Continue to Site

Welcome to our site!

Electro Tech is an online community (with over 170,000 members) who enjoy talking about and building electronic circuits, projects and gadgets. To participate you need to register. Registration is free. Click here to register now.

  • Welcome to our site! Electro Tech is an online community (with over 170,000 members) who enjoy talking about and building electronic circuits, projects and gadgets. To participate you need to register. Registration is free. Click here to register now.

Design a PCB with the manufacturing cost in mind

Status
Not open for further replies.

Davy De Waele

New Member
Hi,

We're in the process of doing a small redesign on an initial set of 5 PCB prototypes we've received. This redesign a number of "patches" we needed to do on those 5 prototypes to get them operational, and some improvements we noticed after seeing the PCBs.

The goal is now to ramp up manufacturing (20 -> 50 -> 100 -> 500).

We would also like to take this redesign as an opportunity to decrease our PCB manufacturing cost.

We started by removing all thru hole components and eliminating all components that we don't really need in a production environment (some LEDs for debugging, headers for testing, some connectors for easy external access).

This will have an impact on the board layout / size and number of components. (It's a double-sided 4 layer PCB).

In terms of the overall cost of manufacturing a PCB, what are the major cost factors that we need to take into account ?

We have a clear view on the price of the individual components and a rough idea on the price of the PCB, but what determines the price tag associated with putting the components on the PCB (pick and place / reflow / ......) ?

I can imagine that the following items an important role in the actual cost:
  • the number of components on the board
  • the different type of components
  • single / double sided board
  • all SMD components
  • size of the PCB (?)
  • the quantities (obviously).
What else can we take up in the design that would help lower our PCB manufacturing cost ?

Thanks...
 
Hi,


We started by removing all thru hole components and eliminating all components that we don't really need in a production environment (some LEDs for debugging, headers for testing, some connectors for easy external access).
This will have an impact on the board layout / size and number of components. (It's a double-sided 4 layer PCB).
In terms of the overall cost of manufacturing a PCB, what are the major cost factors that we need to take into account ?
We have a clear view on the price of the individual components and a rough idea on the price of the PCB, but what determines the price tag associated with putting the components on the PCB (pick and place / reflow / ......) ?
I can imagine that the following items an important role in the actual cost:
  • the number of components on the board
  • the different type of components
  • single / double sided board
  • all SMD components
  • size of the PCB (?)
  • the quantities (obviously).
What else can we take up in the design that would help lower our PCB manufacturing cost ?
Thanks...
The items you listed are indeed the major ones, especially board size and quantity. I hope you are asking your pcb supplier in addition to this forum.
Additional items that directly affect pcb cost and items that affect assembly cost might include:
- can you panelize your board so that you are running more than one at a time through pick&place?
- is your pcb or pcb-panel using the available area of a blank panel efficiently ( https://pcdandf.com/cms/home/246-2012-articles/9058-panelization )
- can you take advantage of low cost methods of separating your individual boards from the panel, like using v-score instead of routing
- does your board have slots in it that need to be routed. slot routing costs money.
- does your board include controlled impedance traces? Why? they cost more than not specifying them
- do you have via-in-pad? Why? These can cost more if you specify that they be filled.
- typically, costs go up as the number of holes go up, if the hole sizes include very small ones like less than .016in dia
- typically, costs are higher if you have very fine spaces between traces, or if you have very fine trace widths (for example, spaces/traces less than 0.008in start to add to cost)
- what surface finish is used. HASL is typically cheapest as opposed to ENIG for example.

