Before asking you guys for help I want to say thank you to the people behind dirtypcbs! I have used their service a couple of times and each time I was amazed by the quality of the boards! And the price.... a-ma-zing! Two thumbs up for our buddies in China!
After ordering singular boards, I am now trying to panalize my designs. However, the Mayhew Labs online gerber viewer as wel as ZofzPCB aren't showing what I was hoping concerning the board outline. Below an example of some hammond 1551G pcb's. I'm using the latest version of Cadsoft Eagle. All lines are layer 20 Dimension. The gaps are 2.0mm wide and the mouse bite drills are 0.5mm spaced 0.65mm apart from eachother.
Can anyone confirm the board house will accept this? ZofzPCB did show the correct outline, however it did not process the internal gaps.
haven't seen a gerber viewer that does display the internal slots correctly. THey all had some errors in the renedering
take a look at other topics about this:
viewtopic.php?f=70&t=7777 (http://dangerousprototypes.com/forum/viewtopic.php?f=70&t=7777)
viewtopic.php?f=70&t=7758 (http://dangerousprototypes.com/forum/viewtopic.php?f=70&t=7758)
At first glance your boards look ok and think you get the slots smaller (see my post in the second topic)
hi t3dd,
Would you care to send the outline file, or better something more - like add one of the layers, to bug (at) zofzpcb (dot) com ?
Hi Sjaak!
I already had a look at those links. They were helpful. The boards are now in production, when they have arrived ill post the result.
@zofz
I have send you an email earlier today.
Thanks!
t3dd,
Thanks for the files. I see problem in places marked by circles.
[attachment=1]
The problem is a lack of imagination in the outline-drawing processing algorithm. When talking to machine, please mark only the board outline and remove the help lines.
[attachment=0]
I do not know, what criterion to use, to be able to process legitimate human 2 human technical drawing, in such case. The CAM operator for sure know what you mean.
ZofzPCB was trying to find all combinations (2^n) it took about 30 min on my PC, and it was targeting to extract the biggest field.
Actually I am very happy that it is not a 3D drawing, I have to analyze :)
[attachment=2]
Your board design looks fine, that is how I did my latest order too. Just a 0mil outline on the 20-dimension layer, leaving a bit of room and rounding the corners. I left at least 3mm of clearance, but I don't think it matters too much. No gerber viewer had a clue what to do with it, so I sent it off and crossed my fingers that it'd work!
Got the board back today, worked perfectly! (I was worried I'd get a bag full of holes... but seems there is a dirty human somewhere in the mix who knows what to keep and what to cut).
[attachment=1]
So for anyone wondering, here the steps for Eagle:
- Design your PCBS one by one, making a new .pcb file for each one
- Create a new blank PCB, not attached to any schematic
- Place each PCB into your panelized PCB by choosing File, Import, Eagle Drawing and selecting the .pcb file
- Turn on all layers, then use the group select tool to move them around and position them
- Delete all your board outlines
- Use the line and curve tool to draw new board outlines
- Use the hole tool to make your mouse bites
- Export gerbers (check that the routing lines don't go through your mouse bites)
- Double check and triple check gerbers
- Place order
[attachment=0]