What's new
What's new

Thread Mill Programming By Hand

MillGuy88

Aluminum
Joined
Mar 13, 2024
Location
Saskatoon
I only use a thread mill for holes with a minor dia. larger than 1". I use a Kennametal indexable thread mill which is like a single point tool but with multiple flutes.

100031871.jpg

For ease of programming, I feed down to the bottom of the hole, arc into my cutting radius from the center of the hole without a Z-axis movement and then helix out of the hole. I like this method because I can use a simple macro for various threads and the thread at the bottom of the hole looks great

Kennametal provides an example that has a Z-axis movement while arcing into the cut, which I could see if I was using a tool with a cutting edge for a specific pitch to maintain the thread form. It also uses cutter comp. I've written a macro using the Kennametal example except I don't use cutter comp (G41), the toolpath is compensated in the macro itself. I haven't tested it out yet.

Screenshot (1).png

Is it absolutely necessary to move the z axis while arcing into cut while using a cutter that matches the pitch? The less the radius arcing into the cut, the less likely it will essentially cross thread or split the thread without using Z-axis movement. Does any one have experience with this?
 
Is it absolutely necessary to move the z axis while arcing into cut while using a cutter that matches the pitch?
It will make a little arc at the bottom that is not at the helix of the thread but so what ? If the bolt bottoms out on the thread the bolt will stop there anyhow and if the bolt doesn't reach the bottom of the thread it will never touch the unhelical arc, so .... can't see that it will make any difference at all.
 
I once milled a 2 3/4-12 thread in a part for a tensile tester load cell. I didn't even bother with the arc leading in just went straight to the diameter and then repeated an incremental subroutine to finish the threads. Using a HSS toolbit on a boring bar, things were pretty slow. I recall going for coffee while it finished.

But pretty much the same thing as you described here just didn't worry about the bottom thread and helix angle.
 
Add math to your macro.
N10 Hole D - Cutter D = Tool path D.
N20 Tool path D X Pi = tool path circumference.
N30 Tool path circumference/ Pitch height (ARC TAN) = cutting angle.
Approach via the center.
N40 Take tool path D/2 for approach Arc D.
N50 Approach arc D X Pi /2 (since its a half arc) for approach arc distance.
N60 Approach arc Distance X Cutting angle (SIN) for approach Z move.
Do one pass and arc back out with previously figured out Z move value

I think I've got all that right. I've never done it as a macro but once did it as a straight approach and escape for external threads. only had one or 2 pitches to do and didn't know macros at the time but it made good parts.
 
Last edited:
This is the macro I wrote but have not tested and proven based on the Kennametal Example. It's a TOSNUC 999 controller so it uses variables a little differently. I was thinking of adding some if statement alarm checks to ensure there are no crashes if the inputs are wrong.

The numbers seem to work in a spread sheet.

[VN=1.5] (THREAD NOMINAL DIA.)
[VM=1.375] (THREAD MINOR DIA.)
[VP=.125] (PITCH)
[VL=2.000] (LENGTH OF THREAD)
[VD=1.000] (TOOL DIA.)
[VG=.003] (FEED PER TOOTH)
[VT=3] (# OF TEETH)
[VW=.21] (TIP OF TOOL TO THREAD ROOT DISTANCE)
[VC=.02] (MINOR DIA. CLEARANCE AMOUNT)
[VA=90.] (ENTRY ANGLE/ALFA ANGLE)

( *** DO NOT ALTER *** )
[VI=[V1403-V[2500+[V1102]]]] (CURRENT Z AXIS COORDINATE, "I" POINT)

[VH=[[[[VN/2]-VC]*[[VN/2]-VC]]+[VM*VM]]/[VM*2]] (RADIUS OF TANGENTIAL ARC/HYPOTENUSE)
[VB=VA+ATAN[[[VN/2]-VH]/[SQRT[[VH*VH]-[[[VN/2]-VH]*[[VN/2]-VH]]]]]] (BETA ANGLE)

