What's new
What's new
By:
Advanced search…

Thread Milling on Haas VF2

J

jwracer14

Plastic
Joined
Jun 30, 2009
Location
Joliet,IL USA
I am trying to thread mill on our 1997 Haas VF2 mill. I have a carbide 5/8-11 hob and I'm trying to mill a 5/8-11 thread 1" deep in 304 SS. The cutter manufacturer recommends 4-5 passes to do this. I have tried every thread milling generator online that I can find. I always get some kind of alarm when I try to run it. The cutter is .470 dia. The hole size is .540. I keep getting tool too big or cutter interference. Can anyone point me in the right direction? Thanks JW
 
here is a climb and conventional cut threadmill

M1
N1 (.470-TML-MTS0500C13-11UN)
T1 M6 (CLIMB CUT)
G0 G90 G54 X0 Y0 S3000 M3
G43 Z1. H01 D01 M8
G1 Z-1.1114 F10.
G41 D1 X.1458 Y-.1458
G3 X.2916 Y0 Z-1.1 I0 J.1458
Z-1.0091 I-.2916 J0
Z-.9182 I-.2916 J0
Z-.8273 I-.2916 J0
Z-.7364 I-.2916 J0
Z-.6455 I-.2916 J0
Z-.5546 I-.2916 J0
Z-.4637 I-.2916 J0
Z-.3728 I-.2916 J0
Z-.2819 I-.2916 J0
Z-.191 I-.2916 J0
Z-.1001 I-.2916 J0
Z-.0092 I-.2916 J0
X.2346 Y.1732 Z0 I-.2916 J0
X.0307 Y.2039 Z.0114 I-.1173 J-.0866
G0 G40 X0 Y0
Z1.
Z.2
G1 Z-1.1114
G41 D1 X.1491 Y-.1491
G3 X.2983 Y0 Z-1.1 I0 J.1491
Z-1.0091 I-.2983 J0
Z-.9182 I-.2983 J0
Z-.8273 I-.2983 J0
Z-.7364 I-.2983 J0
Z-.6455 I-.2983 J0
Z-.5546 I-.2983 J0
Z-.4637 I-.2983 J0
Z-.3728 I-.2983 J0
Z-.2819 I-.2983 J0
Z-.191 I-.2983 J0
Z-.1001 I-.2983 J0
Z-.0092 I-.2983 J0
X.24 Y.1772 Z0 I-.2983 J0
X.0314 Y.2086 Z.0114 I-.12 J-.0886
G0 G40 X0 Y0
Z1.
Z.2
G1 Z-1.1114
G41 D1 X.1525 Y-.1525
G3 X.305 Y0 Z-1.1 I0 J.1525
Z-1.0091 I-.305 J0
Z-.9182 I-.305 J0
Z-.8273 I-.305 J0
Z-.7364 I-.305 J0
Z-.6455 I-.305 J0
Z-.5546 I-.305 J0
Z-.4637 I-.305 J0
Z-.3728 I-.305 J0
Z-.2819 I-.305 J0
Z-.191 I-.305 J0
Z-.1001 I-.305 J0
Z-.0092 I-.305 J0
X.2453 Y.1811 Z0 I-.305 J0
X.0321 Y.2132 Z.0114 I-.1227 J-.0906
G0 G40 X0 Y0
Z1.
Z.2
G1 Z-1.1114
G41 D1 X.1575 Y-.1575
G3 X.315 Y0 Z-1.1 I0 J.1575
Z-1.0091 I-.315 J0
