7. Computer Controlled Machining

The group assignment for this week was to;
1. Complete our lab’s safety training for our FabLab’s Shopbot
2. Test our machine’s runout, alignment, fixturing, speeds, feeds, materials and toolpaths

Ideally we could test all, but because we spent 1 whole day on getting a good enough cut (due to bad quality endmill), we could only manage to do the offset test during the groupwork day.

Test	Description	Result
Runout	The rotation inaccuracy which occurs when the tool is no longer aligned with the main axis. (Ideal a tool with 1/4 inch should leave a trace of exactly 1/4 inch.)	1/4inch should be 6.35mm.
Alignment	Check for slanted workspace by printing a square.	No bad angle or slants on our test piece
Fixturing	The use of specialized tools to hold workpieces in place during machining on a CNC machine. Fixtures are essential for ensuring accuracy, repeatability, and efficiency	We used nails
Speeds and feeds	“Feeds” refers to the amount of engraving per cut, i.e., how fast the cutter moves through the material. If the sawdust is very fine, you could raise the speed to have more coarse sawdust. Spindle Speed is the endmill rotational RPM. Plunge Rate is vertical motion…speed of entry into material…slower is safer	We referred to manufacturer’s recommendation
toolpaths (Kerf, offset)	Offset value for height and width	No offset was needed for our shopbot with our almost brand new endmill

Our Shopbot:
We used the Shopbot at FabLab Minatomirai

Specs	SHOPBOT PRS Standard 96-48
Machine size ( X×Y×Z )	3050 x 2000 x 1700mm
Workable Area ( X×Y×Z )	2615 x 1245 x 200mm
Cutting Speed	XY：max 150mm/sec　/ Z： max 50mm/sec
Minimum cutting distance	0.015mm

Our Material:
Softwood plywood (合板 ランバーコア) 15mm thickness, 910x1820mm

Our Endmill:
1/4 inch Solid Carbide router, 2 flute, Downcut extreme heavy duty
(1/4 inch = 6.35mm)

Safety Precautions

Attire:
- Wear safety glasses
- No sandals
- No scarves or loose-fitting clothing
- Long hair must be tied up
- No gloves while operating equipment
- But use gloves when handling screws and wood.
- Recommended to wear earplug and masks while the machine is cutting.

Mindset:
- Do not use it when you are not in a good mental state such as when feeling anxious, tired, sleepy, etc
- Take plenty of time and do not rush
- Stay vigilant even after you start feeling comfortable with the machine
- Do not operate machines alone
- DO NOT touch any tools when they are energized
- Know how to perform an emergency stop before starting equipment
- Don’t leave the machine while operating, pay attention to machine works, and stop immediately if anything trouble happens

Know what the emergency procedures are

The Offset test

We calculated the necessary offset value for secure fit.

• Our wood width was supposedly 15mm, so we decided to test offsets of +0 to +1mm, with 0.1mm intervals.
  (However we found out that some parts of our material were thicker than our order of 15mm. Lesson learnt to always measure our material beforehand (at several different points)!!)

Preparing data

We used the Kerf Generator made by Atsufumi Suzuki (2022 Graduate from Kamakura), with dimensions: 15 mm - 16mm with 0.1 intervals.

Setting up

Preparing CAM data

We used the Vcarve-Pro software to make the CAM Toolpath.

VCarve Pro is a software program that helps users design, lay out, and machine parts using a CNC router. It’s used for sign making, engraving, and other CNC manufacturing. - VCarve-Pro

“Job setup” and “Job material” were set as follows;

Parameter	Setting	Memo
Job type	Single sided
Job size	900 (Width/X) x 450 (Height/Y) x 15 (Y)	Face the Shopbot PC to determine the direction of XY
Zero Position	Material Surface
Use offset	No
XY Datum Position	Left Bottom

Import .dxf data and rotate as necessary.
Draw the hole for the nail (We set 6 nails).

For Endmill settings it is recommended to use the Blade manufacturer’s recommended values.
However since there was no recommendation for the 1/4 Downcut endmill for Soft Plywood, we refered to 2 values below, and ended up using the default value on Fablab Minatomirai’s PC.

