vias
3. Buried-blind holes
To achieve high-density interconnection, buried-blind holes must be used in the multi-layer board. However, if the dielectric thickness of each layer can be appropriately adjusted, we can use any layer interconnection technique to achieve all kinds of buried-blind holes.
4. Depth control drill
4-1. Back drilling
4-2. Depth control routing
Copper plating
Layup
Sometimes, the lamination is unreasonable and too thin, which can easily cause problems such as delamination in the substrate, a too-thin dielectric layer and current breakdown, especially for thick copper plates. In addition, the amount of glue filled is large, quickly leading to insufficient thickness of the dielectric layer. Sometimes, we will press the raw base material without copper and the PP sheet together to get a thicker dielectric layer.
Sometimes, TU-872lk material is defined in the spec., but this base material is not suitable for blind holes. If used, it will cause delamination. Some customers have previously reported that this problem occurs in the SMT process. At the same time, due to your laminated structure and blind hole, our company recommend using tu-768 material in our stock to make it; At the same time, we have slightly adjusted your design to meet the board thickness and impedance value.
If multi-layer flexible, such as our 6L below for reference.
Our regular 1.0mm HDI 1+N+1 stack-up is below.
Meanwhile, the quality department will check each dielectric layer thick before delivery, just like below.
Cam’s design
1. BGA design
BGA layout suggestion below:
To optimize the BGA power supply’s filtering and energy storage effect, placing more than 22uF capacitors around BGA is recommended. The excellent layout below:
Sometimes, some BGA pads around 0.2mm are so small that it becomes hard to control their size and shape during the etching process. Therefore, we advise choosing the solder mask defined pads technique(solder mask opening less than its corresponding copper pads) just like below.
2. Impedance simulation
And the detailed impedance analysis list is just like the one below.
3. Panel
Most of the time, customer files are single PCBs. However, we will always give suggestions to customers and provide suitable panels which are easy to handle both in PCB manufacturing and PCB assembly process. There are two types of panels commonly: panel with v-cut and panel with mouse bite. Please refer to the following frustration. The advantages and disadvantages of v-cut and mouse bite are:
- V-score design adjustment to meet customer needs
- 30 ° V-score, the distance between copper and the V-score centre line should be > 0.35mm to avoid exposing copper on the board's edge.
- 45 ° V-score, the distance between copper and the V-score centre line should be > 0.4mm to avoid exposing copper on the board's edge.
- The thickness of the board is ≤ 0.40mm. Therefore, it is recommended that the customer use single-sided V-CUT and reserve the residual thickness of 0.20 ± 0.10m. the distance between copper and the V-score centre line should be > 0.4mm to avoid exposing copper on the board's edge.
- If the board thickness is more than 1.0mm and less than 1.6mm, the remaining thickness is 0.4 ± 0.1mm.
- The thickness of the plate is more than 1.60mm, and the remaining thickness is 0.5 ± 0.1mm.
- It is recommended that all sharp edges be rounded - to prevent the bag from being punctured.
4. Copper layer design
Common rules for copper layer design and engineering:
Enlarge the graphics as a whole according to the MI instructions, and Check whether the minimum clearance meets the requirements of MI.
When the minimum gap cannot be met after the overall compensation, the large copper and pad can not be compensated, and parts of the line can be reduced as well; But we need to ensure that (pad or IC or line width etching amount) ≥ 80%.
If the line needs to be moved due to insufficient clearance, the outer layer can be moved within the range of ≤ 0.05mm. (except for the impedance line, which cannot be moved) if it moves beyond 0.05mm, you must ask the customer in writing, and you can move it only after the customer confirms and replies.
Check that the minimum gap between the exposed pad and large copper covered with solder mask after compensation should be ≥ 0.08mm.
Check that the minimum gap between the windowed pad and pad after pre-enlargement is ≥ 0.1mm.
Relatively independent etched characters generally need to be compensated on the overall compensation base (the pre-enlarged number depends on the size of etched characters and copper thickness) to ensure that the independent characters after etching are ≥ 0.15mm.