Z-.9182 I-.315 J0
Z-.8273 I-.315 J0
Z-.7364 I-.315 J0
Z-.6455 I-.315 J0
Z-.5546 I-.315 J0
Z-.4637 I-.315 J0
Z-.3728 I-.315 J0
Z-.2819 I-.315 J0
Z-.191 I-.315 J0
Z-.1001 I-.315 J0
Z-.0092 I-.315 J0
X.2534 Y.1871 Z0 I-.315 J0
X.0332 Y.2202 Z.0114 I-.1267 J-.0935
G0 G40 X0 Y0
Z1. M9
G0 G91 G28 Z0
M1
N1 (.470-TML-MTS0500C13-11UN)
T1 M6 (CONVENTIONAL CUT)
G0 G90 G54 X0 Y0 S3000 M3
G43 Z1. H01 D01 M8
G1 Z.0114 F10.
G42 D1 X.1458 Y.1458
G2 X.2916 Y0 Z0 I0 J-.1458
Z-.0909 I-.2916 J0
Z-.1818 I-.2916 J0
Z-.2727 I-.2916 J0
Z-.3636 I-.2916 J0
Z-.4545 I-.2916 J0
Z-.5454 I-.2916 J0
Z-.6363 I-.2916 J0
Z-.7272 I-.2916 J0
Z-.8181 I-.2916 J0
Z-.909 I-.2916 J0
Z-.9999 I-.2916 J0
Z-1.0908 I-.2916 J0
X.2346 Y-.1732 Z-1.1 I-.2916 J0
X.0307 Y-.2039 Z-1.1114 I-.1173 J.0866
G0 G40 X0 Y0
Z1.
Z.2
G1 Z.0114
G42 D1 X.1491 Y.1491
G2 X.2983 Y0 Z0 I0 J-.1491
Z-.0909 I-.2983 J0
Z-.1818 I-.2983 J0
Z-.2727 I-.2983 J0
Z-.3636 I-.2983 J0
Z-.4545 I-.2983 J0
Z-.5454 I-.2983 J0
Z-.6363 I-.2983 J0
Z-.7272 I-.2983 J0
Z-.8181 I-.2983 J0
Z-.909 I-.2983 J0
Z-.9999 I-.2983 J0
Z-1.0908 I-.2983 J0
X.24 Y-.1772 Z-1.1 I-.2983 J0
X.0314 Y-.2086 Z-1.1114 I-.12 J.0886
G0 G40 X0 Y0
Z1.
Z.2
G1 Z.0114
G42 D1 X.1525 Y.1525
G2 X.305 Y0 Z0 I0 J-.1525
Z-.0909 I-.305 J0
Z-.1818 I-.305 J0
Z-.2727 I-.305 J0
Z-.3636 I-.305 J0
Z-.4545 I-.305 J0
Z-.5454 I-.305 J0
Z-.6363 I-.305 J0
Z-.7272 I-.305 J0
Z-.8181 I-.305 J0
Z-.909 I-.305 J0
Z-.9999 I-.305 J0
Z-1.0908 I-.305 J0
X.2453 Y-.1811 Z-1.1 I-.305 J0
X.0321 Y-.2132 Z-1.1114 I-.1227 J.0906
G0 G40 X0 Y0
Z1.
Z.2
G1 Z.0114
G42 D1 X.1575 Y.1575
G2 X.315 Y0 Z0 I0 J-.1575
Z-.0909 I-.315 J0
Z-.1818 I-.315 J0
Z-.2727 I-.315 J0
Z-.3636 I-.315 J0
Z-.4545 I-.315 J0
Z-.5454 I-.315 J0
Z-.6363 I-.315 J0
Z-.7272 I-.315 J0
Z-.8181 I-.315 J0
Z-.909 I-.315 J0
Z-.9999 I-.315 J0
Z-1.0908 I-.315 J0
X.2534 Y-.1871 Z-1.1 I-.315 J0
X.0332 Y-.2202 Z-1.1114 I-.1267 J.0935
G0 G40 X0 Y0
Z1. M9
G91 G28 Z0
G91 G28 Y0
T1 M6
G103 P1
M98 P9503
G103
M30
%
 
