Thread Mills

[robk]

Are you sure that you minor Ø is correct? Are you hitting bottom if hole is blind?  I don't know what your code looks like but below is what my threadmilling spread sheet gave me for results. I selected Lakeshore Carbide threadmill #L1/4-20THRDZ  Ø.180 for cutter dia. and .254 thread depth using 350sfm @ .0007 ipt . I don't use mastercam so my NX setting would be useless for you. Attached is a spread sheet for thread milling to help you out.

BTW, I have never used that brand of threadmills so I can't vouch for them.

 

ONEPASSINCREMENTALPROGRAM

S7427 M03

G91 X0 Y0 Z0

G01 Z-0.2853 F25.

G41 X0.0175 Y-0.0175 F10.92

G03 X0.0175 Y0.0175 Z0.0063 I0 J0.0175 F4.37

G03 X0 Y0 Z0.0500 I-0.0350 J0

G03 X-0.0175 Y0.0175 Z0.0063 I-0.0175 J0 F6.55

G01 G40 X-0.0175 Y-0.0175 F50.

G00 Z0.2228

ONEPASSCYCLETIME :3.02SECs

 

 

TWOPASSINCREMENTALPROGRAM

S7427 M03

G91 X0 Y0 Z0

G01 Z-0.2853 F25.

G41 X0.0134 Y-0.0134 F10.92

G03 X0.0134 Y0.0134 Z0.0063 I0 J0.0134 F3.35

G03 X0 Y0 Z0.0500 I-0.0268 J0

G03 X-0.0134 Y0.0134 Z0.0063 I-0.0134 J0 F5.03

G01 G40 X-0.0134 Y-0.0134 F25.

G01 Z-0.0625

G41 X0.0175 Y-0.0175

G03 X0.0175 Y0.0175 Z0.0063 I0 J0.0175 F4.37

G03 X0 Y0 Z0.0500 I-0.0350 J0

G03 X-0.0175 Y0.0175 Z0.0063 I-0.0175 J0 F6.55

G01 G40 X-0.0175 Y-0.0175 F50.

G00 Z0.2228

TWOPASSCYCLETIME :6.04SECs

 

 

THREEPASSINCREMENTALPROGRAM

S7427 M03

G91 X0 Y0 Z0

G01 Z-0.2853 F50.

G41 X0.0134 Y-0.0134 F10.92

G03 X0.0134 Y0.0134 Z0.0063 I0 J0.0134 F3.35

G03 X0 Y0 Z0.0500 I-0.0269 J0

G03 X-0.0134 Y0.0134 Z0.0063 I-0.0134 J0 F5.03

G01 G40 X-0.0134 Y-0.0134 F25.

G01 Z-0.0625

G41 X0.0161 Y-0.0161

G03 X0.0161 Y0.0161 Z0.0063 I0 J0.0161 F4.03

G03 X0 Y0 Z0.0500 I-0.0323 J0

G03 X-0.0161 Y0.0161 Z0.0063 I-0.0161 J0 F6.04

G01 G40 X-0.0161 Y-0.0161 F25.

G01 Z-0.0625

G41 X0.0175 Y-0.0175

G03 X0.0175 Y0.0175 Z0.0063 I0 J0.0175 F4.37

G03 X0 Y0 Z0.0500 I-0.0350 J0

G03 X-0.0175 Y0.0175 Z0.0063 I-0.0175 J0 F6.55

G01 G40 X-0.0175 Y-0.0175 F50.

G00 Z0.2228

THREEPASSCYCLETIME :9.06SECs

[The Cathedral]

1) check your speeds and feeds. Are you internal or external milling? If you're internal, you have to slow the feed, external you should actually speed it up. Remember the feeds the manufacturer gives is for linear movements; you have to calculate the actual feedrate using the formula  (Hole dia - tool dia) / Hole dia for internal and (Hole dia + tool dia) / Hole dia for external. Multiply your linear feed rate by the value you get for your actual feedrate

 

2) Rigidity rigidity rigidity. Sounds like you have that done with a new tool holder

 

3) Runout

 

4) Deflection. Rigidity and stickout affect this, but so does the shape of your flutes. I personally never order or use straight-flute endmills because with a straigh flute you have the entire length of cut in the cut at the same time which causes deflection, especially on smaller diameter mills.

 

5) Your program seems way, way wrong. It looks like you're doing an internal thread since you start and end at X0 Y0; the minor diameter of a 1/4-20 is .201" so having your tool move a radius of .1185" means you're plowing the whole tool way past where it's supposed to go. If your tool has a cutting diameter of .170, the biggest I/J you should see in the cut is .04" Your numbers should look more like what ^^^^^ posted.

[robk]

It seems that I can't attach an excel file.

Send me your email address and I will send an excel threadmill spreadsheet.

It's always good to have a backup plan.

[specv]

I also noticed that the code looks wrong but thought he may have been using control comp instead of wear comp.

[The Cathedral]

I also noticed that the code looks wrong but thought he may have been using control comp instead of wear comp.

Good point. Didn't think of that.

[SpecialtyTool]

I am using control comp. I've got my feeds down pretty low. Ramping in at 2 IPM then cutting at 3 IPM. I think the program should work. We did a test in aluminum that worked fairly well and left a proper thread but steel is totally different. I think a better tool holder would really help especially considering the spindle its in has seen its better days. I haven't had a chance to check the runout yet.  Thanks for all the help.