What are common upcharges that can be avoided with simple design changes?
2 Likes
Common upcharges (in my experience include):
- Being a new designer. Not a new customer, a new designer. Sales people can spot novices from a hundred miles away (true of any profession.) You donât know how much things cost, so everything seems reasonable. Thatâs why I triple-quote all projects. Even if I do know how much things are supposed to cost, I donât get daily reports of stock shortages/tariff changes/etc. so if prices are up across the industry, theyâll be up across the quotes. If itâs one company trying to get a little extra, Iâll get that information too. Additionally, once you have the three quotes, you can start to work with the various sales people on getting the best price possible. âCompany A can do it for x dollars. Would you like the opportunity to match/beat that quote?â Sometimes the answer is yes, sometimes itâs no. On my last quote (single panel) the difference was >$350
- You pay for speed. Letâs say youâve got two projects, One on a 10-day fabrication / 10-day assembly turn time, and another on a 3-day fabrication / 3-day turn. Whatâs the difference? On the 10-day turn, they start working on your boards on day 7. How do you use this to your advantage? Well, if a company canât beat the price due to fixed costs, perhaps you can negotiate a better time-frame. Youâre not going to get a 10-day moved to a 3-day. But you might get 5 or 7.
- Donât use Via-in-Pad unless youâre willing to pay to plate it. Your fabrication partner wonât care. Not their problem. But when you go to stuff your board, the assembly partner is going to tell you that all your solder is wicking into the hole and youâve now got voids under your BGA and itâs going to cost xxxx dollars to respin the board or xxxx dollars to manually rework the components. So either a) donât put vias in your pads or b) pay to put vias in pads
- There is an upcharge to have the assembly house kit your parts. In most cases you should probably just pay it. People who save money kitting their own parts arenât properly valuing their own time. And theyâre probably not properly storing the parts in their home labs, controlling moisture, etc. That being said â the last few projects Iâve done, Iâve kitted my own parts. I shouldnât have.
- What plating do you really need? HASL / ENIG / ENIPIG? Well, the cheapest is HASL where your entire board gets covered in molten solder â unfortunately, HASL isnât very flat â so if youâre going to put a solder stencil on afterwards, itâs not going to properly gasket, and youâre going to get assembly problems. If you stencil, you should probably pay for ENIG. However, thereâs new tech out there called a Jet-Paste Printer. It puts down solder paste like an ink-jet printer puts down ink. It doesnât care how flat the board is â it shoots the solder out right on top! So ask your assembly house if they use a jet-paste printer and if HASL is okay for you.
In my opinion, smart salespeople do not âupchargeâ customers. If they do, the customer inevitably finds out, and then the customer abandons the company altogether. Iâm not saying itâs impossible for them to upcharge, just saying itâs not happening in mass.
One last thing â fabrication houses usually have a double-digit profit margin. Assembly houses tend to have single-digit profit margins. Itâs a lot easier to negotiate with fab-houses than assembly.
2 Likes
- Donât design to the process minimums. The number of boards that were passed on to the customer compared to the number of boards that were made is called the yield. And itâs rarely 100%. At some point on the yield curve, the loss is just too high, and that becomes the process minimum. Beyond that youâre throwing away more boards than you keep. So move away from that point! Increase to 5 mil / 5 mil trace space, add 2 mils to the diameter of your via pads, etc. More copper & more space = less risk = lower cost.
- Know the MOQ of your materials. In a fab-house, the materials are the copper and dielectric material. Some materials are commonly stocked, some are a one-day wait, and others are 8 months and a $150k minimum purchase. Order commonly stocked materials wherever possible, or work with your fabricator to find a reasonable substitute. Governments â you just keep doing you. Accept no substitutes.
2 Likes
You are doing great, Mark. I just recalled that incident about micro via that I shared. I would love to share my experience If I can connect my thoughts to other questions as well.
1 Like
Youâve said that once you add a single microvia, you might as well add 10,000. What is charged per usage? Are mechanical drill hits per-hole? Is plating over the hole per-via? Castellation or gold fingers? Is there much value in mostly avoiding minimums that you canât entirely avoid?
Hi JimJJewett, thanks for joining! I think when I was writing that particular comment, I had in mind that the gentlemen who needed a fine-pitch heavy copper board, and my inclination was to perhaps separate the design into a small thin HDI + a separate heavy copper board as a possible solution.
