PCB Stencils?

My new board might need to have components as small as 0402... but I'd prefer to even go to 0201 if I can. But I hear that a PCB stencil can make life very easy. The issue is, where to get one made? Are there any such services available in Pakistan?

Pick n' place isn't a viable option because we won't be getting 100 boards made at once - rather, the plan is to phase out the old machines with the new ones.

I wonder if you will work under microscope with 0201 components :)

PCB stencils are not made here locally. I always use machine assembly with stencils and I get them made from a European company.

Stencil is a costly item because transportation / courier charges are high. I can not give you exact idea about cost unless I have PCB file.

Haha, I think I will need a microscope for 0402 as well. Any suggestions for one? I'm about to order some parts anyway.

The PCB, so far, is 6 x 5" 4 layers. But I haven't completed it yet, so the final board maybe slightly bigger.

Stencil is costly, but considering once our circuit is finalized it will stay the same for a few years, I think two stencils would be invaluable. Whenever we want new machines, we get the PCB fabricated, put it under the stencil, apply paste and voila! :)

In order to use stencil, you will also need some kind of stencil printer (a fixture which holds the stencil) so that you can apply solder paste.

Personally I am against manual soldering of PCBs. Problems do pop up after some time or some years due to manual soldering.

Remember, if it can happen, it will happen no matter sooner or later...

Are you referring to hot plate + stencil as manual as well? Hmm, if you think about it, it is anyway because you are placing components by yourself.

If so, what do you say is the preferred method for soldering/assembling about 5 to 10 boards? Won't passing these through a Pick n' place be costly? The board is as I mentioned 6" x 5", has through-hole connectors. Rest of the components are smd but to reduce size, I'm placing quite a few on the bottom layer (none of the chips. Just about half of the buffer transistors I require).

No, I am just talking of Solder Paste Printer ( a small jig in which you fit your stencil and then use solder paste to apply to your PCB).

Here is one : http://www.essemtec.com/products.asp?ArtNr=SP002

Double side SMT assembly is more tricky since it has to be assembled in two passes and you also need glue dispensing under the components so that they don't fall down when you reflow the 2nd side of the board.

If you are comfortable with manual assembly, go ahead.

Alright, as I'm inexperience with this, I seek your advice:

The current boards that I'm designed are "semi-prototypes" in that I've already demonstrated the concept and this is actually a full fledged wiring harness tester with all the features we require, except it's total testing points are just 74. This too is ok - the point of this exercise is to actually use these boards on the factory floor and see how well they work.

Up until now, 0603 components were ok as this was not a dense board but now I have a lot more devices on it (SD Card, 2 CPLDs, LOTS of buffering MOSFETs and a quite a few resistor buses) - even this isn't that big of a problem. The problem is that 0603 decoupling caps are far too large for my 0.5mm pitch CPLDs. Have a look at the picture below:

Please ignore the shorted trace with ground - an error on my part. Notice how the 0603 caps are blocking so many of my pins! I'm unable to use the IO pins because I can't route them - I suppose I could use a via, but I'm saving that as a last resort. With a 0402 cap, this issue is minimized (not gone!). This is why I felt the move to 0402 would benefit the layout. Of course, the lower inductance of a smaller package would also be beneficial.

Considering this and the fact that we probably won't be making more than 10 boards at once, would you recommend pick n' place or stencil + stencil printer?

How much do those babies cost?

[quote=", post:, topic:"]

The problem is that 0603 decoupling caps are far too large for my 0.5mm pitch CPLDs.
[/quote]

Vias are there to help you, don’t be afraid of them. I would run the power traces towards the center of CPLD and use vias to take the de-coupling caps on bottom side.

[quote=", post:, topic:"]
Considering this and the fact that we probably won’t be making more than 10 boards at once, would you recommend pick n’ place or stencil + stencil printer?
[/quote]

Generally the cost is setup charges (around 10-15K one time) + Rs. 1/component. Now you can calculate how much it would cost you.

[quote=", post:, topic:"]
How much do those babies cost?
[/quote]

LOL - these babies are more expensive than babes, a normal SMT pick and place setup costs around 60,000-150,000 USD.

