I have a design for a PCB that I have been thinking about producing. One thing that I have found is that I need is something called an assembly drawing. So far, all I have been able to come up with is that they are used to describe which components go where for PCB assembly. But I think they are also used for turnkey supplying as well.

What are the key things that fabrications houses look for in a good assembly drawing?

If I am using turnkey manufacturing, how do I describe what parts I want, and how specific do I need to be for things such as capacitors, resistors, and IC's?

What does a good assembly drawing look like? And is there an easy way to create them with Eagle?

If I order, say 500 PCB's, it is common practice for a supplier to create the first 10, ship them, make sure they work as required, and produce the rest?

  • \$\begingroup\$ Fabrication is making a bare PCB. No assembly drawing required. The bare PCB may be referred to as a "bare fab" also. After fab, the PCB's go to the assembly house where components are installed. The assembly house will want an assembly drawing. And will also need a BOM, and pick-and-place file. The assembly drawing shows where all the components go. If there are any wires or anything that have to be soldered on, those can be listed on the assembly drawing, too. \$\endgroup\$
    – user57037
    Mar 5, 2018 at 6:47
  • \$\begingroup\$ For Fab, I have never heard of splitting it that way. For assembly, if you can go to the assembly house and test the first units off of the line, they may give you an opportunity to do a go/no-go. But they don't like leaving the line set up while you do testing. I don't think they will go for it unless you can complete the testing really quickly on-site. But you can discuss it with them. \$\endgroup\$
    – user57037
    Mar 5, 2018 at 6:57
  • \$\begingroup\$ The assembly drawing is the master drawing to assemble a completed assembly. Not all the information to achieve that is necessarily in the usual fabrication and assembly outputs - bonding of components and conformal coat information come to mind. I have used such drawings for decades. \$\endgroup\$ Mar 5, 2018 at 11:12
  • 2
    \$\begingroup\$ If someone you know has a copy, IPC-D-325 is the standard. \$\endgroup\$ Mar 5, 2018 at 11:21

4 Answers 4


Assembly drawings are the master prints to completely assemble a unit.

They should contain (at a minimum):

  1. The quality standard to be used for assembly and inspection (usually IPC-A-610 class 2; class 3 is difficult to achieve unless you are willing to pay a premium).

  2. A reference to the schematic with current revision (which you should also supply).

  3. A reference to the Bill of Materials with current revision which, once more, you should supply. The Bill of Materials should specify the bare board and revision information.

  4. Any special instructions (not everything required to completely assemble the board will be in the normal tool outputs):

Bonding of components perhaps for high vibration environments where you should also specify the material type (at least the standard to which they must be made). I usually specify a particular bonding agent. You should clearly identify on this drawing which components are to have instructions applied to (using a callout)

Any modifications to be performed - we do not spin a PCB for every modification which may require a wire or two.

Any conformal coat requirements, including masking information (you can do this on a fabrication layer, but that layer information needs to be called out).

Any test requirements (you may need to provide test equipment or work with the assembler to define the tests).

Any other information: perhaps some Kapton (r) tape needs to be applied to avoid short circuits.

A view of any surface with components with reference designators clearly visible.

An isometric view is useful for some information.

The applicable standard is IPC-D-325.

I usually require a certificate of conformance to the instructions provided and that assembly has been carried out to the quality standard referenced.

Note that I also generate fabrication master prints in addition to gerbers / ODB++ and the other various outputs; that is a subject in its own right.

There are other things that may end up on the drawing, but this should get you going; I do not use Eagle, so I do not know if there is a simple way of doing this (I use Altium with the drafstman tool)

Edited for comments. Most passives are commodity parts; it is your responsibility to identify the parts that can be eaaily changed.

  • \$\begingroup\$ How specific do I have to be for things such as resistors and capacitors? Will stating their package size and resistor/capacitance be enough if I don't need any other special characteristics? Or should I describe them down to the manufacture and part number that I want? \$\endgroup\$ Mar 5, 2018 at 20:34
  • \$\begingroup\$ For things that are truly commodities, the bom can contain a note specifying "or equivalent." This will be the clue to the assembly house that they can substitute. Sometimes if you don't list the vendor and vendor part number, they will just ask you for it, which can be tedious on a long BOM. \$\endgroup\$
    – user57037
    Mar 6, 2018 at 5:47
  • \$\begingroup\$ Generic resistors may be something like this: RES 4.7K 5% 1/8W 0603 \$\endgroup\$
    – user57037
    Mar 6, 2018 at 5:50
  • \$\begingroup\$ Generic ceramic capacitors need to specify dielectric type and voltage rating. CAP 22UF 6.3V X5R 0805 \$\endgroup\$
    – user57037
    Mar 6, 2018 at 5:51

I never heard of the need for an "assembly drawing" for producing circuit boards. Assembly drawings are required when you want to produce a fully assembled device (including plastic shells, screws, spacers, brackets, free-hanging wires and connectors, whatever...). They are usually mechanical drawings.

Now, if you want to order assembled PCBs (just the circuit board with all components soldered), you simply have to provide:

  • The gerber files and drill files for producing the PCB (including the silk-screen masks where the component designators are given). These files are produced by your cad tool, using a standard format.
  • A Bill of Materials sheet, identifying each and every component with their designator, and giving their values (for resistors/capacitors), the manufacturer from which they are purchased and the manufacturer part number (especially for chips), and eventually the package (e.g. the size for passive components, standard package code for chips, ...). Basically all information that is relevant for purchasing and identifying the components. There is no standard format for this information. Usually a excel spreadsheet or a CSV file is fine. See this other question for details and an example of BoM.

Now, with just this, the fab house should be able to produce boards. The BOM allows them to source the components, and the silk screen gerber files let them know where to place them on the board (be sure to clearly indicate the component orientation: pin 1 mark for the chips, anode/cathode clearly shown for diodes, polarity for capacitors, ...). If there are some particular instructions (non-standard way of mounting a specific component, additional manual assembly steps, ...), be sure to clearly indicate this somewhere, too.

If the fab house is using automated SMT pick-and-place for assembling the board, you can also give them a pick-and-place file (generated by your CAD tool). It gives the position and orientation for each component on the board. This will ease the job at the fab house and avoid mistakes. I am not sure there is an actual standard format for these files, however. The CAD tool usually let you configure the format.


Parts: if the brand is important specify it, or specify device properties else you'll get whatever was easiest for the manufacturer.

Drawing depends on the product - it must have sufficient detail that it describes an acceptable product and does not describe an unacceptable product. all dimensions need tolerances.

500 units is a small order. If you order 500 units you will pay the cost of starting a second run if you insert a stoppage after 10 parts.


It's usual to have a couple of prototype boards made if you are contemplating a run of 500. You can then sort out any problems at relatively little cost. Board manufacturers cannot interrupt a large production run so that you can check the first few boards.


Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

Not the answer you're looking for? Browse other questions tagged or ask your own question.