[FuriousGeorge]

Anyone have any good info on how to calculate Feeds and Speeds for thread Milling? I have to thread mill a M12x.5 hole in Delrin (and soon 6061).

Currently, I'm running a carbide 0.372" 4 flt single profile thread mill at 90 ipm and 5100 RPM. I got this using G-wizard where I set my parameters by calling my tool a 60 deg. dovetail (I thought this was the closest tool they had to my thread mill) with a .5 mm width of cut (my pitch) and a 0.25 mm DOC (I'm running 2 passes).

Is this an accurate method? The Feeds and Speeds work fine in Delrin, but most feeds and speeds do. When I plug the same parameters in for 6061, G-wizard tells me to run at 5100 RPM and 40 IPM. Does that sound right? I've never tried thread milling aluminum and would rather not destroy my tool with too aggressive or soft of a cut. I have no idea if I can actually substitute a thread mill for a dovetail in G-wizard.

[gjvander]

What feed rate can you achieve in an M12 hole? I have found that I cannot get to the requested feed rate when I do thread milling - but it was on a smaller hole.

Geo

[FuriousGeorge]

"What feed rate can you achieve in an M12 hole? I have found that I cannot get to the requested feed rate when I do thread milling - but it was on a smaller hole."

Geo,

I didn't even think to check the actual feed rate, I guess I'm more of a newb than I thought haha. I'm maxing out at around 20 IPM. G-wizard tells me that I should be running at a speed of 700 RPM if I hold my feed at 20. I just tried this and it cut terrible. I could hear the thread-mill screeching (rubbing, I assume?) in the plastic and I stopped before the operation was even finished.

Funny thing is, at 5100 RPM and around 20 IPM (what I originally thought was 90), the thread cut great.

[gjvander]

I feed at 2.5 IPM on aluminum, but I am not in a hurry, and the thread mill is a single point 0.032" shank that is 0.750" long, so it is just looking for an excuse to break.

I would suggest you start with slow feed rate (5 IPM?) and do override on it as you become more comfortable with the tool.

Geo

[SCzEngrgGroup]

For RPM, you always go by the cutter diameter, and recommended SFPM for the tool material and work material - just like for an endmill. For feedrate, look at the manufacturers recommended chipload, and feedrate is chipload * RPM * #Teeth - also just like for an endmill. For very fragile or flexible tools you sometimes have to back off a bit, but that should be baked into the manufacturers chipload recommendations. If in doubt, start at half the calculated feed, and work your way up until surface finish starts to degrade, or something else bad starts to happen, then back off a bit from that point. Going too slow is often as bad, if not worse, than going too fast. With threadmilling you should be doing relatively light cuts, so should generally have fairly high feedrates.

Regards,
Ray L.

[TurboStep]

Don’t forget to account for the fact that you’re cutting a circular contour. The effective feed rate will usually be much higher than the programmed feed rate (unless your CAM software already compensates). Check out the following article:
Get The Feed Rate Right When Thread Milling : Modern Machine Shop
or if you have GWizard the “Interpolate” button will call up a useful calculator.
Step

[FuriousGeorge]

"Don’t forget to account for the fact that you’re cutting a circular contour. The effective feed rate will usually be much higher than the programmed feed rate (unless your CAM software already compensates). Check out the following article:
Get The Feed Rate Right When Thread Milling : Modern Machine Shop
or if you have GWizard the “Interpolate” button will call up a useful calculator."

This is gold. I had never heard of this before, but it makes total sense. It also explains why my cut at 20 IPM and 5100 RPM worked the best. Using the interpolation feature in G-wizard, I see that to Feed at 90 IPM for a 12mm hole is about 20 IPM... so effectively, I started off cutting at the right feeds and speeds despite the fact that A) I didn't realize that the tormach's motors max out well below 90 IPM for a circular cut and B) a cut at a given feed rate is, in actuality, way above that actual speed.

I wish making two mistakes at the same time always canceled each other out so perfectly...

[btu44]

Here is a formula I found in SPC thread mill catalog for adjusting the feed.

(Major dia. - tool dia.) / major dia x NAFR = AFR

NAFR = not adjusted feed rate for selected tool diameter.
AFR = adjusted feedrate.

Or what I did was put in an Excel file and use this formula.
=((C1-B1)/C1)*A1

A1 = NAFR, B1 = tool dia, C1 = major dia. of thread.

Barry