Cart-logo
0

The Guidelines provided below not just help to reduce the cost of your boards but also minimise the risk of manufacturing errors. For details, you may refer to our services overview. In the following section you can get familiar with:


  • Data formats accepted by PCB POWER for production of your PCB prototypes and small series.
  • Requirements for design data to comply with the PCB POWER specifications to allow a smooth production of your PCB prototype.
  • Guidelines for Drills ( PTH as well as NPTH).
  • Design guidelines for the copper pattern.
  • Design guidelines for the mechanical layers ( contours, slots, etc ).
  • Design guidelines for generation of soldermask, legend, carbon pads, peel-off mask, via fill, and heat-sink paste.
  • Design guidelines for Panel.

Input Data Format: Accepted data formats for PCB layout data are:


  • Gerber RS-274X (Extended Gerber with embedded apertures – developed by Gerber Systems).
  • DPF (Dynamic Process Format – developed by Ucamco NV).
  • Gerber RS-274D (Standard Gerber with a separate aperture file – developed by Gerber Systems).

By PCB layout data we mean all the copper layers, soldermask and legend layers, board outline or mechanical layer, SMD pasta layers, carbon layers, peel-off layer, etc. We step up the accuracy and efficiency of tooling by encouraging the designer to output the Gerber file in a RS-274X output and hence relieve the PCB manufacturer from loading apertures during the tooling process. NC data: NC data refers to the drill and profile data with the following accepted formats:


  • Excellon (1 or 2) + appropriate tool list (ideally embedded).
  • Sieb&Meyer + appropriate tool list (ideally embedded).
  • Gerber format RS-274X or RS-274D (only true drill data, no drillmap).
  • DPF (only true drill data, no drillmap).

IMPORTANT: Please supply ONLY ASCII-encoded files. These files are man-readable which enable our engineers to check them visually if needed during data preparation. CAD PCB design data is NOT at all accepted by us!


  • Converting CAD data into production data may lead to errors which cannot be cross-checked.
  • It is impossible to have legal copies of every CAD PCB design package in the market or the knowledge required for their correct usage. Since all designers do not use the same software version, we would have to provide a whole range of update patches as well.

Gerber being clear and unambiguous has since years been the industry-standard format for PCB manufacture. Every PCB design package can output Gerber data. A complete description of the process has been provided in your CAD PCB design package handbook and help-files. You can check the accuracy of the Gerber output data by downloading one of the many free Gerber viewers available on the Internet. We recommend GC-Prevue available as freeware from www.graphicode.com. Input data requirements:


  • Preferred data formats are:

For PCB layout data — Extended Gerbers (RS-274X) For Drilling — Excellon1 + appropriate tool list (ideally embedded)

  • Provide us ONLY with the data files needed for production. These are:

  • 1.Gerber files for the copper layers, soldermask and legend layers, mechanical layer and SMD paste layers in addition to carbon, peel-off and via-fill layers as needed as per the service selection criteria.
  • 2.Excellon drill file(s) for drilling.
  • 3.If you want us to prepare a customer panel (“array”, “matrix” or “biscuit”) from the single board data to your individual specification, the panel plan can be supplied as a Gerber of DPF file.

  • Please do not provide any additional files such as original CAD data, Graphicode GWK files, PDF files, Word files (doc), Excel files (xls), part lists, placement and assembly information, etc.
  • Please check wherever possible your generated output data (Gerbers & Excellon) with a Gerber viewer before you send it on to production. Make sure that all instructions or other necessary input needed for making the boards are included in the Gerber and Excellon files.
  • Please use clear and easy to understand filenames and avoid long filenames as far as possible. Make it easy for us to determine the layer function from the filename or add readme file for file identification.
  • Please do not scale your data. All data provided must be scaled 1/1 (100%).
  • Please make sure that your Gerber files do not contain apertures with a zero-size (size = 0.00mm) and that your Excellon data does not have zero-sized tools (size=0.00mm).
  • Please use the same offset for all your Gerber layers and the Excellon drill data. We do not prefer different offset.
  • Please use the same units (mm or inch) in your Gerber & Excellon output files as in your CAD PCB design software. This will prevent conversion or rounding of errors.
  • Please use the same resolution (grid) for your Gerber & Excellon data to allow a perfect match. Please also make sure that the resolution (grid) used for your output (Gerber & Excellon) is at least a factor 10 better than the resolution (grid) used in your CAD PCB design software.

