Practice for Final Exam (MasterCAM)

Advertisements

MasterCAM Practice (Pocket Facing, Contour, Pocket Standard, Spot Drill, and Drill)

Drawing

Practice Test

Review The Term Test2 (Contour, Pocket Facing, Pocket Standard, Spot Drill, and Drill)

Term-Test2

Term-Test2

Set up the Material

Set up the Material

Set up the Material

Set up the Material

Contour

Contour

Contour

Contour

Contour2

Contour2

Contour3

Contour3

Contour4

Contour4

Contour5

Contour5

Contour6

Contour6

PocketFacing_Boss1

PocketFacing_Boss1

PocketFacing_Boss2

PocketFacing_Boss2

PocketFacing_Boss3

PocketFacing_Boss3

PocketFacing_Boss4

PocketFacing_Boss4

PocketFacing_Boss5

PocketFacing_Boss5

PocketFacing_Boss6

PocketFacing_Boss6

PocketFacing_Boss7

PocketFacing_Boss7

PocketFacing_Boss8

PocketFacing_Boss8

PocketFacing_Boss9

PocketFacing_Boss9

PocketStandard-1

PocketStandard-1

PocketStandard-2

PocketStandard-2

PocketStandard-3

PocketStandard-3

PocketStandard-4

PocketStandard-4

PocketStandard-5

PocketStandard-5

PocketStandard-6

PocketStandard-6

SpotDrill

SpotDrill

Drill

Drill

CAM Practice

Drawing

The Angled Holes

To draw the angled holes:

1. Make one circle then select it.

2. Go to the “Xform” menu then click the “Rectangular Array” submenu.

  • Input the number “7” to create X direction holes in the blank of the Direction 1.
  • Input the number “3” to create Y direction holes in the blank of the Direction 2.
  • Input the number “1/2” for the X, Y distances of the Direction1 and 2.
  • Click the “Done” button.

3. Delete the two circles of the right side of the first and third rows.

4. Move “-1/4” the second row circles to the left side by using the “Xform Translate” method.

5. Rotate all circles by using the “Xform Rotate” method.

.

The Rotated Holes

 To draw the rotated holes in the circle

1. Go to the “Created” menu and select the “Bolt Circle…” submenu.
2. Click the bolt circle’s center point.

√ Input the size (1”) of the bolt circle.

√ Input the number “16” to create 16 holes.

√ Input the initial angle of the first hole.

√ Enable the “Points”, “Arcs”, “Center Pont” and “Reference”.

√ Input number “3/4” (hole size) in the “Arcs” box.

√ Click the “Done” button.

...

.

Setting the machine properties (Tool Settings)

Setting the Machine Properties (Tool Settings)

Stock Settings

  • Change the parameters to match the following “Stock Setup image”
  • Define the stock size (0.625 X 8.125 X 10.82) and type (ALUM. 6061T6).

Stock Setup

Setting the Machine Properties (Tool Settings)

  • Profile outside contour, where necessary, with a ø 7/8″ Flat Endmill (Take a 0.05 finishing cut)
  • Use a ø 3/4″ Flat Endmill to machine boss. Pocket type (island facing)
  • Use a ø 5/8″ Flat Endmill to machine pocket. (1 X 0.17 Roughing and one 0.03 finishing depth cut) Finish pocket walls with a 0.02 finishing pass.
  • Spot drill (ø 3/8″) and peck drill all holes.

* Each tool of the cutting speed is “200fpm”.

the completion of my practice

The Completion of My Practice

Adviser and Reference

Adviser and Reference

CNC (Analysis of the Circular Interpolation Assignment)

List of Coordinates:

1 X0 Y0.30 / 2 X0.695 Y-0.9 / 3 X-0.695 /4 X-1.75 Y1.2 / 5 X-1.15 Y1.8 R0.6 / 6 X-2.316 / 7 X2.316

8 X1.15 / 9 X1.75 Y1.2 R0.6 10 X-2.457 Y-0.85 / 11 X-1.47 Y-2.144 R2.6 / 12 X1.47 R2.0 / 13 X2.457 Y-0.85 R2.6

14 X4.0 Y4.05 R4.05 / 15 X-4.25 Y-2.625 / 16 Y2.625 / 17 X-3.125 Y3.75 R1.125 / 18 X3.125

19 X4.25 Y2.625 R1.125 / 20 Y-2.625 / 21 X3.125 Y-3.75 R1.125 / 22 X-3.125

The program to machine as follows:

