Thread Milling question

[within a thou]

Good afternoon I would like to ask you guys for your advise. I would like to thread mill a 75mm x 1.5 pitch holes on a mill but not sure what I need in terms of cutters (preferably indexible for cutter comp reasons) type of cycle so I can synch in case I need to recut and also speeds and feeds. Any and all suggestins are greatly appreciated and thank you in advance.

[Jrygus]

I use contour ramp on an full arc and set depth to pitch distance. Then use wear offset. Allows you to adjust and run again. I really do not do much thread milling so i am sure others will have more info for you.

[Guest]

resync???

 

If you take it out of the machine it's done.

 

If you need to go back and and recut because it is undersize, threadmill handles this issue it will also allow you to take multiple passes if you need.

 

Speeds and feeds are generally set quite similar to if you were actually milling the part

[David Colin]

It depends if you have many holes to machine... If just a few, i would go with a turning threading tool with 1 insert, then thread milling cycle.

[Tinny]

I would threadmill it with wear comp, its ultimately more controlable than anything else. The Mastercam threadmill toolpath makes it simple.

[Mr. Wizzard]

I first create the tool. Typically, i use Carmex solid carbide thread mills. For example, on an M80 x 3mm internal thread, I bought a MT0625C16 3.0 ISO Carmex thread mill. It has a 3.0mm pitch and will make anything over a 25mm diameter. I usually create a dove mill with a 45 degree taper on the bottom. For this tool, the diameter is straight from the book. The flute length is the standard equivalent of the metric thread pitch. 3.0mm / 25.4 = .1181.

Then, I create a point at the center of the hole and use the thread mill toolpath. From there, you just fill in the blanks. I also convert the thread pitch in the toolpath box to standard.

If you use 1 for active teeth, you should get a pretty accurate picture of the thread when you verify it.

[gcode]

quote:

---

I create a point at the center of the hole and use the thread mill toolpath

---

You can also drive a thread mill toolpath

by selecting an arc..For ID threads draw the

arc at the major diameter. That's one less data

field to fill out in the toolpath paramters and once less chance of a mistake.

[Don M]

I use thread mills for this.

As JP says, if you remove it from the machine your sunk.

As for resynching, that would only matter if your tool broke (like when your threading very hard material).

To account for that, I use the tool presetter to pick up the sharp v of the last tooth on the thread mill.

If my length offset comes from a known spot like that, I can always replace my tool by picking up from the same spot, and I can re-machine the thread with the new tool.

I hope this helps.

[htm01]

quote:

---

As JP says, if you remove it from the machine your sunk.

---

i think he said your "done" not sunk.you should be able to put it back in machine and run aqain all day long

[Don M]

quote:

---

i think he said your "don" not sunk.you should be able to put it back in machine and run aqain all day long

---

Fair enough.

I suppose there could be instances where you could re-load the piece.

[crazy^millman]

Tom one problem with that method of using points. On older machines they do not comp very nicely so you have to use a point so that you do get the box. Then let the guy cut the threads then you can adjust it where as by using the arc you have to adjust the size of the circle and if a solid was tired to that circle now it creates all types of problems.

 

Just something to think about I like using circle on machines where I know it is not a problem.

 

HTH

[gcode]

quote:

---

if a solid was tied to that circle

---

my solids are always dumb imports from SolidWorks.

Points are a pet peeve of mine. I don't use them for anything but defining the origins of WSC's

and toolplanes..

I drive all drill and circlemill toolpaths with arcs. To me it makes for a less cluttered file

that is easier to understand when you have to make an edit a year later.

I really like driving drill toolpaths with arcs

because you can mass select them by hole size

using the diameter filter.

Arcs are good for circlemill and helix bore

because the size of the arc drives the toolpath.

You can machine multiple hole sizes with the same toolpath when you drive them with arcs.. you can't do that with points