Help with threading

[protrxrptr17]

I need to cut some 2"- 4.5 TPI thread on 1018, 6.5 inches long. I'll be using a high speed tool for the first one and when the brown truck comes I'll be using an insertable carbide tool. I have a Fanuc 6-T control. What G-code should I use? An example would be great. The manual says G92 is the canned cycle for threading, but I can't understand how to write it. I could use G28, but that would take forever to write. What RPM and depth per pass should I use for each tool? I have only cut threads with a manual lathe. What infeed angle will this machine use? Thanks for any help or suggestions.

[tobyaxis]

Originally Posted by protrxrptr17 I need to cut some 2"- 4.5 TPI thread on 1018, 6.5 inches long. I'll be using a high speed tool for the first one and when the brown truck comes I'll be using an insertable carbide tool. I have a Fanuc 6-T control. What G-code should I use? An example would be great. The manual says G92 is the canned cycle for threading, but I can't understand how to write it. I could use G28, but that would take forever to write. What RPM and depth per pass should I use for each tool? I have only cut threads with a manual lathe. What infeed angle will this machine use? Thanks for any help or suggestions.

G92 is a good Canned Cycle but you may want to use G76 instead.

G28 is a Home Position Return example home X and Z
G28U0W0


G92 goes like this. It is a little long because the Material was Inconel X750

G0G40G80G97G99M5
G28U0W0M9
G50S2000M41
M1

N1(THD .5 20 UNJF-3A KENNAMETAL)
T0707 S1000 M13
G0 X.75 Z.08
X.62
G92 X.496 W.22 F.05
X.49
X.484
X.479
X.474
X.469
X.464
X.46
X.456
X.452
X.449
X.447
X.445
X.443
X.442
X.441
X.44
X.4395
X.4395
X.439
X.439
G0 X.52 Z-.0167 S2500
G1 U-.12 W.06 F.0008

G0G40G97Z.1M9
G28U0W0T0700
M1
----------------------------------------------------

G76
X= the minor diameter of the thread
Z= the length of the thread plus deceleration distance
I= taper from start to end radially {Tapered NTP Threads}
K= depth of the thread = D major - D minor / 2] D [depth of the cut on the first pass
F(E)= the thread lead {F has 4 place decimal programming}{E has 6 place decimal programming} EX. F.0001 E.000001
A [the angle of the thread normally 30,55, or 60 degrees]

G00 will cancel both G76 and G92 Threading Cycles.

Here is a good rule of thumb. Take the same Depth of Cut with your CNC that wou would on an Engine Lathe. That is a Nasty Large Thread that you have to cut in 1018. Speeds are going to be relative to the Setup Rigidity. The Feed will be the Thread Lead so that can't be changed. The Lead on that thread is F.2222
I would use E.222222


1018 CR is gummy and tears. It is difficult to get a good finish without using Cermet Inserts like Seco Carboloy FF1's

[protrxrptr17]

Thanks for the example. What about infeed angle? I don't remember what inserts I ordered, but I think it required a 29 degree infeed angle. On my old manual I took about .020 at first and then backed it down as I got deeper. What RPM sounds right for that? The bar is 40" long and it's just going to be chucked.

[protrxrptr17]

Can you suggest a better material for this? They are essentially just big bolts. 6.5 inches of thread on one end and just enought to thread anut on the other. Then I weld the nut on the short end. I make 2 about every 3 months for a local lumbermill. They break them somehow?? I don't really want to make them any stronger because I want to keep making them. They specified 1018 the first time I made them. I guess they are kind of like shear bolts. Maybe something easier to thread but with the same strength.

[tobyaxis]

The infeed angle is set by the G76 Canned Cycle it is a little difficult to explain without a drawing.

I'll post an example Picture for you.

RPM I'd start at 300 to 600 RPM and use G97S300M3. G97 is Constant Surface Footage Cancel. You don't want your RPM going up when threading or drilling for that matter.

In this picture the first depth of cut is RED and the Rest are Green.

[protrxrptr17]

Originally Posted by tobyaxis The infeed angle is set by the G76 Canned Cycle it is a little difficult to explain without a drawing. I'll post an example Picture for you. RPM I'd start at 300 to 600 RPM and use G97S300M3. G97 is Constant Surface Footage Cancel. You don't want your RPM going up when threading or drilling for that matter. In this picture the first depth of cut is RED and the Rest are Green.

I should have been a little more specific. Is the infeed angle automatically instated? If so, how can I know what it is? I sure appreciate your help. This forum and it's people a a very valuable tool for me.

[tobyaxis]

Originally Posted by protrxrptr17 Can you suggest a better material for this? They are essentially just big bolts. 6.5 inches of thread on one end and just enought to thread anut on the other. Then I weld the nut on the short end. I make 2 about every 3 months for a local lumbermill. They break them somehow?? I don't really want to make them any stronger because I want to keep making them. They specified 1018 the first time I made them. I guess they are kind of like shear bolts. Maybe something easier to thread but with the same strength.

