thread milling advice needed - tolerances

So I bought a threadmill and milled some nice 1/2-13 holes and the studs from my workholding go right in however... the fit is really tight. I suspect I'm cutting the threads way too close to the specs.

Without doing a ton of trial and error, I was hoping to get some advice from the machinist experts on here. Here is what I did.

I pre-drilled 27/64 which according to my GWizard shows 78% thread diameter.

I used a single pitch threadmill with a .3720 diameter and 4 flutes.

I did the programming for a 0.5000 diameter feature so the g-code produced helicals such that the outer diameter of the threads will be exactly 0.5000

What do you guys usually do for threadmilling. Do you add in some overage on the outer diameter say something like 0.5050 to add 5-thou to the outer thread diameter or use a larger pre-drill which I assume would produce more flat inner edges on the threads such as a 7/16 (62%) or 29/64 (46%). or do you do both. I'd love to have some advice from experts on some best practices. Thanks!

We use a tap!

Quote:

---

Originally Posted by hawkeyeammo

So I bought a threadmill and milled some nice 1/2-13 holes and the studs from my workholding go right in however... the fit is really tight. I suspect I'm cutting the threads way too close to the specs.

Without doing a ton of trial and error, I was hoping to get some advice from the machinist experts on here. Here is what I did.

I pre-drilled 27/64 which according to my GWizard shows 78% thread diameter.

I used a single pitch threadmill with a .3720 diameter and 4 flutes.

I did the programming for a 0.5000 diameter feature so the g-code produced helicals such that the outer diameter of the threads will be exactly 0.5000

What do you guys usually do for threadmilling. Do you add in some overage on the outer diameter say something like 0.5050 to add 5-thou to the outer thread diameter or use a larger pre-drill which I assume would produce more flat inner edges on the threads such as a 7/16 (62%) or 29/64 (46%). or do you do both. I'd love to have some advice from experts on some best practices. Thanks!

---

what kind of passes are you taking? how many spring passes what depths?

Quote:

---

Originally Posted by hoffmannm

what kind of passes are you taking? how many spring passes what depths?

---

OK, I'm new to this. I didn't realize multiple passes were necessary or advisable since Bob Cad doesn't even have an option for this in the Thread Milling feature. This is crazy!

It seems the only way to accomplish this is to copy the feature like 3 times and lie about the OD of the thead to get multiple passes. This should absolutely 100% be built into the feature.

It would take like 2 additional questions in the dialog box.

Number of rough passes: 4
Number of finish passes: 1

Here is the logic for BobCad to use. No royalty necessary.

NRP = Number Rough Passes
NFP = Number Finish Passes
NP = Number Passes = (NRP + NFP)
PD = Pass Diameter
OD - Outer Diameter (Feature Diameter)
H - Thread Height
ID = Inner Diameter = OD - H

FOR PASS = 1 TO NP
IF PASS <= NRP THEN
PD = ID + (H * (PASS / NRP))
ELSE
PD = OD
********************
Existing G-Code Logic for Helical Interpolation starting with Z=Top of Feature substituting PD for OD in current posting logic
********************
NEXT PASS

Wish I had access to the Bob Cad Source Code. I could have this added in like 15 minutes. Using this programming logic you could program existing the feature with 1 pass and 0 finish passes and it would work exactly like it does now.
Or you could program it with 2 passes with 1 finish pass and it would make 3 passes 1 rough pass 1 OD pass and then a finish pass with no extra material removed.

Bob Cad PM me if you want me to do the programming for you. :)

You need to check something like the machinery's handbook for allowable sizes on major/minor/pitch diameters for certain classes of thread. Without expensive measuring tools and gauges, one would simply start with a conservative dimension (as you did) and then modify from there based on the test item until the fit was as desired. Once you get an idea of the fit you want/need, you can just make all your 1/2-13 holes the same without having to do the guess and check routine.

Or, you could do the calculations (from Machinery's Handbook).

