Technical Guideline WEdirekt

General Information

Online, Offline, Pool and Non-Pool

Printed circuit boards that you configure and order online are manufactured at particularly low cost. Due to the standardized online processing, certain technical specifications apply.

If you have your own specifications or requirements please contact us. We will be happy to coordinate your individual offer together.


What applies to online configured PCBs and what does "Best Price" (Pool) and "More Technology" (Non-Pool) mean?

Pool / Best Price: We combine a lot of orders for different boards into a single production step and manufacture them "together." This way we can use our panels to capacity. We gladly pass on the resulting cost savings to you!

WEdirekt produces all Best Price (Pool) circuit boards according to IPC A 600 Class 2. 

Non-Pool / More Technology: If you select the "More Technology" option in the circuit board configurator, it is not possible to combine your order with other orders for production. Such an order will then be produced as a single order (Non-Pool).

WEdirekt produces all "More Technology" circuit boards based on IPC A 600 Class 2.

Number of layers and layer stack-ups

Rigid printed circuit boards

In the WEdirekt calculator, we offer you the opportunity to order printed circuit boards from 1 to 16 layers.

Depending on requirements we manufacture Best Price (Pool) or More Technology (Non-Pool):

Best Price (Pool):

  • up to 8 layer (0,80mm, 1,00mm, 1,55mm and 2,40mm material thickness)

More Technology (Non-Pool):

  • up to 16 layer (0,50 mm, 0,80mm, 1,00mm, 1,55mm, 2,00mm, 2,40mm and 3,20mm material thickness)
HDI Microvia printed circuit boards

At WEdirekt, we offer the following HDI Microvia layer stack-ups:

  • Layer stack-up 1-x-1 without buried vias (4 layers in 0.50mm, 0.80mm, 1.00mm or 1.55mm material thickness, as well as 6 and 8 layers in 1.00mm or 1.55mm material thickness)
  • Layer stack-up 1-xb-1 with buried vias (4 layers in 0.80mm, 1.00mm or 1.55mm material thickness, as well as 6 and 8 layers in 1.00mm or 1.55mm material thickness)


Flex-rigide, Flex with Stiffener and Flex

For WEdirekt, we offer the following layer stack-ups:

  • Flex-rigide 1F-1Ri (2-layer / 1,00 or 1,55mm)
  • Flex-rigide 1F-3Ri (4-layer / 1,00 or 1,55mm)
  • Flex-rigide 1F-5Ri (6-layer / 1,00 or 1,55mm)
  • Flex with Stiffener 1F-Ri (1-layer / 0.30mm)
  • Flex with Stiffener 2F-Ri (2-layer / 0.30mm)
  • Flex 1F (1-layer / 120 µm)
  • Flex 2F (2-layer / 170 µm)

Download Stack Ups

Thickness and material

For WEdirekt, you will get TG150 FR4 material for rigid boards. You will be automatically provided with polyimide (without adhesive) for Flex printed circuit boards.

We offer the data sheets for downloading here:

  • FR4 TG135
  • FR4 TG150
  • Flex


Rigid printed circuit boards

Basically, for our rigid printed circuit boards we offer material thicknesses of 0.80 mm, 1.00 mm, 1.55 mm, 2.00 mm, 2.40 mm and 3.20 mm. Here is a compact overview of how the material thickness of rigid printed circuit boards affects the availability of other options.

Depending on the material thickness and combination with other options, we manufacture Best Price (Pool) or More Technology (Non-Pool):

Best Price (Pool):

  • 0,80mm, 1,00mm, 1,55mm and 2,40mm thickness

More Technology (Non-Pool):

  • 0,50mm, 0,80mm, 1,00mm, 1,55mm, 2,00mm, 2,40mm and 3,20mm thickness
Microvia HDI printed circuit boards

For WEdirekt we offer you the following Microvia HDI material thicknesses, depending on the layer structure:

  • Layer stack-up 1-x-1 (4 layers in 0.50 mm, 0.80 mm, 1.00 mm or 1.55 mm material thickness as well as 6 and 8 layers in 1.00 mm or 1.55 mm material thickness)
  • Layer stack-up 1-xb-1 (4, 6 and 8 layers in 1.00 mm or 1.55 mm material thickness)
Flex-rigid circuit boards

For WEdirekt we offer you the following material thicknesses:

  • Layer stack-up 1F-1Ri: 1.00 mm or 1.55 mm material thickness
  • Layer stack-up 1F-3Ri: 1.00 mm or 1.55 mm material thickness
  • Layer stack-up 1F-5Ri: 1.00 mm or 1.55 mm material thickness
TWINflex® circuit boards
  • Layer stack-up 1F-Ri: Stiffener 0.30mm total
  • Layer stack-up 2F-Ri: Stiffener 0.30mm total

The FR4 stabilizer for TWINflex will be applied only one-sided.