1018 Cold Rolled is pretty damn strong. Keep making them LOL. It pays the bills. They want 1018, they get 1018. Pray that your customer doesn't ask for 17-4ph Stainless Heat Treated 45Rc. Or worse yet 13-3ph Stainless.

[tobyaxis]

Originally Posted by tobyaxis G92 is a good Canned Cycle but you may want to use G76 instead. G28 is a Home Position Return example home X and Z G28U0W0 G92 goes like this. It is a little long because the Material was Inconel X750 G0G40G80G97G99M5 G28U0W0M9 G50S2000M41 M1 N1(THD .5 20 UNJF-3A KENNAMETAL) T0707 S1000 M13 G0 X.75 Z.08 X.62 G92 X.496 W.22 F.05 X.49 X.484 X.479 X.474 X.469 X.464 X.46 X.456 X.452 X.449 X.447 X.445 X.443 X.442 X.441 X.44 X.4395 X.4395 X.439 X.439 G0 X.52 Z-.0167 S2500 G1 U-.12 W.06 F.0008 G0G40G97Z.1M9 G28U0W0T0700 M1 ---------------------------------------------------- G76 X= the minor diameter of the thread Z= the length of the thread plus deceleration distance I= taper from start to end radially {Tapered NTP Threads} K= depth of the thread = D major - D minor / 2] D [depth of the cut on the first pass F(E)= the thread lead {F has 4 place decimal programming}{E has 6 place decimal programming} EX. F.0001 E.000001 A [the angle of the thread normally 30,55, or 60 degrees] G00 will cancel both G76 and G92 Threading Cycles. Here is a good rule of thumb. Take the same Depth of Cut with your CNC that wou would on an Engine Lathe. That is a Nasty Large Thread that you have to cut in 1018. Speeds are going to be relative to the Setup Rigidity. The Feed will be the Thread Lead so that can't be changed. The Lead on that thread is F.2222 I would use E.222222 1018 CR is gummy and tears. It is difficult to get a good finish without using Cermet Inserts like Seco Carboloy FF1's

Originally Posted by protrxrptr17 I should have been a little more specific. Is the infeed angle automatically instated? If so, how can I know what it is? I sure appreciate your help. This forum and it's people a a very valuable tool for me.

A is the angle 30,55,60 degrees
K is the first Depth of Cut

G76X1.8528Z-6.0K.0721A60E.222222

The in Feed as you call it I don't think matters. A is the Included Angle of the Thread 60 Degrees

[Hursty]

A 2" x 4.5 tpi needs about 25 passes to produce. If using only the G92 cycle then the depths would be 0.016, 0.012, 0.011, 0.009, 0.007, 0.006x2, 0.005x3, 0.004x7, 0.003x7 & 0.002. I would use both cycles first a G92 then the G76 something like this.
G92 X1.968 Z#### F(E)0.222
G76 X1.732 Z#### K0.134 D28 F(E)0.222 - D = Total depth 1st +2nd depth

The G76 cycle will take 23 passes plus 1 for the G92 = 24 passes. If you try the G76 ONLY with this depth of cut there is a good chance the tool will break hence the first pass with G92.

[protrxrptr17]

Well, it didn't go to well for me today. I kept on chipping inserts. I tried 175 RPM all the wat to 600 RPM. Chatter was also a problem. I used a Kennametal NSR-164D and Interstate ITN-52004J inserts. I even tried going only .002" per pass and then dropping to .001" as it got deeper. That is with diameter programming, so it's really half that. I think it has something to do with the infeed angle because the chatter marks were on both sides of the thread. I think the tool was feeding straight in. I used G92. I never tried G76.

[protrxrptr17]

Toby, after carefully studying your post again, I see what you were trying to tell me. I will try G76 and see if that works. Is there a parameter to change the angle on G90? It would be just like changing the angle on the compound slide on a manual machine.

[tobyaxis]

Originally Posted by protrxrptr17 Toby, after carefully studying your post again, I see what you were trying to tell me. I will try G76 and see if that works. Is there a parameter to change the angle on G90? It would be just like changing the angle on the compound slide on a manual machine.

One thing you have to get used to on CNC's, there is no Compound and no way to Change the Infeed Angle.

Select a C7 Grade of Carbide Insert. It is Tougher than C2. C2 will chip very easily. Call Kennametal on the phone and tell them what your cutting. They will be able to select a Carbide Grade that will suite your needs.

BTW: You maybe better off using G92 because it allows you to Taylor Each Depth of Cut you make. Use Cutting Oil to. If you were getting Chatter your RPM was too High or the Tool had too much surface contact. 2 thousanths Depth Cuts should do the trick combined with a Lower RPM. BTW put the Spindle in Low Gear Too.