CNC Mill

CNC Converted Little Machine Shop Mini-Mill
Location: Machining Area Ownership: Breaks Everything (Loan) Status: Fully Working Usage Restrictions: Preapproval Required?
CNC Mill
Brand: Little Machine Shop Model: UNIT-00 Coordinate System: Cartesian Quality: Prosumer/Professional Axis Travel: X: 120mm, Y: 288mm, Z: 210mm

The Mini-Mill is a loan from Mr. "Breaks Everything".

Standard Operating Procedure

CNC Instructions

   1. Turn on Computer
   2. Flip power Switch to up Position
   3. Turn Estop Clockwise 
   4. Login User: maglab 
      Password: magcat
   5. Click on “metric” or “merica” for metric or standard interface
   6. Click Home All (important, bad things will happen if you don’t
   7. Click on file on top left and click open navigate to your g-code file
   8. Click on help for help menu
      

Notes:

   • Do not store g-code locally use USB drive
   • If Estop is pressed have to re-home
   • Use LinuxCNC post-processor
   • Power Off Controller Before Computer

Quirks

Conversion was a project.

Supplemental Resources

Brandon's Notes

He does not make good notes.

Use the following settings in the Fusion 360 postprocessor (after selecting the emc2 linuxcnc post):

• Safe Retracts and Home Positioning
  • Safe Retracts: G28

Try to use G54 instead of G53 because it's less scary.

FlatCAM Parameters

There are three different types of operations that go into CNC milling a PCB: hole drilling, trace isolation, and edge milling. Each of these operations will get its own section under this guide.

Hole Drilling

Hole drilling is accomplished with the variety of 1/8" shank jobber drills provided next to the CNC. The following equation is used to calculate the length that the drill needs to be passed into the PCB in order to clear a hole: ${\dfrac {d_{drill}/2}{\tan(65^{\circ })}}+1.65{\text{mm}}$. A tabular version is provided below for each 0.1mm increment:

Drill Diameter	Depth
0.6	1.77
0.7	1.79
0.8	1.82
0.9	1.84
1.0	1.86
1.1	1.88
1.2	1.90
1.3	1.92
1.4	1.94
1.5	1.96
1.6	1.98
1.7	2.00
1.8	2.02
1.9	2.04
2.0	2.06

The following parameters apply for drilling operations. Note that the following machine settings may need to be changed for larger jobber drills: Feedrate Z, Spindle Speed.

Parameter	Value
Diameter	{Auto-filled from the DXF file import}
Cut Z	{Use the provided look-up table above}
Multi-Depth	⬜
Travel Z	2
Feedrate Z	300
Spindle Speed	7200
Dwell	⬜
Offset Z	0

Trace Isolation

The tool parameters should be stored in the tool database which is loaded by default when you open FlatCAM. This section exists in case those parameters were somehow erased.

The main parameters for the v-cutter are specified when purchasing the cutter. The main ones at the makerspace are specified at 0.1mm tip, 20 degree v-angle.

The following table contains the milling parameters for the V-cutter.

Parameter	Value
Shape	V
V-Dia	0.1440
V-Angle	20
Tool Type	Finish
Tool Offset	Path
Custom Offset	0
Cut Z	-0.15
MultiDepth	⬜
DPP	0
Travel Z	2
ExtraCut	⬜
E-Cut Length	0.1
Feedrate X-Y	240
Feedrate Z	60
FR Rapids	1500
Spindle Speed	12000
Dwell	⬜
Dwelltime	1

The tool library settin⬜gs for the cutter's isolation parameters are unchanged because it is assumed that the passes and overlap are going to be decided on the isolation tool panel instead of from the tool library.

There are two parameters for isolation milling:

Parameter	Value
Passes	{Determined on a case-by-case basis}
Overlap	20%

The determination for number of passes should be based on the minimum passes to ensure trace-to-trace clearance. This is largely determined by the maximum trace clearance on the PCB. Careful design and the generous use of copper fills is recommended since flatcam is not the friendliest software for non copper clearing. The following example should determine your minimum passes to be five by counting from the innermost pass to the outermost pass:

Edge Milling

Edge milling is performed with the 1.5mm burr. These are inexpensive carbide burrs originally intended for use with fiberglass, but they can be used with the PF material preferred by the makerspace.

Manually entering parameters for edge milling is important because the software likes to crash if a tool is deleted from the tool table when performing edge milling. The following parameters should be entered instead of imported from the tool library:

Parameter	Value
Dia	1.5
Cut Z	-1.65
Multi-Depth	⬜
Travel Z	2
Feedrate X-Y	200
Feedrate Z	72
Spindle Speed	7200
Dwell	⬜