Text Box: SUNY at Farmingdale
Met 127
Professor Maltezos

Spring 2002
 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

Text Box: Initials Project
Prepared by: R. Hayes
 

 

 

 

 

 


 

 


Table of contents

 

 

Page number

Title

1

Description

2

Feed and Speed Calculations

3

Time Calculation

4

Route Sheet

5

Drawing

6

G-Code

 


Description

 

In this project we will be program our initials on a plate with the CNC machine.  We will incorporating some basic g-code commands.

 

(RH)

N0020G70

N0030G90

N0040M06

N0050T1

N0060M03

(R)

N0080G00X.400Y.400

N0090G01Z.10F30

N0100G01Z-.125F5

N0110G01Y2.60

N0120G01X1.331

N0130G02X1.831Y2.100I1.331J2.100

N0140G01Y2.000

N0150G02X1.331Y1.500I1.331J2.000

N0160G01X.400

N0170G01X1.331

N0180G01X1.831Y.4

N0190G01Z.1F30

 

First we will deal with some set up commands, which appear in most any cnc program.

 

Please note lines N002-N006. These lines tell the machine some basic information about the part we will be machining. G70 means we will be machining in inches as apposed to millimeters. G90 says we are in absolute mode, meaning we will reference all our points from a common origin in the lower left corner of the part. Refer to the AutoCAD drawing.

 

M06, T1 and M03 is the tool change sequence. M06 rapids the machine to its home position and stops. T1 tells the machine it needs a tool defined as Tool number 1 to be inserted into the spindle. M03 turns on the spindle in a clockwise motion.

 

The machine is now ready to machine the part.

 

Note line N008. G00 is a rapid move. Its speed is usually some where around 300 ipm. This is used when moving the spindle a long distance up off the part. It saves time. In this instance the spindle will rapidly move to the start point, which is X.400, Y.400.

 

Line N0090G01Z.10F30, is a linear move to the feed plane at z.1. F30 tells the machine to move at 30 ipm, Slower than the G00 but still not cutting material.

 

Line N0100G01Z-.125F5 and N0110G01Y2.60 starts the actual cutting of the part. Note the F5; this is 5 ipm, the cutting feed rate.

 

When the part is finished machining, the ending sequence of code is read;

                                                            N0320G01Z.1

                                                            N0330M02

                                                            END

The tool feeds at 5 ipm to the feed plane, z.1, then reads M02. M02 tells the machine to end program, rapid to the home position, and turn the spindle off.


 

Feed and Speed Calculations

 

Speed (Revolutions Per Minute)

CS=300, from table in text.

D= .25

 

RPM=                        RPM==4800 rpm

 

Feed (Inches Per Minute

F=.002, from table in text

N=4

 

IPM=F*N*RPM                     IPM=.002*4*4800=38.4 ipm

 

NOTE:

We used a feed of 5 ipm and speed of 1500 rpm in machining this part. The reason for this is that we are choosing to be conservative. We are cutting for the first time and we like to be sure the program is ok before increasing the feed and speed.

 


Time Estimate

 

To calculate time estimate for this piece, we need to know the total distance of the cutting tool. To do this we will add the dimensions in the following picture.

 

 

 

 

Total cutting distance 2+.931+1.571+.931+1.208+2.200+2.200+1.431

Total cutting distance = 12.47

 

So at 5 ipm, which is our actual cutting speed, we will divide 12.47 by 5. This is 2.49 minutes. We can round this to 2.5 minutes.

 

The actual machining time for this project is about 2.5 minutes.

 

 

 

 

 


SUNY at Farmingdale

Route Sheet

Name of Part:        Initials                                                 Drawing No.:          0001                    

No. of Parts to be manufactured:         1                           Order No.:                                        

Sheet Writer:         R. Hayes                                            Sheet 1 of 1

Approved by:                                                                 Date:           2/11/01                           

 

Oper. no.

Operation

Tool Used

Machine

10

Cut sheet aluminum to 4 1/8 x 3 1/8.

 

Band Saw

20

Break sharp edges

File

 

30

Mill to finish length and width

End mill

Vertical Milling Machine

40

Create 2d AutoCAD Drawing of part

AutoCAD

Computer PC

50

Write G-code

Notepad

Computer PC

60

Load G-code into Controller

Computer

CNC Mill

70

Set up Machine and program zero

Computer

CNC Mill

80

Set up part in Fixture

Vise

CNC Mill

90

Verify G-code

Computer

CNC Mill

100

Run Program

1/4 Ball end mill

CNC Mill

110

Remove Part

 

CNC Mill

120

 

 

 

130

 

 

 

140

 

 

 

150

 

 

 

160

 

 

 

170

 

 

 

180

 

 

 

190

 

 

 

200

 

 

 

210

 

 

 

220

 

 

 

230

 

 

 

240

 

 

 

250

 

 

 

260

 

 

 

270

 

 

 

280

 

 

 

290

 

 

 

300

 

 

 

310

 

 

 

320

 

 

 

330

 

 

 

 

 

 

 


 

G-Code for the Dynapath Controller

 

 

 

(RH)

N0020G70

N0030G90

N0040M06

N0050T1

N0060M03

(R)

N0080G00X.400Y.400

N0090G01Z.10F30

N0100G01Z-.125F5

N0110G01Y2.60

N0120G01X1.331

N0130G02X1.831Y2.100I1.331J2.100

N0140G01Y2.000

N0150G02X1.331Y1.500I1.331J2.000

N0160G01X.400

N0170G01X1.331

N0180G01X1.831Y.4

N0190G01Z.1F30

(H)

N0210G00X2.231Y1.500

N0220G01Z-.125F5

N0230G01X3.662

N0240G01Z.1F30

N0250G00X2.231Y.40

N0260G01Z-.125F5

N0270G01Y2.600

N0280G01Z.1

N0290G00X3.662Y.40

N0300G01Z-.125F5

N0310G01Y2.600

N0320G01Z.1

N0330M02

END