Author Topic: Checklist for MCPCB design  (Read 4742 times)

0 Members and 1 Guest are viewing this topic.

Offline HackedFridgeMagnetTopic starter

  • Super Contributor
  • ***
  • Posts: 2029
  • Country: au
Checklist for MCPCB design
« on: March 20, 2012, 11:55:10 am »
Just designing my second board (which is strange for an otherwise quite experienced engineer).
It will be an single layer MCPCB for mounting Cree leds.

I have never panelised a board before. So I would like to do it right, and I would like to avoid as many pitfalls as possible.
I have watched Dave's videos on preparing boards for manufacture.

Here is my panelising checklist.
  • put a 10mm border around my boards
  • provide tooling holes (3mm? whatever the manufacturer wants)
  • add fiducials
  • add a separate layer for Vgroove cuts.
  • use standard drill sizes
  • impedance tracks (I am only considering these so that I know the copper thickness)
  • I don't want any testing done.

Anybody got any further comments. Especially in regards to MCPCBs.

Offline miranday

  • Newbie
  • Posts: 3
Re: Checklist for MCPCB design
« Reply #1 on: May 09, 2012, 06:47:58 pm »

There is a tool that will help you with the Panelization feature called FAB 3000 Professional. A free trial is available to use at

Hope that is helpful.

Offline free_electron

  • Super Contributor
  • ***
  • Posts: 8518
  • Country: us
    • SiliconValleyGarage
Re: Checklist for MCPCB design
« Reply #2 on: May 09, 2012, 07:49:56 pm »
Don't bother. leave that to the PCB fab guys. they will panelize according to their rules .
Unless you need matrixes for automated assembly.. and then it's your rules that apply.

Borders are only required of you are going to run matrixes through automated assembly.

Some 'pcb jargon' :

Panelization : this is the preparation of artwork to be placed on a PCB panel.  Panel in this temrinology means : the panel used by the PCB manufacturer. this is NOT your panel size !!
PCB manufacturers use 18x24 inch panel ( typically ). Thi spanelisation you cannot do as you do not know what the clearances are , end keepouts , where the registration and lamination holes sit and lots of other process related stuff. this shifts from pcb manufacturer to manufacturer...

Matrix : this is the end users 'panel' . this s your mini 'panel' that can be used for automated assembly.
If your board is large enough , and parts are kept more than 3 mm away from the edge of the board then there is no need to create a matrix. Dave's microcurrent is too small se he needs matrixes.

Fiducials are only for pick and place. 3 are needed. typically 1 square , 2 round ones in an L-shap pattern. Square fiducal is board coordinate 0:0. i did a post on the forum already about the how and why. if you got fine pitch parts qou can add 2 fiducial markers per part there. For those fiducials special rules apply : they need to be at the intersection of the pin centerlines ...

Impedance coupons are again done by the board fab house. in order for this to work YOU need to specify the stackup ... so you need to know the dielectric, and prepreg thickness post fusing. They place these internally on their 'panel' , not on your 'matrix'.

if you want one you can put one on your board or you can put one on the matrix frame ( what you call the 'border' ). but it is a waste of space. if you need the info , the pcb house will happily supply you with the coupons from the panels they ran. Thickness of the copper has little or no impact on the impedance ( there are some stray effects , but minimal ) it is purely layer to layer and dielectric.

'standard drill sizes' . there are no 'standard' drill sizes. they have any drill from 6 mil up to 80 mils or so in steps of 1 mil , after that it becomes routing.

If you need v-grooves : check the minimum clearance they need. also keep in mind that you cannot place any fragile parts close to the groove. breaking the board may break the part ! Especially ceramic caps and resistors. if you need grooves then you need to mill slots where the parts are... Same goes for mousebites.
V grooves are going to cost you extra as this is an extra separate step in the process. Mousebites don't cost extra. its just drilling and milling and those steps are there by default ...

Now , you talk about metalcore pcb's ... that is whole different animal.... you may want to tal woth your pcb maker bfore you embark on this ... there are special rules for those things..
milling and v-scoring is expensive... depending on volume they may want to make a punch and die approach ...

Professional Electron Wrangler.
Any comments, or points of view expressed, are my own and not endorsed , induced or compensated by my employer(s).

Offline HackedFridgeMagnetTopic starter

  • Super Contributor
  • ***
  • Posts: 2029
  • Country: au
Re: Checklist for MCPCB design
« Reply #3 on: May 09, 2012, 11:13:58 pm »
I actually sent the board off a few weeks ago, to some dirt cheap company that I can't remember the name.
It should return soon.
All it is supposed to be is a good way to get a lot of aluminium mounts for cree leds.
I just hope their dielectric is good for 40 volts.
If they can manage that I should be ok.

Your are right they panelised it and did they VScore to their standard cuts.
I am just going to hand mount the leds.

I will post back the results of this experiment.
Ideally it should be 550 good led bases for $220 dollars, including all costs. And in shapes to make it easier for me to make light fittings.

ps. thanks for the input.


Share me

Digg  Facebook  SlashDot  Delicious  Technorati  Twitter  Google  Yahoo