Thread milling with PathPilot

Just messing around today, in case I need to do this someday.

I ground up a single point tool from an old endmill. I haven't found any dimensions for this type of tool. I used a surface grinder so I know the top is right on the center line, and has a zero rake on the top face. Ground the lead angle with the grinder also. Back side I had to do by hand. Since PathPilot graphics seem to show cutting with the lead angle, a little off shouldn't be a problem.

Considering how long it took I probably should have just turned a piece of O1 and heat treated it.

Just found a video by NYCNC that explained why I was undersize, (sharp point tool vs the proper radius for the root.) Do I lie in the tool table about the cutter diameter to compensate or enter a larger outside thread diameter in the to compensate?

Is my Z zero point the sharp edge or would it be the bottom of the tool. I had set it by eyeball to the sharp edge but it did not mill as deep as I thought it would. If I had set from the bottom of the tool it would have been off even more. I am not clear how to predict how deep in Z the end of the pass will be. With either a flat bottom or a short tool this could be a problem,

Dave

On my mill, not a Tormach, I always use cutter comp when thread milling and start with cutter maybe 0.015 oversize and reduce diameter until the nut or bolt fit with the thread.

Jeff

Yeah, I tried to get all scientific about it but in the end just kept nudging the diameter until things fit.

Quote:

---

Originally Posted by rdsi

Yeah, I tried to get all scientific about it but in the end just kept nudging the diameter until things fit.

---

I use to draw models at required size so cam software would not show a gouge detection error! Now I turn gouge off and do all the nudging in the cam operation setup. Note the dia used for a very nice fitting 0.5 -13 i.d. thread. This setting uses an standard published i.d for minor hole size.

Attachment 386140

Quote:

---

Originally Posted by rdsi

Yeah, I tried to get all scientific about it but in the end just kept nudging the diameter until things fit.

---

There's nothing scientific about thread sizes - its just a question of mechanical tolerances. The tolerance of the pitch diameter for a 1/4-20 2B (I'm not familiar with imperial tolerances but this appears to be fairly standard) is about 0.004" which is well within the capabilities of a Tormach. To me, a thread needs to be within tolerance, everything else is just a spiral groove (we've all seen plenty of those on Youtube :))

Quote:

---

Originally Posted by toyshop

Considering how long it took I probably should have just turned a piece of O1 and heat treated it.

---

Uhhh, it sounds to me like you should have just bought a thread mill! I wouldn't have gone to all that trouble...

Quote:

---

Originally Posted by toyshop

Do I lie in the tool table about the cutter diameter to compensate or enter a larger outside thread diameter in the to compensate?

---

Lying is never a good strategy and that also applies here. One of the few benefits of a single form thread mill is the ability to cut threads of different pitches. Lie once and you're like to get caught when you try to machine a different pitch. For single form thread mills (ground to a theoretical point) I use their actual diameter and program the CAD to mill the larger spiral.
Step

I'm using the conversational in PathPIlot. So this is not in my tool table for the cad/cam.
Just trying to figure it out with a cheap tool, money not time, before I broke a $ 50 tool.
Do the purchased ones have a flat or radius for the thread root?

Dave

Sorry I should be more specific to the topic or question. I use single point thread mills that look like picture above. Only difference is there are 4 teeth/notches. The root is a point and the reason I need to use a oversized tool path to get the correct fit. I use a formula published in programming cnc by Peter Schmidt. I mentioned my process for cad and cam because I mostly start with a design model and if model has certain sizes or features it makes selecting them for use in drill, threading and chamfer operations more straight forward, fast and also not generate errors.
Anyway setting up a conversational program would use same values if the same profile tool is used.

There absolutely is something scientific about it - and it can be easily calculated. Because you are using a sharp point tool, you need to cut to that - which is NOT where the thread definition is, so thread will always be tight as that little extra from the thread definition to the sharp point is not accounted for. It is not a "tolerances" thing - its a definition thing. This is true for both internal and external thread - and the little extra is roughly twice as much on an external thread that it would be on an internal thread.

