Thread mill non-standard large pitch modified Acme thread

[implmex]

Hi again Overland:
I've used and liked AB Tools in California for customs of all kinds.
Cheers

Marcus
www.implant-mechanix.com
www.vancouverwireedm.com

 

[Overland]

Once again showing my ignorance, but also showing a willingness to learn, haha !
With a solid carbide multi-flute cutter, is it realistic to "sharpen" them occasionally ?
May be touch the face, therefore extend life and reduce tooling cost.
Thanks
Bob

 

[implmex]

Hi again Bob:
Since you're just cutting mild steel, your biggest hazard to the cutter will be from re-cutting chips.
If you have HP through tool coolant or air, you can blast the little bastards right out of the pocket and your tools will last forever.
You might have to get the cutter grinding house to drill coolant passages though, or you can do it yourself if they whine and cry about doing it for you.

It's gonna make quite the fountain though, so keep the door closed when you hit cycle start.

Cheers

Marcus
www.implant-mechanix.com
www.vancouverwireedm.com

Edit:
Don't get them to make you a solid carbide cutter...it'll be way too expensive.
A 4140 HTSR body with brazed on carbide teeth will do brilliantly and cost a fraction of a solid carbide cutter.
Besides, you can drill coolant holes in it easily.
MC

 

[Overland]

Once again, thanks Marcus.
My machine is a Mazak VTC-20. No HP through coolant.
I was thinking that about the chips. The threadmill should start with a clean hole after drilling, but I guess it'll fill up fast. I figure start from the bottom, and leave the "little bastards" in the bottom of the hole, but probably not that simple.
Maybe I can set up an airblast. Fixed table machine, so as we say in the South "might could work".
Great suggestion about the brazed on carbide !
Some calls to make on Monday.
I have 2 vices, so maybe 4 at a time, but hard to see an overall cycle much less than 15 minutes on the VMC.
Plus cutting blanks, and turning the pointy end.
Appreciate your input.
Bob

 

[gregormarwick]

As far as tooling goes, I'm pretty sure you'd be able to find a bigger double chamfer kinematic mount insert that would work to cut that thread. You'd probably need to find the next narrowest insert and take two passes with an axial shift to get the right form width. That would avoid the need for custom tooling at the expense of a little longer cycle time.

eg:

 

[Overland]

As far as tooling goes, I'm pretty sure you'd be able to find a bigger double chamfer kinematic mount insert that would work to cut that thread. You'd probably need to find the next narrowest insert and take two passes with an axial shift to get the right form width. That would avoid the need for custom tooling at the expense of a little longer cycle time.

eg:

Greg,
Excellent suggestion, thanks.
I've checked a couple of sites, Carmex, etc and have only found fairly narrow tools that would require multiple passes. The crest of my thread is 0.180", so I can find square groove tools wide enough.
For example, Carmex does a 0.167" wide tool, with 1.38" cutting diameter, 6 flute; and a chamfer cutter same 6 flute, 1.38" dia.
This would require 3 passes, 1 to cut groove and 2 more to cut top and bottom flanks.
So with a cutting speed of maybe 400 fpm, tooth load of 0.004", 2 inch thread dia, each full rotation would be about 15 seconds. Need to cut 5 threads (5 rotations), So 1.25 minute per pass, times 3 passes, say 4 mins with toolchange, etc.
Do my estimates sound reasonable ?
Maybe not too bad. Cost of two toolholders.
Thanks
Bob

Edit: Looks like about $650 for 2 toolholders and inserts $140 each, Carmex.

 

[Overland]

I have just done some analysis on the effect of the diameter of the milling cutter on the thread geometry.
This is a point that Marcus brought up earlier, that I didn't fully appreciate - the tool diameter needs to be as small as possible to minimize the distortion in the thread flanks.
Very interesting learning experience.
Bob

 

[Overland]

I've spoken to a several tool companies that can produce specialized tooling for thread-milling, and waiting for their quotes.
It seems there are 2 options: either full length solid carbide or "single point" brazed tipped tools. Both these options would be about 1" cutting dia with 4 or 5 flutes.
With a cutting depth of 0.080" I imagine it would need multiple passes of full length solid carbide, 2.5" depth of cut.
For a "single point" brazed tip cutter it would need 5 revolutions for the thread depth plus maybe multiple passes due to 0.080" depth of cut.
Could I get some suggestions on the number of passes required for these 2 options please ?
I'm thinking tooth load of 0.004", and 400 ipm, realistic ?
I'm trying to estimate cycle times.
Recap:
Major dia 2.00"
Minor dia 1.84"
Pitch 0.5" (1/2").
Depth of cut 2.5".
1018 or similar.
Mazak VTC-20 with 15 hp spindle.
Thanks,
Bob

 

[implmex]

Hi again Bob:
I believe the first thing to do is to establish just what this thread is supposed to do.
If it has to mate with something, that's a very different proposition than if it's just going to be filled with grout.
Finding that out decides if this is even going to be a workable strategy or if it's just hopeless.

So before you get too deep into this...find that out.
The trial I proposed with a single or two flute home made boring bar is a good and cheap way to do that.

Cheers

Marcus
www.implant-mechanix.com
www.vancouverwireedm.com

 

[dandrummerman21]

Here, this pdf from SCT should give you an idea of speeds/feeds. Their acme doesn't go to 2"-2 like you are looking at, but you can at least use their speeds as a guide for yours.

http://sct-usa.com/wp-content/uploads/2015/08/Catalog2015_81015_SPTM_STUBACME_ACME.pdf

Idk if anyone mentioned this, but I wonder if it "doesn't look like an acme because of the flank angle" because of overcutting with the threadmill. If someone already commented that, cool.


