PCB Cost Question

[Noway2]

I am working on an SMT circuit design using a four layer PCB. I am presently debating the merits of placing components only on one side of the board versus placing passive components, such as termination resistors and bypass capacitors on the bottom side of the board. My concern in doing so is the added cost to the production manufacturing process due to the added process steps.

Does anybody have a suggestion or a "rule of thumb" regarding how much additional cost placing components on the bottom side of the board incurs?

 

[VEBill]

Automated machines such as pick and place machines and wave soldering machines typically do only one side at a time.

Probably worth keeping all the parts on one side.


Disclaimer - wait for other answers from those with more direct experience.

 

[logbook]

There is no way to put a number on it for a general unspecified job. You need to do two lots of placement and two lots of re-flow. You need two solder paste masks as well.

You could say that the cost of populating the board is doubled, but how big that cost is relative to the cost of parts and the cost of testing is impossible to state in general.

Having said that the cost of placement is doubled, you then get "two pass" boards. Suppose the placement machine has 100 head placement capability and you require 150 heads worth of parts. This means you need to run two passes through the machine anyway, in which case the cost of putting bits underneath is not as great as double.

 

[itsmoked]

logbook is right on in his assessments.

It will cost MORE for another side because the board houses can charge for an "obviously more effort". Often board stuffing is one of the most expensive aspects of the finished part. In lieu of this you would save money by using a slightly larger board to comfortably get more parts on one side even though board size/expense increases.

Remember too that you would need two stenciles ~$200/a piece. Then the digitizing set up fee (tooling). Then the two machine set up fees because they treat it as separate jobs.

I only use two sided if the product *demands* it.

 

[MacGyverS2000]

Since most of my products tend to be designed for tight size constraints, I normally place SMD on both sides. When possible, place only small/light components on one side (i.e., don't place large BGAs on both sides).

If only small components are placed on one side, this is the first side that gets populated and reflowed. Once the second side (with the large/heavy components) is populated and run through the reflow oven a second time, the small components on the bottom side from the first run will stay attached to the board by surface tension. If large components are on both sides, at least one side (the first to be populated) will need the components glued to the board before reflow to prevent them from falling off when the board is flipped.

Compared to the increase in cost for a larger 4-layer board, I'll choose the extra mask cost every time (unless we're talking prototype quantities, but at that point costs vary so much it's irrelevant).


Dan
Owner

http://www.Hi-TecDesigns.com

 

[InstruEngineer]

Hi
Whether to use single side mounting or double side mounting will depend on the following factors
1) Cost involved in designing PCB layout (it might be easier if you have a both side mounting but in case of heavily dense one side mounting it may be time consuming and hence more cost will go in designing itslef)
2) Cost involved in Soldering (Obviously both side mounting is expensive and time consuming)
3) Troubleshooting (some time its easy to trouble shoot a ckt if its one side mounted only)
4) Capabilities (capability of the manufacturing process to support both side mounting, capability of your layout design team to design a dense one side layout (if its dense) )




Instruite
--------------------------------------
Ideas that works
Concepts that sells
--------------------------------------

 

[itsmoked]

Good points Instu: I skipped that layout difficulty/cost.

I just had a very small sized 2.8" X 1.6", VERY dense four layer two sided board done. And after struggling with it for 2 weeks. I paid my expert buddy,(big price break), do it for $2,200. So the layout can definitely bite you.

 

[Noway2]

I want to thank everybody for their advice on this issue.

Based on the feedback, I have determined that I am going to proceed with a single sided layout. It looks like the two biggest determining factors for my application are the process capabilities of the manufacturer that will be used and low product volume, which would drive the per unit cost up.

I think the single sided layout will be managable, but I found I had to move some decoupling caps a little farther away from the FPGA to squeeze the traces in, which is the part that prompted my question. I am still able to keep them within 0.125" of the power pins but with a two sided layout they could be a lot closer.

From reading other thread lines, I think my desire to keep the traces at least .010" is somewhat concervative by todays standards but I am concerned about reliability if I go much smaller as I have been seeing some field returns where the cladwork was cracked by somebody flexing the board too much.

 

[itsmoked]

Noway: I have always had the same concern. Those narrow traces are reeeeeeeeealy weak looking but in recent years I have been forced slowly down to 8-8 rules and lately 6-6 rules. Vias from 20mil down to 12mil in some cases.. The expected problems have never occured. You do start raising fab cost cuz the board houses don't like using 10mil drills (for 12mil vias)but they're getting used to it.

By the way PC mother boards often have 4-4rule traces on them and a whole lot of them at that! If those huge boards can manage it, smaller boards should perform better yet.