Aalto Fablab
Child pages
  • PCB Milling with Roland SRM-20
Skip to end of metadata
Go to start of metadata

Here you can find information about Roland monoFab SRM-20 and how to start using it at the Aalto Fablab.



1. Introduction

This is a 3-axis milling machine, we usually use it to make PCB (Printed circuit board) in FabLab. You can install the bit on the machine, set the .gerber file to the tool path file, then the machine can remove the material on the board based on the tool path file.

The basic process for one-side PCB milling is:

  1. Set the file as a tool path file by CopperCAM
  2. Set up the material
  3. Install the milling bit
  4. Clean up


2. Set the file as a tool path file by CopperCAM

We use CopperCAM to create milling files. Every .gerber file can be used in this software.

2.1. Import file

  1. Open CopperCAM
  2. File → Open → New circuit. Select your front-side file. If your files don't show up, try to change the file type to "All files (*.*)"
  3. There's a message asking you to confirm the highlighted track net is card contour path, which is the cutting edge of your board. Select "Yes". If this message doesn't appear, right click on your board's outline → Define as card contour → Set card contour: outside contour → OK
  4. File → Dimensions → margin: 1mm, Z thickness: 2mm (a little thicker than your material)→ OK
  5. File → Origin → X:0, Y:0 mm → OK

2.1.1.  Multi-layer and Drilling holes

  1. If you have more layers: File → Open → Additional layer
  2. If you have drilling holes on your PCB design: Open → Drills → Select the drilling file. If your files don't show up, try to change the file type to "All files (*.*)" or "Gerber X2".
  3. Repeat Import file step 4 & 5 for all the layers. If all your layers have a cutting outline, remember to remove them so only the first layer has a cutting line.
  4. If the additional layer doesn't line up with your first layer: 
    1. Select a pad that appears on all the layers → right click → Set as referenced pad
    2. Select another layer → Select the pad that should be at the same place as the referenced pad → right click → Adjust to referenced pad #1
    3. Now all layers should be aligned
  5. Regarding double-side PCB milling, please ask the FabLab master for more information.


2.2. Tool Setting

Assign specific milling tools to different jobs.

  1. Parameters → Selected tools 
  2. Select tools for different jobs, you can find the information about Tool.1~3 on the sheet next to the machine.
    1. ENGRAVING TOOL: Tool.1 or Tool.3. Depth: 0.1mm/ Margin: 0mm/ Engraving speed: For Tool.1, the speed can be 5~10 mm/s, and for Tool.3 is recommended to use 5mm/s.
    2. HATCHING TOOL (If you want to remove the remaining material of your board): the same setting as the engraving tool.
    3. CUTTING TOOL: Tool.2. Depth: a little thicker than your material/ Cutting speed: 5~10 mm/s are recommended
    4. DRILLING TOOLS: Use one single tool for all drills → Tool.2 (you can only drill a hole that is bigger than 0.8mm in diameter)/ Drilling depth: a little thicker than your material/ Speed: 5mm/s
  3. OK


2.3. Contours Setting

  1. Select "Calculate contours" icon on the toolbar
  2. Set how many paths you want to engrave:
    1. Number of successive contours: How many times the bit will engrave outside the tracks and pads. Usually, 3~4 is good.
    2. Extra contours around pads: How many times the bit will engrave around the pads after successive contours
  3. OK

💡Tip: If you want to engrave some texts on your board, do this before calculating contours: right click on the text → Engrave tacks as centerlines.


2.4. Export the file

Now we can export files as the tool path file for the machine.

  1. Select "Mill" icon on the toolbar
  2. Select Section # 1: Engraving layer#1
  3. Select Section # 2: Drilling (single tool)
  4. Select Section # 3: Cutting out
  5. XY-zero point: South-West corner
  6. Z-zero point: Circuit surface
  7. OK. And save the files. You will get multiple files depending on how many milling tools you will use. In this example, we'll use Too.1 & Tool.2 so there're 2 files exported.


3. Set up the material

You can find most of the tools you need in the drawer which is under the table.

  1. We have both one-side and double-side copper boards in Fablab. You can find them in the leftover box (REUSABLE PCB STOCK), which is put on top of the drawer. If there's no board suitable for you, you can find more in the bottom layer of the drawer.
  2. Use the double-sided tape to fix your board on the machine's working platform. You can find the tape in the first layer of the drawer

        


4. Install the milling bit

  1. open VPenel for SRM-20 on the desktop. We use this software to control the machine.
  2. Make sure that both sides are set to User Coordinate System.
  3. Setup →Command Set :RML-1, Unit: Millimeters, Y axis using keypad: Move cutting tool to desired location → OK
  4. Make sure the value of Spindle Speed is in the middle.
  5. Use the arrow bottom to move the tool holder in the middle so it's easier to install the bit.
  6. Choose the bit you need from "IN-USE PCB MILLING BITS" box. Usually, the order of the jobs is engraving → drilling → cutting. So in this example, we use Tool.1 fist to engrave the circuit.
  7. Use the hex key, which is attached to the machine by a magnet, to install the bit on the tool holder. Don't tighten too much, just make sure the bit is fixed.
  8. Be careful to take and install the bit, the point of the bit is very fragile.

       

4.1.  Set the Z-origin

  1. Use the arrow button to move the bit close to the material's surface, but remember to leave some space for moving down later during the job.
  2. Use the hex key to release the bit, moving the bit down till it slightly touches the material's surface, and tightening it again. 
  3. Press "Z" button under Set Origin Point to set Z-origin. Select "Yes" to the pop-up message, then you will see the value of Z is "0.00mm"
  4. Use the arrow button to move up the bit.


4.2. Set the XY-origin

  1. Make sure the bit doesn't touch the material.
  2. Use arrow buttons to move the bit to the starting point you want. Remember the bit will start from the bottom-left corner.
  3. Press "XY" button under Set Origin Point, and you will see that both values of X and Y are "0,00mm".

💡Tip: Choose the smaller steps for Cursor Step setting to move the bit more precisely.

4.3. Import file

  1. Cut → Delete All → Add
  2. Choose the job file you need. Make sure the job is according to the milling bit you are using. If your files don't show up, try to change the file type to "All files (*.*)" → Output
  3. Select "Resume" on the pop-up message.
  4. Then the machine starts!


4.4. Change the tool

After finishing the engraving job, we need to change the tool to do the drilling and cutting job.

  1. You can press the "View" button to move the working platform closer to you. Use the vacuum machine and the brush to clean up the dust.
  2. Replace the bit with Tool.2, which is for drilling and cutting.
  3. Only repeat Step 4.1. to reset the Z-origin, do not reset the XY-origin.
  4. Repeat Step 4.3. to start the job.


4.5. DONE!  🎉🎉

  1. Take out your board.
  2. Remove the tap on the backside.
  3. Finish!

5. Clean up

Remember to clean up after every time you finish using the machine.

  1. Take off the left material and remove the tape on the backside, putting it back in the leftover box.
  2. Clean the dust in the machine.
  3. Make sure the hex key and all the bits are back in their original place.
  4. Put all the tools back in the drawer.

Thanks!


💡For more advanced techniques, consult the Fablab staff💡

6. Troubleshooting


6.1.  The drilling file didn't show the proper holes or show nothing

6.2.  The engraving part wasn't engraved evenly

6.3.  The engraving traces were too thin

6.4.  About through-hole components and rivets


Mainenance

Kris to fill in this.

  • No labels
Write a comment...