Thread Milling Question

[Rob B]

I am trying to thread mill a metric acme(TR60 x 9)internal thread on a mill. I am using a single point lathe threading bar. I have my thread to major diameter, but now that my thread depth is right, my root width is to wide. I think it is to wide because the is not feeding in inch per revolution, like a tap would. What can I do to fix my problem or is there any fix for this.

[kennebec]

What Machine / Control

[jgary]

In my machine G95 is feed per revolution..

 

hth

[Mr. Wizzard]

I've thread milled many metric threads. You have to convert the metric pitch into english threads per inch if your machine is set-up for standard units.

[jeff]

Your code should look something like this:

(Assuming center of hole is X0Y0)

G00G40X0Y0

Z.1

G01Z-1.F50. (IPM)

G91

G01G41X1.181F10.

G03X0Y0Z.3543I-1.181J0

G03X0Y0Z.3543I-1.181J0

G03X0Y0Z.3543I-1.181J0

G03X0Y0Z.3543I-1.181J0

G03X0Y0Z.3543I-1.181J0

ETC...

[taperlength]

Either the insert on the threading bar is too big for that thread, or the bar is wobbling. Feeding at inches per rev (G95) will break the tool.

[Rob B]

My machine is Mazak with 32B Mazatrol controller.

 

I didn't think about G95.

 

My bar isn't wobbling and the insert fits the threaded rod perfect.

 

It looks like I need to modify my post so it outputs I's & J's. I checked the Linearized Output switch, but still no I's & J's.

 

I am using a basic MPMaster post.

[hugh jars]

If you checked for linearized output then you would not get arcs with I & J - you would get a large number of small line segments in XYZ approximating a helix. Is this what you are getting? Let's see a code sample.

 

How noisy was this job running? That's a fairly chunky thread for this method. Perhaps a stability problem?

[Rob B]

I got the post to output I's & J's.

 

Things aren't looking good for me. I did some searching on the net. Here is a interesting post on internal thread milling. One of the guys in the post says it can't be done. I think I'm starting to believe him. Read the post and see what some of you guru's think about this subject.

 

post on thread milling

 

I'm up against a deadline. It looks like we might be going to the manual lathe with these blocks.

 

The parts are square blocks: 3.15x5.511x5.905

Did I mention they were made of 863 bronze. It sucks being me today.

[jhjr]

Do it in the lathe if you don't have a tap to finish the thread. I ran into this a few years ago & after a scrap part did the next one in the lathe. Now we have a tap. I don't think a smaller insert will work either because of the angle of the helix. Only with acme. You almost have to see it yourself to understand why it won't work & even when you see it you still scratch your head a bit. I've been through it. Good luck.

[htm01]

milling will cut wider than the tool unless you can tip the cutter to the helix angle. been cutting special threads in miller for 30 years and we would adjust the thread form to compensate.

[jhjr]

How did you adjust the angle. Do you have a special adjustable threading bar? I've never seen one, was it homemade or bought. Not to say they don't make them like I said I've never seen one.

[htm01]

the tool grinder had formula's for changing the thread tool, he would adjust the width and angles. when i first started we used a threading table in a bridgeport and could tip the head to the helix angle.

[Rob B]

The owner says there should be a way to time the spindle so it does 1/1 ratio with the pitch. He pretty much said I didn't understand how to get the machine and the software on the same page. My machine's minimum rpm is 60. my pitch is 9mm(.354). should my feedrate be 21.24 ipm (60 x .354) to do one revolution of pitch to one revolution of spindle. Boss wants the tool to stay in contact at all time with the part, just like a lathe. I say you can't stay in contact with the part continually like a lathe when you are thread milling. If it can be done without modifying the threading insert. I would like to know how to do the thread mill. I say it can't be done without modifying the threading insert.

 

What say you MC guru's??

[jeff]

quote:

---

The owner says there should be a way to time the spindle so it does 1/1 ratio with the pitch.

---

What is he smoking? He clearly doesn't know jack about a mill does he?

Unless you're tapping, then you can't time it, and there is no need to do so.

When threadmilling, the amount that you move in Z axis is your thread pitch, like in my post above, 9mm pitch move on Z.

[Saultspics]

Rob, Try looking a PH Horn tools. My book has internal Acme and metric trapezoidal thread milling cutters in it.

[hugh jars]

If the boss wants to time the rotation of the bar to the Z movement there is a way to do it. Put the job in the spindle so you are rotating the job, clamp the threading bar to the table, flip the machine on its side and call it a lathe.

Better still, get a lathe.

[jhjr]

Wow I'm glad that's not my boss. . See about getting a special internal acme threadmilling tool. Jeff I don't think code is his problem. It'd be ok if it was a 60 degree thread but a regular acme turning insert will not work for internal threadmilling. It cuts to wide. I imagine the insert needs to be thinner than the actual thread profile. He needs a special insert for this. I just looked at the ph horn website. They do make acme internal threadmills as Stephen said. I'd look up there # & give them a call. I'm sure they could get you what you need.

[Superman]

Hey Jeff,

I think you're Okuma savvy, There is an Okuma that can syncro the spindle with all axes, so you may have seen this option, they term it a "TURNCUT", on a horizontal MA600HB

 

 

http://video.google.co.uk/videoplay?docid=...urncut&hl=en-GB

 

To be able to threadmill large pitches, the tool must be able to arc in/arc out without cutting on the flanks of the thread lead.

 

ie bore ID = 2", the lathe threading bar should be small as practical to hold the tip, say a 1" rotating dia ( 3/4" shank ) or smaller.

 

You may have to rough with a 60° V tip first, but the 9mm pitch on a 60mm dia will be hard to do.

[jhjr]

Whoa that's trippy

[Mr. Wizzard]

I've done internal acme threading with a lathe threading bar. I had to grind it to relieve the shank so as not to rub on the internal minor diameter. I don't get the rpm sync thing. It does not matter what rpm you run the spindle. The feed does not matter either.

Obviously, with a single point threading bar, you want high rpms and slow feed to get a smooth cut.

Just draw your tool, save as undefined, and use the drawing. Then, use thread mill toolpath and adjust your metric pitch to threads per inch and set your major diameter in the parameters. It shouldn't be a big deal.

If you've thread milled with regular thread mills before, it should work out.

[jeff]

Well yes, he definitely needs an internal threading insert, and the bar has to be relieved as needed.

I thought that was "id threading 101" so I assumed he had that already,but perhaps not.