Assembly services with very small boards

[MarkR42]

Hi all,

I'm making a PCB which is a very small speed controller with radio receiver, for small robots. The final PCB that I want to make is about 19x24mm,

My current plan is to get it assembled (one side) by JLCPCB assembly, who are very good value and have all the parts that I want to use in their catalogue. I have ordered a few boards from jlc before but not assembly!

I've built a few prototypes by hand (it is very tricky because I don't have a good SMD setup at home, and I cannot go to the hackspace now), and one even works, so the design seems fundamentally ok.

My board is too small for JLCPCBA's assembly service and in any case, it doesn't have any space for the tooling holes that they need to add.

So I decided to panelise two boards and add some tooling strips so jlc can put their tool holes there. I put the "stamp holes" to snap-off the unneeded parts of pcb.

I contacted jlcpcb support and they seem to think it's ok.

Before I commit $100 to order this thing, can anyone tell me:

* Have you done something similar before (with a smt assembly place) and did it work?
* Does it look like it will work?
* Is 6mm wide of stamp holes enough to hold this board together during assembly?

Here is a picture, attached, and the Gerbers are here: http://vectrex.org.uk/mark/nanox-panel5.zip

Thanks, Mark

PS: I have also updated forum member essele's kicad plugin to work with panelised boards.

[Mangozac]

What you're planning here is very commonplace. You might want to panelise into a grid of 2x2 to provide a little more "heft" and ensure there's definitely no issues with being too small in one dimension.

The "mousebites" (as the break off tabs are called) look fine. There are guides for the optimum hole to space ratio but I don't remember off the top of my head.

Is 6mm wide of stamp holes enough to hold this board together during assembly?

Can you please rephrase that question?

[MarkR42]

It is good to know. Actually since I posted this, I realised that Julian Ilett had already done almost the same, ordering a panel of 2x boards because they are too small individually,

The mouse bites width is about 10mm, which is slightly less than half the height, 24mm, I think it should be robust enough, I'm not sure if I should get 1.6mm or 1.0mm boards, I might try the thicker ones for more strength during construction (even though I'd prefer less board in the application)

[SMTech]

What you can see on Julian's boards is that there is absolutely nowhere for a conveyor system to hold the board in place while it is being assembled, this means they have almost certainly built it as part of a larger panel and then cut it out, either the handling or the cutting machine makes anything smaller than 20x20 impractical so that where they put their limit. However JLC can do that because they are JLC, seeing a lots of what they are treating as one-off designs concurrently that they can juggle around to build this way.

Anywhere more conventional and the minimum panel size is going to be bigger typically 50x50 is where conveyor systems stop, your example with tooling strip on the edges is better but I would agree 2x2 would be even better. Where possible I would always try to put Fiducials on the individual PCB too, having those and including them in your XY data means the data you supply has easily relatable data linking the fiducials and the components, on our Essemtec system that makes setting up a new design much easier even if during production I switch to using fiducial marks in the tooling strip.

[ANTALIFE]

What you have is a good starting point, here is what I would change:

• Change your panel from a 2x1 to 2x3. You want your panel to be at least 50x70mm otherwise the assembly house will have trouble feeding it through their line
• Your mouse-bites are a bit long (13mm), I would reduce to 5-7mm to make de-panelling easier. Also make sure that mouse-bites have at least 15-20mm between them
• Gotta add fiducials man, an assembly house can try and use holes/vias but you have to be aware that holes are less accurate than etched copper. So for components smaller than 0603 you might run into placement issues if you use drilled holes
• Finally your mouse-bite holes are too close to SMD pads, so you will have to be extremely careful when de-paneling the boards, otherwise you will pop some pads/components. My recommendation is that you grow your board size so that SMD pads are 1-2mm away from mouse-bite holes

[Gribo]

Why aren't you using V-cut?

[ANTALIFE]

Why aren't you using V-cut?

Looks like they are placing some sort of SMD wireless module which is super close to PCB edges, so that's probably why no v-cut/groove

[dietert1]

The modules shown may be good for hobby, yet no good engineering. For something reliable you need at least two or three times the size of the part as distance from the edge. Those multilayer caps break easily when separating the modules.

Regards, Dieter

[GerardG]

Hello MarkR42,

Make a panel like suggested 2x3. Tooling holes on the break edge.
Minimum distance of fiducial to the edge of the panel to be 4mm.

I use 5 holes of 0.6mm with center to center spacing 1mm.
The attached picture uses 0.8mm. But this is way too big for most designs.

At some designs I have used breaking tabs at the corners of the PCB as there are mostly no components close to the corner.

[MarkR42]

Why aren't you using V-cut?

JLC does not give the option of using v-cut for smd assembly. They have their own rules, honestly, I think they've got their own way of doing things, possibly they panelise several customers boards together during assembly then snap them out (so they already use v-groove for their own stuff?)

I did not really want to panelise myself but there is no choice as the boards are too small for them to be made individually and there's no room for tool holes.

Anyway, thanks everyone for the many helpful comments, I cannot really do all of these things due to the small desired size.

It seems it is not feasible to move the smd parts further from the mousebites or use v-groove. I will remember about the mlcc breaking when the boards are snapped, and try to be very careful. If I have to rework a few boards it's ok. There is a LED and resistor quite close to the mouse bite, and a mlcc a bit further away.

Looks like they are placing some sort of SMD wireless module which is super close to PCB edges, so that's probably why no v-cut/groove

I am placing a wireless module, but I will hand-assemble that on the other side of the board after all the smaller smt stuff is done by the assembler. Soldering those is super-easy anyway. I will probably snap the boards before I solder that on.

It is a short production run of boards for hobbyists with a fairly limited market, it's really the first test production run so I don't want to do too many boards at once (especially if they are badly broken and need to be reworked or thrown away)

[JLCPCB Official]

Yes, we penalise several customers boards together during assembly then snap them out. You get me, friend. 

[NivagSwerdna]

"penalise"

You mean panel-ise.  Different meaning! 

PS
My boards are currently going through production... the ability to watch progress in realtime and see small videos of the stage is so cool.