Example: If you use a 10 mill resolution to draw your board in your CAD PCB design software, then use a 1mil output resolution for your Gerber & Excellon output.


  • Please make sure that your data is supplied as seen from top to bottom through the PCB. Do not mirror (or reflect) any data layer – image or drill. Viewing a PCB from top to bottom through the board is the universal practice in the PCB industry. We view and handle your data in that way, as does your CAD PCB design software.
  • This means that when viewing your Gerber data, text on the top side of your board (copper, soldermask, legend) should be readable and text on the bottom side (copper, soldermask, legend) should be non-readable.
  • Please use top viewed right-reading text to label every gerber layer to prevent mirror board production.
  • RECOMMENDED: In your Gerber files use flashed pads as often as possible.
  • RECOMMENDED:. In your CAD PCB design software try to create an aperture list for Gerber output showing only the apertures used in the design.
  • Make sure to include the board outline on all layers. This will enable us to properly align all layers in case of an offset problem. Also include the board outline in a separate Gerber mechanical plan.

Technical Capabilities: General Board Specifications


  • Laminate: FR-4.
  • PCB Thickness: 0.8mm / 1.6 mm/2.4mm.
  • Start Copper Thickness: 17.5 Microns/ 35 Microns/ 70 microns.
  • Min. Track Width/ Spacing: 0.17/ 0.15mm (7 Mils/ 6 Mils).
  • Min. Hole: 0.40mm (16 Mils) FINISH.
  • Min. SMD Pitch: 0.5mm (20 Mils).
  • Solder mask: Green/ Blue/ Black.
  • Surface Finish: Hot Air Leveling (HAL)/ Lead Free HAL/ Immersion Tin / Immersion Gold (ENIG).
  • Legend: White/Black/Yellow (White is default , other colors are subject to availability, please contact our sales team for further details.).

Product Specifications :


SPECIFICATION STANDARAD PROTOTYPE
Minimum Conductor Width (TW) 5 Mils/ 0.127 mm 4 Mils/ 0.10 mm
Minimum Conductor Spacing (PP, TP, TT) 5 Mils/ 0.127 mm 4 Mils/ 0.10 mm
Minimum Plated Hole Size 10 Mils/ 0.25 mm 8 Mils/ 0.20 mm
Maximum Board Size (Active) 610 Mm X 400 mm 820 Mm X 400 mm
Maximum Number Of Layers 18 24
Maximum Outer Layer Cu. Thickness 4 Oz (140 Micron) 6 Oz (210 Micron)
Maximum Inner Layer Cu. Thickness 2 Oz (70 Micron) 3 Oz (105 Micron)
Board Thickness Tolerance + / - 10% + / - 10%
SMD Testing 20 Mils/ 0.50 mm 15 Mils/ 0.38 mm

PTH-NPTH Tolerances
PTH HOLE SIZE PTH TOLERANCE NPTH HOLE SIZE NPTH TOLERANCE
0.50-3.50 mm +/- 0.10 mm < 3 mm +/- 0.10 mm
>3.50 mm +/- 0.15mm > 3 mm +/- 0.15 mm

PCB Size Tolerances
SIZE TOL.
<150.00 mm +/- 0.20 mm
>150.00 mm +/- 0.50 mm

Other Tolerances
Thickness of PCB +/- 10%
Tolerance for Track width / spacing +/- 20%
Tolerance for Finished copper thickness (Plating in hole is considered) > 20 micron

Product Finish : 1) PROTOTYPES

I) LEAD-FREE FINISHES


  • ELECTROLESS NICKEL IMMERSION GOLD
  • IMMERSION TIN
  • LEAD FREE HAL

II) ELECTOROLYTIC GOLD PLATING


  • HASL
  • CARBON PRINTING.
  • PEELABLE MASKING.

2) SOLDER MASK FINISH


  • PHOTO IMAGEABLE LIQUID SOLDERMASK.
  • SMOBC (GREEN, BLACK, RED, BLUE).
  • DRY FILM SOLDERMASK.

3) PRODUCT RAW MATERIAL


  • 3) PRODUCT RAW MATERIAL.
  • RT DUROID ( ROGERS ).
  • SPECIAL LAMINATES.