Flex printed circuit boards
  • 1F = material thickness 120 µm
  • 2F = material thickness 170 µm


Dependencies to other Options

Thickness and material

  0,80mm 1,00mm 1,55mm 2,00mm 2,40mm 3,20mm
1, 2, 4 layer
6 layer X
8, 10 layer X X
12 layer X X
14, 16 layer X X X

Material Thickness and Smallest Via

  0,80mm 1,00mm 1,55mm 2,00mm 2,40mm 3,20mm
≥ 0.25mm
≥ 0.10mm X X X


We can also offer other material thicknesses. Please send us a request via email to We will pass your request on to your local Würth CBT representative.

Copper thickness

You can get a final copper thickness of 18μm, 35μm, 105μm or 70µm at WEdirekt. Here is an overview of which copper thickness you can order depending on the type of manufacture and/or production location.

Please note that an end copper of 18µm is only possible in conjunction with etching technology without a copper plating process.

For the outer layers we start with a thinner film, which is then built up in the production process to reach your required final copper thickness. The copper in the hole is 20 microns on average. The thinnest permissible copper in the hole is 18μm.

For the final copper thickness we ask you to consider the following:

  • The inner layers correspond to IPC 2221B Table 10-1
  • The outer layers correspond to IPC 2221B Table 10-2

Copper surface design tip

In order to ensure a uniform deposition of metal for your PCB, your layout should have a uniform copper distribution. We encourage you to fill free space with copper balancing.


Note for end copper thickness

You may wonder why we create the outer layers using a copper foil, which is not the same as the final copper thickness. Due to the processes used, copper is plated on to the board. This means that, for example, the use of an 18μm copper foil results in 35μm nominal final copper thickness.

The final copper thickness is governed by the tables stated in IPC 2221A above. Please note that the actual thickness of your copper PCB may be thinner. In the PCB industry, we use the terminology, final copper thickness, however this is nominal and the actual result may turn out thinner. This is not the rule, but can occur in the standard process. If you need to define your PCB copper thickness, we encourage you to send us an enquiry to We will pass your request on to your local Würth CBT representative.

Conductive Pattern and Structures

The following overview shows our specifications for the conductive pattern structures and distances for online orders. These apply regardless of how your circuit board is manufactured and the production location.

Outer Layers (18µm final copper)  85µm Structures 100µm Structures 125µm Structures 150µm Structures
Track width  ≥ 85µm  ≥ 100µm ≥ 125µm  ≥ 150µm 
Spacing track to track  ≥ 85µm  ≥ 100µm ≥ 125µm  ≥ 150µm 
Spacing pad to pad  ≥ 170µm ≥ 170µm ≥ 170µm ≥ 170µm
Spacing track to pad  ≥ 85µm  ≥ 100µm ≥ 125µm  ≥ 150µm 
Outer Layers (35µm final copper)  100µm Structures 125µm Structures 150µm Structures
Track width  ≥ 100µm ≥ 125µm  ≥ 150µm 
Spacing track to track ≥ 100µm ≥ 125µm  ≥ 150µm 
Spacing pad to pad ≥ 170µm ≥ 170µm ≥ 170µm
Spacing track to pad  ≥ 100µm ≥ 125µm  ≥ 150µm 


Outer Layers (70µm final copper)  192µm Structures
Track width  ≥ 150µm 
Spacing track to track  ≥ 192µm 
Spacing pad to pad  ≥ 192µm
Spacing track to pad  ≥ 192µm 
Außenlagen bei 105µm Endkupfer 250µm Structures
Track width  ≥ 150µm 
Spacing track to track  ≥ 250µm 
Spacing pad to pad  ≥ 250µm
Spacing track to pad  ≥ 250µm 


Inner Layer Structures 85µm 100µm 125µm 150µm 192µm 250µm
Final Copper Thickness 18µm*  18µm, 35µm 18µm, 35µm  18µm, 35µm  18µm, 35µm, 70µm 18µm, 35µm, 70µm, 105 µm
*Please note that an end copper of 18µm is only possible in conjunction with etching technology without a copper plating process. 


