I plan on in the near future using Batch PCB to create 6 circuit boards for a project I am designing. The cad program I use is called DipTrace. As you can probably see in the screen shot, every layer is exportable in DipTrace as a Gerber. I need some clarification on several questions about the layers and what I need to supply. Please answer them all.
The Top Assy (assembly?) is assume means the mechanical components (like mounting screws, etc). Correct me if I am wrong. I probably do not need any Gerbers here.
The Top Silk is the silkscreen. I need to supply this Gerber.
The Top Mask is the solder mask for the top layer. This is where I am the most unclear. Do I need to supply a Gerber for this? If I do not, a solder mask will just be added i assume? If I do, what do I need to put on this layer? Do I have the option of altering the solder mask? How does this work? :?
The Top Paste is for the solder paste. Do they include this for stencil creation? I probably do not need a Gerber for this. Correct me if I am wrong.
The top is just the top copper layer. I need to supply this Gerber.
Also, in Diptrace there is a difference between mounting holes and regular through holes? How is this handled in BatchPCB? Do I just use regular through holes for mounting holes or can I use both>
All the bottom layers are the same as the top, only they are on the bottom of the board.
You’ll need to supply copper, silkscreen, and soldermask layers for both top and bottom. In the PCB editing tools I’ve used the solder mask layer is automatically generated from component libraries and such. I think it determines the solder mask by adding it always around pads and vias (the radius is the minimum annular ring as a DRC rule). You can view the output of the gerber generation by using a viewer like gerbv.
I’m guessing that mounting holes are non-plated through, which means there’s no electrical connection between the two layers. BatchPCB says that all holes will be plated through, so don’t rely on this for your board.
Put each board files into a folder not containing other things.
Save all of those files using “Export All” for simplicity, and then run a batch file to delete the ones you don’t want, and rename some of the files to save you some time:
del “Bottom Assy.gbr”
del “Bottom Paste.gbr”
del “Top Assy.gbr”
del “Top Paste.gbr”
ren “Bottom Mask.gbr” BottomMask.gbs
ren “Bottom Silk.gbr” BottomSilk.gbo
ren “Bottom.gbr” BottomCopper.gbl
ren “Top Mask.gbr” TopMask.gts
ren “Top Silk.gbr” TopSilkscreen.gto
ren “Top.gbr” TopCopper.gtl
You also need to export an N/C drill file ; name it something.drl
You will want to run gerbv after installing it. The following command may be right for you:
Zip up the above files as well as one of either “Board Outline.gbr” or Board.gbr for use as the outline, unless you have added an outline to one of your silkscreens.
I found that the bot increased my board dimensions by .010 for dimensions that were already at an even .010 number. others just got rounded up to the next .010 level. I hope they don’t actually cut my boards more than .010 big.
When you do your exports, have “Use design origin” selected. The lower left corner of my boards it at 0,0. I don’t know if that was important or not.
I created a small circuit board with a few holes and an Easy Radio RF Module. I will not be sending this out for production but am using it as example to see if Diptrace created the Gerber files correctly. Did it? Especially for the soldermask ones, should the pads and holes appear like a photographic positive?
Upload it to your BatchPCB account and see if it passes the DRC. You’ll get an email telling you what’s wrong, if anything. Then you can delete it from your account. There is no charge for uploading designs!