Annular Ring: Annular Ring = 1/2 (Circuit layer pad diameter – PHD) Where PHD = Production Hole diameter or Tool ize = finihed hole size + 0.15 mm for Plated Through Holes = finished hole size + 0.05 mm for Non Plated Through Holes


Minimum Annular ring for Outer layers:0.125 mm Minimum Annular ring for Inner layers:0.125 mm IMPORTANT: Annular Ring calculations are carried out from the production TOOL SIZE for the holes, not from the finished hole ENDSIZE. For connected non-plated (NPTH) holes we recommend a minimum annular ring of 0.50 mm. As NPTH holes have no plated barrel, a smaller annular ring may lift during soldering or break away even during normal operating conditions. Holes:

MIN. FINISHED HOLE SIZE MAX. BOARD THICKNESS
0.20 mm 1.60 mm
0.35 mm 2.00 mm
0.40 mm 2.40 mm
0.55 mm 3.20 mm

Minimum drill – drill clearance: 0.15 mm. This is measured edge to edge of the drill TOOLSIZE.Please do not overlap drill holes. These can cause broken drill bits and the small pieces of material left behind may cause voids in the plated hole barrels. Note:  Please do not use overlapping drill holes to define slots.

1. Tool lists for drill files are ALWAYS read by our CAM systems as finished hole sizes (ENDSIZE).

2. All PCB drills are manufactured in step of 0.05 mm so wherever possible combine the drill sizes that are within 0.05mm with each other. So we convert the drill sizes given in the drill files or tool lists into millimeters and round up to the nearest 0.05mm. For example:


  • Drill size of 31mil is converted to 0.7874mm and then rounded to 0.80mm.
  • Drill size of 32mil is converted to 0.8128mm and then rounded to 0.80mm.
  • Drill size of 33mil is converted to 0.8382mm and then rounded to 0.85mm.

3. If possible, provide separate drill files for plated (PTH) and non-plated (NPTH) holes. Or else, please specify different tools for PTH and NPTH holes and mark clearly which tools are PTH and which tools are NPTH.

4. When no PTH/NPTH info is provided we use the following rules to determine PTH/NPTH: For 0-layer and 1-layer boards: All holes are considered as NPTH by default. For 2-layer and multilayer boards: All holes are considered PTH except the following cases which are considered NPTH:


  • Non-connected holes without copper pads.
  • Non-connected holes where the copper pad size is equal to or smaller than the drill TOOLSIZE (the copper pad will be removed in single image preparation).
  • Connected holes with a copper pad on 1 side (outer), no connection on any other layer (outer or inner) and no copper pad on the other side (outer).

5. To allow for the plating in the hole we drill holes prior to plating at a larger size (drill over-sizing). The conversion rules from finished hole ENDSIZE to production TOOLSIZE are: TOOLSIZE = ENDSIZE + 0.15mm for Plated Through Holes (PTH) + 0.05mm for Non Plated Through Holes (NPTH)

6. Standard tolerances on drill ENDSIZE diameter. NPTH holes:  +/- 0.10mm  (for drill size <3.0 mm) +/- 0.15mm (for drill size >3.0 mm) PTH holes:    +/- 0.10mm  (for drill size <3.5 mm) +/- 0.15mm (for drill size >3.5 mm) In case there are no tolerances specified in your data, we will produce according to our standard tolerances.

7. Drilled holes that overlap the board contour can be, NPTH holes without copper pads: these NPTH holes will be treated as part of the board outline. PTH holes with copper pads: these PTH holes will be considered as plated holes on the board edge.

8. Overlapping drill holes. Please do not overlap drill holes. These cause broken drill bits and small remaining material parts may cause plating voids in production. Copper layer:


  • When generating output, use “flashes” for pads and avoid “drawn pads” (i.e. pads filled with small draws)

  • Avoid drawn planes, filling large copper areas or copper planes with small draws (“painting”). Where possible, use contours or polygons to construct areas or planes. Contourized areas or Polygon Area fill are standard features in Extended Gerber output (RS-274X).
  • When generating output include the board outline in your copper layers.


  • Remove copper pads from NPTH holes if these pads are not used or connected to other copper. If you require copper pads on NPTH holes then it is advisable to use a minimum Outer Annular Ring (OAR) of 0.50mm.
  • Minimal clearance between PCB edge and copper pattern.

