PCB Panelization

[Luka C]

I'm done with routing two PCBs which I'll be sending to fab house this weekend hopefully. While using the price calculator, I found out that if I am able to put both of them in the same order, it would turn out to be like 50% cheaper and I could use the saved money for BOM parts. Now the thing is these are two different boards, one of size 42x84mm and the second one 42x92mm (I entered the total value of 100x100mm in the calculator for price quote). They are both of rectangular shape, nothing irregular there. Since I have never made a panel before, I'd like to ask if anyone has any experience with it that he would like to share?

This is what I've found so far. There are two frequently mentioned options, V-scoring and break tabs + mouse bites. I kind off like the latter, so I browsed on how to do it properly in Eagle.

I've found this post:

"I make a slot of 50 mill wide (which is well bigger then what is allowed: 32mil (0.8mm)). To add mousebites I use the line tool with layer dimension, width 0 and draw an arc to make the end of a slot round. the width of the mouse bite I use is 75 mil. Next I place the smallest hole possible 25 mill apart on both sides."

http://dangerousprototypes.com/forum/download/file.php?id=11775&mode=view

I've also taken a look at PCB Panelizer tool:

http://blog.thisisnotrocketscience.nl/projects/pcb-panelizer/

https://hackaday.io/project/19202-small-pcbs-for-panelizing-tutorial/log/59210-panelization-using-gerberpanelizer-on-windows-linux-possible

Has anyone used this tool?
I downloaded it and tried it out, the included gerber viewer seems to display everything correctly in the final panel layout. I'm just a bit worried whether there may be any bugs that could cause displacement of inner layers (power+ground planes) in relation to the outer layers as I place components manually a lot using a very fine grid (which means X and Y positions of components typically have many decimal places), but I guess someone would have already reported such problems.

[Allen Dutra]

Hi Luka,

Allen Dutra, professional PCB designer currently working for Apple and with a lot of first hand experience with PCB panels.

In your case you want to use mouse bites to combine two different sized rectangles. V-Scores won't work here. The mouse bite instructions from dangerous prototypes will work well for standard 0.064" designs. Question, are you soldering these boards by hand or having them built on an assembly line? (I could guess your answer but no assumptions from me) Assembly lines will want tooling rails for best results but these are easily forgotten.

I haven't use the PCB Panelizer tool that you linked to. Generally I design my panel in the ECAD tool (Eagle CAD, Allegro, Altium etc.) I'm already using to ensure Gerber accuracy.
 
Let me know if you have other questions,

Allen

On Friday, December 8, 2017 at 5:07:06 PM UTC-8, Luka C wrote:

[gregebert]

Are you making a lot of boards ? If not, chuck-up a thick cutoff wheel on your Dremel, and cut slowly. And of course, respirator + eye protection.

I've had poor results with a hacksaw.

[Roddy Scott]

Slightly OT to the discussion.

I worked in the PCB industry for over 17 years in machine maintenance and process line install and found that designs for multiple board manufacture varied a lot over the years from simple two sided 'punch and crunch' with routing and perforated break lines to individual 24 layer boards with complex routing profiles.

The advent of the cellular phone industry was where V-scoring came into its own on a scale never seen before with large multi-unit main boards with routing and V scoring to divide into smaller sub-boards containing up to 8 units per section that were broken off after population.

There was a small company I used to service who, with limited financial resources, would create large boards with multiple sized rectangular circuits bound for different customers separated them by V scoring and after final test, split them into the different orders. This was a waste reduction exercise for them and proved successful in its operation.

[Luka C]

@Allen I'm planning on assembling them "by hand", manually pick and place SMD components and bake them inside a reflow oven. I guess I'll try following the Dangerous Prototyping post today.
The only thing I do not understand is the part I've marked in yellow on the picture here: https://i.imgur.com/HmpFPwv.jpg
Those break tabs contain outlines of both the first and the second board as well as the arc. I suppose the technician at the fab house then alters this in a way that the machine only cuts the arcs and not the board outline directly around it as it would cut the two boards apart?

@gregebert I'm was thinking about cutting them with something like that indeed, I'd just like to make it easier by having empty space between them and having mousebites to simplify cutting them apart.

[allen dutra]

Hi Luka,

You are correct. Everyone that I've ever talked to, looks at that mess of board outlines you've circled and says "Mouse Bite". Ultimately any board outline is provided to a CNC technician and interpreted to create tool routing. Tool routing that is offset from the board outline by the drill radius and concave acute angles rounded. Often a good PCB Fabricator (fab shop) will point out areas that can't be CNC routed and work with the customer on a solution.

Take way: board outlines and mouse bites are always interpreted by a technician to make sure the CNC routing works correctly. I've yet to see mouse bites done incorrectly though I've have seen the drill size, spacing, and count adjusted based on board thickness. If your building a thinner than standard boards a fab shop may adjust the mouse bite specification for reliability. Translation, make sure the mouse bite doesn't break in the factory but can be snapped latter by the customer.

Done correctly you shouldn't need cutting tools to snap mouse bites.

