Thread Milling Help

[BriscoBones]

I'm having trouble thread milling on the first attempt. Threads cut fine, but every time I have to cut a new thread size, it takes me a few attempts to get it to fit.
I am using a single-point thread mill, doing (mostly) "proprietary" threads.
Using Mastercam 2021, I am a student and neither of my instructors has ever used a thread mill, so I have basically taught myself.
I use theoretical machinist to get my cut specs, and on a manual lathe (or on our cnc lathe), I can cut threads with no issue.

But this thread milling is kicking my butt! Usually need to adjust deeper and deeper cuts with the thread mill to get it to fit.
I draw my part to my major diameter, and under my cut parameters I override my geometry and set it to cut to my minor.

Most of the time, by the time my threads fit, my minor diameter is completely out of spec.
Friday I cut my stock to my 1.4125 major, and my theoretical minor should have been between 1.3688" and 1.3571"
My first attempt was 1.36" minor, ended up having to cut all the way down to 1.34"

My brother (who owns a machine shop out of state), argues the point of thread milling, is to experiment/run tests until you find a recipe that works and just re-use that recipe.
Problem is, for my senior project, I have to cut 4 proprietary threads. That's a lot of test parts and work to make one part I may never have to make again.

TIA for any help on this one.

 

[mhajicek]

First, make sure you have the pitch exactly right. The further off that is, the more you have to oversize the thread to get the gauge or screw to fit. Second, what percentage of thread do you need? That will determine the actual minor. In soft materials like plastic or aluminum, I go for 75% thread, in hard materials like steel or titanium I'll go for 50%. Most threadmills are setup for the 50% thread, as it allows for a thicker, stiffer tool.

Edit:

It sounds like you might be talking about an external thread? If so, then the measured minor will depend on the tip flat size of the threadmill. Check your pitch diameter with thread wires and a mic.

 

[Booze Daily]

Threads are measured at the pitch diameter. Depending on the radius, or lack of, on the thread mill your minor will be different at the same pitch diameter.
Like your brother said, figure out how much “extra” you have to go to get a good thread and apply that to other thread cutting.
Besides, minor is kind of for reference.

 

[MaxPrairie]

Sounds like you are milling external threads. Not sure how you are measuring minor diameter unless you are figuring it based on the programmed radius and cutter diameter.

How we machine external threads…
1-Get specs for major diameter, pitch diameter, minor dia (for programming)
2-Machine the major diameter and make sure it is in tolerance.
3-Program thread cycle using cutter comp at high side of minor diameter.
4-Measure pitch diameter.
5-Adjust tool offset to bring pitch diameter to middle of pitch tolerance.
6-Rerun threadmill cycle.
7-Recheck thread.

 

[mhajicek]

To add, threadmills are usually a couple thou undersized from spec, so that on that first run you're always material safe. Then you comp it in until it gauges out.

 

[Larry Dickman]

Your mastercam instructors have never done any threadmilling? That's a pathetic statement right there.

When you enter your parameters for a threadmill op, it's common to enter the major dia of the thread, and the od of the threadmill. What you're actually going to measure is the pitch diameter. What does the pitch dia have to do with the thread major and the mill OD? Absolutely nothing, but it'll get you close.

Normally you use your dia comp to bring it in. It usually works out to about .009 / .012

Here's a little exercize for you. Draw your thread using the pitch diameter for the diameter, then calculate where your threamill is going to intersect that diameter. You will find it to be around .0045 off (per side)

 

[Dan from Oakland]

If you want to look into this further from a theoretical standpoint, put your threading tool on a comparator and determine how far from the tool tip the actual
tool width matches half the thread pitch. Pretty sure you are going to find that the pitch diameter on the tool is not at the theoretical distance.

 

[BriscoBones]

First, make sure you have the pitch exactly right. The further off that is, the more you have to oversize the thread to get the gauge or screw to fit. Second, what percentage of thread do you need? That will determine the actual minor. In soft materials like plastic or aluminum, I go for 75% thread, in hard materials like steel or titanium I'll go for 50%. Most threadmills are setup for the 50% thread, as it allows for a thicker, stiffer tool.

Edit:

It sounds like you might be talking about an external thread? If so, then the measured minor will depend on the tip flat size of the threadmill. Check your pitch diameter with thread wires and a mic.

Practicing in steel, final part is in stainless.
I have to do two internal and two external threads.
This project is reverse engineering, so I have to decide the thread engagements. I was just shooting for 75% cause that seemed like the standard; but that 50% makes sense.

 

[BriscoBones]

Sounds like you are milling external threads. Not sure how you are measuring minor diameter unless you are figuring it based on the programmed radius and cutter diameter.

How we machine external threads…
1-Get specs for major diameter, pitch diameter, minor dia (for programming)
2-Machine the major diameter and make sure it is in tolerance.
3-Program thread cycle using cutter comp at high side of minor diameter.
4-Measure pitch diameter.
5-Adjust tool offset to bring pitch diameter to middle of pitch tolerance.
6-Rerun threadmill cycle.
7-Recheck thread.

Damn, I never thought to double check my pitch Ø with my thread mikes. I mean I would do it that way on manual lathe, going to do that next practice run.

 

[BriscoBones]

Your mastercam instructors have never done any threadmilling? That's a pathetic statement right there.

When you enter your parameters for a threadmill op, it's common to enter the major dia of the thread, and the od of the threadmill. What you're actually going to measure is the pitch diameter. What does the pitch dia have to do with the thread major and the mill OD? Absolutely nothing, but it'll get you close.

