Frequently asked questions

Yes, these technologies can be combined and applied independently of each other, though the vast complexity of the manufacturing process and the required technological equipment will result in a significant price increase.

Blind vias and buried vias can be requested individually. Buried vias vary in complexity and therefore require individual evaluation. Please email your requirements to kontakt@leiton.de.

Packaging refers to simultaneously routing and drilling several stacked boards resulting in time saving. Various stack sizes are possible depending on board material thickness and size of the applied drilling and milling heads. Hence usage of large drilling diameters and thin material strengths are optimal during this process.

Nibbling refers to a particular drilling process whereas it is possible to carry out multiple interleaving drillings with so called nibbling drill heads, which are more rigid than conventional drill heads. This process is particularly adequate when crafting plated-through slots, as the adhesion of copper onto the boards’ material is increased as opposed to routed surfaces.

This term refers to interlayer connections within inner layers, which do not connect to the outer layers of a multi-layer board. They do not show from outside the board and thus are referred to as buried vias.

This term refers to interlayer connections, which plate through multiple layers beginning with one outer layer, but without connecting to the other outer layer. Thus the drill-hole does not penetrate the entire board.

During the pressing process of PCB’s, minor offsets within the various layers may occur. Thus it is necessary to increase the pads’ extensions in the inner layers. The optimum is considered to be 0.5 mm (outer layers: 0.3 mm) plus the final drilling diameter.

Smaller pads in the inner layers are producible, however the drilled pads may turn out to form a so called sickle within a layer, the drilling not being centrical to the pad that is. Though electrically irrelevant, the sickle-shaped pad is an undesired feature and thus avoided by correct pad sizes.

If plated-through drillings are desired which are not supposed to be connected to the respective inner layers, appropriate clearances from surrounding copper have to be applied. Plated-through drillings, which connect to an adjacent copper area due to minor offsets within the inner layers, can cause an electric short if these clearances are insufficient.

Thus the clearances in the inner layers should be approximately 0.7 mm larger than the final drilling diameter (r = 0.35 mm).

The drilling process itself does not set limitations to continuously decreasing drill-hole diameters. Drillings with diameters smaller than d = 0,4 mm are perfectly possible, though the eventual metallization process inside the drill-holes will become more difficult as liquids flowing through become more inert with increasing strength of the board. The drilling diameter equals d = 0.4 mm and FR4 with d = 1.55 mm by default.

The dimension of the drillings specified by the designer represent the final dimension from a manufacturers’ point of view. Due to the through-plating, the surface finish and the copper build-up in particular, the drillings’ diameter has to be carried out larger to eventually reach the desired size. Plated-through drillings without an annular ring provide significantly less stability to the final product.

The drill-hole allowances for the fabrication of printed circuit boards may vary among manufacturers. In the boards’ outer layers, an allowance of 0.3 mm for drill pads (plus the final diameter) by default is considered as sufficient. For a low-cost PCB mass production even larger allowances may be required.

Examples for drill allowances in the fabrication of printed circuit boards (source: Leiton GmbH):

Surface finish chemical gold: drill allowance +0.10 mm to +0.20 mm
Surface finish chemical tin: drill allowance +0.10 mm to +0.20 mm
Surface finish HAL (non-leaded): drill allowance +0.15 mm to +0.25 mm

If an allowance of 0.15 mm is applied, the annular rings’ width is 0.075 mm only (standard width: 0.3 mm plus the diameter of the drill-hole).

Desired size: 0.3 mm final diameter / 0.6 mm pad = 0.15 mm annular ring

Fabricated size: 0.45 mm drilling diameter / 0.6 mm pad = 0.075 mm annular ring

No, allowances for drillings vary with the desired surface. More or less of the surface finish material is settling in the drill-holes during processing which therefore requires varying allowances:

No, these allowances are specified by the manufacturer or the respective CAM-department.

Aside from technical difficulties concerning the metallization process in extreme narrow drill-holes, the complexity of the drilling process increases significantly. Boards are commonly drilled in so called packets, whereas several copper coated materials are stacked and drilled simultaneously. When applying very thin drilling bits with diameters smaller than d = 0.6 mm and assuming standard board materials with d = 1.55 mm, the packet stack size decreases from 3 to 2 boards. This increases drilling time and therefore requires additional efforts.