For routed boards:                      – 0.30 mm on outer layers
                                                – 0.50 mm on inner layers
For boards with scoring (V-cut):    – 0.50 mm on outer and inner layers
             If you require a copper area or plane to extend up to the board edge, then clearly indicate this in the mechanical layer.
             If you require the board edge or part of it to be plated, then clearly indicate this in the mechanical layer.

  • All copper text must be correctly readable.
  • Avoid peelables & same net spacing errors.

Multilayers: When designing multilayers, the following should be considered:


  • Always design in an even layer count, such as 4, 6, 8, 10…layers. This will produce a symmetrical lay up which in turn please minimizes warp.
  • ALWAYS provide the proper layer sequence for a multilayer board. The layer sequence can be given in several ways: Indicate the layer numbers in the copper image by placing a logical number in each layer (1 for top layer, 2 for inner1, 3 for inner2, etc….).


  • Stack ups should be left to us to determine the most cost effective layup. All multilayers should be symmetrical in stack up.Symmetrical stacks up is achieved by balancing the top and bottom of the stack up equal in relationship to the center most cores. Keep in mind that plane layers should also follow this rule. Therefore if a power and ground plane are to be used, then if in a 8-layer PCB the power plane is on layer 2, the ground plane should be on layer 7.
  • INNER LAYER PAD ISOLATION (IPI): We recommend keeping the isolated pads on inner layers 0.95 mm greater than the drill size. Since we drill 0.15 mm over the desired finish hole size (to allow for plating), the clearance pad should be 0.80 mm + the production hole size and not the finished hole size.

  • Drill to track clearance: We recommend keeping the clearance from drilled hole to nearby track by 0.40 mm.
  • Thermal definition: Make sure your thermal relief pads are properly defined and comply with the production requirement for Annular Rings (AR), Track Widths (Thermal Segment Width) and Gaps. Good practice for Thermals is to work with a Gap of 0.25mm (10mil) and a Thermal Segment Width of 0.20mm (8mil).

  • Avoid thermal isolation.

Soldermask & Legend Print: There are minimal concerns when considering solder mask and silk-screen design rules. Our standard process is LPI (Liquid Photo Imageable) which produces the best registration around pad features.



  • Mask Opening: Typically solder mask should have a minimum of a 0.10 mm “growth/mask opening” around the pad to allow for any mis-registration.
  • And the minimum solder mask “dam” should be 0.10 mm (a dam is the minimum track size of solder mask).
  • Once the “dam” goes below 0.10 mm, it becomes more dfficult to process without the “dam” lifting off the the PCB.

IMPORTANT: Solder mask dam smaller than 0.10 mm will be removed and will be converted to the image below.


  • For Legend print, the main consideration is font size and its hight. We recommend a 0.15 mm font minimum.

  • The legend print will ALWAYS be broken – or clipped – against the corresponding soldermask layer.

General Note:  Legend clipping is done with respect to solder mask layer & drill layer as our standard to make sure legend ink doesn’t come on pad for better soldering. Clipping rules:

  • Legend clipping clearance is 0.10mm (4mil). This means that we clip the legend 0.10mm (4mil) back from the soldermask openings.
  • Any bits of line smaller than 0.17mm (7mil) are removed.
  • In absence of a soldermask layer, the legend print is clipped against the corresponding copper layer. If there is no copper layer, the legend is clipped against the drill layer.

Design Tip: To avoid your legend being clipped maintain a minimum distance of 0.20mm (8mil) between your legend elements and the copper image. This 0.20mm (8mil) = 0.10mm (4mil) Soldermask Annular Ring + 0.10mm (4mil) Legend Clipping Clearance. Mechanical Layer: A mechanical layer should minimally contain: 1.The exact board outlines, ideally including dimensions (mm or inch). 2.Exact positions and sizes for all inside milling, slots or cutouts, ideally including dimensions (mm or inch). IMPORTANT: When no dimensions are given we will always take the center of the contour lines to be the exact outline of the board, regardless of their thickness. Additional information that should be included in the mechanical plan when needed:

  • A reference hole: the distance from one drill hole in X and Y to the PCB outline. This is particularly important when you only have NPTH holes without copper pads.
  • Positional indication of all drills using symbols (=drill map). Use different symbols for each different drill size.
  • PTH/NPTH indication for holes and slots.
  • If you supply panelized data include proper indications for break-routing and/or scoring (V-cut).
  • A clear layer sequence or buildup drawing including all copper layers, soldermask and legend layers, any additional layers like peel-off or carbon, in the correct sequence viewed from top to bottom and with the correct corresponding data file name.

