| Electronics > Projects, Designs, and Technical Stuff |
| Cloning a Commodore PET-2001 |
| << < (29/33) > >> |
| BrianHG:
--- Quote from: GK on December 16, 2018, 06:40:23 am ---In each case I have the board outline defined in the mechanical layer (GM1). From here: https://support.jlcpcb.com/article/42-how-to-export-altium-pcb-to-gerber-files --- Quote ---Please make sure you have the clear outline in mechanical layer. --- End quote --- :-// In almost 20 years of Protel now an hundreds of boards manufactured, I've never had a request for anything beyond that. Can you define a board shape in 99SE like you can in AD13? I don't know because I've never had to do it before, and right now I have to go out. --- End quote --- You are correct. Yes, I've done PCBs since the early 90s. However, over the past 27 years, all my gerber files were inspected by a human operator loading the files and seeing the board outline right there on their gerber viewer. (At the time, my prototype PCBs also cost hundreds of dollars, over a thousand or two for a 4 layer, all made here in North America unlike today's highly all automated shops which would end up being under 100$.) JLCPCB has no human in the loop when you upload a .zip of gerber files on their website. Withing seconds, it just shows you a 3D quality rendering of your final PCB, that is if it can determine the PCB outline. Otherwise, a human would need to do a degree of work. I'm not sure if it's a quirk with P99se, but all I have done is tell you how I define my PCB outlines in P99se & when I send my P99se .zip gerbers to JLPCB, it instantly reports back my board dimensions and show me a preview of my PCB. Note than in P99se, it is usual practice that the board outline is defined on the 'Keep Out Layer'. Using this layer, you draw the shape you like, and you can even create multiple PCB on 1 cad document this way. I just draw a rectangular trace around the PCB. The reason I copy and paste my board outline from that layer to the mechanical layer is to have the board outline visible on every gerber file layer. This makes it obvious to the automatic detection software which JLCPCB uses to find the PCB outline. I usually send my .zip to JLCPCB as a test before I make a design public since the render they give you on the web page is instant and represent what they and others will give you if others have lazy inspection engineers and just hit the 'AUTO' button on their gerber viewers. |
| BrianHG:
Here is an example upload I've done on this site which you can play with / look at the protel PCB / send the .zip to https://jlcpcb.com/quote 's website to see what happens: Protel project file to inspect / or copy my source PCB in protel, you may play with it and inspect the board outline: https://www.eevblog.com/forum/projects/free-subwoofer-audio-processor-project-for-forum-members/?action=dlattach;attach=403539 Gerbers (upload these at https://jlcpcb.com/quote ): https://www.eevblog.com/forum/projects/free-subwoofer-audio-processor-project-for-forum-members/?action=dlattach;attach=403538 Click on 'ADD your gerber file', send the .zip, and all JLCPCB's fields should automatically be filled in. You should read: "Detected 2 layer board of 70x100mm(2.76x3.94 inches) ." and everything else on the web page should have the correct default values... You can click on 'Gerber Viewer', and, on the new page, use you mouse wheel to zoom in and out. At the top, you can select which layer of the PCB to view as well as PCB mechanical statistics. You can also turn ON/OFF each layer, IE silk, drill, outline, copper, which make the PCB. |
| GK:
--- Quote from: BrianHG on December 16, 2018, 07:19:40 am ---You are correct. Yes, I've done PCBs since the early 90s. However, over the past 27 years, all my gerber files were inspected by a human operator loading the files and seeing the board outline right there on their gerber viewer. (At the time, my prototype PCBs also cost hundreds of dollars, over a thousand or two for a 4 layer, all made here in North America unlike today's highly all automated shops which would end up being under 100$.) --- End quote --- Well, I've had these boards (the exact same Gerber files) and a ~dozen other designs made by PCB cart and Elecrow now, and this is the first time there has been an issue. I just uploaded the Gerber files for the motherboard to JLPCB's viewer. It's having a fit over the alignment/outline of the drill guide. |
| BrianHG:
Ahhh, ok, just do / try this (I've seen this before with my friend's board miller.) : Follow my settings in the attached screenshots: For the Gerbers Films, Select Imperial or Metric, with the highest resolution of 2:5. For the film coordinates, use the relative origin. (This means the coordinates used in the gerber file places 0.0 X 0.0 at the position of your set origin marker in your PCB.) I usually use the bottom left corner of the PCB. Now for the NC Drill settings. Use the same units and resolution as the Gerber File settings, and !!! Use " Reference to relative origin " just like the Gerber Films so that your drill hole has the exact same coordinates as the pads on your Gerber Film which is also now set to the same reference relative origin. This used to be aligned manually by the tech at you PCB manufacturing shop, so, the NC drill used to never have to match the coordinates of the gerber film. See my PCB screenshot for relative origin position... |
| GK:
--- Quote from: BrianHG on December 16, 2018, 10:21:48 am ---This used to be aligned manually by the tech at you PCB manufacturing shop, --- End quote --- It still is I'd guess, it's probably just that JLPCB here are trying to be too smart in their on-line automated quoting system. I made sure to follow the Elecrow guide here (as this is who made my boards): https://www.elecrow.com/wiki/index.php?title=How_to_export_gerber_files_from_Protel Note that they demand neither a keep out nor a mechanical layer and say nothing about the NC Drill file origin having to match the copper layers. Also 2:4 format is specified for the copper layers and 2:3 for the NC Drill. 2:5 is beyond the manufacturing capabilities of a lot of these cheap fabs. Do you think it is wise to default to 2.5 for both? A manufacturer might balk if the format resolution of the submitted Gerber files exceeds their manufacturing abilities. I think I'll just re-upload my Gerber *.zip folder with a .txt "readme" giving the board dimensions. That should be enough if required to get anyone out of trouble and I can't magically and simultaneously accommodate the possible quirks of every manufacturer out there. |
| Navigation |
| Message Index |
| Next page |
| Previous page |