No, as it would cause the drill bit to break once the standard bit bottoms out into another drill-hole. An alternative represents the nibbling process.

The difficulty in fabricating blind vias is caused by the fact that these drillings cannot be thoroughly flushed by the chemicals involved. The bigger the blind vias are, the better they can be coated with copper. The aspect ratio of diameter to depth should be >1, the width should exceed the depth of the drill-hole that is.

No, punching may be an inexpensive way of cutting boards, however particular punching tools are needed for this purpose. These once-only costs do pay off in mass production only. The punching procedure is often applied in low-involvement consume goods, e.g. toys, since they are extremely price-sensitive and manufactured in large quantities.

If circuit paths (traces) or grounded areas are located too close to the outlines of the printed circuit board (PCB), the possibilities of shorts in the eventual product is significantly higher. Solder waves, which can leave tin residues on the outlines, as well as conductive casings can form undesired connections, or the applied solder mask can chip off the routed copper through mechanical load.

The clearance maintained should be at least 0.3 mm on routed boards (PCB) and at least 0.5 mm on v-cut material.

Yes, v-cuts are possible. This additional production step involves handling and compiling the machine data. Please email kontakt@leiton.de for individual conditions.

Yes, a multi-panel counts as a sole panel only and is fabricated and delivered in one piece by default. Routings may be applied to separate the individual boards at an extra charge. A marking with a line thickness of 2mm is required for these inner routings and should be included in the delivered layout data. If these markings are carried out differently or are missing in the data delivered, additional efforts and an increase in price may occur.

Yes, though the possibilities of arranging several boards onto one panel depend on their individual size. In principle, we recommend fabricating in one panel when ordering multiple small boards. The size of the board should not exceed 160 mm by 100 mm. Upon request, we arrange the panel individually for you at a surcharge. Size of the panel, positioning and quantity are then being determined by Leiton. Additional costs may occur if you should require specific panel sizes.

Yes, this is always possible with single designs, though the choice of milling heads may be then slightly restricted. The standard milling bit has a diameter of d = 2 mm. Inner routings, inner-edges or slots which require a radius of less than r = 1 mm cost a surcharge if applicable. Thinner routings will make packaging more difficult as operating with the milling head has to be decelerated to prevent damages to the tool. We will of course brief you before acknowledging your order if any additional efforts are required.

Yes, additional costs for inner routings are then included if they represent a functional neces-sity. This does not apply to individually set inner routings to separate multiple boards.

Yes, though adjustments in price that may occur concerning extreme board designs are subject to an individual consultation.

In the fabrication of printed circuit boards, milling heads with a diameter of d = 2 mm are commonly used, resulting in a minimum radius of r = 1 mm. If a rectangular shape is desired, it is possible to create a perfect 90° angle by routing from two sides into the printed circuit board (PCB) and thus removing the radius, without cutting into copper areas.

Smaller routing radiuses till 0.35 mm are possible, but may increase costs. Packaging multiple boards is then inapplicable and routing speed is decreased. Appropriate milling heads are expensive and more likely to break.

Please consult the details in our « Technology » tables for PCBs and FPCs.

The standard milling head has a diameter of d = 2 mm, and smaller routings can be carried out down to d = 0.7 mm. However, routings with smaller diameters should be avoided due to additional complexity and costs that may occur, if they do not represent a necessity in view of the boards’ functionality.

On one hand, the packet stack size in combination with plated-through routings makes it inevitable to process one board after another to avoid damage to the tool, depending on the type of milling head. On the other hand, the milling speed is significantly slowed down. The single routing at reduced speed therefore requires additional efforts.

Via-filling is most commonly applied if a thorough filling of plated-through drillings is desired. This provides a better eventual borad assembly on machines equipped with a vacuum gripper for fixation.

Yes, is it possible. Merely the mask clearance has to be removed in this case. However, this lacquer does not always thoroughly fills out the drillings and is no legit substitute for Via filler.

