Board Outline and Cutouts Not Showing Up for PCB Manufacturer

Hi!

1. Open Export > Artwork.
2. In the Artwork Control Form, look at your Outline film.
3. Expand the film (click the + next to the film name) and verify that BOARD GEOMETRY / DESIGN_OUTLINE and BOARD GEOMETRY / CUTOUT are actually listed there.
4. If they are missing, right-click the film name, select Add, and pick those layers from the class/subclass list.
5. Ensure the Undefined line width in the Artwork Control Form is set to a small positive value (e.g., 0.1) to ensure zero-width lines are rendered.

Please post a screenshot of how your Export > Artwork form looks like. 

Hi!

1. Open Export > Artwork.
2. In the Artwork Control Form, look at your Outline film.
3. Expand the film (click the + next to the film name) and verify that BOARD GEOMETRY / DESIGN_OUTLINE and BOARD GEOMETRY / CUTOUT are actually listed there.
4. If they are missing, right-click the film name, select Add, and pick those layers from the class/subclass list.
5. Ensure the Undefined line width in the Artwork Control Form is set to a small positive value (e.g., 0.1) to ensure zero-width lines are rendered.

Please post a screenshot of how your Export > Artwork form looks like. 

Hi Juan,

Thanks for answering.

I've attached a screenshot of my Artwork window. For now, I decided to place BOARD GEOMETRY / DESIGN_OUTLINE and BOARD GEOMETRY / CUTOUT into separate Gerber files (BOARD.art and CUTOUT.art) to see if generating two files would solve the problem.

Previously, both layers were included in the same BOARD.art file. When they were exported together, neither the board outline nor the cutouts were recognized by the manufacturer's DFM tool. However, after separating them, at least the board outline is now recognized.

I'm also not sure if I'm creating the cutouts correctly. At the moment, I'm simply drawing a closed shape on the BOARD GEOMETRY / CUTOUT subclass.

Back when I was using Altium Designer, I would draw a line (or another closed shape) and the convert that entity into a board cutout. I'm not sure if the workflow is different in Cadence PCB Editor.

HI SB.

I had not used the JL PCB DFM tool but for gerber creation the following might be of help.

On your layer structure some board house prefer that the physical design outline exists on all layers of your design, so for example assuming the top layer that would be.

TOP
board geometry/design_outline
ETCH/TOP
PIN/TOP
VIA CLASS/TOP

This can help them when creating a panel as all layers will be aligned using the physical board outline.
"Basically your design_outline is incorporated into every gerber layer you export"

Note: typically a design will use a Board Origin, this is used as a reference point, typically bottom left of the board. So go to setup change drawing origin so as to set that on your board. More than likely you have this in place already.

In addition to the gerber export, it may be worth checking the gerber format. On the general Parameters tab check

Device Type - Gerber RS274X
Suppress - Leading Zeros "Checked", Equal Coordinates "Checked"
Format - Typically allegro sizes this but Integer places - 2, Decimal places 5 work fine
Output Units - Inches or Millimeters, Depends on design.

You mentioned a cutout, do you mean that a certain part of the board will be physically milled out or something else ?.

Best Regards.

Hello,

Yes, I needed to make a cut (slot) between some components to ensure electrical isolation between them.

I actually found the solution today. Instead of using BOARD GEOMETRY / CUTOUT, I used BOARD GEOMETRY / NCROUTE_PATH and drew the slot using thick lines. That worked perfectly.

I also had to generate the board outline in a separate Gerber file containing only the BOARD GEOMETRY / DESIGN_OUTLINE layer. Otherwise, the JLCPCB DFM tool couldn't recognize the board outline correctly.

Thanks for your help!

Excellent. glad you got it to work.

BTW NCROUTE_PATH also shows up in the 3d view of your board, so you can get a nice visual if needed. The added advantage of ncroute_path is that one can generate a route file from it, similar to how NC drill works.

All the best.