Design and Manufacture Guidelines for Surface Mount Technology

[Ralba]

Hello all,

I am working with an SMT electronics CM, and we ran into some issues with problematic designs for manufacture from customers, such as lack of rails or poor component placements. Some inside my organization mentioned their previous companies would issue a "Guidelines to Design for Manufacture" type of document to the customer detailing characteristics necessary to make a board reliably manufactureable. Many of our customers are small or are not part of a compliance system, so I cannot do something like PPAP.

Does anyone have a document they issue to customers for this kind of purpose? While obviously an electronics related document would be great, I am mostly looking for a format, so this type of document from any industry would be helpful.

 

[outdoorsNW]

The IPC 22xx series of documents cover design. There are general documents for rigid and flex PCBs and documents for more specialized design needs. I would ask customers to use these documents.

However the reality is only some customers will. Even our large customers (Forture 500 types) sometimes have poor designs when there are easy ways to improve the design that will not hurt performance or cost. And one of our engineers, a former PCB designer, complains about how often he is ignored when he makes easy to implement design recommendations to customers early in the design process.

The reality is most electrical engineers receive little to no training on how to design a good PCB for manufacturability.

Your only solution may be to charge the customers your added cost and highlight the cost saving if they improve their design.

 

[John Broomfield]

Being as better manufacturability results in lower costs (and better reliability?) how about selling your design expertise?

I’d recommended designing your design enhancement service and validating it with your favorite customers first.

This new design support service may increase the sales of your manufacturing services too.

 

[Ralba]

The IPC 22xx series of documents cover design. There are general documents for rigid and flex PCBs and documents for more specialized design needs. I would ask customers to use these documents.

However the reality is only some customers will. Even our large customers (Forture 500 types) sometimes have poor designs when there are easy ways to improve the design that will not hurt performance or cost...

Well that is disheartening, but not surprising. I doubt there is any industry that never skips over something that would make everything easier on everyone. I will try to get the IPC 22xx documents you mentioned. I was just wondering what some example "design for manufacture" documents might look like so I could communicate effectively when I craft one for things we commonly run into (e.g. 'yes, you must have a complete gerber file with the solder mask included. No, you cant put parts at the edge of the PCB with no rails.')

If anyone in this industry was willing to share, I was also wanting to see what they include on it so I do not miss something obvious.

 

[outdoorsNW]

There is a lot to consider, hence the multiple documents. You may not need all of the 22xx series documents.

Things that often cause us problems are rails-wrong size, customer wanting a non standard condition after rails removed (sometimes the customer does not understand the natural break lines of the various ways of attaching rails), the customer fails to allow for a worse case tolerance condition, or forgets that scoring is a v groove and not the centerline on the drawing. We ask to design the panelization ourselves whenever possible.

Other common problems are components too close to the edge, wrong land size or pattern, lack of soldermask between lands (some soldermasks have better resolution than others). I have seen a couple of cases of through hole parts on both sides (difficult, may mean hand rather than selective solder is used) and one case with where to board is threaded rather than using an insert (not going to hold over time). Bottom termination components are best avoided as well. Balanced stack up and design helps maintain flatness.

Large boards need to be thick to maintain coplanarity. A .062 thick 16 inch wide board can be designed, but it will move and flex from reflow heat and create problems with BGAs, especially those with non-collapsing balls. When the PCB cools, it can be flat again. The hypothetical 16 inch wide board probably needs to be at least .096 inches and possibly thicker to have enough rigidity for anything other than a small BGA. A long narrow board may have similar problems; I don't have enough experience to be sure. Even with a fixture, keeping a wide board flat can be a problem. Possibly if fixture attachment points were designed into the board middle in the correct places and a rigid enough fixture could be fit through the reflow oven, cheating the thickness might be possible. Otherwise low yields are likely and the big expensive BGAs will be the ones causing problems.

Fiducials need to be in different locations on each side and between similar parts. We had a case where a PCB was loaded upside down but because the fiducials were in the same place, the machine accepted the part. Some newer SMT equipment can switch products by reading the fiducials if the components are in the machine. If you run product families, there is potential for time savings especially if you can either rapid change your stencil or have jet print equipment for your solder paste.

Gerber is outdated as a format and should not be used for new designs. ODB++ is better than gerber, and IPC 2581 is taking over (45+% of our business, growing every year) and is the best format until someone develops something even better.

If you are purchasing IPC-2223 for flex and rigid flex PCBs, make sure you get the E version. I got an email from IPC today saying it had been released, along with 6012 E for bare PCB manufacturing and quality.

 

[Ralba]

That is one impressive post! I will be meeting with the production team and some very experienced operators to build our list, and I will keep what you said here with me to make sure we include it.

We have asked all of our customers to use ODB++. That said, some of them, especially some of the smaller companies, do not have that capability yet, so we get many gerber files.

And thank you for the heads up about the revision changes.

 

[Ralba]

OutdoorsNW , could you perhaps help me with another thing? I have made this document and I am in the process of having my co-workers review it, but there is one aspect of the design that I can't seem to locate. Is there a chart/matrix somewhere that shows the relationship between board size and board thickness? That is, what is the minimum recommended thickness for boards with X surface area?

I found a table in one of the IPC standards that says there is a risk, but it doesn't attribute any numbers to it. I am mostly looking for a general guideline on maximum panelization for small boards, as the savings in throughput of a highly panelized board eventually will be overshadowed by the sag and coplanarity risk of a very large, thin board with many V-scores/mousebites.

 

[outdoorsNW]

I am not aware of a chart. I just know about cases where my company has had problems. Factors are board size and thickness, BGA size (smaller is easier, bigger is more likely to have problems) and BGA ball type, collapsing (easier) vs non-collapsing.

You have a basically flat, rigid BGA that you are trying to solder to a potentially slightly curved PCB surface. Anything that minimizes the effect of or conforms to a slight curve is helpful. You are trying to keep everything within .006 inches of flat within the BGA area.

Bare PCB design (balanced vs unbalanced construction and amount of copper in an area) is also a factor but is hard to predict ahead of time.

 

[Ralba]

I had hoped there was a guideline resource, but after looking into it more, it appears there are just far too many variables for a usable matrix like I wanted. Thank you for all your time in your responses.

 

[msbettyhunt]

Thank you for bringing the document issue here. I too get to learn so many things.