Table of Contents

1. PCB layout

2. Component placement plans

3. Pick & Place file

4. Bill of materials (BOM)

5. Stencil

6. Components

7. Soldering SMD (vapour phase)

8. Soldering process THT (selective wave)

9. THR (Through Hole Reflow)

10. Component placement variants

11. Panel

12. Lead time

13. Terms and definitions

14. Instructions on how to create the BOM and component placement plan for EAGLE

15. Instructions on how to create the BOM and component placement plan for Altium

16. Instructions on how to create the BOM and component placement plan for Target 3001!

17. Instructions on how to create the BOM and component placement plan for GERBER


This guide is designed to aid in allowing a problem-free component placement. Please consider the following points when placing an order with us.

1. PCB layout

The first mistakes often occur at this initial stage and can affect the whole project.
 
Component labeling and footprints on a green PCB Footprints and component labelling
Footprint
Please make sure that the footprints (land pattern), that is the component landing points of the components to be assembled, comply with the specifications of the respective manufacturer.
IPC
Alternatively, the IPC-7351 also contains recommendations and design specifications: http://www.ipc.org/
Footprints from standard libraries
Footprints from the standard libraries such as eagle "rcl.lib" tend to differ greatly from these specifications. They are suitable for a manual component placement, but not for automatic machine placement.
Vias
Please avoid placing vias on the soldering surfaces of components pads, this causes the solder paste to flow during reflow and will not guarantee a reliable solder joint. This can also cause the 'tombstone' effect where components are lifted vertically during reflow.
Paste data
A component also includes the paste data in addition to the footprint. Unfortunately, it happens time and time again that (e. g. in QFN housings) the exposed middle pad under the component is often forgotten. Since the paste data is used to manufacture an SMD stencil required for PCB assembly we recommend that you double-check before ordering.
QFN package with exposed pad
Reference points
Please include at least two or more preferably three reference points in your PCB layout. There is often a corresponding library within the PCB layout program with such reference marks (Eagle = marks.LBR).
Alternative for reference points
If this is not the case, simply place 2 or 3 reference marks/fiducial (Ø = 0.5 mm - 2 mm), which should not be covered with the solder mask, as far away from each other as possible. Generally, these should be placed diagonally in the corners of the PCB. The pick and place machine finds these points using a camera and all components are placed on the coordinates relative to these points.
 
If during the component placement, we notice that components do not match the designated location in the layout, we reserve the right not to place these components.

2. Component placement plan

Component identifiers
All component names should be clearly legible. With poled components, make sure that clear and unique identification is present. A simple dot (.) is often not clear enough for LEDs or electrolytic capacitors. It is much better to use the typical symbols such as “+/-” or “A / C”.

Also, connectors, terminal blocks and sockets are often drawn only as a rectangle. Please enter details for the orientation (e.g. indicate cable feed).

If any components stick out beyond the edge of the board, please indicate these accordingly. This is important for the creation of the PCB panel data.

If you order a double-sided PCB assembly, make sure that the bottom layer is mirrored when printed in, for example, a PDF. Component names and polarities must also be clearly legible here.
GERBER
For any order using the “GERBER” format, please note that we also need the X and Y coordinates of the lower left corner of the PCB as well as the marking of the at least two reference marks (fiducials), which also need be present in your Pick & Place file.

For an optimal presentation, we recommend hiding PCB tracks or copper planes and to show only the PCB outer contour, component contours and component names (make sure the printout has sufficient contrast).

Correct and incorrect creation of the component placement plan

- Clear assignment of the component name
- Legible component name
- Polarity of components is drawn
- Assignment of the component name does not exist and/or illegible
- Polarity of components is drawn

3. Pick & Place file

 
The Pick & Place file is used to generate the data for the automatic placement machine. If you order from us using the supported formats such as Altium, Eagle or Target, we will export this file for you - directly from your PCB layout file.
Pick&Place via Gerber
When ordering using the “Gerber format”, please note that we do not have the PCB layout file and we need you to provide the Pick & Place data. Please see the example on the right which details how the Pick & Place file should be supplied.
Sample file GERBER Pick&Place
Identical component values BOM
It is very important that the component values are identical to those supplied in your BOM, as otherwise incorrect placements will occur. Please use millimetres (mm) as a unit of measure.
Reference points
Also note that the reference marks (fiducials) drawn in the component placement plan are listed here with the corresponding X and Y coordinates. The bottom left corner of the PCB outline should be selected as the origin / (0,0) point.
Altium
An important note for customers who order from us using their Altium file: The component value must be entered in the “Comment” field, as this is required to generate the Pick & Place file correctly.