I wrote a little iPhone app that does the calculation for me, and I get perfect threads first time, every time. "x-end" is the value for minor diameter on an external thread, and "Maj D" is the value for major diameter on an internal thread. Those are the values that take the sharp point into account. I don't know why Tormach doesn't build this calculation into their conversational threading.

Working 7 out of 8 days now,so I won't get back in the shop to work on this til the following weekend. The shop is cooled back down, so no evening work either. It's been tough keeping the shop warm enough this year.

Thanks for the info

Dave

What Dannir said. An engineering thread form has a rounded bottom. Your tool has a sharp point. Look up the reference Standards.
Two things you can do:
Knock a tiny bit off the point of the thread mill (which makes for a stronger thread anyhow)
Allow a compensation parameter to the calculations. This tends to require some experimentation.

Both are 100% valid engineering. (Which means some of us have been doing both for years.)

Cheers
Roger

Quote:

---

Originally Posted by dannirr

There absolutely is something scientific about it - and it can be easily calculated.

---

This is just school trigonometry. If this is science then I've been a scientist since the age of about 13 and didn't even know!
Getting back to Daves last question:

Quote:

---

Originally Posted by toyshop

Do the purchased ones have a flat or radius for the thread root?

---

The single form thread mills that most of us here are using are intended to cover a range of thread pitches, so in contrast to multiform thread mills (which is out of scope here) they can't have the correct form and will have "sharper" points than their multiform counterparts, but as Roger pointed out, a really sharp point is less that ideal for strength.
The image below shows one tooth of my Maritool "Single Form Thread Mill .180 Diameter" (1310-.180-1) I use for 1/4-20. You'll see that the tip has a small ground flat as standard.
Attachment 386332
On my poor mans optical comparator I measured this flat to be about 2.2 thou. (I'm sure this varies considerably between thread mills) which reduces the actual outside diameter of the cutter by around 3.7 thou compared to what the cutter would have measured before the flats were ground. From what I can see the app from dannirr (sorry, Dr. dannirr) relies on the cutter having a sharp point so if we rely on either the measured diameter, or the specified cutting diameter (e.g. from Maritool) this would give you an incorrect value, the resulting thread would have a slightly wider groove than expected, but this is often still ok as I'll explain.

Continuing with the same example, the minimum major diameter of an internal 1/4-20 is 0.250 but on the one hand this is the minimum value and on the other hand, as we've seen here, it isn't very easy to handle. This minimum value corresponds the the minimum pitch diameter (see Unified Screw Threads and Tolerances (Inch) for more info on pitch diameters). You'll find values for both the minimum and maximum pitch diameters and the difference between them for a 1/4-20 2B is 4.8 thou (according to the amesweb values). Therefore, if you aim for the minimum diameter, with this little bit of extra groove width you're still well inside the tolerance band (yes those tolerances are relevant) so you're good to go.
Obviously tool runout and backlash will be there but hopefully they are small in comparison to the allowed tolerances.

You don't have an optical comparator? Well, being on this forum I'm sure you all have some pretty good tooling already and probably the only additional part some of you might need can be purchased from Banggood for under $50. I've been planning to make a video to demonstrate this - maybe now's the time.

@dannirr: If I understand the values in your screenshot correctly, you are showing the programmed OD for a sharp pointed thread mill to be 0.255". How did you arrive at this value?

Experimentation an "nudging" are fine for one offs but if you're producing for paying customers you'd better make sure you're using a thread gauge as your reference and not just an undersized bolt!
Step

Of course there is a science to threads, lots of standards, definitions and tolerances. I have plenty of books on the subject. The issue is the PP conversational for millings them. The tooling bits sold by Tormach look to have the same sharp point as the ones I have from SCT. Trying to modify a carbide thread mill with a known root form is not that easy if you’re trying to meet specifications.

So the question is using the standard sharp point tool what are the parameters to use in the conversational to get a decent fit. I view this conversational as just a quick & easy way to get a thread made with an off-the-shelf tool. If I had to meet a certain “class” I don’t know that I would use this methodology.

I didn’t spend a lot of time trying the scientific approach because I just wanted to get it done (the point of this conversational) but I did make some notes and could not reconcile them with how the conversational should work thus my statement.