jwracer14 said:
I am trying to thread mill on our 1997 Haas VF2 mill. I have a carbide 5/8-11 hob and I'm trying to mill a 5/8-11 thread 1" deep in 304 SS. The cutter manufacturer recommends 4-5 passes to do this. I have tried every thread milling generator online that I can find. I always get some kind of alarm when I try to run it. The cutter is .470 dia. The hole size is .540. I keep getting tool too big or cutter interference. Can anyone point me in the right direction? Thanks JW
Click to expand...

I guess I should of stated it is an internal R.H. thread and I want to climb mill from bottom up.
 
Shawnrs said:
here is a climb and conventional cut threadmill

M1
N1 (.470-TML-MTS0500C13-11UN)
T1 M6 (CLIMB CUT)
G0 G90 G54 X0 Y0 S3000 M3
G43 Z1. H01 D01 M8
G1 Z-1.1114 F10.
G41 D1 X.1458 Y-.1458
G3 X.2916 Y0 Z-1.1 I0 J.1458
Z-1.0091 I-.2916 J0
Z-.9182 I-.2916 J0
Z-.8273 I-.2916 J0
Z-.7364 I-.2916 J0
Z-.6455 I-.2916 J0
Z-.5546 I-.2916 J0
Z-.4637 I-.2916 J0
Z-.3728 I-.2916 J0
Z-.2819 I-.2916 J0
Z-.191 I-.2916 J0
Z-.1001 I-.2916 J0
Z-.0092 I-.2916 J0
X.2346 Y.1732 Z0 I-.2916 J0
X.0307 Y.2039 Z.0114 I-.1173 J-.0866
G0 G40 X0 Y0
Z1.
Z.2
G1 Z-1.1114
G41 D1 X.1491 Y-.1491
G3 X.2983 Y0 Z-1.1 I0 J.1491
Z-1.0091 I-.2983 J0
Z-.9182 I-.2983 J0
Z-.8273 I-.2983 J0
Z-.7364 I-.2983 J0
Z-.6455 I-.2983 J0
Z-.5546 I-.2983 J0
Z-.4637 I-.2983 J0
Z-.3728 I-.2983 J0
Z-.2819 I-.2983 J0
Z-.191 I-.2983 J0
Z-.1001 I-.2983 J0
Z-.0092 I-.2983 J0
X.24 Y.1772 Z0 I-.2983 J0
X.0314 Y.2086 Z.0114 I-.12 J-.0886
G0 G40 X0 Y0
Z1.
Z.2
G1 Z-1.1114
G41 D1 X.1525 Y-.1525
G3 X.305 Y0 Z-1.1 I0 J.1525
Z-1.0091 I-.305 J0
Z-.9182 I-.305 J0
Z-.8273 I-.305 J0
Z-.7364 I-.305 J0
Z-.6455 I-.305 J0
Z-.5546 I-.305 J0
Z-.4637 I-.305 J0
Z-.3728 I-.305 J0
Z-.2819 I-.305 J0
Z-.191 I-.305 J0
Z-.1001 I-.305 J0
Z-.0092 I-.305 J0
X.2453 Y.1811 Z0 I-.305 J0
X.0321 Y.2132 Z.0114 I-.1227 J-.0906
G0 G40 X0 Y0
Z1.
Z.2
G1 Z-1.1114
G41 D1 X.1575 Y-.1575
G3 X.315 Y0 Z-1.1 I0 J.1575
Z-1.0091 I-.315 J0
Z-.9182 I-.315 J0
Z-.8273 I-.315 J0
Z-.7364 I-.315 J0
Z-.6455 I-.315 J0
Z-.5546 I-.315 J0
Z-.4637 I-.315 J0
Z-.3728 I-.315 J0
Z-.2819 I-.315 J0
Z-.191 I-.315 J0
Z-.1001 I-.315 J0
Z-.0092 I-.315 J0
X.2534 Y.1871 Z0 I-.315 J0
X.0332 Y.2202 Z.0114 I-.1267 J-.0935
G0 G40 X0 Y0
Z1. M9
G0 G91 G28 Z0
M1
N1 (.470-TML-MTS0500C13-11UN)
T1 M6 (CONVENTIONAL CUT)
G0 G90 G54 X0 Y0 S3000 M3
G43 Z1. H01 D01 M8
G1 Z.0114 F10.
G42 D1 X.1458 Y.1458
G2 X.2916 Y0 Z0 I0 J-.1458
Z-.0909 I-.2916 J0
Z-.1818 I-.2916 J0
Z-.2727 I-.2916 J0
Z-.3636 I-.2916 J0
Z-.4545 I-.2916 J0
Z-.5454 I-.2916 J0
Z-.6363 I-.2916 J0
Z-.7272 I-.2916 J0
Z-.8181 I-.2916 J0
Z-.909 I-.2916 J0
Z-.9999 I-.2916 J0
Z-1.0908 I-.2916 J0
X.2346 Y-.1732 Z-1.1 I-.2916 J0
X.0307 Y-.2039 Z-1.1114 I-.1173 J.0866
G0 G40 X0 Y0
Z1.
Z.2
G1 Z.0114
G42 D1 X.1491 Y.1491
G2 X.2983 Y0 Z0 I0 J-.1491
Z-.0909 I-.2983 J0
Z-.1818 I-.2983 J0
Z-.2727 I-.2983 J0
Z-.3636 I-.2983 J0
Z-.4545 I-.2983 J0
Z-.5454 I-.2983 J0
Z-.6363 I-.2983 J0
Z-.7272 I-.2983 J0
Z-.8181 I-.2983 J0
Z-.909 I-.2983 J0
Z-.9999 I-.2983 J0
Z-1.0908 I-.2983 J0
X.24 Y-.1772 Z-1.1 I-.2983 J0
X.0314 Y-.2086 Z-1.1114 I-.12 J.0886
G0 G40 X0 Y0
Z1.
Z.2
G1 Z.0114
G42 D1 X.1525 Y.1525
G2 X.305 Y0 Z0 I0 J-.1525
Z-.0909 I-.305 J0
Z-.1818 I-.305 J0
Z-.2727 I-.305 J0
Z-.3636 I-.305 J0
Z-.4545 I-.305 J0
Z-.5454 I-.305 J0
Z-.6363 I-.305 J0
Z-.7272 I-.305 J0
Z-.8181 I-.305 J0
Z-.909 I-.305 J0
Z-.9999 I-.305 J0
Z-1.0908 I-.305 J0
X.2453 Y-.1811 Z-1.1 I-.305 J0
X.0321 Y-.2132 Z-1.1114 I-.1227 J.0906
G0 G40 X0 Y0
Z1.
Z.2
G1 Z.0114
G42 D1 X.1575 Y.1575
G2 X.315 Y0 Z0 I0 J-.1575
Z-.0909 I-.315 J0
Z-.1818 I-.315 J0
Z-.2727 I-.315 J0
Z-.3636 I-.315 J0
Z-.4545 I-.315 J0
Z-.5454 I-.315 J0
Z-.6363 I-.315 J0
Z-.7272 I-.315 J0
Z-.8181 I-.315 J0
Z-.909 I-.315 J0
Z-.9999 I-.315 J0
Z-1.0908 I-.315 J0
X.2534 Y-.1871 Z-1.1 I-.315 J0
X.0332 Y-.2202 Z-1.1114 I-.1267 J.0935
G0 G40 X0 Y0
Z1. M9
G91 G28 Z0
G91 G28 Y0
T1 M6
G103 P1
M98 P9503
G103
M30
%
Click to expand...