4. Bill of materials (BOM)

Specific BOM format
For the component placement, we can only accept the BOM in our specific format: make sure that all components are listed according to their value. Components that are not to be populated must be marked with "No" in the "Place Yes / No" column.
Spelling values
You should definitely avoid different spelling values such as: 100nF=0.1uF or 100_nF=100nF (example file BOM / row 3 + 4).
Component values should not be assigned more than once: e.g. 100n, 100nF etc. the specifications here must be absolutely identical to those used in your layout (Altium, Eagle, Target). The output of your Pick & Place data is taken from your layout file, which prepares the data for the automatic placement machine. If there are any differences, this may lead to incorrect placement or unnecessary delays because we will need to consult with you.

Also check that the order numbers of the components are correct. Specified values may be different (e.g.: BOM = 3k32 > order number = 3k3). Here we cannot determine if the value can still be placed (example file BOM / row 8).
 
Any deviations between the quantity specified in column QTY and the actual quantity specified in the column Parts can lead to delays. This may result in too few components being ordered, which only becomes noticable once the actual PCB assembly process begins.
It is crucial that the correct number of components to be ordered is listed in the column QTY (example file BOM / row 5).

If you assign components in your BOM as BETA stock components, that are NOT listed in our current stock list, we have to omit these items. Subsequent reloading or soldering is not possible. (example file BOM / line 9).

The necessary format templates can be found on our website. You can find instructions from item 14 on this page. The components that we currently have in stock can be found in the current stock list (.xlsx).

5. Stencil

Paste data
The SMD stencil used in the PCB assembly process is created on the basis of your “Paste data”. Therefore, it is very important to verify that all SMD solder pads have been taken into account. When ordering PCB assembly, please make sure that all pads created in the paste data can also be printed with solder paste and soldered. 
If THR components are also to be placed, please ensure the data for these pads are included in the solder paste data.
Please note that we will not send you the SMD stencils which we use for PCB assembly orders.

 

 

6. Components

 
You can choose whether we order the required components for you or you provide them to us. If we order the components for you, we can only accept distributors with on-line order options (shopping cart), EURO as currency and without credit card payment.
Tray



Reeled goods
The components should be delivered in a machine-compatible production packaging, such as rod, tray, roll or reel.
Reel goods feed
Please note that these should be provided as a contiguous section and that there should be no “multiple snippets”. In addition, a feed (> 24 mm) is necessary so that the straps on the machine can be setup. It is often the case that various distributors provide corresponding information on the packaging. If this is not the case you should always check with your distributor before ordering.
 
Cap as component placement aid
 
For plugs, sockets and pin connectors, a placement aid / cap is absolutely necessary, so that they can be equipped by our automatic placement machines.

Any components that are not supplied in machine-compatible production packaging cannot be assembled, in certain cases, they may have to be replaced or the component assembly can be completed manually with an additional charge (calculated on the basis of time required).

When selecting your components, check all packaging as well as the availability and lead times. We can only begin the PCB assembly process once all the required components are received.

If you provide components, ensure that they have been properly stored. For older components where this has not been the case, this can lead to problems with the soldering joints. The components you provide must be delivered in a dry condition (see IPC/JEDEC J-STD-020D; IPC/JEDEC J-STD-033B.1).
 
This works on the basis of the BOM you provided, so please label the components with the appropriate name (e.g.: R1, R2, R3,... /10k/0805).


If you send us components for different projects, make sure they are marked accordingly, for example they should also have the project name. Components that are used in different projects must not be present on a single reel section, but they have to be delivered separately with the desired excess amount because we may process different orders separately and on different machines.
Excess components
The following applies for excess amounts:
Package 0603 or larger: 20% more components (min. however 10)
Package 0402: 100% more components (min. however 20)

With high-value components, an excess amount (typically 1-2 pieces more) can be accepted if these components are supplied machine-compatible with the appropriate reel feed or in a rod or tray.

7. Soldering SMD (vapour phase)

 
Our assemblies are all soldered after the SMD component placement in our vapour phase. This soldering method has the benefit that a relatively low soldering temperature (240 ° C) is required and the assemblies can be soldered without overheating.
Suitability of the components for the soldering process
Please make sure that your components are suitable for the soldering process. This information is usually in the corresponding data sheets provided by the component manufacturer. Often, microphones or sensors are not suitable for soldering with this vapour phase method. If you have any doubts, please contact the manufacturer beforehand.