Dimension of Single PCBs and Delivery Panel

Single PCB

Please select this option if your board does not require a delivery panel. Generally, individual circuit boards are routed. The PCB may contain inner cut-outs, so long as the conductor pattern is not broken. If the copper tracks are to be broken, then we will produce the board, and refer to the PCB, as a delivery panel.

If your PCB is smaller than 30mm x 15mm in size, please create a delivery panel using the "Delivery panel using online configurator" option. PCBs smaller then this dimension may cause issues during production and may damage machinery.

The maximum PCB dimension that we offer at WEdirekt is 426 x 271 mm.

Delivery panel

Delivery panel from data or attached documentation:

Do you already have the single PCB data and a delivery panel drawing? Then this option is the right choice for you. We will produce your printed circuit board in a delivery panel according to your specifications. If you need break-off tabs, please include them in your data. An additional marking on the delivery panel is recommended. The dimensions of your delivery panel may not be smaller than 30mm x 15mm or greater than 426mm x 271 mm.

If you need a nested or mirrored panel, please send us the completed panellised PCB data at order entry. The same rule applies for multipanels i.e. a delivery panel which contains different PCB designs.

Delivery panel using online configurator

Do you already have the single PCB data but no delivery panel drawing, yet want to have your PCB delivered in a panel? You can use the Online Configurator to state how you want your panel to look. The dimensions of your delivery panel may not be smaller than 30mm x 15mm or greater than 426mm x 271mm. If you need break-off tabs, please state where they should be positioned in your data.


Fiducials in the panel frame
On request, we will add fiducials on the delivery panel frame of your boards. These will be executed according to our WEdirekt standard. This means, that 3 copper pads with a diameter of 1,00 mm will be placed in the center of your panel frame. In the solder mask, there will be a clearance of 2,00mm.

Bad parts on a delivery panel
It’s possible that our quality department will mark individual parts of a delivery panel with a black cross. Please don’t use these PCBs since they are not matching our quality standards. We never discard more than 50% of a delivery panel. Furthermore, we restock the missing quantity by sending you more delivery panels as you have ordered to make sure that you receive the quantity you need.

Special features for Flex printed circuit boards

  • The distance between the single PCBs in the delivery panel has to be ≥ 8.00 mm.
  • A delivery panel frame of ≥ 7.50 mm is mandatory on all four sides.
  • If there is a copper free area, we always add copper cross-hatching in the delivery panel frame on top and bottom to help avoid your board warping.
  • The delivery panel frame will always be coated with flexible soldermask on top and bottom (also if you have a 1F stack-up).


Notes to the dimension

The size of your PCB is measured from the centre of the PCB contour to the centre of the opposite PCB contour. This also applies to routing. Therefore we advise the use of a 200µm contour line to avoid confusion.

The outer contour of your PCB can be created using routing, v-scoring or a combination of both. Single PCBs without a delivery panel will be routed.

When routing a delivery panel, the PCB is held in the panel by tabs. The standard routing tools available are 1.60mm, 2.00mm or 2.40mm.

If v-scoring is used at WEdirekt, we place your PCBs edge to edge in the delivery panel.



Plated through holes (PTH holes)

For plated through holes, edge to edge the holes must have a distance of at least 400 µm. Please use the finished hole diameter to measure this.

Half-open plated through holes which are located on the contour of WEdirekt orders will be milled by us during the final cutting process. This can lead to burring on your PCB. In rare cases, it is possible that the plated barrel can be separated from the hole. Please consider this when you place an order through our WEdirekt Online Shop.

Note: If you need this technology, please contact us. Würth Elektronik will be happy to submit you an offer.

Non-Plated through holes (NPTH holes)

Non-Plated Holes are open after our manufacturing process. This means that these holes are not metallized.

Unique for HDI Microvia

Microvias are tiny holes in your PCB created using a laser. The most important parameter you need to consider is the aspect ratio (the ratio of hole diameter to the hole depth).