I guess I should of stated it is an internal R.H. thread and I want to climb mill from bottom up. I tried the climb mill code that you posted and I get tool too big alarm. Thanks but it is apparent that I don't have a clue what I'm doing on this.
 
What value do you have in your dia. comp?

Your code is going to have to account for the diameter of your endmill and only use D comp. as adjustment.
If you're trying to comp half the diameter of your tool you'll get an alarm because in that situation your lead-in move needs to be bigger than your comp amount which it isn't.
 
Shawnrs said:
here is a climb and conventional cut threadmill

M1
N1 (.470-TML-MTS0500C13-11UN)
T1 M6 (CLIMB CUT)
Click to expand...

Shawn, thanks for posting that, but the OP just needs a single helix, as he's using a multi-pitch cutter, not single pitch.

I mostly use single pitch cutters, and don't bother with an arc lead in when cutting Al. Just feed down at the center of the hole, linear to pitch diameter (or less if multi-pass), then helix out however many turns. With stainless a curved lead in is probably a good idea. All my thread milling is done to tool centerline, I don't invoke offsets.
 
Booze Daily said:
What value do you have in your dia. comp?

Your code is going to have to account for the diameter of your endmill and only use D comp. as adjustment.
If you're trying to comp half the diameter of your tool you'll get an alarm because in that situation your lead-in move needs to be bigger than your comp amount which it isn't.
Click to expand...

I set the cutter dia. at .470 on the tool offset page
 
Try this:

Set dia. comp at zero.

Code should account for cutter size.