Normally you use your dia comp to bring it in. It usually works out to about .009 / .012

Here's a little exercize for you. Draw your thread using the pitch diameter for the diameter, then calculate where your threamill is going to intersect that diameter. You will find it to be around .0045 off (per side)

I don't know about pathetic, definitely unfortunate, neither one of them ever had to thread mill in industry. I think between the two of them they have some 50 years industry experience. They just tapped or turned all threads.

But you mention diameter comp, although I know how to program it and probe cutter comp, Ive never run it. I might give cutter comp a try monday, as well.

 

[guythatbrews]

I'll bet your trouble is the single point tool you are thread milling with has a truncation that does not match the spec for the thread pitch. It is ok to use a sharp vee tool unless you are cutting a controlled root radius thread like a J series thread. Look at the thread tables in machinery's handbook and you'll see minor diameter is a max reference dimension. Read all that stuff about threads in machinery's handbook!!!

If you truncate your sharp vee tool to spec the minor diameter will fall into place. Or if you use a full profile topping insert it will fall into place.

If it doesn't no worries as stated above. Your CAM software is assuming a proper threading tool for the pitch you are cutting, and likely you are not using that tool. You should expect to have a smaller minor diameter.

It is worth mentioning the pitch diameter exists at the diameter where the thread and thread space are the same width. That is the definition of pitch diameter.

Again, a wealth of info about all things machining in machinery's handbook. Read it!

 

[mhajicek]

But you mention diameter comp, although I know how to program it and probe cutter comp, Ive never run it. I might give cutter comp a try monday, as well.

If your instructors haven't taught you cutter comp yet, that's far more pathetic. You cannot be a CNC machinist in the modern world without using cutter comp, unless you're doing super simple hobby level stuff with tolerances you can throw a cat through. But there's light at the end of the tunnel, you can surpass your instructors and be a better machinist than they ever were.

 

[IninefingersI]

I'm still on my first Monday morning cup of coffee, but I'm a little confused here. Your instructors have given you an assignment that they don't know how to do themselves and you aren't familiar with cutter comp? I'm also not following the probing cutter comp statement. Just change your toolpath compensation type to wear and walk your tool in at the control. You also need to be careful about the shape of your leads. Cutter comp has to be turned on and off on a linear move, otherwise you get an annoying red light.

 

[BriscoBones]

I'm still on my first Monday morning cup of coffee, but I'm a little confused here. Your instructors have given you an assignment that they don't know how to do themselves and you aren't familiar with cutter comp? I'm also not following the probing cutter comp statement. Just change your toolpath compensation type to wear and walk your tool in at the control. You also need to be careful about the shape of your leads. Cutter comp has to be turned on and off on a linear move, otherwise you get an annoying red light.

For our senior project we get to pick our part. We have to write up an estimate and everything.
I like to challenge myself, so I picked a part that involves processes Ive never used
And I was just referring to probing the diameter of the tool for cutter comp.
Normally we just probe the length if we cutting something quick

 

[BriscoBones]

If your instructors haven't taught you cutter comp yet, that's far more pathetic. You cannot be a CNC machinist in the modern world without using cutter comp, unless you're doing super simple hobby level stuff with tolerances you can throw a cat through. But there's light at the end of the tunnel, you can surpass your instructors and be a better machinist than they ever were.

I mean we were taught it, just have never used it. I've already made a few parts where the teachers had to ask me how I did it

But compared to the next closest machining program, my teachers seem like geniuses.
The instructor at the other school was teaching kids to use their live centers (from the lathe) as center punches! lol

 

[MaxPrairie]

I had to show our tech-ed instructor at the local school how to read a caliper. I didn't even chance trying to show him a mic.

 

[BT Fabrication]

thread mills never fit first attempt....... always better to sneak up on it then overshoot it and scrap parts

 

[rklopp]

I tend to use the theoretical cutter diameter at the pitch line as my compensation diameter input. That way, I can use the thread's pitch radius as my G02 or G03 radius, and tweak the cutter wear value to hit the pitch diameter dimension. Three slight drawbacks with this approach are that the theoretical cutter pitch line diameter varies with the pitch, I have to calculate that diameter based on a guess of the size of the flat at the tips of the cutter, and I have to make sure the cutter clears on entry and exit because the cutter's physical diameter is bigger than the pitch-line diameter. Using the cutter OD as the compensation diameter also has the first two drawbacks, and, to me, it is less natural to program the major (for internal) or minor (for external) diameter in G03 or G02.

 

[IninefingersI]

For our senior project we get to pick our part. We have to write up an estimate and everything.
I like to challenge myself, so I picked a part that involves processes Ive never used
And I was just referring to probing the diameter of the tool for cutter comp.
Normally we just probe the length if we cutting something quick

If you are expecting to mill a thread and get it right out of the gate, you are probably going to be disappointed. I've always had to play with them a bit, especially if you are shooting for a Class 3. Set your compensation type to wear in cut parameters. Add a little bit of 'D' to the tool at the control to give yourself room to work with, walk it in to where you like it, and call it a day. When I'm proving a part, and I get it where I like it, I go back into the program file and add 1/2 of my D comp to my overcut allowance. If you start simple, you usually have the problem solved before you get to complicated.

 

[mhajicek]

I'm threadmilling some 000-120 holes in Ti right now. I had to comp it in three thou to get it to gauge out. Then after a few parts I had to move it another thou.