 

8. Soldering process THT (selective wave soldering)

 
THT components are usually soldered using a selective solder wave technique.
THT & SMD components
When completing the PCB layout, it is important to ensure that no SMD components are placed in the immediate vicinity of the corresponding solder joints of these THT components. Also, solder joints between high components are difficult or sometimes impossible to reach. We also perform manual soldering using a conventional soldering irons, but this method is not feasible for large quantities..
Spacer / installation aids
If components are to be mounted and soldered at a certain distance from the PCB, we require the appropriate spacers or installation aids. Otherwise, details such as “please solder on LED with 10 mm distance to the PCB” cannot be implemented. Larger quantities of wired components must be supplied as machine-compatible goods similar to SMD components. Further requests such as e.g. bending / shortening resistors and diodes are not possible.

 

9. THR (Through Hole Reflow)

THR-soldering process
THR/PIP
THR (Through-Hole-Reflow) or also PiP (Pin-In-Paste) is becoming ever more popular. This is not surprising: Two techniques can be combined resulting in a single process step.
Vias
For this purpose, solder paste is introduced into the appropriate vias of the THR components. This happens during the same work step as the paste of the SMD components using the stencil. Therefore, it is very important that you take these “vias” into consideration with your paste data, otherwise these pins will not be soldered. Subsequent soldering is not easy, since the pin of such components only protrude minimally out of the circuit board or sometimes not at all.


 

10. Component placement variants

 
If you require different assembly variants for your PCB design, we need to create separate orders for each variant. A suitable BOM and a corresponding component placement plan are required for each order.

 

11. Panel

 
Your PCB will be manufactured in a frame for assembly purposes and we will take care of these details.
PCB edge length < 20 mm
However, protruding components need to be identifiable in the PCB layout so that the lands and the frames can be created correctly. PCBs with an edge length of less than 20 mm are always supplied in panels and not as single units. This is due to quality assurance reasons.
If you order PCBs in a self-created panel format, these panels will not be separated.

 

12. Lead time

 
PCB assembly begins once we have received all the necessary components and PCBs required for your order. When selecting and ordering your components please check current availability and delivery times.
Sum of the components
Sum of the components = Sum of the SMD and THT components x number of PCBs to be placed with components.

The following options are possible when you place your order:

Order with ≤ 300 components
Please note:
With 2 WD, 10 PCBs (max qty) and
300 components (SMD and THT, max qty) at the most can be ordered. 25 THT (max per order – not per PCB) 

2 WD 
Order with ≤ 499 components 12 WD standard
8 WD 
4 WD 
Order with 500 - 999 components: 14 WD standard
10 WD 
8 WD 
Order with ≥ 1000 components: 16 WD is standard, no expedited service possible.
Status: January 2019
 
The lead-time required for PCB assembly is also added to the production time of the PCB. Therefore, please order your components that are required for the assembly in good time. Our general specifications can also be found at the following link:
https://uk.beta-layout.com/pcb/technology/specifications/


13. Terms and definitions

  • ESD - Electrostatic Discharge
  • SMD - Surface Mount Device
  • SMT - Surface Mount Technology
  • THT - Through Hole Technology
  • THR - Through Hole Reflow
  • BOM - Bill of Material
  • P&P - Pick & Place Table
  • AOI - Automatic Optical Inspection

    Comparison of the metric system and of the imperial system

    In the metric system, the basis is the meter, in the imperial system the inch. mil stands for milli-inches or 1/1000 inch; this corresponds to 0.0254 mm.

 

14. Instructions on how to create the BOM and component placement plan for EAGLE

The standard components, which we keep in stock are listed in the file “Beta_Stock_day_month_year.BOMdb”.
You can use these components on request in your EAGLE BOM file.

For this, components such as R-EU_ resistors, C-EU and CPOL-EU capacitors must come from the original EAGLE rcl.lbr library.

In EAGLE, use the function “Component Placement Variants”, we need a separate order for each variant, indicating which variant is to be filled with components.
1. Download the file “eagle_e.zip”.

Unzip the file into the directory: C:\Beta LAYOUT\PCB-POOL BOM\
2. Start EAGLE and open the file “test.sch”. The *.brd file must be located in the same folder.