Tool List

T10 – 1.5″ DIA TWO FLUTES ENDMILL

(RPM:12*280/3.141592*1.5=713) / (IPM:713*0.008*2=11.4) / (Down IPM:11.4*0.4=4.56)

T04 – 3/8″ DIA TWO FLUTES ENDMILL

(RPM:12*280/3.141592*0.375=2852) / (IPM:2852*0.003*2=17.112) / (Down IPM:17.112*0.4=6.8448)

T02 – 1/4″ DIA TWO FLUTES ENDMILL

(RPM:12*280/3.141592*0.25=4278) / (IPM:4278*0.002*2=17.112) / (Down IPM:17.112*0.4=6.8448)

%: Start Code – Begining of File Transfer

O0023: Program Identification (PART#O0023 CIRCULAR INTERPOLATION)

(PROGRAMMER: HARRY BAEK)

(MACHINE:HAAS-VF1)

N10 G17: XY Plane Selection  G20: Input Inches  G40: Cutter Compensation Cancel  G49: Tool Length Compensation Cancel G80: Canned cyce cancel G90: Absolute programming – Safety Codes with Initial Setting And Cancellations

N20 G28: Return to Reference Point G91: Incremental programming Z0 – Safety Codes Send Z Axis Home Incrementally

N30 G28 X0 Y0 – Safety Codes Send X and Y Axis Home Incrementally

N40 T10: Tool Fuction, Number M06: Tool change (1.5″ DIA TWO FLUTES ENDMILL) – Tool Change For T06 and Toll Description in Brackets

N50 G00: Rapid Positioning G54: Work Coodinate System Offset G90 X0 Y4.05 S713: Spindle Speed (RPM) M03 Spinde CW. Rotation – Restart Block

N60 G43: Tool Length Compensation Z2.0 H10: Offset Number M08: Miscellaneous Function, Coolant pump on – Tol LG Offset, Clear Plane 2″ Above Part

N70 G00 Z0.1

N80 G01: Linear Interpolation Z-0.25 F4.56: Feed Function

N90 G02: Circular Interpolation (CW) J-4.05: Y Axis Arc Center F11.4

N100 G00 Z2.0

N110 X-4.25 Y-2.625

N120 Z0.1

N130 G01 Z-1.03 F4.56

N140 Y2.625 F11.4

N150 G02 X-3.125 Y3.75 I1.125: X Axis Arc Center

N160 G01 X3.125

N170 G02 X4.25 Y2.625 J-1.125

N180 G01 Y-2.625

N190 G02 X3.125 Y-3.75 I-1.125

N200 G01 X-3.125

N210 G02 X-4.25 Y-2.625 J1.125

N220 G00 Z2.0 M09: Coolant pump off

N230 G28 G49 G91 Z0 M05: Spinde stop

N240 M01: Optional stop

N250 T04 M06 (3/8″ TWO FLUTES ENDMILL)

N260 G00 G54 G90 X0 Y0.3 S2852 M03

N270 G43 H04 Z2.0 M08

N280 Z0.1

N290 G01 Z-0.1 F6.84

N300 X0.695 Y-0.9 F17.1

N310 X-0.695

N320 X0 Y0.3

N330 G00 Z2.0

N340 X-1.75 Y1.2

N350 Z0.1

N360 G01 Z-0.1 F6.84

N370 G03 X-1.15 Y1.8 I0.6 F17.1

N380 G01 X-2.316

N390 G00 Z2.0

N400 X2.316

N410 Z0.1

N420 G01 Z-0.1 F6.84

N430 X1.15 F17.1

N440 G03 X1.75 Y1.2 J-0.6

N450 G00 Z2.0 M09

N460 G28 G49 G91 Z0 M05

N470 M01

N480 T02 M06 (1/4″ DIA TWO FLUTES ENDMILL)

N490 G00 G54 G90 X-2.457 Y-0.85 S4278 M03

N500 G43 Z2.0 H02 M08

N510 Z0.1

N520 G01 Z-0.1 F6.84

N530 G03 X-1.47 Y-2.144 I2.457 J0.85 F17.1

N540 G02 X1.47 I1.47 J-1.356

N550 G03 X2.457 Y-0.85 I-1.47 J2.144

N560 G00 Z2.0 M09 – Rapid to Clear Plane 2″ Above Part and Coolant Off

N570 G28 G49 G91 Z0 M05 – Home in Z only, Cancel Tool LG Offset and Spindle Off

N580 G28 X0 Y0- Home in XY only

N590 M30: End of program

%: Stop Code – End of file transfer