Allen

--
You received this message because you are subscribed to a topic in the Google Groups "neonixie-l" group.
To unsubscribe from this topic, visit https://groups.google.com/d/topic/neonixie-l/Y0gwQHuCzoE/unsubscribe.
To unsubscribe from this group and all its topics, send an email to neonixie-l+unsubscribe@googlegroups.com.
To post to this group, send email to neoni...@googlegroups.com.
To view this discussion on the web, visit https://groups.google.com/d/msgid/neonixie-l/67036d33-d5a0-465e-8f20-57f96a9acbe2%40googlegroups.com.

For more options, visit https://groups.google.com/d/optout.

[Luka C]

Thank you very much for your valuable feedback.
Just to make sure, this would be alright:

--------------------------------------
|       SMALLER PCB       |
--------------------------------------
   )¤¤¤(      )¤¤¤(      )¤¤¤(
----------------------------------------------
|          LARGER PCB              |
----------------------------------------------

the shorter PCB above the longer one connected by mouse bite tabs?

Oh, and since I will be ordering a stencil along with the PCBs, while googling something related to it, I found this: https://learn.adafruit.com/smt-manufacturing/laser-cut-stencils

The only thing I find interesting is where they suggest to make modifications to the gerbers in order to shrink the size of the SMD pads: "You'll now see that your pads are thinner. This prevents bridging since the laser is not perfectly precise and tends to 'go over' the boundaries by a few mils."
Is it really needed? I have some QFN components with small pitch between pads, I will be ordering the electropolished stencil for added precision.

Dana subota, 9. prosinca 2017. u 22:36:39 UTC+1, korisnik Allen Dutra napisao je:

Hi Luka,

You are correct. Everyone that I've ever talked to, looks at that mess of board outlines you've circled and says "Mouse Bite". Ultimately any board outline is provided to a CNC technician and interpreted to create tool routing. Tool routing that is offset from the board outline by the drill radius and concave acute angles rounded. Often a good PCB Fabricator (fab shop) will point out areas that can't be CNC routed and work with the customer on a solution.

Take way: board outlines and mouse bites are always interpreted by a technician to make sure the CNC routing works correctly. I've yet to see mouse bites done incorrectly though I've have seen the drill size, spacing, and count adjusted based on board thickness. If your building a thinner than standard boards a fab shop may adjust the mouse bite specification for reliability. Translation, make sure the mouse bite doesn't break in the factory but can be snapped latter by the customer.

Done correctly you shouldn't need cutting tools to snap mouse bites.

Allen

On Sat, Dec 9, 2017 at 5:26 AM, Luka C <luka.culi...@gmail.com> wrote:

@Allen I'm planning on assembling them "by hand", manually pick and place SMD components and bake them inside a reflow oven. I guess I'll try following the Dangerous Prototyping post today.
The only thing I do not understand is the part I've marked in yellow on the picture here: https://i.imgur.com/HmpFPwv.jpg
Those break tabs contain outlines of both the first and the second board as well as the arc. I suppose the technician at the fab house then alters this in a way that the machine only cuts the arcs and not the board outline directly around it as it would cut the two boards apart?

@gregebert I'm was thinking about cutting them with something like that indeed, I'd just like to make it easier by having empty space between them and having mousebites to simplify cutting them apart.

Dana subota, 9. prosinca 2017. u 04:17:25 UTC+1, korisnik Allen Dutra napisao je:

Hi Luka,

Allen Dutra, professional PCB designer currently working for Apple and with a lot of first hand experience with PCB panels.

In your case you want to use mouse bites to combine two different sized rectangles. V-Scores won't work here. The mouse bite instructions from dangerous prototypes will work well for standard 0.064" designs. Question, are you soldering these boards by hand or having them built on an assembly line? (I could guess your answer but no assumptions from me) Assembly lines will want tooling rails for best results but these are easily forgotten.

I haven't use the PCB Panelizer tool that you linked to. Generally I design my panel in the ECAD tool (Eagle CAD, Allegro, Altium etc.) I'm already using to ensure Gerber accuracy.
 
Let me know if you have other questions,

Allen

On Friday, December 8, 2017 at 5:07:06 PM UTC-8, Luka C wrote:

--
You received this message because you are subscribed to a topic in the Google Groups "neonixie-l" group.
To unsubscribe from this topic, visit https://groups.google.com/d/topic/neonixie-l/Y0gwQHuCzoE/unsubscribe.

To unsubscribe from this group and all its topics, send an email to neonixie-l+...@googlegroups.com.

To post to this group, send email to neoni...@googlegroups.com.

[Allen Dutra]

Hi Luka,

That panel configuration looks good. What is your mouse bite spacing?

I general don't use a stencil when hand soldiering a board. Don't find then useful. That said there is a fine art to design to prevent defects during mass assembly. Elongating paste shapes, changing paste shapes, getting a stencil with the correct thickness, etc.

Seeing your not making hundreds or thousands of these, this isn't a huge concern.

Allen

[Luka C]

@Allen I was thinking about 1mm spacing between the centers of mouse bite holes, each one of 0.5mm diameter? As for the distance between breakaway tabs themselves, 25mm between the breakout tabs, this gives me space for 3 tabs connecting the two PCBs

[Allen Dutra]

@Luka

That is good spacing. Some designers put in to few mouse bites but you have good spacing.

Allen

[Luka C]

@Allen Thank you for all the help you have provided. I will let everyone know how the project turns out once I'm done with acquiring the BOM parts and assembling the boards, most likely in January :)