For online orders the Aspect Ratio needs to be 1:0.8.

In addition to the aspect ratio, the pitch plays a particularly important role in production. If you follow these three rules, there risk of issues with your layout and your PCB will be significantly reduced. This avoids queries and delays.

  • 0.75 mm BGA pitch (distance from center of the pad to center of the pad)
  • Our guidelines for clearances and structures
  • 350μm Microvia pad size

If your microvia pads do not meet our design rules, WEdirekt may amend the pad diameter to at least 350μm to ensure reliability.

Bond or BGA Pads <300µm

Bond or BGA pads <300μm cannot be displayed in the online shop standard process currently. You can request a corresponding quote here.


Buried Vias (HDI Microvia 1-xb-1)

A buried via refers to a hidden drill hole. It involves a via of at least two inner layers that have no direct connection to the outer layers. When selecting vias you must take into account drill hole diameter to the ratio of hole depth (the aspect ratio). The value must not exceed 1:10.

Important: Buried vias must be defined in the layout data as a separate drill file.



The Annular Ring

You should always consider the following rule when designing your data:

Pad Ø = Finished Ø + 0,35mm

For the nomenclature:

  • The Pad Diameter describes the solder pad
  • The final/finished diameter of your hole is often also called the nominal diameter or drilling diameter
  • The tool diameter is determined by us, which is also stated under the term drill diameter
  • The annular ring is the solderable ring after drilling


Design tip

If the annular ring in your layout does not conform to our specification then we will adjust the finished hole size or the pad diameter. As a result of this the price can increase.

Our advice: During the design of your PCB data consider the following rule of thumb: Pad diameter = finished hole diameter + 0.35mm

Routing and V-Scoring


The outer contour of your PCB will be routed. We use standard routing tools of 1.60 mm, 2.00 mm or 2.40 mm.


When v-scoring, we carve notches into your PCB to leave a thin defined residual ridge. The standard ridge thickness is 0.30 mm, with a tolerance to ± 0.10 mm. The scoring angle is 30°, on both the top and bottom side. If your panel design is unbalanced, we require a scoring path of 10.00 mm.

We will use v-scoring on your delivery panel, if your data dictates this process. V-scored boards have the advantage that they can be very easy to break apart. This can result in a small strip of residual material of up to 0.15 mm per side. Please note that your printed circuit board may be 0.30 mm larger due to this process.

In the manufacturing process, we can v-score in the horizontal and vertical direction.

Apertures and slots

Apertures and slots are routed or nibbled by us. Depending on your layout, we will plate or leave them non plated as required.

If a cut-out is less than 1.60 mm (radius ≤ 0.80 mm), please select the appropriate cutting tool for your PCB in the calculator.

For manufacturing reasons we have to mill non-plated cut-outs ≤1.5mm using a milling tool 0.2mm smaller than the cut-out. The cut-out won’t be any smaller due to this, but we need to follow this procedure to ensure that no residues from the milling process remain in the cut-outs. Plated cut-outs are not affected by this procedure.

Design tip

Please note, that we cannot consider plans that differ from your CAM files. This applies, for example, for openings or additional mechanical details. Every note has to be part of the CAM data.


To avoid burring on your WEdirekt PCB, please consider the following distance rules. If your design includes distances smaller than required, we will amend these for you. If the design requires smaller distances, please contact us.

Material Thickness Copper to V-Score Copper to Routing  SMD Pads
0,80mm 0,40mm 0,25mm 20%
1,00mm 0,40mm 0,25mm 20%
1,55mm 0,50mm 0,25mm 20%
2,00mm 0,60mm 0,25mm 20%
2,40mm 0,70mm 0,25mm 20%
3,00mm 0,80mm 0,25mm 20%


Tolerances / Mechanic

Plated through holes   +0,10 / -0,05mm 
Non-Plated through holes   +0,10 / -0,10mm 
Hole to hole in one run    +0,05 / -0,05mm 
Contour routed  ≤ 0 - 30mm
> 30 - 120mm
> 120 - 200mm
> 200 - 400mm
> 400mm 
+0,10 / -0,10mm
+0,15 / -0,15mm
+0,20 / -0,20mm
the more 100mm
+/- 0,050mm 
Contour scored
Scored and routed 
DIN ISO 2768 middle
DIN ISO 2768 middle
Outline to non-plated hole, contour routed    +0,10 / -0,10mm 
Outline to non-plated hole, contour scored   +0,15 / -0,15mm 
Contour routed
Contour scored
Contour routed/scored
Contour routed/scored  

