CNC machine protocol

CNC machine protocol

CNC Protocol for Cortical Cell Chamber

version 6.0

Sierra, Yuan, Houpu

I.     File translation to .stl

I.1.    use AutoCAD to Convert dwg file to stl file (see figure 1)

a.    select each geometry individually for each file per one cutting job

b.    Choose “file” in the upper left hand corner, click “other formats” option,

c.    Export and “save as” a “stl” file.

II.  File conversion to G code (.nc)

II.1. Upload saved stl file to MeshCAM

II.2. Choose “Two sided cutting”

II.3. Defining the stock (See figure 2)

a.    measure the dimension of the raw material and enter this number, typycally used polycarbonate stocks are 150*150*6.35 mm.

II.4. Support Dimensions- two sided cutting requires substrates to hold the geometry in place (see figure 3)

a.    Choose the width and height of the supporting material. Thicker support would offer stronger support. Should not be thinner than 2*2 mm. it would be cylinder, not cubic.

b.    Select the “top”, “middle”, “bottom”, or “other” where the substrates will be cut to hold the geometry in place. This is dependent on the thickness and geometrical components of the design.

II.5. Height above stock- the position the drill retracts back to move to various positions and returns to rest after cutting is completed (see figure 4)

a.    Enter at least 1.00 mm

II.6. Setting the program zero- This defines the zero of the cutting positions, which ensures the symmetry of the geometry  (see figure 5)

a.    Choose the first option- “top of geometry”

b.    For the “XY position” select the middle of the geometry and the X and Y values will automatically change to the halfway values

c.    Choose “Set to Geometry Zero” to lock the dimensions( not necessary, output g code should be relative coordinate)

II.7. Maximum cutting depth- the deepest the machmill will be able to cut (see figure 6)

a.    This value is the thickness of the raw stock

II.8. Toolpath Parameters (see figure 7)

a.    “Select tool” to cut geometry with preset settings

b.    Roughing

          Depth per pass- is the distance in the z direction the drill cuts away each pass

          Stepover- dependent on the diameter of the drill for overlap of each cutting pass

          Feedrate- the velocity at which the x and y directions are cut

          Plunge rate- the velocity at which the drill cuts in the z direction

          Stock to leave- the amount of stock left to smooth and finish in the final steps

c.    Finish

          Smooths out the remaining uncut raw material (stock to leave amount) in the x and y directions ensuring precision and accuracy

d.    Waterline

          Smooths out any surface angles or grades ensuring precision and accuracy

e.    Pencil Cleanup

          Smooths edges and final finish to the geometry ensuring precision and accuracy

f.     To set the parameters click “Ok”

III.             CNC milling

III.1.                       Machmill3 software (see figure 8)

III.2.                       Raw stock fixation (see figure 9)

a.    Fix sides of raw material onto CNC machine using metal pieces connected to the bottom channels of the  bottom steel support

b.    Firmly fixate via metal pieces and position via screws for the x and y directions of the raw material

c.    Alternative fixating using polycarbonate and screws attached to the bottom steel support is also an option

III.3.                       X, Y, Z Configurations

a.    Choose “Spindle CW15” button to start spindle

b.    Y configuration:

          Using the arrow keys, place spindle at the edge of the raw material- Y1

          Using the arrow keys, move the spindle to the exact opposite edge of the raw material (Y1->Y2)

          Move the spindle to the midpoint of the raw material- (Y1+Y2/2)

          Zero the y coordinate by clicking “zero Z” (Ymidpoint->0)

c.    X configuration:

          Using the arrow keys, place spindle at the edge of the raw material- X1

          Using the arrow keys, move the spindle to the exact opposite edge of the raw material (X1->X2)

          Move the spindle to the midpoint of the raw material- (X1+X2/2)

          Zero the x coordinate by clicking “zero X” (Xmidpoint->0)