When the bottom copper is ≤ 1oz, the minimum gap between the hole and the line is generally 0.20mm. In exceptional cases, it must be ≥ 0.15mm. Meanwhile, the tin ring must be reserved based on the minimum gap required by MI during fabrication, and the tin ring must be ≥ 0.085mm simultaneously. (For the holes and tracks after compensation)
Rules about IC pin and non-functional circuits
When the line width connected with the IC pin is greater than the width of the IC pin, the line can be thinned to equal the width of the IC pin. When the gap is affected, it must be refined. (only the overlap with IC can be changed, and the length of line thinning can only be 0.5mm longer than the IC bit at most)
Remove the non-functional circuit with the original ≤ 0.1mm to prevent it from falling off after brushing and grinding after etching for functionality on large copper sheets. The line width should be ≥ 0.12mm after etching.
When a line ≤ 0.12mm is in the board, this functional line width can be as large as the line.
Copper on the edge of the board:
Rules about the copper on the edge of the board
The distance between the large outer copper and the line from the contour line when the routing board is≥ 0.20mm; The minimum size is 0.15mm. Punching: ≥0.20mm. The minimum size is ≥ 0.15mm.
The distance between the large outer copper or the single side of the line and the V-score line is ≥ X+0.10mm.
Generally, it is made of x+0.20mm. Normally, add 1.0mm fiducial marks on the waste strip and copper sheet to balance the plating.
Meanwhile, to make routing easier, we have to add four tooling holes.
Solder mask opening of fiducial marks should be ≥ 1.0mm. Sometimes, we need to add protecting ring around fiducial marks to make them resist etching.
Generally, its outer diameter is 5.0mm, and the ring width should be ≥ 0.20mm after etching; if the customer has no special requirements, a copper pad can be added to the frame area.
If the customer has unique needs, it should follow the customer's requirements. The size of the pad on the frame area is generally 1.50mm, and the spacing is generally 2.0mm. Generally, layout them just like the one below.
5. Drill
The general size of the isolation clearance between the NPTH drilled at the first time and the outer copper is ≥ 0.20mm, and the minimum clearance is ≥ 0.15mm; (increase the minimum gap between npth hole and line to prevent the welding resistance of silk screen line from reddening)
Second drill hole copper digging: If it is the second drill after etching, the copper cut in the center of the second drill is 0.10mm smaller than one side of the hole.
If it is the second drill before routing, the minimum distance from the edge of the second drill to the copper or trace edge is 0.10mm.
Ensure that the second drilled annular ring is min.0.3mm single side after etching, especially second-drilled rings based on 2oz copper. The minimum annular ring should be more than 0.3mm on one side.
6. Solder mask design
- Check the solder mask Gerber file to avoid them on pads as usual.
- The solder mask shall be exposed to minimize the leakage of the substrate, and the opening size shall be one mil larger than one side of the pad.
- If the solder mask dam is at the golden finger, we will advise deleting it and exposing it to both ends of the slot position if it is unreasonable.
- BGA is too small, which leads to poor control of etching. Changing the BGA size to choose the solder resist defined by the pad is suggested.
- Vias around BGA shall be plugged with solder mask ink to lower the risk of the open-short circuit.
- Solder mask design for PTH and NPTH.
Solder mask design for PTH
- Check the soldHoles less than or equal to 0.5mm are not blocked by the solder mask.er mask Gerber file to avoid them on pads as usual.
- For the hole with a larger opening than the hole and smaller than the pad, and S/M ink is not allowed to enter the hole, the solder mask blocking light point is 0.1mm more than the holes.
Solder mask design for NPTH:
- When the hole diameter of NPTH is ≥ 0.6mm, the solder mask blocking light point is made 0.05mm smaller than the single side of the hole diameter;
- When the hole diameter of the NPTH hole is less than 0.6mm, the solder mask blocking light point is made 0.05mm larger than one side of the hole diameter
- Cancel the solder mask blocking the light point for plugging holes.
Principle and two important factors for film
Principle: Do not change the position of the original S/M exposure and the area reserved by the solder mask. Pay special attention to retaining the solder bridge of the original design (except those that are too small to be retained).
Two important factors: One is the window size; The other is the distance from the window to the line.
Solder mask opening principle in case of different copper thickness
When the bottom copper is less than 1oz, the S/M opening is 0.05mm more than the pads on one side of the line pad. Generally, it is made of 0.08mm. Suppose 0.08mm edge, resulting in many exposed lines, or the minimum solder mask dam cannot be retained. Then, the minimum S/M opening should be at least 0.03mm.