Run the following ULP:
“C:Beta LAYOUTPCB-POOL BOMPCB-POOL-BOM-17.ulp”
This ULP was originally based on the BOM.ulp, which was provided with EAGLE in 2004 and improved over the years by Robert A. Rioja.
The original version can be downloaded from the CadSoft web site.
 

3. Your schematic tab should look like the picture on the right.

The setting “Grouped by” in the lower left corner must be set to “Same values”.

All parts that are in the
“Beta_Stock_day_month_year.BOMdb” file are automatically integrated into your Bill of Materials.

 
4. Verify that the Data Inventory tab contents corresponds to this Beta_Stock Data Inventory.

If not, you can open the file “Beta_Stock_month_year.BOMdb” with the button “Open Database”.


 
5. Make sure that the setup file“PCB-POOL.BOMsu” is loaded in the output tab.

If not, please download the file with the “Get setup” button in the lower-right corner.

The “PCB-POOL.BOMsu” setup file must be loaded after the “Beta_Stock_day_month_year.BOMdb” database file. (See point 4).

 
6. Save your "Bill of Materials" file with the button "Save output".

Make sure that you have selected the table format (spreadsheet).

 
7. Import your "Bill of Materials" file in Excel.
 
If you are having trouble reading a * .csv file (there is no separation of the individual field), try the following:
  • rename the extension *.csv into *.txt
  • open Excel
  • click “open file”
  • select “All files (*.*)”
  • select your *.txt file
  • select the text conversion wizard:
    • original file type: separated
    • Separator: Comma
Now please fill in the following fields:
  • Place_YES/NO - Should we place this component?
  • Provided_by_customer_YES/NO - Do you provide this component?
  • Distributor - Where can we purchase this component?
  • Order number - Under which order number does the distributor provide the component?
  • Weblink - please help us find your component, especially if it is an exotic product
  • Remarks_customer - your comment for this component
We fill all remaining fields for you.

The component placement plan for your EAGLE-File

We require the component placement plan stored as a pdf file as additional information for component placement of you PCB.

Please note that the component placement plan also serves as a template for the final visual inspection!
Therefore, the components, component names and contours of the PCB should be clearly visible in the component placement plan.
The orientation of poled components are also indicated here (e.g., diodes, electrolytic capacitors, ICs, connectors, etc.).


Which layer do I have to show in Eagle for this?

   
For the component placement plan of the TOP layer, please show the following layers:

    LY17:    Pads
    LY20:     Dimension
    LY21:    tPlace
    LY25:    tNames
    LY48:    Document
    LY51:    tDocu

For the component placement plan of the BOTTOM layer, please show the following layers:

    LY17:    Pads
    LY20:     Dimension
    LY22:    bPlace
    LY26:    bNames
    LY48:    Document
    LY52:    bDocu


How do I print the component placement plan as a PDF?

To do this, in your EAGLE layout editor select the menu item “File” > “Print”.

For printer, select a pre-installed PDF writer and adjust the scale to the format DIN A4
(make sure that the DIN A4 page is well filled).
Select the sheet limit when printing to PDF to “1”.

Make sure the bottom layer has a mirrored output so that the labels are readable.
To do this set the tick under Options “Mirrored” located on the left side.
 

15. Instructions on how to create the BOM and component placement plan for Altium

In order for Beta LAYOUT to assemble your PCBs we need a Bill of Materials (BOM) supplied according to our specifications and we also require a component placement / assembly drawing plan.

 

1. Download the file “altium_e.zip”. Find the root directory of Altium Designer on your hard drive.

There you will find the subfolder “Templates”.

 

2. Now save the previously downloaded “assembling_beta_altium.xlt” file to this folder.

Note that in this example the specified target path / memory address may differ from that on your computer!

 

3. Next, open your layout with Altium Designer and select “Bill of Materials” under "Reports" in the menu bar.

A new window opens with the required information to the components present in your project.

 

4. To export this data to the Beta BOM template, select “Grouped Columns” in the top left of the window area by ticking the terms “Comment” and “Footprint”.

In the lower section there is the “Excel Options” with the selection box "Templates". Now select the “BetaBOM-Prototype.xlt” file previously saved to the subfolder.

Then press the “Export” button and enter the destination folder for the BOM save operation.

You should find a BOM in Excel format corresponding to our specifications.

 

5. Finally, we request that you fill in the missing information (yellow highlighted cells).

If specific information about components is required, enter this in the column “Customer Remarks”.