All drillings with sufficient copper pads are carried out plated-through. Single-sided pads are unusual and will be carried out plated-through as well if the existent pad is adequate in size and a pad is placed on the other side of the printed circuit board (PCB). However, such contradictory aspects should be mentioned beforehand to determine if pads shall be applied entirely or not.

The design of a single layer board requires solely photolithographic processing, etching and drilling. When omiting the through-hole plating, single-layer printed circuit boards (PCB) become more cost-effective. If plated-through drillings are desired, the application of pads on the rear side is recommendable. Hence the same procedures for two-layered boards become necessary and the cost benefit of single layer boards is void.

HAL is an abbreviation for Hot-Air-Leveling. After the boards are immersioned into molten tin, they are extracted and blown with high pressure to remove residues from drillings or routings.

Yes, since January 1 2006, all our PCB products are compliant to the RoHS/WEEE guidelines. We provide the following surface materials:

Available finishes:

Upon request:

When ordering with this option, Leiton will determine the surface material to provide you with a cost-effective product. The printed circuit boards (PCB) will then be delivered with one of the following surfaces:
- Immersion tin
- HAL lead free
- Immersion gold (ENIG)

All boards are RoHS/WEEE compliant. If you specifically require lead-free HAL, the reduced ability to combine your order with boards requiring other finishes, such as immersion tin, can cause additional effort. Please email kontakt@leiton.de for the required finish and individual conditions.

No, chemical nickel-gold (NiAu) and hard gold (galvanic gold) are distinguishable by the following criteria:

Yes, Leiton provides immersion nickel-gold (ENIG) surfaces for printed circuit boards. Please email kontakt@leiton.de for an individual quotation.

Hard gold is commonly required when switches or connector strips are exposed to an increased mechanical load, e.g. in a PCI card slot in a personal computer. In this case the connectors are hard gilded to increase abrasion resistance und to protect other contacts from corrosion.

Yes, these are synonyms for an identical surface treatment. The term hard gold relates to the grade of hardness, connector strip gold to the application and galvanic gold to the fabrication process.

The commonly used material is FR4. This material consists of pressed glass fibre and expoy resin. It has an amber-beige colour which does not show after the application of the solder mask.

The standard FR4 material has a Tg of 130° C (266° F) and a maximum continuous operating temperature of approximately 110° C (230° F).

This depends on the applied material : standard FR4 material has a maximum continuous operating temperature of approximately 110° C (230° F). Newer materials bear up to 130° C (266° F) and 160° C (320° F) using high-temperature consistent laminates. As a safety tolerance, 20° C to 30° C should be subtracted from the respective Tg to determine the maximum continuous operating temperature.

Theoretically, the lifespan of a PCB is unlimited. Though environmental influences like temperature, humidity and vibrations may have a strong impact on the operating ability of a PCB. However, the board itself is commonly not the primary source of error, but the applied components or their soldered joints.

FR means "flame retardant".

FR1 = Phenolic resin + hard paper
This is an obsolete and very cheap material. It is higly hygroscopic, it absorbs humidity that is.
FR2 = Phenolic resin + hard paper
An old and cheap material formerly used in mass production and separated by blanking. It had to be warmed up for this process otherwise it would splinter. Like FR1 it is hygroscopic and is not used anymore due to its qualitative deficiencies. Furthermore, phenolic resins emit small amounts of phenol and formaldehyde and represent a health risk. Nowadays epoxy resin is commonly used as a substitue for Pertinax (paper containing phenol and formaldehyde).
FR3 = Epoxy resin + hard paper
This is a budgt-priced material for consumer electronics.
FR4 = Epoxy resin + glass fibre fabric
The most utilised material in the fabrication of printed circuit boards (PCB) is RoHS/WEEE compliant and does not contain any harmful bromine compounds. FR4 has a Tg of 130° C (266° F) and a maximum operating temperature of 110° C (230° F). Thin inner laminates for multi-layer boards are also made of this material.
FR5 = Epoxy resin + thermostable glass fibre fabric
Like FR4, but thermally more consistent. FR5 has a Tg of 160° C (320° F) and a maximum operating temperature of 140° C (284° F).