When 1oz ≤ base copper <2oz, the S/M exposure is 0.05mm larger than one side of compensated line or pads.
When 2oz ≤ base copper <3oz, the S/M exposure is 0.03mm larger than one side of compensated line or pad.
When 3oz ≤ base copper <4oz, the S/M exposure is 0.02mm larger than one side of compensated line or pad.
When base copper≥ 4oz, the S/M exposure is 0.01mm larger than one side of compensated line or pad.
For BGA opening, the minimum S/M exposure is 0.03mm larger than one side of compensated line or pad to prevent poor exposure.
7. Carbon design
The printing pad is min.10mil larger than the copper pad, and the minimum line thickness is 10mil.
The minimum distance between the printing pad is 10mil, and the distance between the line pad is min.30mil(when there is green oil between the carbon oil fingers).
The minimum spacing between the printing pad is 30mil, and at this time, the spacing between the line pad is min.50mil(when there is no green oil between the carbon oil fingers).
Carbon oil is not allowed to seep into the hole ring and other pads, so the minimum distance from the printing pad of the carbon oil film to the hole ring and other pads is 10mil.
8. Silkscreen
Word width: 5MIL; (base material surface), 6mil (line surface) word height: 0.8 mm (min) Minimum word gap: 6mil; The minimum character spacing pad is: 6mi.
The characters are reversed. Sometimes, the characters on the bottom side are not mirrored, resulting in the characters being changed, which affects discrimination. It will be adjusted in time. And then Inform the customer to pay attention to the subsequent wiring adjustment and improvement.
The silk screen printing will need to be clarified due to the small character line. The character line width will be adjusted in time to make it clear and easy to recognize, and the customer will be informed to pay attention next time.
Characters on pads shall be found in time, and these characters shall be removed to prepare for the subsequent SMT process.
It is generally recommended to add the UL logo and date code on the silkscreen layer, which can protect customers’ interests under particular circumstances and provide a reference basis for subsequent traceability.
9. Cam working analysis and optimize
Software and network analyst:
The genesis2000 system mainly includes the following main functions:
Input (data input), DFM (data optimization), editing function, analysis (data detection), output (data output), etc.
When transferring files, we must transfer all customer files into Genesis, especially network files; When the customer provides network documents, the customer network must be used to compare whether the network generated by the production draft is consistent and confirm with the customer if there is any abnormality.
Network analysis documents and network analysis to help customers find potential open and short circuit problems.
10. Copper layer design and optimization
Annular ring inner layer
Teardrop
You can use the detection function in the software to detect whether there is a wiring pad.
When the inner line width corresponding to the bonding pad is less than 0.12mm, a teardrop design is added according to the following instructions to increase the connection reliability between the PTH hole and the inner layer. After adding teardrops, ensure that the minimum gap meets Mi requirements.
Inner functional pad
Number of inner functional pad connecting wires ≥ 2.
Size of inner functional pad isolation ring: generally made of 0.25mm. In exceptional cases, the minimum isolation clearance of the inner layer can be the same as the Minimum clearance (the minimum shall not be less than 0.12mm, and the resolution capacity of the coated plate is limited).
11. Some other further optimization
Cancel all non-functional independent pads in the inner layer (except blind, buried holes, unless the customer has unique requirements) to reduce the possibility of internal short circuits.
To reduce resin filling, when adding power grabbing copper sheet in the inner layer of the groove, each corner should be made into a fillet (generally R ≥ 2mm). Please do not make it into a right angle, let alone an acute angle, to facilitate the flow and exhaust of resin.
Inner layer network check Net-list (network) check is to check whether the electrical performance of the production line graphics changes during the production process based on the raw data, reducing the production design risk.
Get an Instant Online Quote Today
Viasion Technology is your trusted partner & one-stop shop for PCB fabrication, components sourcing, PCB assembly and electronic manufacturing. With more than 16 years of experience, we have been supplying high-quality PCBs with competitive pricing for 1000+ customers worldwide. Our company is ISO9001:2015 Certified & UL Listed, and all our products are 100% E-tested and inspected by AOI & X-RAY to meet the highest industry standards. So please get an instant quote from our sales team now, and we will take care of the rest.
