Author Topic: How to output solder mask in gerber files?  (Read 2561 times)

0 Members and 1 Guest are viewing this topic.

Offline Lukas

  • Frequent Contributor
  • **
  • Posts: 408
  • Country: de
    • carrotIndustries.net
How to output solder mask in gerber files?
« on: June 05, 2017, 02:28:40 pm »
Hi there,

I'm in the process of re-thinking how to handle exporting solder mask layers in my EDA package horizon: https://www.eevblog.com/forum/eda/new-work-in-progress-eda-package!/msg1124424/

Two options came to my mind:
1. Export solder mask pads as regular pads (i.e. flashed aperture). May leave structures that are to small to be manufactured.
2. Export solder mask as polygons, removing sections that would cause DRC errors. see http://support.seeedstudio.com/knowledgebase/articles/447362-fusion-pcb-specification "Width of Solder Mask Dam". Kicad does it this way.

So what's the way to go? To me the second one seems to be the right one, since it more accurately represents what you'll get back from the factory. But why do the big boys (Altium, Allegro) export solder mask as pads (1st option)?

Lukas
 

Offline Mattylad

  • Regular Contributor
  • *
  • Posts: 142
  • Country: gb
Re: How to output solder mask in gerber files?
« Reply #1 on: June 05, 2017, 05:11:54 pm »
Use flashes wherever possible.
Because flashes are easier, smaller in amount of data etc. Rather than draw here, draw there, draw over there and draw back to here etc. Its just a flash this shape and size.
We stopped using draws many many years ago, it may even be better to also output ODB++ or IPC(2581 or whatever the number is).

The fab house will hate you if its all polygons, they have specific routines to convert draws to flash!
(try contacting a fab house and ask them, Steve at Eurocircuits support is very helpful)

Your solder mask pads should be 1:1, we no longer need to add 0.01" etc. and can give them as 1:1 to the manufacturer who will oversize them to suit their processes.
This way you can produce the same set of data and send it to different fabricators who may have differing requirements.

If you think flashing leaves structures too small to be manufactured then you are possibly doing it wrong, what would be too small?
Perhaps a row of QFP type pads? these will likely be gang masked if the pitch is so fine that it breaks the minimum resist rules of the fab house.
If you want specific oversize for certain pads then there is usually a way of achieving this in your PCB package so that you can still output at 1:1.

Within CADSTAR I can add an oversize to the pad code on specific layers, so if say I wanted a mounting hole to have a larger resist clearance around it then I simply oversize it on the resist layer so when I output my pads at 1:1 for the resist layer it is how I want it.

That said, I can still see some older PCB tools and designers still using really old values, probably whilst still using XP, a 17" crt monitor and having rolls of black tape in the draw.

Matt
CID+
« Last Edit: June 05, 2017, 05:15:55 pm by Mattylad »
Matty
CID+
 

Offline Lukas

  • Frequent Contributor
  • **
  • Posts: 408
  • Country: de
    • carrotIndustries.net
Re: How to output solder mask in gerber files?
« Reply #2 on: June 05, 2017, 10:33:50 pm »
Your solder mask pads should be 1:1, we no longer need to add 0.01" etc. and can give them as 1:1 to the manufacturer who will oversize them to suit their processes.
This way you can produce the same set of data and send it to different fabricators who may have differing requirements.
I guess this depends on the manufacturer: http://www.seeedstudio.com/blog/2017/05/23/solder-mask-design/ They specify that you should oversize the solder mask opening.

If you think flashing leaves structures too small to be manufactured then you are possibly doing it wrong, what would be too small?
Perhaps a row of QFP type pads? these will likely be gang masked if the pitch is so fine that it breaks the minimum resist rules of the fab house.
That's what I've been thinking of. See fig. 41 in the link above. If I understand their suggestions correctly, they want me to deliver the soldermask already preprocessed with the dams too thin removed.

Or maybe seeedstudio is an outlier in that regard...?
 

Offline Mattylad

  • Regular Contributor
  • *
  • Posts: 142
  • Country: gb
Re: How to output solder mask in gerber files?
« Reply #3 on: June 06, 2017, 04:38:15 pm »
Given that seedstudio are el cheapo and they want minimal front end work then yes, they probably want you to do the job for them.
Whatever oversize they specify, another supplier may require something different.
One may want 10th clearance while another is happy with 4th - what to do?
Either do it for each supplier or supply 1:1 and tell them to do it to suit their processes :)

Perhaps add the option for both in your program, user adjustable outputs, zero, 4, 6, 8, 10 th oversize etc. LEt the user configure it in the gui.
« Last Edit: June 06, 2017, 04:40:07 pm by Mattylad »
Matty
CID+
 

Offline Lukas

  • Frequent Contributor
  • **
  • Posts: 408
  • Country: de
    • carrotIndustries.net
Re: How to output solder mask in gerber files?
« Reply #4 on: June 09, 2017, 06:43:00 pm »
Thanks for the insight, looks like I'll implement (somewhat) parametric footprints to get the right pads (flashes) instead of going the cheap way of dumping all solder mask pads into one polygon and expanding that one.
 


Share me

Digg  Facebook  SlashDot  Delicious  Technorati  Twitter  Google  Yahoo
Smf