Jump to content

Welcome to eMastercam

Register now to participate in the forums, access the download area, buy Mastercam training materials, post processors and more. This message will be removed once you have signed in.

Use your display name or email address to sign in:

Thread Mill

Paul Felger
 Share

Recommended Posts

Paul Felger Newbie

Paul Felger

Posted
Posted

We have a HASS mini mill that Ive jst been doing some simple programming.  Im use to Mastercam and this company has Solid Works and Solid Cam that Im still getting use to.

Was hoping someone here could help out with a program?

Thread milling 1.047-24 ID threads on the HASS.

Using a 1/2 12-32 carbide thread mill (.372 cutting diameter)

 

Matl we are threading is actually a 2" 5c collet.  pretty soft steel.

 

 

Thanks everyone! 

Link to comment
Share on other sites
Guest

Guest

Posted
Posted

T1 M6                

S3000 M3              

G0G90 X 0.0000 Y 0.0000            

G43 Z 2.3500 H 1            

G1 Z -0.6500 F 20            

G41 X 0.1688 Y -0.1688 D 1        

G3 X 0.3375 Y 0.0000 J 0.1688 Z -0.6461 F 10

G3 X 0.3375 Y 0.0000 I -0.3375 Z -0.6148    

G3 X 0.1688 Y 0.1688 I -0.1688 Z -0.6109    

G1 X 0.0000 Y 0.0000            

G0G40

Z 2.3500

M9              

Link to comment
Share on other sites
  • 1 month later...
Paul Felger Newbie

Paul Felger

Posted
  • Author
Posted

Hello again..   Finally got back to this threadmill project and having some trouble.

Below is the code I am using and it doesn't like the "D1"

I am not using any tool comp.

 

  %

O3232 (1.047X24 INTERNAL THREADS)
T9 M6 (1/2 12-32 THREAD MILL)
S3000 M3
GO G90 X0.0 Y0.0
G43 Z1.350 H9
G1 Z-0.650 F20.0
G41 X0.1688 Y-0.1688 D1
G3 X0.3375 Y0.0 J0.1688 Z-0.6461 F10.0
G3 X0.3375 Y0.0 I-0.3375 Z-0.6148
G3 X0.1688 Y0.1688 I-0.1688 Z-0.6109
G1 X0.0 Y0.0 
GO G40
Z1.350
M9
M30
%
 
 
Any help would be great...
 
 

Thread milling 1.047-24 ID threads on the HASS.

Using a 1/2 12-32 carbide thread mill (.372 cutting diameter)

 

need .5 to .625 of thread

 

 
 
Link to comment
Share on other sites
Paul Felger Newbie

Paul Felger

Posted
  • Author
Posted

Just noticed the GO..

Tool Im using is a  1/2" 12-32 TPI

Its a 4 flute single tip thread mill (.372 cutting dia)

 

This program looks like it for a full form thread mill..

 

Someone help with a program for a single tip?

 

One time project and this place doesn't have mastercam.

They have solid work/solid cam  which im still learning :(

Link to comment
Share on other sites
crazy^millman Veteran

crazy^millman

Posted
Posted

Here by hand off the top of my head.

 

G0 X0 Y0 Z.1 (CENTER OF THE HOLE USING X0 Y0 SD OUR POSITION)

G1 G41 X.3375 D1 (MOVE THE DISTANCE OF THE RADIUS OF THE HOLE MINUS THE DIAMETER OF THE TOOL)

G3 X-.3375 Y0 Z-.02083 R.3375 (MOVE A HELICAL MOVE TO X- THE OTHER SIDE THEN Z MINUS HALF OF THE PITCH)

G3 X.3375 Y0 Z-.04166 R.3375 (MOVE A HELICAL MOVE TO X+ THE OTHER SIDE THEN Z MINUS HALF OF THE PITCH)

(REPEAT THE ABOVE AS MANY TIMES AS NEEDED TO GET THE DEPTH)

G1 G40 X0

 

Sorry, but many years I never had a CAM system and learning some basic CNC programming would do you a world of good.

 

Encase you don't trust the numbers off the top of my head here is a CNC program using the tool defined above cutting the thread you originally called out. This is starting from the bottom and coming up from a depth of -1.0:

