milling 1 1/4-7 threads

[Greg White]

This would be on a 1991 lagun knee mill,40 taper.
It does not seem possible my looking in the msc catoalog,but perhaps I am confused.
Please type slowly as this(if possible) will be my first attempt,thru holes,1 3/4 thru,mild steel,large pipe flanges,any help would sure beat hand tapping.
Thanks
Gw

 

[MetalmanTi]

Try drilling through with the tap drill and then mount the tap into one of your tool holders or an old drill chuck and put the mill in low gear and the slowest speed and power tap the threads. Push down just hard enough to get the tap started and then let go and let the tap pull the spindle down. you can even turn the spindle on and off if you feel it is threading too fast.
Once you break through just reverse the spindle and power out. let the tap do all the work. Once the tap nears the top on the way out give it a little help to clear the hole. I have done this many times on through holes and it does beat hand tapping.

 

[Greg White]

I am wanting to know aboot thread milling,but thanks for your thoughts,she(Lagun )did not like 1 1/8-7 tap at all,so power tapping 40 or 60 holes is out.
gw

 

[johnoder]

Though your are posting in the CNC forum, you have not said the Lagun is CNC. If it is not, or not the right flavor of CNC, there will be no thread milling.

John Oder

 

[MetalmanTi]

I assumed by the first post that it was not CNC, maybe a bad asssumption.

 

[Greg White]

huh?

sorry folks,it is indeed a 3 axis CNC,I must sound dumber than I am.
I have been using helical milling for years,even when the controller wouldnt,I would write linear data and scale to get er to plunge in a circle,me biggest ? is tooling to use,the BIG book is lacking
Gw

 

[HuFlungDung]

There are a couple of ways to do it. First you'd have to figure out if your machine can do a helical interpolation. Check the manual or try adding a Z value (equal to the decimal thread pitch) to a circle cutting command and see if it accepts it, and feeds slowly in Z for the duration of time it is cutting the circle. If it errors or does not do the motion as required, then you'll need to write the code using some CAM software.

In the software, you'll need the facility to draw a helix, and then interpolate it into short 3 axis linear movements to approximate true helical interpolation. This will work well. However, determining the diameter of the helix is the trick, because you need to know the radius of your thread mill (which could be a single point tool), deduct the radius from the thread OD and then construct the helix and interpolate it with the software. It may take a few guesses to get it working correctly, so some practice pieces would be in order after you've cut a little air first

 

[Greg White]

THE MACHINE WILL CUT A CIRCLE AND ALLOW THE Z TO RAMP,THE MACHINE WILL DO IT!!!!!!!!!I AM INTERESTED IN TOOLING AND METHOD.
Gw

 

[HuFlungDung]

Check Scientific Cutting Tools. I think they'll have a thread mill that will do the job.

As for method, what more is there to know if you know how to make the machine do a helical interpolation? Start at the bottom of the hole and climb mill coming up, assuming you are using standard RH rotation tools. It looks a lot more complex than it really is

 

[Hdpg]

You could even 'single point' it using a lathe threading tool on a boring bar held in a collet. Soemwhat slower than a multi-teeth threadmill but for 7tpi through 1-3/4 not that slow.

 

[WILLEO6709]

if you have a radial drill just make the hole, take it to the radial and drive that puppy through. buy a morse taper tap driver and you are all set.

 

[HuFlungDung]

Oh gawd, run Willeo, run. He's already typed one reply in all caps, who knows what will be next......maybe a big RED font

 

[Metalcutter]

THE MACHINE WILL CUT A CIRCLE AND ALLOW THE Z TO RAMP,THE MACHINE WILL DO IT!!!!!!!!!I AM INTERESTED IN TOOLING AND METHOD.
Gw

Get a Woodruff type cutter. It will take longer but there is not so much side pressure.

I usually start at the bottom and unwind it counter clockwise for right hand . Unless you can't do that. It does let the chips fall through the bottom where they don't impact the cutting.

It will take a while to get the thread diameter just right. The good news is it always starts in the same place.

Regards,

Stan-

 

[Greg White]

