Thread milling

[jimk1960]

I am trying out some thread milling, starting with a 1/4-20 in 6061.

I am using MC 2021 and have the code figured out I think, made the circle for the helix .001 larger than the major diameter and have set the code to use machine wear.

Spindle Speed 3000
Feed 3.2592
Single form 4 flute cutter

The problem I am having is the thread is just too tight.
I have added wear to the tool.
I have changed the drill to a #6.
The thread is still tight.

What am I missing?

Thanks Jim

 

[Booze Daily]

Need to see the code.

 

[Mtndew]

I am trying out some thread milling, starting with a 1/4-20 in 6061.

I am using MC 2021 and have the code figured out I think, made the circle for the helix .001 larger than the major diameter and have set the code to use machine wear.

Spindle Speed 3000
Feed 3.2592
Single form 4 flute cutter

The problem I am having is the thread is just too tight.
I have added wear to the tool.
I have changed the drill to a #6.
The thread is still tight.

What am I missing?

Thanks Jim

Add more wear to make the thread larger.
You have to account for things like tool pressure,tool diameter, point of the tool in relation to pitch diameter, etc...
I've never programmed a thread mill path where I didn't have to adjust the wear to make it on size.

 

[Larry Dickman]

I always wondered about this, so one day I took some time and worked it out.

So, your using .251 as your diameter of the hole, and you're using the actual diameter of the tool as the tool diameter.
That would seem logical, but what do these two diameters have to do with your pitch diameter? Absolutely nothing. (well, not really, but close to nothing)

It was my observation that I always had to comp the tool -.008/ -.012 If you were to draw this out and look at where your pitch dia is relative to your major diameter, then look at exactly where your tool profile is intersecting the pitch diameter, you will find it is off around .004 /side. So the diameter would be off .008, which is what it is.

 

[Mtndew]

I always wondered about this, so one day I took some time and worked it out.

So, your using .251 as your diameter of the hole, and you're using the actual diameter of the tool as the tool diameter.
That would seem logical, but what do these two diameters have to do with your pitch diameter? Absolutely nothing. (well, not really, but close to nothing)

It was my observation that I always had to comp the tool -.008/ -.012 If you were to draw this out and look at where your pitch dia is relative to your major diameter, then look at exactly where your tool profile is intersecting the pitch diameter, you will find it is off around .004 /side. So the diameter would be off .008, which is what it is.

Yep. One of the things I try to teach new employees is that in this trade, it almost never works out like it does on paper. Too many intangibles to take into account.

 

[TeachMePlease]

Your threadmill doesn't come to a perfectly sharp point, either, so you've gotta comp for that. Same as having to comp diameter after touching off a chamfer mill, to account for the flat on the tip.

 

[ChipSplitter]

It's like threading in a lathe, I've always had to go a bit deeper than calculated thread depth.

Threadmilling works great for nasty materials and weird threads.

But why are you using it for a 1/4-20 thread in aluminum?

I'd tap that........(sorry, cliche )

 

[GENERALDISARRAY]

did CNC software actually fix something? When did geometry besides a point work for threadmilling?

 

[jimk1960]

All, thanks for the thoughts.
Went to -.006 in comp and it worked great.
I figured it just needed more comp but was second guessing myself.
I did alum in hopes of not breaking my nice new shiny expensive tool, yes I also normally use a tap for alum.

 

[Bobw]

All, thanks for the thoughts.
Went to -.006 in comp and it worked great.
I figured it just needed more comp but was second guessing myself.
I did alum in hopes of not breaking my nice new shiny expensive tool, yes I also normally use a tap for alum.

Years ago, I had a guy working for me. And he was good, he was careful. He was setting up something one day that needed a tap, and I had a meeting to go to. I figured he would be pretty much done with the job when I got back. I get back and there is no parts done. None.

Turns out he wanted to double check the tap (I don't remember the size, maybe 3/4), like you do when you pull a drill out of a drill drawer. All the taps of that size where too big and he didn't want to scrap the job. Like .008 too big...

I think it was the first time he had ever measured the OD of a tap.

 

[litlerob1]

It's my assumption (yes Ox, I am). I've never taken the time to really compare the Angularity. But it seems that it's almost always that much comp. because of the actual 3D Helix. Meaning the "pitch line" is not Perpendicular to the Face of, or Parallel to the Body of the Thread. The Thread data that you find in MH is 2D (theoretical), the actual pitch line is (math, math, pythegoria, math) several degrees off of Parallel from the Body of the Thread.

R

 

[ChipSplitter]

>>>OP, you still haven't 'splained why you're threadmilling this hole.

Just for fun..??