T1 M6
G54 G90 G0 X0 Y0 Sxxx M3
G43 H1 Z.25 M8
G1 Z-1.0 Fx.
G1 G41 D1 X.0775 Fx. (.625 - .470)/2
G3 I-.0775 Z-.909 (code for one turn of thread)
G40 G1 X0
G0 Z.25

Comp value of any more than .0775 will give an alarm. Just use comp to tweak in the size so that it gages correctly.
 
Booze Daily said:
Try this:

Set dia. comp at zero.

Code should account for cutter size.

T1 M6
G54 G90 G0 X0 Y0 Sxxx M3
G43 H1 Z.25 M8
G1 Z-1.0 Fx.
G1 G41 D1 X.0775 Fx. (.625 - .470)/2
G3 I-.0775 Z-.909 (code for one turn of thread)
G40 G1 X0
G0 Z.25

Comp value of any more than .0775 will give an alarm. Just use comp to tweak in the size so that it gages correctly.
Click to expand...

My trick for getting a tool to drop in on center while still using a lead in arc...

radius difference between tool and hole diameter. (.625-.470)/2 then multiply times .414.

Now take that # (.03208) and put it in for lead in line and also the lead in radius.. And
give the lead in arc 135 degrees.

The tool will drop right on center every time.
 
I agree a lead-in arc is the best approach, but I rarely do any big threads.
Would you also helix up in Z on the lead-in arc. In this case 3/8 of a complete arc so 3/8 of a pitch?
 
Booze Daily said:
I agree a lead-in arc is the best approach, but I rarely do any big threads.
Would you also helix up in Z on the lead-in arc. In this case 3/8 of a complete arc so 3/8 of a pitch?
Click to expand...

Yes, it would look something like this





()
()
N1
()
()
G28 G91 Z0
( Tool 1, THREAD MILL)
T01 M06
(OPERATION: 1)
()
( --- 2Dmill_begin --- )
G0 G90 G58 X0.0 Y0.0 M03 S2000
M08
G43 H1 Z0.25
Z-0.3091
Z-0.495
G1 X0.0275 Y-0.025 F2.0
G41 D1 Y-0.05
G3 X0.0775 Y0.0 I0.0 J0.05 Z-0.4803
X-0.0775 I-0.0775 J0.0 Z-0.4349
X0.0775 I0.0775 J0.0 Z-0.3894
X0.0275 Y0.05 I-0.05 J0.0 Z-0.3748
G40 G1 Y0.0265
G0 X0.0 Y0.0
Z0.25
 
The cutter comp on a Haas is the radius of the tool. It’ll need to be G41 for an internal thread bottom to top, and if the cutter dis is 0.470” you’ll need to have the radius set at 0.235” as that is what the G41 D? Will read. Vargas have an excellent calculator which has worked for me everytime, it gives you the tool diameter as reference but the machine reads the rad from the tool offset page.


Sent from my iPhone using Tapatalk
 
I don't think it is possible for someone to give a clear-cut answer without knowing what your cutter comp settings are. 43 and 58 I think?
 
You must log in or register to reply here.

Similar threads

E
Tips/Tools for machining large diameter threads on mill
2
Replies
37
Views
2K
magno_grail
M
WakelessFoil
Milling Thin and Deep Channel on Vertical Mill
2
Replies
32
Views
2K
Paolo_MD
P
I
Making a dovetail fixture for the 5 axis...make it square or rectangular?
2
Replies
24
Views
3K
implmex
I
J
Recreating an interesting hardened part.
Replies
12
Views
1K
john.k
J
S
Threading on Old Mitchell Lathe
Replies
11
Views
813
strokersix
S








 

ABOUT PRACTICAL MACHINIST

With more than 10.6 million unique visitors over the last year, Practical Machinist is the most visited site for metalworking professionals. Practical Machinist is the easiest way to learn new techniques, get answers quickly and discuss common challenges with your peers. Register for the world’s largest manufacturing technology forum for free today to stay in the know.

Learn more about us.

STAY CONNECTED

Facebook Instagram YouTube LinkedIn Pinterest Twitter Tiktok

Register Become a forum member. Register today.

Sign Up Sign up for our e-newsletter.

© 2024 Copyright Practicalmachinist.com. All Rights reserved.

Back
Top