“Tg” denotes the temperature where the base material starts to soften, it loses its mechanical stability that is.

FR4 175 - 250
PTFE > 600
Insulation material group I CTI > 600
Insulation material group II > 400 < 600
Insulation material group IIIa > 175 < 400 (FR4)
Insulation material group IIIb > 100 < 175

A printed circuit board (PCB) represents with the basematerial (dielectric) and copper layers above and underneath (electrodes) a capacitor. The influence of the dielectric material of a capacitor is described with the dielectric constant Epsilon ɛ. This dimensionless constant indicates the factor by which the capacity will alter if another dielectric medium with same thickness other than air is used. Thus air represents the reference the dielectric constant DK and equals ɛ = 1. Some examples for ɛ values:

FR4 with a thickness of 1.55 mm is a standard material for prototypes and medium-volume PCBs. Differing thicknesses and base materials cannot always be combined with other orders due to lower demand, so setup costs cannot be shared. This additional effort has a greater effect on small quantities. Typical non-standard thicknesses are 1.0 mm or 0.5 mm. Please email kontakt@leiton.de for an individual quotation.

Yes, e.g. black FR4 material is often requested by our clients. This type of FR4 serves particularly for opto-electronic applications which require a photo-resistant base material. We would be glad to provide you with an offer meeting your individual needs.

Yes, upon request we provide you with an offer for printed circuit boards (PCB) for hf-applications. These boards are carried out with Rogers (Ro4000 series) or Isola (IS4000 series) materials.

If you require several high frequency PCB layouts at the same time, it is possible to fabricate them together to cut costs. However, single boards for hf-applications are not combinable.

A cauterisation allowance is an enlargement of circuit paths to carry out the desired circuit path thickness after the cauterisation process. The size of this allowance depends on various fabrication and layout factors.

To ensure the correct orientation of the board, it is necessary to display text in at least one copper layer. PCB layouts without text may lead to fabricating boards with inverted layers.

The copper layers of printed circuit boards (PCB) are commonly exposed using the positive-technique method. This implies that the image of the circuit path layout on the film is black or red-brown, and that small gaps in grounded areas or text are exposed as well. After processing, these small laminate residues often become loose and stick to other parts of the PCB. This prevents a thorough eventual copper and cauterisation stop build-up; the concerning area will be etched as well. Thereby small loosened laminate residues on copper circuit paths could cause eventual disconnections on the PCB.

Thus it is recommended that the gaps in letters or screened grounded areas correspond to the applied PCB technology. A minimum of 0.15 mm by 0.15 mm has to be maintained. Smaller gaps should be filled out.

The application of text and logos is carried out using the same method as common circuit paths. If text is printed using an insufficient thickness, it may be etched away. Letters placed too close to each other or gaps in between may merge during the eventual build-up process.

A minimum line thickness for text and logos in copper layers of 0.20 mm is recommended.

It is possible to convert films into an appropriate data-fomat if you require this, however the costs involved in this process depend heavily on the additional efforts.

It is possible to convert photos into an appropriate data-fomat if you require this, however the costs involved in this process depend heavily on the additional efforts.

If a printed circuit board (PCB) has e.g. some very thin, single bound circuit paths, these are carried out with additional cauterisation allowance other that those, which are adjacent to several parallel bound circuit paths. Single bound circuit paths are enlarged with up to 4mil (0.1 mm) cauterisation allowance. This is uncritical if there are not adjacent copper areas or circuit paths. A common example for cauterisation allowances of a PCB in 6mil technology is the enlargement to 7mil (0.175 mm) of circuit paths, at the expense of lesser clearances of mere 5mil (0.125 mm). The cauterisation allowances ensure that the copper in the eventual PCB corresponds to the desired requirements of the layout. In case of doubt, the allowances should be dimensionated slightly larger than usual. An exception are PCBs for high-frequency applications. Though cauterisation allowances are possible and partially necessary, these have to be adjusted precisely to the respective fabrication conditions and function of the hf-board.