Parameter	1/4” Upcut EndMill for Soft Plywood	1/4” Downcut EndMill for Softwood	We used:
Cut	1 x D	N/A	1/2 x D (.125inches)
Chip Load per leading edge (inches)	.004-.006	.007-.009	0.0075
Flutes	2	2	2
Feed Rate (inches/sec)	1.2-1.8	4.2-5.4	3
Spindle speed, RPM	18,000	18,000	12,000

The Toolpath settings were as follows:
(We selected “Profile Toolpath” as we are only cutting. For pockets, also need to select “Engrave Toolpath” )

Parameter	Setting
Cutting Depths, mm	Start Depth: 0, Cut Depth: 15.3 (1st try, too shallow), & 16 (2nd try)
Tool	1/4 Inch Downcut Endmill
Machine Vectors	Outside
Tab	Add Tab (Length: 10mm, Thickness: 3mm), 4 tabs

We specified the Tab by selecting “Edit Tab” and clicking on the desired points. When done, press “Close”.

Create Toolpath by selecting “Calculate”.
We then set the Toolpath for drill hole of 3.0mm.
We checked the Toolpath Preview, to make sure the drill hole is cut first.

CAM toolpath is complete, so we saved Toolpath and exported for Shopbot.
(As Post Processor, select Shopbot TC (MM)(.sbp))
If the file is made in an external PC, transfer the .sbp file to the Shopbot PC, and move it to a local drive (Do not access the file on external drive, in case connection is lost during cutting !!)

Setting the Drill bit

Remove the collet and collet screw from the box.

• Set the Mill to collet
  
• Set them to machine (first by hand, then using the screwdriver, set really tightly)
  → Use a glove
  → Set the box underneath in case the mill drops while working and material gets damaged
  → To prevent runout, set at least the third of the length of drill, but make sure it can reach width of material
  

https://fabacademy.org/2022/labs/kamakura/assignments/week07_indonesia.html#install-the-tool

Setting XYZ Origin

• For XY position, type in C3 in the command control. Machine arm will move to the Home position.
  
• For Z position, we use a probe tool.
  → Remove the probe tools from machine arm and Set the metal plate under the mill.
  　→ Place clip around the metal part. Touch the metal plate to point tip the screw to make a connection. (Make sure to touch gently to not damage the screw head!!)
  → Place the metal plate directly under the mill. (Make sure the plate is placed directly under, as the mill will continue to go lower until it touches the metal!!)
  → Type in C2 on the command control to lower the mill. Once the milll touches the metal place, the Z origin will be automatically set. We also check the same number with actual measurement and application panel: it was 25.402mm
  
• Remember to remove the plate after testing!!
  

Finally, drill in nails to secure the material to bed.

Airpass

• It is recommended to do Airpass before actual cut to check that there are no strange movements and to make sure the pass doesn’t cross any nails.
  
• For Airpass, press C3 to get back to XY origin, raise Z by around 20mm and presss Start cut.
  
• After Airpass, make sure to set XYZ origin again.

Start cutting

Final Checklist:
[ ] Attach the extraction attachment.
[ ] Turn on the Air duster. (Press the green button)
[ ] Close the curtain.

• Finally, when ready, turn the machine on with key, type in FP in command console, open the .sbp file, and press “Start cut”.
  

fp command	turn on	start cut

Processing…

After cutting

• Turn off the machine key and Air duster.
  
• Vacuum clean the wood surface before removing it to minimise chips scattering everywere.
  
• Unscrew, cut off tabs, sand down splinters.
  
• Put all tools back to its origin and clean and organize the workspace. (Dirty environment increases the risk of accidents happening!!)

Results

Our first test was a big failure.

Problem analysis:

Result	Reason	Action
The finish is extremely bad quality. The slot width is very uneven.	The drill bit is in very bad condition, with rust and breakage	Make sure to inspect the drill before use.
Chip load is too fine	Rico suggested setting it to a slower cut speed
The depth of cut is too shallow	We forgot to measure the material and the thickness of the board was uneven. Also the cut depth was too shallow (we had set it to 15.3cm)	Next time, we should measure the width in multiple locations before cutting. Also cut depth should be about + 1mm

Differences of drill bit quality - Upper: bit with rust / Bottom: clean new bit

Our secont test …

← 2 test results alongside each other
With our almost brand new mill, we found that no Clearance was necessary.

Files and Codes

Toolpath for Testkit
Toolpath for Drill

Useful links

• FabLab Kamakura Tutorial
  
• Fablab Kuriyma 2022
  
• Kamakura (Indonesia) 2022
  
• Kamakura 2023
  
• Useful documentation
  
• Rico’s guide