[quote=", post:, topic:"]

Vias are there to help you, don’t be afraid of them. I would run the power traces towards the center of CPLD and use vias to take the de-coupling caps on bottom side.

[/quote]

Do you mean to place the caps on the bottom layer and use vias to connect to power/gnd pins? If so, wouldn’t that increase the loop between the power/gnd pins a lot which is generally a no-no, isn’t it?

*

[quote=", post:, topic:"]
Generally the cost is setup charges (around 10-15K one time) + Rs. 1/component. Now you can calculate how much it would cost you
[/quote]

That’s not so bad, certainly doable for 10 boards. Probably not that feasible for 4. Can you please describe what files I need to generate for Pick N Place? And what companies here offer the service? I assume I get the PCB fabricated from elsewhere and then hand them the components and the PCB?

Do the components need to be in complete reels or are strips ok? What about TQFP chips?

[quote=", post:, topic:"]
LOL - these babies are more expensive than babes, a normal SMT pick and place setup costs around 60,000-150,000 USD.
[/quote]

Haha, I meant about stencil printer not a SMT pick and place :P. And, finally, what about BGA packages? If that is possible here, then I’d sure go for pick n place simply because it would vastly help me.

[quote=“PsychedelicBreakfast, post:9, topic:15989”]

Do you mean to place the caps on the bottom layer and use vias to connect to power/gnd pins? If so, wouldn’t that increase the loop between the power/gnd pins a lot which is generally a no-no, isn’t it?

[/quote]

Yes, place the caps on bottom side under the chip using vias. The purpose of de-coupling caps is not to stabilize the VCC but to eliminate the ground bounce. ICs can tolerate certain variation in VCC but ground bounce is a killer. Generally the de-coupling capacitor should be as close to GND pin as possible but as you said your board is a 4-layer (I assume you have at least one GND plane) so a cap placed near to chip is ok.

[quote=", post:, topic:"]
Can you please describe what files I need to generate for Pick N Place? And what companies here offer the service? I assume I get the PCB fabricated from elsewhere and then hand them the components and the PCB?

Do the components need to be in complete reels or are strips ok? What about TQFP chips?

[/quote]

Which PCB design software you are using ? Usually in post processing, you have the option to generate the Pick & Place file along with your Gerber files. Normally components are required in Reels but cut-tape can also do if it is longer than 1 foot. TQFP chips are usually shipped in trays and are fed onto different feeders on machine. If you don’t have the tray, it can be arranged.

[quote=", post:, topic:"]
And, finally, what about BGA packages? If that is possible here, then I’d sure go for pick n place simply because it would vastly help me.
[/quote]

BGAs are possible without any problem. How many pins and how dense ?

Finally as I told you earlier, machine assembly of SMT on both sides of board requires glue dispensing under the components on the side which is assembled first. The reason is that when you assemble the second side, and put the board into reflow oven again then the bottom side components (on the side which was assembled and soldered first) would fall down.

Unfortunately I know of no source in Pakistan who is doing SMT assembly on both sides of the board. However I will check again.

PS: Instead of discrete FETs, didn’t you find the FETs in array package ?

Is this how you meant it?

Maybe I placed it wrong, but the loop area seems bigger now. :(

Yes, it's a four layer PCB, arranged like this:

Signal layer

Ground

Power (3.3V)

Signals

I am using Altium Designer. In the past I have tried Eagle, OrCAD and I didn't really like their approach. OrCAD was the better of the two but Eagle's interface is appalling. I have most of the components in strips but I haven't really bought anything in mass, which will ofcourse be later. My TQFP didn't come in trays though!

I'm looking at BGAs like 324-Pin FineLine Ball-Grid Array. Two of these, plus a smaller 100 pin TQFP, on a board would be able to check our largest wiring harness without any issue. My initial approach was cascading three 144-pin TQFPs, for output and input - so in total of 6. Goal is to have 320 IO pins. The 324-pin FBGA will obviously not have 320 IO pins so the additional 100 pin TQFP would still be needed.