If someone has a method to use with the conversational to utilize a sharp point tool that does not require some trial & check fit I would like to know what it is? Tormach only states:

Quote:

---

NOTE: The values entered in these tables assume a full form thread tool. If using a fine point threading tool to cut coarse threads, the root diameter must be modified to account for the smaller tool nose radius of the fine point threading tool.

---

"dannirr" has his app but doesn’t really state if it’s output is applicable to the conversational, what the calculations are, or if it deals with fine, coarse, metric threads correctly.

"rcaffin" notes their will still be some experimentation…

Yeah I know there are calc’s that "dannirr" uses but the one’s I found on the internet & my handbooks only got me closer using the Tormach conversational. Still had some trial & error.

So in the mean time as I learn what parameters work for me I just add them into the custom thread file that Tormach provides in:

operator/gcode/thread_data/custom_threads_xxx.txt

Note: Replace “xxx” with either “metric” or “sae”.

Then it’s just one click to make a thread that I know works.

As "dannirr" points out it would be nice if Tormach included this calc in the conversational but my feeling is that it just doesn't work hence the custom files.

Quote:

---

Originally Posted by TurboStep

@dannirr: If I understand the values in your screenshot correctly, you are showing the programmed OD for a sharp pointed thread mill to be 0.255". How did you arrive at this value?


Step

---

It's just the science you derided in your post above. Given that you've been an expert at trigonometry since the age of 13, I'm sure you can figure it out.

@rdsi:

My app works with coarse and fine threads. I have not tried it with metric threads, but I think the same calculations would apply - I'll try that and report back. Yes, I wrote it for use with Conversational, as the values from Tormach and standard books gave threads that were too tight, sometimes to the point of not fitting at all. I now get a great fit, first time, every time.

Quote:

---

Originally Posted by dannirr

It's just the science you derided in your post above. Given that you've been an expert at trigonometry since the age of 13, I'm sure you can figure it out.

---

I ask simply because I get a different value :)
Step

Yes, have some good thread gauges is required. The 'real' ones are quite expensive, but if you have some good taps and dies you can make 'derived' or secondary thread gauges using brass rod. It also helps to keep a record of what compensation factor is needed for each thread mill - in what material.
I do a lot of thread milling, from M3 to M24.

Cheers
Roger

Quote:

---

Originally Posted by RCaffin

Yes, have some good thread gauges is required. The 'real' ones are quite expensive, but if you have some good taps and dies you can make 'derived' or secondary thread gauges using brass rod. It also helps to keep a record of what compensation factor is needed for each thread mill - in what material.
I do a lot of thread milling, from M3 to M24.

Cheers
Roger

---

I started with used thread gauges but they're not easy to find in good condition at a reasonable price. I tried the cheap Chinese variety, thinking that $10-$15 "lost" isn't going to break the bank but they appear to be pretty good. I checked them with the 3 wire method and they're as accurate as I can measure - so that's good enough for me.
Step

the cheap Chinese variety
A very good point.
eBay?
URL?

Cheers
Roger

Quote:

---

Originally Posted by RCaffin

the cheap Chinese variety
A very good point.
eBay?
URL?

Cheers
Roger

---

I figured I'd measure a gauge again, just be be on the safe side before I make a recommendation, but the values were WAY out. I was getting values well over 0.1mm too big! I repeated the measurements, rechecked the tables, my Excel calculations and HSMAdvisor but they all gave me the same result. I tested the gauge in a nut and got the expected result. Measured a bolt, also with the expected result! I thought I was going nuts (pun intended). Then I realised I was using the pitch diameters for an external thread, but this is a gauge for an internal thread. This isn't exactly the first time I've measured a thread gauge!
(chair)
Using the correct values the measurements were exact - which means they were as close as I could measure.

I order from ebay.com.au. Search for "thread gage go/no go" and set Item Location to worldwide (if I include the link it redirects me to my local ebay site).

Most of these seem to come from uxcell so I sometimes order direct:
Uxcell Products Search

These sellers stock just about anything and everything so the products aren't posted by engineers and sometimes the pitch isn't specified - and the have some unusual thread pitches. I therefore only purchase an item when the pitch is clearly stated.
Step

Thanks.

Cheers
Roger