≥ 30,00mm 

+0,10 / -0,10mm
+0,15 / -0,15mm
+0,20 / -0,20mm
+0,30 / -0,30mm 

Image to drill    +0,10 / -0,10mm 


Chamfering and Sideplating


You can choose between 20° PCI and 45° ISA. Top and bottom is always chamfered in the process. Please also follow the information for electroplated gold.

Note: the depth of the chamfer depends on the thickness of the PCB.


We offer sideplating for the outer edges of your circuit boards. We kindly ask you to follow the design parameters to ensure flawless production.

In your layout data, the circuit board edge to be sideplated must be marked with 500µm of protruding copper. A connection of at least 300µm must also be defined.

Layers that are not to be connected should have a clearance of at least 800µm on the outer contour.

Surface Finish

Electroless nickel gold, HAL lead-free and immersion tin surface are offered for all types of manufacture and locations. However, HDI Microvia and Flex printed circuit boards can only be manufactured in conjunction with electroless nickel gold or immersion tin.

The surface finish of your PCB is designed to protect against oxidation. It also allows for easier soldering of your PCB.

HAL lead free

The Hot Air Solder Levelling (HASL lead free) produces a homogeneous tin coating. This finish provides longer shelf life and good solderabil

Electroless nickel / immersion gold and Immersion Tin

For the electroless nickel / immersion gold and immersion tin surface finish, a thin metal coating is applied onto your PCB using a chemical process. An advantage over HASL lead free is the defined thickness of the metal coating. In addition, we can create thinner conductive patterns on the PCB. For this reason, WEdirekt only offers immersion surfaces for our HDI microvia printed circuit boards.

The shelf life of the electroless nickel / immersion gold and lead-free HASL surface finish is twelve months. Immersion tin has a shelf life of a maximum of six months.

The thickness of our ENIG surface is 0,05-0,1µm gold and 4-7µm nickel.

Useful information about our surfaces

Surface Thickness Storability Notes
Chemical nickel-gold (ENIG)  4-7 μm Ni
0,075 ± 0,025 μm Au 
12 months - Low process temperature (approx. 90 °C)
- Smooth coating
- Suitable for aluminium wire bonding
HAL lead-free (Hot-Air-Leveling)  1-40 μm 12 months - High process temperature (D9265-280 °C)
- Increased Cu removal, dependent on layout 
Chemical tin (Sn) 0,8-1,1 μm 6 months - Low process temperature (approx. 70 °C)
- Smooth coating
- Growth in the intermetallic phase between Cu and Sn 
- Layer thickness >1µm required for multiple soldering
- Rapid processing in the assembly process 


You need a surface for gold wire bonding? Than send us your enquiry, we would be pleased to submit you an offer!

Hard gold

Hard gold is only done in combination with connector contacts. Full-area plating is not possible. The thickness of our surface is 1-3µm gold and 4-7µm nickel.

Please follow the rules regarding the gold connectors.

Solder Resist

At WEdirekt, we offer a green, photosensitive solder resist. Please note in your design, the following rule of thumb:

Solder Mask Pad Ø = Copper Pad Ø + 0,10mm

If your board has different values, we will adapt the layout to this rule of thumb. This is to be keep solder surfaces free of solder resist. Our recommended soldermask web is a minimum of 70μm. You can download our solder resist datasheet here:

Remark: We use flexible solder mask for PCBs with a thickness of 0.50mm.

Information regarding the thickness of our solder resist 

Thickness over base material: 20-45 µm
Thickness over track: 10-25 µm
Thickness at the knee of the track: ≥ 5 µm 


Remark for vias in solder mask

At WEdirekt vias are always cleared in the solder mask. If the vias in the solder mask have no clearance in your layout files, we will automatically adapt this so that the vias will be not covered with solder mask. We use the smallest possible diameter for the clearance.

This is not valid for HDI microvia PCBs. Here the laser vias will be covered with solder mask if it’s in your layout.