items more pertinent to assembly and test costs:
- are you careful to limit yourself to easily handled smt part sizes, for example using 0603 or 0402 resistors while avoiding 0201 sizes. Or specifying TSSOP ic package rather than QFN or other leadless types?
- it might be a bit early to remove your engineering components unless you're entirely happy with functionality and performance
- what kind of electrical tester will be used for functional test? Adding probe test points may allow use of a higher speed tester or a lower cost system.
- have you scrubbed your design with an aim to reduce the number of unique resistor values, capacitor values, inductor values, ic types?
- do you have any components that are unusually shadowed, that is, a tiny part right next to a very large part. Or parts literally underneath other parts. This may require more tuning of the solder process.
- is your documentation crystal clear, accurate, and dummy-proof? Something like could cost you time and money if mistakes are made during assembly. Are you providing all the necessary assembly information that could possibly be needed including special handling notes?
- can you avoid unusual soldering requirements like high-temp? How about board cleaning, is no-clean flux ok for your parts?
- are you avoiding special handling of the board after assembly by ruggedizing it against ESD damage?
- are you using simple methods to attach your pcb to its chassis or housing? Can you use snaps rather than screws? Is your final assembly simple, for example all in one direction? Are you able to avoid multiple pc assemblies and inter-board wiring?
- are you ensuring sufficient tolerance in the location and diameter of your mounting holes?
- have you avoided having more than one electrical connector between boards so as to avoid addition of location tolerances?
- are you using the cheapest possible method of heatsinking your hot components?
- do you avoid handling costs by doing pcb assembly and final assembly in one location? Or do you ensure best quality by doing pc assembly in one location and final assembly and test in another (ie. your own shop)? The latter is preferred when doing your initial low volumes. Keep you final and especially your testing close for now.
- minimize your warranty and yield costs (and save your reputation) by meticulously policing the soldering quality of your assembly operation. Do detailed inspections (microscope examination, x-ray etc.) using IPC standards as reference and be aggressive with your assemblers if they make dumb mistakes or just do poor soldering. An assembler with a the right attitude loves negative feedback that is deserved, how else can they improve?
- don't assume anything. Assign one of your people to be responsible for assembly quality.
- on the other hand, don't get carried away with reducing your BOM and assembly costs if you are still testing the market. If you don't have a first customer you may be wasting your time. It is often the case that your first customer will want you to change the design anyways. It is often the case that your first product is not the one that goes to big volumes. Don't spend money on cost reduction if you don't have a good reason.
 
Things that dictate pcb cost are size and geometry.
PCBs are run as panels. You pay for a panel. To lower your cost, squeeze as many boards on the panel as you can. If you remove 50 mil from a board size (let's say, 2.200" vs 2.250"), can you squeeze another row on the panel. Contact your board fabricator and see what size panels they use, what's the usable area (they have rails on the outside). Is your board rectangular or irregular. Irregular boards have to be routed, so there's a .250" gap between them, eating up panel space. If your board is square or rectangular, you can score it as opposed to routing it out.
Given a standard number of layers (the more layers, the more $$$$), the next way to reduce board cost is the geometry size. 5 mil runs? Can't you do it in 8? A lot of times the geometry of a part (BGA) will determine the pitch of the runs. The larger you can accommodate, the cheaper the board. Also drill size, the larger the smallest drill, the better.

On double sided boards, you have two silkscreens which will add to the cost, so if you can keep parts on one side, this will reduce not only PCB cost, but also assembly costs.

See above (very good) post relating to assembly costs.
 
RadioRon:
"- are you using simple methods to attach your pcb to its chassis or housing? Can you use snaps rather than screws?"
Please provide an example of snaps or a supplier.
Thanks
 
Try google Images using keywords "pcb snap posts" for snap components. Snaps are, however, usually designed to be integral to the plastic enclosure rather than separate components. Or they may be used only to hold the plastic enclosure together while details inside the enclosure hold the board between housing halves.
 
Thanks.
I have a small PCB that fits on the inside of the lid of a polycarbonate box.
Two LEDs on this PCB protrude through holes in the lid.
At the moment I simply glue the PCB to the lid with a hot glue gun.
It works but I was wondering if there's more (elegant) ways to do this.
 
Status
Not open for further replies.

Latest threads

New Articles From Microcontroller Tips

Back
Top