Manual Threadmilling Programing: Cutting helical feeding UP or DOWN?

I don't have a tap for a missing part I am trying to make a replacement for that I intend to thread mill the internal threads for.

When manually programing thread milling, what is the proper or typical method for cutting? Do you go down the center of the hole and thread from the bottom up or do you thread mill down? And why?

I guess it has to do with chip evacuation and whether it becomes conventional or climb milling by the thread mill cutter. Also whether its right or left handed threads. But traditionally, looking at various literature and animation, thread milling right handed internal threads is typically done by plunging the cutter into the drilled hole with a rapid, and then at the bottom of the hole feeding the cutter to the cutting diameter, and then helical interpolate UP. Why is that?

The other method will be the more logical method to the uninitiated, which is to simply cut down into the hole every time no matter what. I suppose both method can work but is there a reason one is better than the other? Or is it always strictly a case of conventional vs climb milling? If so which one is best?

Chip evacuation in a blind hole is one reason. As the chips accumulate, it's better to have the mill recede from the depths rather than meet them head-on. My personal preference is to avoid a G00 to the bottom of the hole when you start. Better to rapid to centre and feed to the bottom.

You mention "more logical to the uninitated..." with respect to having the thread mill cut from the top down. I don't understand this comment. The only reason that this would be proper to an amateur observer would be that most every other rotational cutting tool tends to gradually disappear into the work (boring heads, taps, drills et al). Thread milling uses an entirely different method of action. You're gradually getting to thread depth by increasing the diameter of circular interpolation. Whether this occurs at the top of the hole or bottom, the thread mill doesn't care. It's still plunging by increasing the cut diameter, not by advancing in Z.

However, you're better off to have the entire insert taking a cut along the full width to avoid deflection of just the tip. Full engagement will allow this, but requires starting where there is enough hole depth to do so. Also, top requires one tooth of engagement, then the next, then the next until you've covered the entire insert. Just as you mentioned climb milling, which creates a large chip load that decreases as the flute advances, thread milling from the bottom up typically allows the insert to do the same axially rather than radially. Loading decreases as the mill advances in Z+.

I would never conventional mill with a carbide thread mill.

Feeding down means you have to go around as many pitches as you have in your thread . . . i.e. 1/4-20 x 0.4 deep = 8 times around. Feeding up means only one circle is needed . . . from Z-.4 to Z-.35

RC Mech said:

Chip evacuation in a blind hole is one reason. As the chips accumulate, it's better to have the mill recede from the depths rather than meet them head-on. My personal preference is to avoid a G00 to the bottom of the hole when you start. Better to rapid to centre and feed to the bottom.

You mention "more logical to the uninitated..." with respect to having the thread mill cut from the top down. I don't understand this comment. The only reason that this would be proper to an amateur observer would be that most every other rotational cutting tool tends to gradually disappear into the work (boring heads, taps, drills et al). Thread milling uses an entirely different method of action. You're gradually getting to thread depth by increasing the diameter of circular interpolation. Whether this occurs at the top of the hole or bottom, the thread mill doesn't care. It's still plunging by increasing the cut diameter, not by advancing in Z.

However, you're better off to have the entire insert taking a cut along the full width to avoid deflection of just the tip. Full engagement will allow this, but requires starting where there is enough hole depth to do so. Just as you mentioned climb milling, which creates a large chip load that decreases as the flute advances, thread milling from the bottom up typically allows the insert to do the same axially rather than radially. Loading decreases as the mill advances in Z+.

I would never conventional mill with a carbide thread mill.

Click to expand...

Yeah I figure maybe chip evacuation is one. I've seen seco documents where they show some animations doing thread milling down also, although as you say, if its a small diameter blind hole, the cutter is heading towards chips if it threads to the bottom of the hole.

Youre right. Thats what I meant for the 'uninitiated' since people tend to view milling as cutting down. Even say boring a hole, you bore down pretty much always. But thread milling is a unique case of going down first and cutting up.

Red James said:

Feeding down means you have to go around as many pitches as you have in your thread . . . i.e. 1/4-20 x 0.4 deep = 8 times around. Feeding up means only one circle is needed . . . from Z-.4 to Z-.35

Click to expand...

Ah good point, and another reason to explain why its from down up because most of the literature is based on using multi-thread thread mill cutters so its more efficient use of the cutting edges for maximum material removal. I was thinking in terms of single point thread milling in the above, which will be my case when cutting. Would this case (single point thread mill) matter in the direction in this regards (I suppose factoring in some points discussed above)?

Red James said:

Feeding down means you have to go around as many pitches as you have in your thread . . . i.e. 1/4-20 x 0.4 deep = 8 times around. Feeding up means only one circle is needed . . . from Z-.4 to Z-.35

Click to expand...

Whether the Thread Milling starts at the top or the bottom is irrelevant with regards to number of circles that have to be made to complete the Thread. If its a single point tool it will equate to the number of pitches (single start thread), whether from top or bottom. If its a multi point cutter, and the length of the cutter is => than the length of the Thread being cut, then it will be one lead irrespective of whether starting at the top or bottom.

The greatest consideration is avoiding compacting and fouling with swarf at the bottom of the bore, and where practical to do so (almost always), to have the cutter climb mill.

Regards,

Bill

angelw said:

Whether the Thread Milling starts at the top or the bottom is irrelevant with regards to number of circles that have to be made to complete the Thread. If its a single point tool it will equate to the number of pitches (single start thread), whether from top or bottom. If its a multi point cutter, and the length of the cutter is => than the length of the Thread being cut, then it will be one lead irrespective of whether starting at the top or bottom.

The greatest consideration is avoiding compacting and fouling with swarf at the bottom of the bore, and where practical to do so (almost always), to have the cutter climb mill.

Regards,

Bill

Click to expand...

Maybe he means with a multiflute threading tool, you can plunge in, maybe just do a 360 or so degree helix and then basically all the threads are done, but with a single point tool you need to rotate as many times as necessary depending on depth of thread cut.

Yeah climb milling is really important. I noticed during my machining op (dry) and taking multiple masses with progressively deeper depths of cut into the material, that the small chips actually begins to clog the threads, not just chips/swarf clogging a blind hole as you plunge deeper into the hole. So with climb milling, at least the cutter is running away from clogged threads. I think climb milling is the only way to go for thread milling, so I guess it explains whatever it takes to make those toolpaths, it will be threading down to up or up to down depending on left or right hand threads.