[VK=VP*[VB/360]] (Z-AXIS MOVEMENT DURING ENTRY APPROACH)
[VX=COS[VB]*[[[VM-VD]/2]-VC]] (X-AXIS POSITION AT START OF ENTRY APPROACH)
[VY=-SIN[VB]*[[[VM-VD]/2]-VC]] (Y-AXIS POSITION AT START OF ENTRY APPROACH)
[VZ=-VL-VW-VK] (Z-AXIS POSITION AT START OF ENTRY APPROACH)
[VE=VG*VT*V1111] (FEED RATE AT CUTTING EDGE)
[VF=VE*[[VM-VD]/VM]] (FEED RATE AT TOOL CENTRE LINE)

G90 G0 Z[VC]
G90 G1 Z[VZ] F[VE] (FEED INTO HOLE)
G91 G1 X[VX] Y[VY] F[VE] (FEED TO CUTTING START POINT)
G91 G3 X[[VN-VD]/2]-VX] Y-[VY] Z[VK] R[VH-[VD/2]] F[VF] (ARC INTO CUTTING RADIUS)
G91 G3 I-[[VN-VD]/2] K[VP] L[FRUP[[VL+VW]/VP] (HELIX OUT OF HOLE)
G91 G1 X-[[VN-VD]/2] (FEED BACK TO CENTRE OF HOLE)
G90 G0 Z[VI]
(END OF MACRO)
 
Last edited:
Then why the hell did you show an entirely different tool in the first place ? Are you just trying to be annoying ? Because you've succeeded.
You must be a real treat to work with.

I showed a picture of the current tool I'm using as originally stated because I assume when most people think of a thread mill, they imagine one like the solid one that can only be used for a specific pitch.
 
The question is why a Z move on the arc in?
If you were going to try to continue the helix in a runout fashion like on a lathe, then you'd need to do that because otherwise it's just an arc at right angles to the axis of the hole, followed by a helix the rest of the way out.

But since it doesn't matter - with the single-point tool originally posted - it isn't worth the hassle to figure it out.
 
If you were going to try to continue the helix in a runout fashion like on a lathe, then you'd need to do that because otherwise it's just an arc at right angles to the axis of the hole, followed by a helix the rest of the way out.

But since it doesn't matter - with the single-point tool originally posted - it isn't worth the hassle to figure it out.
He updated it in post #4 .
Any difference?
 
He updated it in post #4 .
He didn't "update", he changed. That's like asking about carrying three tons of gravel in a dump truck, then showing an Austin-Healey Sprite.

Any difference?

Of course there is. With a single point tool, you arc in at the bottom which doesn't count, then helix up the hole. With a thread mill, there's teeth all the way up so you will have an arc at right angles to the hole all the way up to the top, followed by the helix. Except the initial arc will not be helical, it'll dig right in to areas you don't want to cut.

Whether it makes a huge difference will matter on the thread size and the helix angle, but still. Not at all the same thing.

If you ask a question about a bridgeport, then you can't just switch to a hydrotel and pretend it doesn't make any difference.
 
He updated it in post #4 .

He didn't "update", he changed.

From my original post.
Is it absolutely necessary to move the z axis while arcing into cut while using a cutter that matches the pitch?
Sorry if the first picture confused you.

It was there to help explain how it works using my current method with my current tooling, for those who might not be familiar with that style of thread mill. I should have added the picture of the solid tool in the first post as well to avoid the confusion.
 
Last edited:
I only use a thread mill for holes with a minor dia. larger than 1". I use a Kennametal indexable thread mill which is like a single point tool but with multiple flutes.

View attachment 437494

For ease of programming, I feed down to the bottom of the hole, arc into my cutting radius from the center of the hole without a Z-axis movement and then helix out of the hole. I like this method because I can use a simple macro for various threads and the thread at the bottom of the hole looks great

Kennametal provides an example that has a Z-axis movement while arcing into the cut, which I could see if I was using a tool with a cutting edge for a specific pitch to maintain the thread form. It also uses cutter comp. I've written a macro using the Kennametal example except I don't use cutter comp (G41), the toolpath is compensated in the macro itself. I haven't tested it out yet.

View attachment 437495

Is it absolutely necessary to move the z axis while arcing into cut while using a cutter that matches the pitch? The less the radius arcing into the cut, the less likely it will essentially cross thread or split the thread without using Z-axis movement. Does any one have experience with this?
I was doing 10-32 thread mill holes..
Fast as a cat. And perfect.
Do not be scared of blowing up a couple thread mills, if you are trying to get the work out and make a profit, you have to go for it.
 








 
Back
Top