  1. Another method to adjust x,y original point. (without touch point sensor/edge finder):
    • Go to one side, x for example, go beyond the material first, left direction first, lowing down the drill to a lower level than surface of the materials (about 0.5 mm). then use arrow keys to move the drill toward the raw material. Flip/tip would be able to move 0.06mm per flip. After hearing the noise of drilling, stop and mark the place as Zero x. then move backward. Change the y direction by a small amount (e.g. 5mm), try feed in x direction again. If this time the drill start hitting at a x value less than 0, then mark this to zero. Repeat 3 times.
    • Then go to the right side of the material, use same method to try the edge. This time write the coordination X1 down rather than set the value. Repeatly test X1 with 3 different place in a line (y change no larger than 20mm), mark the largest value as X2.
    • Then the middle point should be X3 = (0+X2)/2.
    • To set the x zero point, read the current X value X4. Calculate X5=X4-X3. Click on the number displayed in the software, when the number frame showed a lighter color, then use keyboard to type down the number of X5, then hit Enter key to finish the coordinate calibration of x.
    • Same method applies to y.
  2. For maximum accuracy only: Direction test.
    • Move the drill to x = 0, the drill might hit the raw material, or just about to hit it. Then move the drill along y direction, see if the dill hit the material harder when moving, or it leaves the material in noticeable distance. It these happens, it means the direction of raw material is not well aligned with the coordinate.
    • note that both side should be tested, since the raw material might be a square that’s not perfect.

f.     Z Configuration:

          Arbitrarily choose any edge of raw material and lower the spindle to graze the surface of the raw material (auditory confirmation)

          Zero the z coordinate by clicking “zero Z” (Zmidpoint->0)

III.4.                       Running CNC machine and Cutting job

a.    Turn on water, CNC machine power button and press “run” (see figure 10)

b.    Choose the “Load G-Code” button and upload file via flash drive or portable USB drive

c.    Turn the dial for spindle mode to “PC”

d.    Place clear mask over opening of the machine cage

e.    Slip vacuum cover over spindle

f.     Spray milling lubricant onto the milling surface and/or Turn on vacuum

g.    Choose the “cycle start <Alt-R>” button to cut the design (see figure 8)

          If doing Two Sided cutting

          After first side completes cutting, remove one side of metal pieces and screws

          turn over material to the bottom side and slide back into fixed position

          place metal piece and screw back to secure fixed position

          Load new G-Code for “bottom side”

          Use the same X, Y, and Z coordinates; Choose the “cycle start <Alt-R>” button to cut the “bottom” design

h.    After completion, (see figure 11a, 11b)

          Power off the computer

          Power off the CNC machine

          Power off the water pump

          Vacuum the spindle, CNC machine, and surrounding areas of any residue and dust from cutting

          Wipe down the spindle, CNC machine, and surrounding areas of any residue and dust from cutting

 

Tips and Trouble shooting:

stock size is typically 155*152*6.35 mm, but with clamp the actually usable space is only 120*120 mm

Increase the spindle speed would be very helful to avoid the melting of polycarbonate!

(suggested value on controler: 150 to 170.  Most melting occoured when the number reading is lower than 130)

Add milling lubricant to cool the drill tip. (do not spoil onto the tapes to fix the block!!)

Remove the scraps using vacuum cleaner.

If the work is longer than 10 hours, it would be helpful to pause it in the middle and let the drill cool down for 1 hour.

If the spindle is covered by melted polycarbonate, do not remove it by force, it might break the spindle tip. take off the spindle and immerse it in acetone for 3 hours, then the polycarbonate would become soft and easy to remove.

 

misfit of 2 side: caused by Zero point drifting.

Melting: using milling lubricant and increase the spindle speed

CNC simplified checklist

(please read the full manual for the first time)

Starting procedures:

  1. Check the water-cooling system.(it should keep running when plugged)
  2. Start the computer,
  3. Start the controller (under the desk), check the dial switch is turned to “PC” and press “run”
  4. Make sure all 4 clinchers were fasten up.
  5. Choose the “Load G-Code” button and upload file via flash drive or portable USB drive
  6. Test the spindle. If the spindle didn’t response when pressed spindle button, and a message appeared as “minimium PMW required”, click the up butten on the software panel.
  7. Calibration of origin/initial/Zero point (x,y) (MUST be done with every piece of raw materials)
  8. Test Z direction zero point in four sides and four corners, adjust the height of raw materials with tapes and papers. (typically height of one-layer tape is 0.02 mm).

(typically the upper right corner is highest)

  1. Start cutting by click cycle start.
  2. After drilling in one side, use knife blade to remove the rough edge to avoid uneven when this side facing down.
  3. Flip the stock material over x axis. (upside down)
  4. Load the g code of top side and start cycle

If stopped in the middle, select run from here(line xxx) and click cycle start

Shutting down procedures

  1. Lift up the spindle using the up button on keyboard.
  2. Remove the stock
  3. Close the software.
  4. Shutdown the control panel under the table by first press stop and then turn off the switch.
  5. Vacuum the spindle, CNC machine, and surrounding areas of any residue and dust from cutting
  6. Shutdown the computer
  7. Turn off the power suppy to shut down the cooling water.