If the PCBs are to be delivered as an array for assembly, then the mechanical drawing for the array should be included as well. The overall tolerances for mechanical dimensions are +/- 0.25mm. It is important to note that hole sizes should be specified as finished hole sizes. Carbon:

  • 1.Carbon elements or patterns are printed with a conductive carbon ink and can be used for keyboard contacts, LCD contacts, jumpers, etc.
  • 2.Always clearly indicate on which side of the PCB carbon is to be applied. This can be on one side or on both sides. IMPORTANT: Indicate the position by proper file naming and a clear buildup or layer sequence description in the mechanical layer. (See section Input data requirements – point 2, 3 and section Mechanical layer point 3)
  • 3.When generating output include the board outline in your carbon layer(s). This is best done using a small line – e.g. 0.50mm (20mil) wide – where the center of the line is the exact board outline. We will remove this line from the production-ready data.
  • 4.Overall carbon design rule specifications:
  • Minimum carbon line width: 0.30 mm.
  • Minimum carbon – carbon spacing: 0.25 mm.
  • Carbon pad should be 0.15 mm bigger than circuit pad.
  • Mask pad should be 0.15 mm bigger than circuit pads. Means Mask pad = Carbon pad.

1. Peel-off masks are used to:

  • Protect selected solder holes and pads against solder plugging during mass soldering.
  • Protect gold-plated contacts or carbon elements during mass soldering.

2. Generally the peel-off mask is applied ONLY to 1 side of the PCB, usually the bottom side.

  • Minimum width of any Peel-off element (P): 0.500mm (20mil).
  • Maximum coverable hole ENDSIZE (H): 6.00mm (236mil).
  • Minimum overlap on copper pattern (V): 0.254mm (10mil).
  • Minimum clearance to free copper (W): 0.254mm (10mil).
  • Minimum distance from PCB outline: 0.500mm (20mil).
  • Tolerance on position: +/-0.300mm (12mil).

5. Avoid using many different small peel-off areas randomly placed on your PCB. Make the peel-off area as large as possible by connecting the separate peel-off areas wherever practical. This will make it easier to remove the peel-off after soldering.

Via Fill: 

  • Completely closed via holes can only be guaranteed by using ViaFill.
  • The maximum via hole ENDSIZE that can be completely closed is 0.25mm (10mil).
  • ViaFill is done by covering the via pad and via hole with a second layer of soldermask.
  • ViaFill data should be provided as a Gerber file containing only the via pads that need to be filled and the PCB board outline.
  • When generating output include the board outline in your ViaFill layer. This is best done using a small line – e.g. 0.50mm (20mil) wide – where the center of the line is the exact board outline. We will remove this line from the production ready data.
  • Typically ViaFill is applied ONLY to 1 side of the PCB. It depends on the design of the PCB.

IMPORTANT: CLEARLY indicate on which side of the PCB (top or bottom) the ViaFill should be applied. Use proper file naming and clear buildup or layer sequence description in the mechanical layer.

Panel:
If you want your PCBs delivered in a panel for assembly purposes, you have several ways to specify the layout. They are as follows:
  • Order a standard layout from the menu options and we build the panel -available on all services.
  • Provide the fully panelised Gerber data – available on all services. There are some manufacturability rules listed below.
  • Provide the single image and a panelisation drawing and we build the panel for you – available on the On demand service only. There are some manufacturability rules listed below.

Notes:

  • 1.Some conventional manufacturers suggest that you put a number of different circuits on the same panel to improve material utilisation and reduce manufacturing costs. We do this automatically as part of our pooling process, so there is no need for you to waste valuable design time. Only order a panel, if you need it for assembly.
  • 2.Any layout which includes multiple circuits or snap-off borders must be ordered as a panel even if you don’t ask us to profile round the circuits.
  • 3.If your layout uses SMD components we automatically panelise a solder-paste layer which you can download as a Gerber file for stencil manufacture. We can generate the paste files from the SMD pads on a “best-efforts” basis but it is not always clear to us which pads to include and which to leave out. So we recommend that you check these files before you use them. It is much safer to generate a paste file yourself and include it in the data you send us. We will then check it with the rest of the data and step and repeat it into the same assembly panel. If you want your PCBs delivered in a panel for assembly purposes, you have several ways to specify the layout:
  • 4.X-outs Panels may be delivered containing a number of rejected PCBs.
NUMBER OF CIRCUITS PER PANEL MAXIMUM NUMBER OF REJECTED CIRCUITS
02 - 03 1
04 -06 2
07 - 10 3
11 - 15 5
16 - 20 7
>20 10

The position of the defective PCBs will be clearly marked.