Iffin I had a Radial we prolly wouldnt of gotten to have this chat,or all this fun,but as aside ,I have been lookin at Radials.
Dung,I can change colors here?never mind that will cause 24 more posts.(ha?)
So start at the bottom and Z up with the tool,I like that,I looked at the woodruff cutters,I will look again.
The indexables selection seem slim to nun for a 1 1/4-7,they seem to be too large in dia. to do inch and a quarter,I will check on Scienctifics,thanks.
One thing that troubles me pea size brain is ,for example the woodruff cutter idea,does a given dia. of cutter,NOT provide enough clearance to make a proper thread,I am for sum reason thinking as the cutter enters and exits the cut it wood deform the thread......?
Next marble rolling around in my head is the indexables? say the insert is .75 long,so you could cut aprox. .75Plus.1429 in 1 rev. around the bore?if you wanted to cutt 2.00 deep do you continue to travel with the Z.1429 pur lap?or do you go back to center Z up .75 and do it again? This may sound like gibberiss,please forgive,as for the last 40 years I have been too busy makin chips tp inprove my writing skills.
Too clear up sum notions,I touched my 1st N.C, mach. in 79 never left em after that.
Prolly forgotten more than I rember aboot em,never ran production,onecesys ,most parts I ever made the same was 8 supstrates for the "new Ranger" pickup dash. the men I worked for never bought me thread mills, I used taps 2.00 - 4 1/4 was real normal,handling holes,eh?
So what aboot it folks can you tech this old m.f. to thread mill?
Maybe I should buy a Radial,the wifey is just settling down from my last purchase?
REspectfully
Gw

 

[Hertz]

Oh gawd, run Willeo, run. He's already typed one reply in all caps, who knows what will be next......maybe a big RED font

I would believe he was typing in caps because the post right before yours said he can cut helical and that hes been doing it for years. Then you replied with

"There are a couple of ways to do it. First you'd have to figure out if your machine can do a helical interpolation. Check the manual or try adding a Z value (equal to the decimal thread pitch) to a circle cutting command and see if it accepts it, and feeds slowly in Z for the duration of time it is cutting the circle."

Frustration probably kicked in for him. lol.

Anyway Greg, if you have been doing helical milling for years, then thread milling will be a breeze for you. Its the exact same as helical milling except you use a different pitch. (This is for single point threadmilling) If you got a 1-1/4 7 thread. Then program a helical toolpath with a .143 pitch. Just remember to come back to center before retracting, unless you start from bottom. I usually only start from bottom if its a blind hole, otherwise I go from top to bottom. Good luck.

 

[Hdpg]

For right hand threads start at the bottom and helix your way up using G03 so you are climb milling, for left hand use G02 and go down.

If it is a through hole you don't need to get fancy about the tool entry into the cut because you move out to the radius underneath the work.

You do not need to take it full depth in a single cut because you always get back to the same start point with the same X Y Z coordinates.

Remember you are taking a deepish cut so your feed has to be reduced compared to what you would use for helically interpolating a hole.

 

[Hertz]

Yes sorry, I forgot to mention that. If you prefer climb milling then go from bottom to top. I never worry about climb or conv milling when threading, hence why I didn't mention it. :p

 

[Metalcutter]

So start at the bottom and Z up with the tool,I like that,I looked at the woodruff cutters,I will look again.

One thing that troubles me pea size brain is ,for example the woodruff cutter idea,does a given dia. of cutter,NOT provide enough clearance to make a proper thread,I am for sum reason thinking as the cutter enters and exits the cut it wood deform the thread......?
REspectfully
Gw

That is a consideration. It's more pronounced in an ACME thread because of the narrow thread angle and the relatively high helix angle.

But for a 60 degree thread it's not too much of a concern because on the 60 degree thread as the cutter rotates the cutting edge "falls away" fairly quickly.

A 3/4th or 7/8th Woodruff type cutter in an 1.25-7 thread should be doable.

You may want to verify that with your tool grinder. I'm making an assumtion here that this is not a life support, space vehicle part.

Best regards,

Stan-

 

[Hdpg]

The 3/4" 'Woodruff' type, my supplier calls them 60 degree double chamfer tool or something like that, does work; I have done 1-1/4" 8TPI with them.

They do give a very sharp thread bottom, a complete Vee with no radius so in critical work I would not use them due to the probable creation of a significant stress raiser. On an inside thread this is not going to be too bad but for an OD thread I think it would be a No, No.

This is why I suggested the lathe threading tool, it works very well and you can get full profile inserts and make a beautiful full profile thread. You just have to do a bit of fiddling to determine the cutting diameter of the tip of the insert for your tool compensation. I do this by estimating it using calipers and rotating the spindle, then interpolating a hole slightly less than my estimate using a regular mill and finally running the threading tool in carefully as a boring tool; mike the finished bore and there is your cutting diameter.

 

[Metalcutter]

The 3/4" 'Woodruff' type, my supplier calls them 60 degree double chamfer tool or something like that, does work; I have done 1-1/4" 8TPI with them.

They do give a very sharp thread bottom, a complete Vee with no radius so in critical work I would not use them due to the probable creation of a significant stress raiser. On an inside thread this is not going to be too bad but for an OD thread I think it would be a No, No.

I don't think it's rocket science to grind a small flat on the 60 degree point.

A many tooth cutter will get the job done a lot faster than a single point tool.

The one thing that may rule out the Woodruff tool is the depth he needs to go.

Regards,

Stan-