%
O0000(TOOLPATH GROUP-1)
(DATE=DD-MM-YY - 16-11-16 TIME=HH:MM - 10:10)
(MCX FILE - T)
(NC FILE - C:\USERS\RON\DOCUMENTS\MY MCAM2017\MILL\NC\TOOLPATH GROUP-1.NC)
(MATERIAL - ALUMINUM INCH - 2024)
( T1 |  THREAD MILL - 0.372 | H1 )
N100 G20
N110 G0 G17 G40 G49 G80 G90
N120 T1 M6
N130 G0 G90 G54 X0. Y0. A0. S1069 M3
N140 G43 H1 Z.25
N150 Z.1
N160 G1 Z-1. F15.
N170 Y-.2375 F25.
N180 G3 X.3375 Y0. Z-.9896 I.0852 J.2375
N190 X-.3375 Z-.9688 I-.3375 J0.
N200 X.3375 Z-.9479 I.3375 J0.
N210 X-.3375 Z-.9271 I-.3375 J0.
N220 X.3375 Z-.9062 I.3375 J0.
N230 X-.3375 Z-.8854 I-.3375 J0.
N240 X.3375 Z-.8646 I.3375 J0.
N250 X-.3375 Z-.8438 I-.3375 J0.
N260 X.3375 Z-.8229 I.3375 J0.
N270 X-.3375 Z-.8021 I-.3375 J0.
N280 X.3375 Z-.7812 I.3375 J0.
N290 X-.3375 Z-.7604 I-.3375 J0.
N300 X.3375 Z-.7396 I.3375 J0.
N310 X-.3375 Z-.7188 I-.3375 J0.
N320 X.3375 Z-.6979 I.3375 J0.
N330 X-.3375 Z-.6771 I-.3375 J0.
N340 X.3375 Z-.6562 I.3375 J0.
N350 X-.3375 Z-.6354 I-.3375 J0.
N360 X.3375 Z-.6146 I.3375 J0.
N370 X-.3375 Z-.5938 I-.3375 J0.
N380 X.3375 Z-.5729 I.3375 J0.
N390 X-.3375 Z-.5521 I-.3375 J0.
N400 X.3375 Z-.5312 I.3375 J0.
N410 X-.3375 Z-.5104 I-.3375 J0.
N420 X.3375 Z-.4896 I.3375 J0.
N430 X-.3375 Z-.4688 I-.3375 J0.
N440 X.3375 Z-.4479 I.3375 J0.
N450 X-.3375 Z-.4271 I-.3375 J0.
N460 X.3375 Z-.4062 I.3375 J0.
N470 X-.3375 Z-.3854 I-.3375 J0.
N480 X.3375 Z-.3646 I.3375 J0.
N490 X-.3375 Z-.3438 I-.3375 J0.
N500 X.3375 Z-.3229 I.3375 J0.
N510 X-.3375 Z-.3021 I-.3375 J0.
N520 X.3375 Z-.2812 I.3375 J0.
N530 X-.3375 Z-.2604 I-.3375 J0.
N540 X.3375 Z-.2396 I.3375 J0.
N550 X-.3375 Z-.2188 I-.3375 J0.
N560 X.3375 Z-.1979 I.3375 J0.
N570 X-.3375 Z-.1771 I-.3375 J0.
N580 X.3375 Z-.1562 I.3375 J0.
N590 X-.3375 Z-.1354 I-.3375 J0.
N600 X.3375 Z-.1146 I.3375 J0.
N610 X-.3375 Z-.0938 I-.3375 J0.
N620 X.3375 Z-.0729 I.3375 J0.
N630 X-.3375 Z-.0521 I-.3375 J0.
N640 X.3375 Z-.0312 I.3375 J0.
N650 X-.0004 Y-.3375 Z0. I-.3375 J0.
N660 X.2375 Y-.0003 Z.0104 I.0003 J.2523
N670 G1 X0. Y0.
N680 G0 Z.1
N690 Z.25
N700 M5
N710 G91 G28 Z0.
N720 G28 X0. Y0. A0.
N730 M30

Funny a Mastercam forum helping a different CAM, but we are professionals trying to earn a living.

  • Like 1
Link to comment
Share on other sites
htm01 Newbie

htm01

Posted
Posted

 

Hello again..   Finally got back to this threadmill project and having some trouble.

Below is the code I am using and it doesn't like the "D1"

I am not using any tool comp.

 

  %

O3232 (1.047X24 INTERNAL THREADS)
T9 M6 (1/2 12-32 THREAD MILL)
S3000 M3
GO G90 X0.0 Y0.0
G43 Z1.350 H9
G1 Z-0.650 F20.0
G41 X0.1688 Y-0.1688 D1
G3 X0.3375 Y0.0 J0.1688 Z-0.6461 F10.0
G3 X0.3375 Y0.0 I-0.3375 Z-0.6148
G3 X0.1688 Y0.1688 I-0.1688 Z-0.6109
G1 X0.0 Y0.0 
GO G40
Z1.350
M9
M30
%
 
 
Any help would be great...
 
 

Thread milling 1.047-24 ID threads on the HASS.

Using a 1/2 12-32 carbide thread mill (.372 cutting diameter)

 

need .5 to .625 of thread

 

 

there is a setting if you want to use a different D comp # than the Tool # also

Link to comment
Share on other sites
Pilot Plant Supervisor Newbie

Pilot Plant Supervisor

Posted
Posted

For a quick program at the machine, I like to keep it simple. Yes, it is conventional cut for right hand threads, but it is the least amount of code, and least amount of math.

 

T1 M6                

G0 G90 G54 X0 Y0 S3000 M3           

G43 Z2. H1  

Z.1 M8         

G1 Z0 F20.            

G91 G42 X.3375 D1  F9.     

G2 I-.3375 Z-.0417 L15

G1 G40 X-.3375  

G90 G0 Z2. 

M9           

  • Like 2
Link to comment
Share on other sites

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

Guest
Reply to this topic...

×   Pasted as rich text.   Paste as plain text instead

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.

×
 Share
Go to topic listing

  • Recently Browsing   0 members

    • No registered users viewing this page.

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Useful Links

Contact Info

Subscribe to eMastercam News

 

Legal

Privacy Policy

Store Terms & Conditions

Forum Guidelines

Follow us

×
×
  • Create New...