I have not threadmilled acme but looks like SCT takes into account potential overcutting and adjusts their grind to at least minimize the effect.

 

[Overland]

Hi again Bob:
I believe the first thing to do is to establish just what this thread is supposed to do.
If it has to mate with something, that's a very different proposition than if it's just going to be filled with grout.
Finding that out decides if this is even going to be a workable strategy or if it's just hopeless.

So before you get too deep into this...find that out.
The trial I proposed with a single or two flute home made boring bar is a good and cheap way to do that.

Cheers

Marcus
www.implant-mechanix.com
www.vancouverwireedm.com

Photo of similar size "drill rod" with a size 12 for scale.
Bob

 

[Overland]

I'm waiting for a PO for this job that includes thread milling a "modified acme" style thread with 2" major, 1.84" minor, 0.5" pitch, 0.180 flat on crest of thread, 90 deg included angle. Pictures posted earlier in the thread.
I'm trying to figure out the "distortion" in the flank angle from using a standard Tee-slot cutter. Getting a special purpose cutter is going to be pricey and a significant leadtime.
Maybe this could work in this very non-typical application.
If you look at the the sketch attached here, assuming a 1.5" dia cutter, you can see it starts to cut on one edge as it goes into the cut, and continues cutting on the other edge as it leaves the cut, creating a flank angle. I'm trying to estimate what this angle might be.
I can estimate from this sketch the angle at which the cutter enters, and leaves the cut - about 45 deg, so 90 total.
I know the the pitch, so 90 deg x 0.50" pitch is about 0.125".
Or about 1/16" per side.
So the angle would be whatever the tangent is of 0.0625 / 0.080 = 0.781 or 38 degrees. This gives an include angle of about 76 degrees.
This might well work.
Is my logic/math sound ?
Bob

 

[guythatbrews]

The flank won't be flat but some weird contour. Maybe use a stock 90* included shank type cutter with a flat on the od and make 2 passes to get the correct root flat.

 

[GiroDyno]

Make a threadmilling cycle in your CAM and simulate it, then export the stock model and look at the cross section.
You can tinker with various size/shape tools and see how they adjust the profile.

 

[Garwood]

This sure looks like the kind of job that could kick your ass if you're not sure what you're doing.

You're planning to threadmill with a 1.5" T-slot cutter or woodruff type cutter 4" down in a 1.84" bore in steel with a Cat40 machine? That's a hell of a lot of cutter engagement with a big stick out on a lightweight machine. Sure it's possible, but not economically. Are you going to take 20 passes each part?

I'd recommend you go buy yourself a good cnc lathe.

Mills don't make very good lathes and you need a good lathe for this job.

 

[mhajicek]

When I had to do something similar for threads in bone plates, I used Solidworks to do a solid swept cut of the tool profile along the path.

How to use a Solid Body as a Profile for a Cut Sweep in SOLIDWORKS

Did you know that you can use a Solid Body to perform a Swept Cut? In this article I'll show you have to perform a SOLIDWORKS Cut Sweep using a body profile

www.javelin-tech.com

 

[Overland]

This sure looks like the kind of job that could kick your ass if you're not sure what you're doing.

You're planning to threadmill with a 1.5" T-slot cutter or woodruff type cutter 4" down in a 1.84" bore in steel with a Cat40 machine? That's a hell of a lot of cutter engagement with a big stick out on a lightweight machine. Sure it's possible, but not economically. Are you going to take 20 passes each part?

I'd recommend you go buy yourself a good cnc lathe.

Mills don't make very good lathes and you need a good lathe for this job.

Actually about 2.25" overall depth for the thread.
Thinking of an Iscar 20 mm dia holder with about 3" or less stickout.
Thinking max diameter of cutter to get max angle on the flank. But take your point a lot of tooth contact in the job.
A lathe would require single point with lots of passes and pretty slow speeds with that thread pitch. Any way, don't have a big CNC lathe.
We'll see......
Bob

 

[Garwood]

2.25" is a lot better. I read 4" earlier in this thread.

A smaller tool is going to be a lot easier cutting. And whatever you buy make sure it's side cutting.

 

[Overland]

Gar,
The job is 4" overall, 2.25 depth of thread.
From what I can tell the estimated cycle time is about the same with a 1.24" dia tool. Smaller dia, higher rpm.
Smaller dia cutter would give smaller included angle.
Image of Iscar cutter. They will custom grind the flanks, but I fear long lead times, and $$$.
Thanks for your interest.
Bob

 

[implmex]

Hi again Overland:
Just a stray thought, but have you considered setting these up on a rotary tilted over to the helix angle?
With that steep helix, getting the plane of the saw on or close to the helix angle will help you.
It looks like the thread is shallow enough and big enough that you might get away with it.

Normally you would use a 5 axis mill to tip over the rotary, but you gotta dance with the girl that brung ya, so in the absence of a big hunky 5 axis, this might be a worthwhile workaround to at least look at.

You still want to put down the smallest saw you can get away with, so you are aiming for a small saw with a big shank, but the shank still has to be small enough that you can make it to the bottom of the thread without crashing the shank into the top corner of the hole while it's tilted over.
You'll also need to make a goofy exit path if your thread happens to end under the undercut (from when the part is tilted over).

You could even carve some clearance into the shank by turning a taper on it kinda like a dovetail...wider at the bottom than at the top.

I encourage you to model it up and see whether you can gain anything by trying it this way.

Cheers

Marcus
www.implant-mecanix.com
www.vancouverwireedm.com