Thread milling help

[dgriffiths]

I am programming my first thread milling operation in Mastercam and was looking for some advicehelp. My first question is should I draw up a custom cutter profile that matches my thread mill? Next, I am thread milling an internal thread 1/2"-13 about 3/4" deep in aluminum. Should I mill bottom up or top down and what kind of chip load would be appropriate for a 4 flute thread mill. Any suggestions or tips would be great.

[kenfromlodi]

no need to draw custom tool unless you would like it to look correct. define as endmill and use your thread tool diameter.

cut from bottom up.

machine hole to minor diameter, make sure that you pick the geometry of the major diameter when picking the chain point,

I always tell it 1 flute and let it do one rough and one finish or spring pass and the chip load is fine for alum. harder materials take a couple passes.

 

hope that helps a little

[dgriffiths]

Thanks Ken. I just did a search of the forum and found a ton of info on thread milling as well. Thanks again. I will give it a try.

[Randy Morton @ Clem Industrial]

Dg, what brand of threadmill you using? Not to smash mastercams threadmilling, but companys like Seco or Iscar have incredible threadmilling wizards geared right for their tooling. We use the seco one for all our seco threadmills and they are always perfect code output, speed, feed and all. =]

 

JM2C

[dgriffiths]

Randy, we are using Scientific Cutting Tools. However I will check our the others as well. We are really just beginning to utilize thread milling on our 5 axis machine and potentially will be doing some thread milling on titanium in the near future. So right now I am open to try anything that others have had success with. I will be running some aluminum parts first and it provided an opportunity to prove out my thread mill code. Thanks for the info.

[Jerosu]

look for "X MR2 SCT Threadmill Assortment.zip" on the ftp for profiles of Scientific Cutting Tools threadmills. I don't know who put it up, but it is great to have.

[Zbuilder]

Thread milling in X2 MR2 doesn't work for me. It always does half of the hole, never a 360° G2 or G3 rotation, except when Linearize Helix is checked. But this is useless for use.

 

Anyone else get this?

[Storkman]

MR2 seems to work fine here. I just did one quick and posted it.

 

 

N1M06T8

G00G17G90G54X-.6642Y1.9254S2150M03

G43H8Z.25

M08

Z.1

G01Z-.5F100.

G41D8X-.7094F1.5

G03X-.6189R.0452

X-.7999Z-.4616I-.0905J0.

X-.6189Z-.4231I.0905J0.

X-.7999Z-.3846I-.0905J0.

X-.7094R.0452

G01X-.7547

X-.7094

G00Z.1

Z.25

M09

G40

G91G28Z0M19

G28Y0

G90

M30

[Tim Johnson]

Works for me too...

 

code:

---

O4263

(ADVENT THREAD MILL 716-TA-05 WITH 20 PITCH INSERT RIGHT SIDE)

IF[#151EQ#0]GOTO1

N18340 G00 G90 X.375 Y-2.625 (B270.) G59

N18350 G43 H48 Z1.495 S13000 M[#933]

N18360 Z1.345

N18370 G01 Z.815 F100.

N18380 G41 D148 Y-2.665 F19.5

N18390 G03 X.45 Y-2.625 Z.8275 I.0268 J.04

N18400 Z.8775 I-.075 J0.

N18410 X.375 Y-2.585 Z.89 I-.0482 J0.

N18420 G01 G40 Y-2.625

N18430 G00 Z1.495

N18440 Z9.25

N1 M99

---

[Henk]

I define them as an tap and name them as mill.

Now i can put the pitch in the parameters, and assign the to the Threadmill cycle in our heidenhain programs.