The single-pitch (single form) thread mill is capable of cutting a range of thread pitches, say from 12 to 28 tpi. The form of the cutter is not a sharp vee, but rather carries a radius (or flat) suitable for the root of the thread at the smallest pitch in the range. To mill a thread with a coarser pitch will require it to make a deeper penetration to get the appropriate clearance for the crest of the external thread mating with it.

The specifications in the Machinery's Handbook are calculated from a theoretical sharp vee thread. The flat or rounded root of the internal thread is to be 0.125Xpitch, and occurs at 0.125X the full thread height of a sharp vee thread. The full thread height for a 13tpi thread is 0.0662”, and 0.125 times that is 0.008”. So, with a sharp vee thread mill, it would be necessary to cut the internal thread on a radius 0.008 (0.016 diameter) greater than the major diameter called for, or 0.516”.

But, your thread mill is not a sharp vee. If the flat dimension is not provided by the vendor, figure it to be 0.125 X the finest pitch the thread mill is designed for. Then, do the heavy math (trig) to determine what your additional cut depth needs to be to get the 0.0096 width at the 0.500 major diameter. It will be less than the example above with the sharp vee.

Quote:

---

Originally Posted by craigmx5

Or, you could do the calculations (from Machinery's Handbook).

The single-pitch (single form) thread mill is capable of cutting a range of thread pitches, say from 12 to 28 tpi. The form of the cutter is not a sharp vee, but rather carries a radius (or flat) suitable for the root of the thread at the smallest pitch in the range. To mill a thread with a coarser pitch will require it to make a deeper penetration to get the appropriate clearance for the crest of the external thread mating with it.

The specifications in the Machinery's Handbook are calculated from a theoretical sharp vee thread. The flat or rounded root of the internal thread is to be 0.125Xpitch, and occurs at 0.125X the full thread height of a sharp vee thread. The full thread height for a 13tpi thread is 0.0662”, and 0.125 times that is 0.008”. So, with a sharp vee thread mill, it would be necessary to cut the internal thread on a radius 0.008 (0.016 diameter) greater than the major diameter called for, or 0.516”.

But, your thread mill is not a sharp vee. If the flat dimension is not provided by the vendor, figure it to be 0.125 X the finest pitch the thread mill is designed for. Then, do the heavy math (trig) to determine what your additional cut depth needs to be to get the 0.0096 width at the 0.500 major diameter. It will be less than the example above with the sharp vee.

---

Yes of course! That's where I made my mistake. I failed to realize that the major diameter in the diagrams I'm looking at was to the flat. You must mill the v deeper to achieve this result. This is exactly what I suspected albeit for a different reason.

I will report back after I make adjustments. It does indeed look like my cutter is a sharp v.

I'm milling 1/4-20 holes right now so I'll be testing a feature diameter of .2610. The specs are .0433 for the thread height so .0433 x .125 = .0055 x 2 + .25 = .2610. I'll be doing 2 passes one at .2300 and one at .2610 with a finish pass at .2610. This should be sufficient and we'll try it out. Thanks so much!

I also did some research and my mill only has a top RPM of 5100 so I looked up a reference on Harvey Tool. This is a great little reference guide for speeds and feeds, passes, and depths for thread mills.

http://www.harveytool.com/secure/Con...s/SF_71000.pdf

So I'm running 5100 with 1.5fpm which is painstakingly slow but that's what i get in the calcs...
Tool Chip Load .180 cutter on aluminum 6160, SFM - 1000, chip load .00097
RPM = (SFM 1000) x 3.82 / (cutter diameter .180)
RPM = 21222 (my machine maxes out at 5000) so i use that going forward

Linear Feed (IPM) = (RPM 5100) x (IPT .00097) x (number flutes 4)
= 19.788 inches per minute roughly 1.5 FPM

It may seem slow but you're milling a circular feed rate, circular feed rates are calculated differently then a linear feed rate.