Every design you submit to a fab house needs a certain number of steps to complete, and there are some choices you make that add a lot of trouble and time, and others that donât. Once you decide to do anything other than a through-hole via, youâve significantly increased the cost of your panel (these are still mechanically drilled.) However, itâs the additional process steps that youâre paying for. Whether you then choose to drill 1 drill per sq. in. or 10, or 20, youâre probably going to see the same charge. That being said, if you start going nuts and put 50k 0.0059 mil drill hits on a panel, you can expect to pay a little more for the privilege.
âadd a single microviaâ â Microvias are made in an entirely separate process â thereâs no mechanical drill. There are lasers! And you have to do one hole at a time, one side at a time, and itâs super slow, so the cost climbs accordingly.
And to your question âplating over the hole per-viaâ the answer is no â theyâll do all the drill hits, desmear, electroless plate, etc. all at once.
âCastellation or gold fingers?â â Iâm sorry, I donât know what youâre asking here â do they make the castellated vias in a batch process? Yes.
Is there much value in mostly avoiding minimums that you canât entirely avoid? Avoid process minimums if you can, but itâs not always possible especially with todayâs component sizes, and, as I mentioned somewhere in a previous post, the published process minimums arenât the absolute process minimums, you can push it, with reduced yields. So no value, no cookies, if you have to put in a bunch of small trace & space copper there, you might as well go ahead and do it.
But there are newer, better processes. Additive, semi-additive manufacturing processes exist and are getting qualified at many fab shops in North America that over the next few years will allow them to create sub 50 micron trace and space width all day long.
1 Like
If I have a 4-layer board with a stack up as SIG-GND-GND-SIG why is it so expensive to fabricate a board like this:
Which has the GND stitching vias just going from GND on L2 to GND on L3? This would save a good amount of space on L1 and L2 making routing in the signal layers way easier and more efficient.
If the core already comes with copper on each side, wouldnât it be easy to treat this on the first stage as a 2-layer board, then laminate the prepreg and outer layers, drill again the signal vias, and finish the board?
1 Like
Hi @manuel.malagon ! Been a little while, but nice to see your name pop up again!
Itâs the buried vias. The buried vias change the way the board is made.
(@lucy.sierracircuits Is it possible to get two travelers for a 4-layer board to illustrate the additional process steps? One for a stackup w/ buried vias and one for a stackup w/ only PTH vias?)
Letâs start with that very same stackup w/ no buried vias. We start w/ the core. It comes off the shelf as copper-clad core and goes to imaging and then etching. Once complete, prepreg & copper sheets are added to the board. Then itâs drilled, imaged, plated, and etched. Finally, itâll go back to the drill/route for non-plated through-hole drilling. (Iâm intentionally leaving out several steps because itâs already plenty complicated, but each of those steps has multiple processes)
Now with buried vias. The core has to be drilled, artwork imaged onto it, electroplated, and then etched. Then prepreg and copper sheets are added, and itâs drilled imaged, plated, and etched. And finally it goes back for NPTH drilling & routing. Youâve substantially increased the number of drilling, electroplating, and etching processes. Drilling isnât such a big deal, thatâs relatively quick, but electroplating and etching canât be rushed.
Your board is going to take longer to go through the system, experiencing many, many more operations, thatâs money the fab house canât make working on another board. So youâre paying for their time.
One last thing â when you add these extra steps, you add risk to the overall process. Rick that something might fail (out-of-spec registration, for example), since no manufacturing process is 100% perfect. And the fab houses pass that risk on to the customers as increased cost â all businesses do â they have to survive.
1 Like
Iâll do my best to find these.
Oh, if you donât have them readily available, donât worry about it. Turn it into evergreen content 
Well, everyone, itâs been a blast. Hopefully, you all enjoyed reading as much as I enjoyed typing! Talk to your assembly/fabrication house and learn everything you can
1 Like
And if you have a complex project, talk to your fab house EARLY in the design. Donât wait!
A huge thank you to the awesome @mjhughes for his dedication during this AMA! 
1 Like
Thanks a lot Mark!
1 Like
Wait ⌠is the per-hole incremental cost more important with a laser drill than with a mechanical drill?
Iâm trying to figure out which â if any â steps contribute to variable cost.
