EENG 393

In Lab 10 - Bill of Materials

Objective

Create manufacturing files for fabrication of your PCB. Have the Lab Instructor or Teaching Assistant sign-off each of the items below.

Common problems

• Included attribution on your PCB!!
  • Your name
  • Board name and revision
  • Date
  • Optional: Your company
• Name the test points with their signal names (I_out, V_out, I_set, V_set) by renaming the test point in your schematic,
• Label the VU meter switch positions settings,
• Check the inverting and non-inverting inputs on op-amp IC3A in the schematic below and make sure that your schematic is the same,
  
  
  
• The heat-sink must be adjacent to the LT30380 metal tab.

Pass Electrical Rule Check

There should be not major errors or warnings left in your schematic.

Pass Design Rule Check

Download PCBway.dru into your project directory. In layout window, make sure that you have run the Ratsnet tool to flood fill with any copper pours

• Tools → DRC …
• In DRC pop-up, in the File tab, click Load…
• In the Load pop-up, navigate to the downloaded PCBway.dru file, select it, click Open
• Back in the DRC pop-up, select Apply, then click Check
• When all the DRC errors are cleared, you will see "DRC: No errors." in the lower left corner of the layout window.

Generate Gerber Files

Gerber files are a hold-ver from the days when PCBs were made by exposing photographic file to a light move by a 2-axis machine.

Gerber file	Name	Included EAGLE layers
layout.out	Outline file	20
layout.sst	Silk Screen Top	21, 25, 27, 51
layout.smt	Solder Mask Top	29
layout.top	Top copper	1, 17, 18
layout.bot	Bottom coppper	16, 17, 18
layout.smb	Solder mask bottom	30
layout.drd	Drill file	44, 45

Before you continue, take a moment to determine the width and height of your PCB in millimeters. You can switch the units in EAGLE layout by selecting View → Grid. In the Grid pop-up select "mm" as the size. Or you can just convert mils to mm, whatever you prefer.

• Download PCBway.cam into your project directory,
• Create a folder named <your last name>
• File → CAM Processor …
• Click on the Load job file icon, select Open CAM File …
• In the Select CAM file pop-up, navigate to the downloaded PCBway.cam file, select it, click Open
• Back in the CAM Processor pop-up, click Process Job,
• In the Select output directory pop-up, click on the folder named <your last name>, click Select Folder,
• Back in the CAM Processor pop-up, you should be greeted with a CAM Exporter: process complete pop-up, click Open folder,
• Open windows File Explorer,
• Navigate to your <your last name> folder,
• Right click on the folder and select Send to → Compressed (zipped) folder …

Check Gerber Files

• Open thejlcpcb.com web page,
• Click on the blue "Add your Gerber file" button,
• In the Open pop-up, navigate to your <your last name> zipped folder,
• Double click on your <your last name> zipped file,
• The web page will show you your board,
• Click on the Gerber Viewer link at the lower right of your PCB,
• On the Gerber View page, you can
  • Move: Left mouse, drag
  • Zoom: Center mouse, scroll up (or down), center mouse, then move
  The following are things that have been sent to out for fabrication and been rejected by the manufacture. So, check your gerber view for the following:
  • Do you have drill files?
  • Do you have tiny traces connecting GND/VCC pads to your copper pour?
  
  
  
  

  Upload your files

  Please make a directory on your Google drive called "final revision" containing your zip file created in the previous step. If I have any problems uploading the designs, I'll get your design files from your Google drive folder.
  
  
  • Put your design files on a thumb drive and take them to the podium computer that the lab instructor is logged into,
  • Make sure that the browser is pointed at: https://jlcpcb.com/quote/#/
  • Process instructions:
    • Layers: 2
    • Dimension: <Auto filled by next step>
    • PCB Qty: 5
    • PCB Thickness: 1.6
    • PCB Color: <Choose your color>
    • Surface Finish: HASL (with lead)
    • Copper Weight: 1 oz
    • Gold Fingers: No
    • Material Details: FR4-Standard Tg 130-140C
    • Panel By JLCPCB: No
    • Flying Probe Test: Fully Test
    • Castellated Holes: No
    • Different Design: 1
    • Specify Order Number: No
    • SMT Assembly: No
    • Stencil: No
  • Click on the blue "Add your Gerber file" button,
  • In the Open pop-up, select your zipped file, click Open,
  • Wait for Processing Gerber files… to complete,
  • In the PCB review page, click "Gerber Viewer",
  • Verify design,
  • Back on the order page, verify board color the click "Add to Cart"
  • On the next page you should see a green check next to "Success, this file has been saved to your File Manager",
  • Click the link for File Manager,
  • Verify that your file with PCB icon is shown.