The solder resist provides multiple benefits. Solder resist can:
  • Protect your board against corrosion and mechanical damage
  • Prevent short circuiting when soldering and wetting of certain areas
  • Isolate components from the PCB surface
  • Improve impact strength of your PCB

Silk screen (legend, partial)

WEdirekt offers you a standard service print in the colour white. Our Non-Pool area gives you the option of choosing the colour yellow, red, blue and black.

If you follow our instructions with respect to the text, we can avoid the merging of the text and improve legibility.

Please do not place silkscreen over solderable areas. If this is present in your design, WEdirekt will remove the silkscreen from the area.

Checkliste for Silk Screen
  • Font Thickness: ≥ 80 microns
  • Spacing between Characters : ≥ 80 microns
  • Font Height: ≥ 1.50 mm
  • Distance to the solder masks opening: ≥100μm


Want to know more? Here we go!

Silkscreen may also be referred to as component legend or legend. It is used to mark the placement of the components on your PCB.

Why do we not print silkscreen on to solder pads? If we were to apply silkscreen to solder pads, issues would occur during soldering, assembly and E-Testing.

Do you use the EAGLE CAD software? In this case, you should change the software settings under "Options", to always select "Vector font ". Without this, text display difficulties may occur.

PCB in black, red and blue

Example image of a printed circuit board with green solder resist and fully coated silkscreen.

Fully coated silkscreen

The fully coated silkscreen is an alternative to colored solder resist. At the edge of the colored print the green solder resist is still visible.

Checkliste for an optimized fully coated silkscreen
  • Distance to the solder masks opening: ≥100μm


E-Testing is free for multilayer printed circuit boards. For one- and two-layer printed circuit boards you have the opportunity to decide whether you require an E-Test or not.

During E-Test, we test your PCB for electrical defects. Between the end points of an electrical network, we run a measuring voltage to check the circuit. Through this, we rule out short circuits or track breaks.

At WEdirekt, we test your PCB in the production panel. Due to this method, it is not possible to mark the edge of the tested circuit board with a black line.

UL Marking

If you want and if there is place, we include an UL marking on your PCB. The marking is in the silkscreen or in the solder resist and will be carried out according to the UL guidelines. If you specify a certain place, we will create the marking where stated.

Please note that the UL marking contains the Würth Elektronik manufacturer's label and the date of manufacture (yy/ww).


Important note: Flex printed circuit boards, circuit boards < 0.80 mm and circuit boards with fully coated silkscreen are not provided with the UL mark.

Certificate of Conformity

We gladly offer you a Certificate of Conformity (CoC). You can easily order the document while you configure your PCB.

You want to know more about the content? Please find an example here.


Missing, unclear, duplicated or incorrect files result in clarifications. This can lead to a postponed delivery date. To help avoid this, please kindly bear the following points in mind:

  • Does your dataset contain all the layers that we need for the production of your PCB? Are the drill files included?
  • If something could be unclear you should add an information as a text document to your data set.
  • Does the layout file match the online configuration? If we get different information we decide according your online order and producibility.
  • If you send your PCB in different data formats we choose the layout of our choice (preferably Ext. Gerber).
  • If you order a “Delivery Panel from Data” with different PCBs in one panel please send us the already designed delivery panel. We only design your panel if we can duplicate the same layout.
  • We produce orders according to our specification. If your PCB data does not meet the specification, yet is still suitable for manufacture, we will produce without consultation.
  • The configuration chosen by you on our calculator has priority over the data attached. For example, if a PCB is ordered without silkscreen yet the data contains silkscreen, the PCB would be produced without silkscreen.
  • We always assume that stubs (tracks without electrical connection) are placed with intent. We won’t contact you to query any stubs.
  • Impedance requirements, given in your data or documentation attached, cannot be met, due to a mixed copper distribution within our production panel. We will process your job according to our standard stack-ups and without further queries.
  • If we have to ask for new data because of missing layers or wrong layouts it generates a high extra effort in our production engineering. We reserve the right to bill this effort with 30.00 Euro per requested data set. This also applies when we get new files after the data check. Both situations can result in a postponed delivery date. Please pay careful attention to the supplied data.

If you have questions we are glad to help you further!

We are happy to make you an offer for your board outside of WEdirekt if you have different requirements. Please send us an enquiry. We will pass your request on to your local Würth CBT representative.