Please fill in the following fields:

  • Place YES/NO - Should we place this component?
  • Provided by Customer YES/NO - Will you provide this component?
  • Distributor - Where can we purchase this component?
  • Order number - Under which order number does the distributor provide the component?
  • Customer Remarks - your comment for this component

 

16. Instructions on how to create the BOM and component placement plan for Target 3001!

The configuration is shown here using the example “Stepper motor” from the Target demo library making use of
Beta LAYOUT components that are available.

1. In TARGET 3001 select! Menu item -> Service -> PCB_service -> Manufacture PCB in PCB-POOL.

After you have configured your PCB according to your requirements, click on the button [Perform component placement]. Please note our instructions regarding the component placement of PCBs and the delivery of components. To do this, click on the question mark to the right of the [Component placement] button.

 

2. Double-click to open the line of a displayed component. Please enter all the required information in the appropriate fields.

 

3. Using the right mouse button you can change the placement properties of several components at the same time.

Under the listed components, you will find a box in which you can enter the desired number of PCBs on which the components are to be placed.

In the field at the bottom right, you are shown the cost of the component placement. Please note that some component costs may be missing, if they cannot be determined automatically.
With the button [Accept Component Placement], the selected placement options are taken over into the calculation of your PCB order.


The component placement plan for your TARGET-File

We require the component placement plan supplied as a pdf file as additional information for component placement of you PCB. The component placement plan is also used as a template for the final visual inspection! Therefore, the components, component names and contours of the PCB should be clearly visible in the component placement plan. The orientation of poled components are also indicated here (e.g., diodes, electrolytic capacitors, ICs, connectors, etc.).

Which layer do I have to show in TARGET for this?

For the component placement plan of the TOP layer, please show the following layers:

  • LY18: Solder mask top
  • LY21: Component placement top
  • LY23: Board outline
  • LY24: Drill holes


For the component placement plan of the BOTTOM layer, please show the following layers:

  • LY04: Solder mask bottom
  • LY07: Component placement bottom
  • LY23: Board outline
  • LY24: Drill holes


How do I print the component placement plan as a PDF?

To do this, in your TARGET layout editor select the menu item “File” > “Print”. For printer, select a pre-installed PDF writer. Tick the options “PCB outline counts” and “Centred”. Entering the scale, adjusts the presentation of your layout in the preview.
Depending on the size of the PCB, it makes sense to rotate the presentation by 90 °. To do this place a tick in “Rotate”. If you need a component placement plan for the bottom layer, then also place a tick by “Mirrored”.

17. Instructions for the component placement with Extended Gerber

In addition to the Gerber data supplied for PCB manufacture, we need extra information to complete the PCB assembly process. You can download the file “gerber_e.zip” for this purpose and review all details which are required..

1. Bill of materials (BOM)
A template showing how the desired parts list should appear can be found in German in this download (“BOM_Vorlage_2003.xls” and “BOM_Vorlage_2007.xlsx”) and in English (“BOM_Vorlage_2003_ENG.xls” and “BOM_Vorlage_2007_ENG.xlsx”).
 
The BOM must include all components, even those that are not to be placed.
Please use the column “Place Yes/No”.

If we are to order the components for you, we need more information about the distributor, as well as a corresponding order number. Please ensure that the components are available in a machine-compatible packaging.

2. Pick&Place file
Export this file from your layout file. In addition to the component names, component values and packaging, this also includes information on the mounting positions such as x-, y-coordinates, rotation angles and which side of the PCB is to be assembled. A demo file can be found in the Download as “Gerber_Pick&Place.txt”.

The individual columns in the file are separated with “TAB”. If relevant information has not been completely exported, you must add this later.

Apart from the components, at least two reference marks with corresponding x and y coordinates must also be listed.
Please note that these points are clearly marked in the component placement plan.
To obtain a reference point for the coordinates of the components, information must be given to the orientation of the PCB.

3. Component placement plan
Therefore, the components, component names and outer contours of the PCB should be clearly visible in the component placement plan. This is also needed for the final visual inspection.

Also, the orientation of poled components (such as diodes, electrolytic capacitors, ICs, connectors, etc.) must be identified here, as well as the reference marks specified in the Pick & Place file.

4. Stencil

So that we can produce an SMD stencil for applying the solder paste, we need the paste data for the PCB. Please include this information with the rest of the production data.