I have designed my first PCB using Orcad for a university research project. I'm somewhat familiar with EAGLE, but definitely still a novice at PCB design compared to most everyone else. I've gained most of my orcad knowledge from watching the kirsch mackey youtube series.
It's a two layer PCB with a partial copper pour on the top for a power plane and a full copper pour on the bottom for a ground plane.
I've exported the .art gerber files for the outline, copper top, copper bottom, silkscreen, and .drl file. However, when I go to export the soldermask_top and soldermask_bottom from the board geometry section, I notice something odd. It exports nothing. Additionally, the PCB manufcaturer i submitted it to, PCBway, noted that the file type was unrecognized. It seems that all of this makes sense because there is indeed no soldermask layer on the top or on the bottom.
I tried to manually create the solder mask by drawing a static solid around the entire board using the polygon tool, as I read in another forum post. I then auto-updated the apertures and created the art files once again. However, the top solder mask layer still does not appear at all when i view it as a gerber file. The bottom solder mask layer appears as a red square the size of the board. Here is a picture of the board. Any help is greatly appreciated. Feel free to add any design critiques as well.
Soldermask details define "holes" in the Soldermask, the assumption being that if you want a Soldermask, it goes "everywhere" apart from the "holes" defined, typically for Pins and, possibly, Vias (and these get defined in the Padstacks), so Pin / Via on Soldermask Top / Bottom need to get added to the Artwork layer(s) to get the Soldermask defined in the Padstacks into the Artwork output. If you define a Shape for a Soldermask and add that to the output, Soldermask will be removed from that area when the board is manufactured.
Thank you very much! That was exactly what I was looking for. I appreciate not only your technical explanation but you're explanation of the top-down view of what a soldermask layer is.
For anyone reading this in the future: this solution worked. I simply added the soldermask_top and soldermask_bottom items from the PIN and VIA CLASS folders to their respective SOLDERMASKTOP and SOLDERMASKBOTTOM folders. I uploaded my file to an online gerber viewer to confirm. Here is what the top soldermask looked like.
Yep, that looks correct. BTW, I use PCBWAY all the time and they do excellent work. Never had an issue with the soldermask so it looks like you solved it. Congrats on getting your board built.