If you need panels which do not include rejected PCBs (X-outs), please order them via the On Demand service and tick the “Panel without cross outs” box.

1. Panelise using menu options: “Power Verified” and “Power On demand” services. Using this service you upload one design and indicate the step and repeat you require. We will automatically construct the panel and add a frame with standard tooling holes and fiducials (optical marks) for assembly machines.

1.1. Manufacturability rules:

  • Minimum dimension of the single PCB is 5.00 mm X 5.00 mm.
  • Maximum panel dimensions on the Power Standard is 250 x 350 mm. For larger panels on the On demand service, please contact sales@pcbpower.com.

1.2. To get a price or place an order.

  • Under the Board Definition tab select “Panel”.
  • Tick on “PCBPOWER” lying on the opposite of “Panel. In the On Demand menu opposite “Panel Rules” tick “PCBPower panel specific” (this is the only option on the Verified and Verified Plus services).
  • “Diff(erent) designs per panel” remains grayed out as only 1 design is allowed. If you want to include two or more different designs please use panelization methods 2 or 3.
  • Enter the dimensions of the single circuit in the “Dimension X” and “Dimension Y” boxes
  • In the “X” and “Y” boxes enter how many times the circuit has to be copied. The system will automatically calculate “Panel Dim X”, “Panel Dim Y” and “No. of PCB Boards”. If the panel dimensions are too large you will receive a warning message.
  • Select the “Board Separation” method on the Verification Plus and On demand services (on Verified only breakrouting is available). Breakrouting, V-cut and “none” which – if you wish to separate the boards yourself- are available on the Verified Plus and On Demand services; and a combination of breakrouting and V-cut (e.g. for non-rectangular circuits) on the On Demand service.
  • Select the “Distance between two PCB’s” from the pull-down table: the options are 2, 5 or 10 mm (a minimum of 2 mm is needed to accommodate the 2 mm cutter). For V-cut the system will automatically enter a zero separation but there must be a 0.45 mm zone free from copper on all sides of the board.
  • Select the “Panel Border” from the pull-down table: the options are 5, 7 or 10 mm (a minimum 5 mm border is needed to give a stable panel and to accommodate optical markers and tooling holes).

1.3. Profile and break-out tabs:

  • Include the profile of the board on at least one (better every) copper layer or on a separate mechanical layer.
  • Our front-end engineers will review the panel and add break-out tabs based on their experience to maintain stability and allow easy breakout of the PCBs after assembly. For stability during handling and transport we recommend that if you need a panel with a large number of small boards, you specify a distance between circuits of 5 or 10 mm and a border of 7 or 10 mm. For circular shaped boards the break-out tabs are preferred to be positioned at 45° angle which results in the pcb to be attached to the panel rather than to be attached the nearby circuit.

Example: “Panel by PCBPower ” with breakrouting 

  • PCB X = X dimension of the single circuit.
  • PCB Y = Y dimension of the single circuit.
  • A = distance between PCBs – for breakrouting the minimum is 2.0mm.
  • B = mandatory border – minimum 7.0 mm required (5.0 mm of laminate border and 2.0 mm for the router cutter).
  • Pan X = auto-calculated X dimension of the panel.
  • Pan Y = auto-calculated Y dimension of the panel.
  • Final result after production :

1.4. Detail of panel border :

Example “Panel by PCBPower” – V-cut

  • PCB X = X dimension of the single circuit.
  • PCB Y = Y dimension of the single circuit.
  • A = V-cut or ‘scoring’ line – a copper-free area of 0.45 mm from the edge of the PCB is mandatory for V-cut scoring. (see also image below).
  • B = mandatory border – a minimum 5.0 mm laminate border is required.
  • Pan X = auto-calculated dimension of the panel.
  • Pan Y = auto-calculated dimension of the panel.