Here's information on the package: http://www.altera.com/devicepackaging/04R00232-01.pdf

I'm using a logic-level MOSFET in a tiny package. They have two inside so it's really quite compact. Here's a 3D view of the board as its layed out so far:

Only started work on this last night so still have the majority of routing left. I don't have the third chip on it and the input side hasn't been placed on the board yet either. Was looking for a suitable resistor-bus for that end.

[quote=“PsychedelicBreakfast, post:11, topic:15989”]

Is this how you meant it?

[/quote]

I would have placed the capacitor where you placed the vias. This would also reduce the trace length. Now you will wonder where to place the vias? Well you can use Via-in-Pad.

I wasn't aware what a via-in-pad was so I googled it. Personally, I'd really rather just route the other signals using vias instead of putting the cap on the bottom layer. It's not that I doubt your approach, I doubt my ability to pull this off. From what I've read, a via-in-pad can open another can of worms that's something I'm desperately trying to avoid, if you know what i mean!

This is one of the reasons I'm still reluctant regarding BGAs. They can be very difficult to get right and if something goes wrong, I'm not sure how I'll inspect the ball-grid. TQFPs are at least accessible. I'm thinking of adopting a extensible approach i.e. have a master PCB and daughter boards can attach to this and expand the test-points. Not sure how to implement this though!

[quote=", post:, topic:"]

From what I’ve read, a via-in-pad can open another can of worms that’s something I’m desperately trying to avoid, if you know what i mean!
[/quote]

Everything has it’s pros and cons. Via in pad has one obvious disadvantage that solder paste flows into it. But on the same hand, this is one of the standard techniques used for routing of BGAs.

[quote=", post:, topic:"]
This is one of the reasons I’m still reluctant regarding BGAs. They can be very difficult to get right and if something goes wrong, I’m not sure how I’ll inspect the ball-grid.
[/quote]

BGAs are difficult to handle especially high density. The only way to route BGA is to either use Via-in-Pad or Dog-Bones. Inspection of BGA soldering is done by X-Rays which itself cost around 100,000 $ to buy such an inspection system.

Yes, that is precisely why I'm reluctant to use BGAs here. I'm thinking we should have a master board which by itself has 114 test points, so basically should have 144-pin TQFP. However, it should have "expansion slots" which would connect more boards to this master board and expand the 114 test-points to how many we need. Each daughter board could have another 144-TQFP. Because the very basis for the testing is a shift register and not a multiplexer, it should be, in principle, easy to extend this to however many test points we require.

Think of it this way, the master board is essentially a 114-bit shift register. The serial out of this shift register needs to be fed to the daughter card which in turn would feed it's serial out to the next card in line. I will need to buffer the serial out, but that shouldn't be too hard. The question becomes difficult when we ask ourselves - how to distribute power to the board? The current plan is to include the switching regulators on the board and if that is the case, I'll need a power connector for each board. But this may stress the regulators as the current requirements increase. Perhaps a better option would be if each board has it's separate regulator and it gets its power from a central power supply PCB which has the transformer + rectification + smoothing caps.

The other approach is not have an extendable system but have three models, one which has 100 test points, another which has 200 and the third which has 300 or so. This will easily serve our current needs but is not extendable.

However, it's almost plug and play. You just program the CPLDs and the uC and you're done. With an extendable board it may not be so easy as it may need some configuration. That will be easy for me to do as Im the designer but for others, maybe not so. Decisions decisions!

PS: BGAs are evil. So are QFN. Is there package you really don't like? When I studied in Karachi, I once went to a teacher with a TO-3 transistor. He claimed that this was not intact a transistor but a diode because it only has pins! I never asked him a question again lol - TO-3 is a pain to work with as well.

Sometime back, I got the opportunity to manually solder an AD LFCSP 4x4mm 20 lead IC (with pad underneath) to a prototype breakout board. It was slightly challenging but fun. Had to do it thrice till I could verify the solder between all leads and their pads with a microscope.

The smaller ICs, while they have their benefits, are not suited to manual soldering for production run nor are they easy to use during development since access to individual leads is very difficult.

Any recommend Pick N Place services in Pakistan? Would prefer their phone or email.

Undersigned :)

Ijaz

Dear All some one please tell me who is providing SMD PICK & PLACE service in Pakistan.

Iftikhar Ahmad