Iâm coming at this as at most a hobbyist, which does affect my perspective. I wonât soon be getting tailored pricing, so I want to figure out what the cost drivers are for a generic order. I assume even skipping a step from the fabâs generic process would require enough manual intervention to be a bad idea at my size. But I donât want to make a step more complicated than it would be otherwise!
I get that a PCB is more like software than a commodity; much of the expense is fixed cost, or at least fixed per-process. But there is some variable cost. The very low volume companies do charge by square inch, maybe with a minimum or per-charge fee.
So I assume the copper-clad cores and pre-pregs are a significant cost.
Iâve read about copper balancing, and fab shops requiring it, but I havenât seen anything to suggest that the percentage of copper removed is a major cost driver.
Drill holes seem like something that has to be done sequentially, so doing twice as many should tie up the machine twice as long â unless positioning the board takes more time than the drilling. And for all I know, it might. But I canât tell from your answers.
I think @ manuel.malagon was asking about this particular stackup. It does require a second drill step (which youâve said isnât a big deal) and an extra plating step, but I think that is all. The extra drilling stage can even be mechanical, despite becoming a buried via. Maybe the vias would need to be plugged and plated over, or something, to keep too much resin from flowing in during lamination?
Misregistration is part of what makes multi-layer boards hard, but this seems like a generic 4-layer board. It seems like the top and bottom wouldnât have to be etched until after lamination, so that registration wouldnât have to be any more precise than with a regular 4-layer; maybe even less, if you use large antipads.
Is it just the tracking to say âhey, drill step before the laminationâ, or is there something I else to make it more expensive?
Hi @JimJJewett ,
Sorry I missed this comment â the AMA closed last week.
The drilling is not a big deal, they can even use x-ray location to get it in there pretty darn accurately. The processes that follow the drill are the big deal. From drill, youâve got to go to a deburr/desmear process, maybe measure internet resistance (to check for shorts/opens), go through dry-film mask, expose the artwork top and bottom, copper plate, clean the dry film, strip etch, maybe planarize, automatic optical inspection, etc. (Sorry, doing this from memory, I could be missing something). And you do all of that before you laminate on more prepreg and copper foil, then do it all again.
Drilling blind/buried vias isnât a big deal. Itâs all the additional work that goes with them that really bogs things down.
1 Like
If I can teach one lesson itâs that youâve got to check with your fabricators and ask them what their cost-drivers are. If you can, arrange a tour of the factory and ask questions.
Companies have different equipment in their shops, and that will impact quoting. What is true in one shop will not be true in the next. What is true in one shop one year might not be true the next.
For example, a fab house near me had some old-old-old-generation CO2 lasers for microvias. I think they were 5W max power output (not sure, but I remember it was a single-digit number) and an engineer had to sit on the machine monitoring every drill hit (probably 1-2 min per hole, again, been a few years, donât remember the exact number I was told.) Microvias with that company took forever, and they charged more once you placed more than xxx microvia hits per square inch (I donât recall the exact number and price). Then, they decided to upgrade to a current-gen laser-drill. Now, with what I assume is 45 W and machine-vision, they could eliminate the operator and drill the holes 10x faster. That limitation of xxx microvias per square inch went away.
Check with your fabricator, check with your fabricator, check with your fabricator.
Sorry â not the detail you were looking for, but I hope it helps.
1 Like
It does help, but now I have two sets of questions. Iâll start with the @ manuel.malagon board specifics.
I get that for vias in general, you have to deburr and desmear, and run connectivity tests. But since the buried vias are strictly between adjacent ground planes, it seems like you could skip a lot of this. Worst case is that one stitching via out of 20 is a stub, rather than a connection.
Is that unacceptable from a quality standpoint (unless customer is explicit?), or weird enough to require manual intervention even more expensive than doing all the steps, or something I havenât thought of?
And how is âdo this to the two-layer board, then later to the full 4 layersâ any worse than having both plated and non-plated through-holes?
More generally, what is the SierraCircuits equivalent of the old laser or the new machine? I would understand if you (or someone else) end up doing this as a separate blog post instead of a reply.
What is fine once per board, but a problem 20 times/board? (variable data, like date or serial number?)
What things do you handle easily, where a competitor might balk? (Controlled Depth drilling?)
What is something helpful that isnât explicit in the order forms, like Steve Carneyâs suggestion Drill holes in boards that 20mil holes are faster than smaller or larger drills?
Hi Jim, weâll get you an answer soon.