Why is DFM needed in PCB production?

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!


    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reasons, such as the long lead time of the specified material type or thickness or the selected material type being no longer active.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.


    1. Tolerance

    Typically, we have to check the hole’s size and tolerance and determine their reasonable range, excluding customer-specific requirements; some other unique holes undefined need specific tolerance, such as Press-fit holes. If we want to improve assemblability, the max.2mil tolerance of press-fit holes must be controlled.

    2. Vias

    If the Vias are too small, the solder mask ink is not easy to be cleaned, resulting in the solder mask ink coming into Vias. Therefore, it is recommended to make a plug hole, etc. If the Vias are too large, it is recommended to reduce them to improve the plugging hole effect. Vias around BGA position, make a plug hole to prevent tin beads from hiding in the hole after SMT and reduce the risk of opening and short circuit.
    Some vias are too close to the SMT pad, and should be moved appropriately.
    To reduce the cost, manually optimize and move the pad on the via; If there is no position movement, select resin plug hole + electroplated hole filling.
    Vias on flexible board For flexible, the through-hole in the flexible area will be preferentially changed to the reinforcement area or the rigid board area to increase the service life of the board; At the same time, it will match the appropriate copper thickness in the flexible area according to the usage habits of customers’ products to improve the bending property of the board.

    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

    Back drilling can be applied to lower costs and technical difficulty. The function of back drilling is to drill out the PCB through-hole section that does not play any connection or transmission role in avoiding causing reflection, scattering, delay, etc., of high-speed signal transmission. And our back drilling capability is below for reference.

    4-2. Depth control routing

    Copper plating

    Ensure the uniformity of board electroplating, and add a copper sheet to the process. When electroplating the working board, the auxiliary copper sheet will be added around to increase the uniformity of electroplating. Electroplating potion has data monitoring, timely detection and adjustment to ensure that the board is plated within the best parameters. After electroplating, the actual copper thickness of each layer of the board will be measured to ensure that it is within a reasonable range, just like below.


    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 solder mask opening=BGA size+ 4mil

    BGA layout suggestion below:

    To better repair BGA, it is recommended not to place components within 3mm around BGA.

    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:


    Divide BGA by cross in the centre, and turn via in the directions of upper left, lower left, upper right and lower right, respectively.


    Ensure that the wire is led out in the middle of two pads and does not offset a pad.


    Both ends of the differential signal need to be fully wired in parallel and introduced into the BGA pin.


    The bonding pad of the via in BGA is not easy to be too large, otherwise it will affect the area of the copper foil channel of the power supply.


    The two ends of the differential signal are fully wired in parallel into the BGA pin. A pair of differential signals are avoided from entering the BGA through their respective channels as far as possible.

    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

    Use Polar software to analyze and simulate impedance values such as below:

    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:

    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

    Solder mask design for PTH

    Solder mask design for NPTH:

    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

    If the hole ring is insufficient, it will be compensated according to the manufacturing process. Size of inner hole ring: 1 oz larger than one side of the hole (diameter of drill nozzle): ≥ 0.10mm; 2 OZ:≥0.13mm; 3 OZ:≥0.20mm; 4 oz: ≥ 0.3mm.


    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.

    Connect with us

    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.