What's new
What's new

Programming a long thread, methods to compensate for flex

laminar-flow

Stainless
Joined
Jan 26, 2003
Location
Pacific Northwest
When threading a high aspect ratio rod supported with the tailstock with a Haas threading cycle, is there a way to compensate for the flex in the middle?

What about with Mastercam?
 
3/8-10 x 5.25?

I think you're gunna need more than taper control!


If it is on a 3/8" bar, and if your threader bar is on the back side looking down, you can doo these with fair results in a Swiss lathe.


In your Haas I would turn it with a box tool and get with Fette for a special set of thread rolls and a high helix head.

You could get by probably with a die head and some "100" series chasers too I guess... (depending on material)
That's a LOT of helix tho....


Unless going with the Swiss, my first call would be to Fette and/or Cleveland Tool (? - the makers of the 100 series chasers?) and see what they have to say about using their tools on that helix.



I kan't imagine trying to fight this by single pointing on a Haas. :wall:



That's not going to leave much uncut stock in the middle either.
That is going to be a DEEP thread for the size of bar.

---------------------

Think Snow Eh!
Ox
 
It will be a .375-10 and about 5.250 long in steel. I can't easily rig up a follow rest on the CNC Haas.

Surely not a V thread! You'd think Acme is bad until you cut a coarse V thread, then realize Acme is a piece of cake for coarse threads.

I think you can write consecutive G33 (thread cycle) commands and run them end to end non stop and so create a multi-vector profile with a tapered thread lead in, maybe a short flat zone near the center, then the opposite taper on the way out. At least this is possible on a Mits controller, probably Haas can do it too.
 
If I was you I'd try a infeed angle of 55deg instead of 60. Kinda get as much load off the training side as I could. See if it didn't cut a little bit more freely.

Brent
 
If I was you I'd try a infeed angle of 55deg instead of 60. Kinda get as much load off the training side as I could. See if it didn't cut a little bit more freely.

Brent

Won't that increase the amount of material getting cut by the trailing edge?

One of the major weaknesses of Fanuc's two line G76 is the lack of control over infeed angle. I'm not a Haas user, but don't they allow ANY infeed angle to programmed (like every other control in existence apart from Fanuc...)
 
The die head sounds interesting, but this is a lead screw for a Schaublin 102 swiss lathe. Yes, the diameter is metric, just under .375. But we can find a .375-10 tap and cut a V thread instead of a acme. We are just thinking about this right now and wanted to see if there was a way to make this happen. We have access to Mastercam and will look to see if there is a way if we can't program the Haas. It will only require a few .000 and in the past I snuck in a piece of wood and acted like a follower
 
I know it's not ''original'' - typical of the Swiss I expect it was 9.5mm OD, ......and those bloody Vee threads on lead screws do wear. ........Anyway I'd go with ACME or better yet stub ACME, at least then you can clean up with a tap and die. - if of course you need to ;)

That said I'd probably buy a piece of ACME rod off the shelf and graft it on to the rest of the works.
 
Won't that increase the amount of material getting cut by the trailing edge?

I thought it decreased it by 5deg?

One of the major weaknesses of Fanuc's two line G76 is the lack of control over infeed angle. I'm not a Haas user, but don't they allow ANY infeed angle to programmed (like every other control in existence apart from Fanuc...)

When I cut some of the larger pitch threads I set my first line P in the 2 line G76 cycle like this P020555. Doesn't that give you a indeed angle 55deg?

I believe if you set your control to use the 1 line G76 cycle you have more angles to use but I agree with what you're saying it does seem like a downgrade for the 2 line cycle.

My bitch is the way you have to do multiple lead threads by shifting the Z start instead just a freaking variable. Lol....

Brent
 
The die head sounds interesting, but this is a lead screw for a Schaublin 102 swiss lathe. Yes, the diameter is metric, just under .375. But we can find a .375-10 tap and cut a V thread instead of a acme. We are just thinking about this right now and wanted to see if there was a way to make this happen. We have access to Mastercam and will look to see if there is a way if we can't program the Haas. It will only require a few .000 and in the past I snuck in a piece of wood and acted like a follower



I would have that ground from a solid, the original was.

Have also used the wooden stick method before, not easy to hold size for a lead screw.
 
The die head sounds interesting, but this is a lead screw for a Schaublin 102 swiss lathe. Yes, the diameter is metric, just under .375. But we can find a .375-10 tap and cut a V thread instead of a acme. We are just thinking about this right now and wanted to see if there was a way to make this happen. We have access to Mastercam and will look to see if there is a way if we can't program the Haas. It will only require a few .000 and in the past I snuck in a piece of wood and acted like a follower


Good grief - if you only need 1 pc, you better find something that you can modify to be what you want.
Way too much of an uphill fight to make one yourself.


------------------------

Think Snow Eh!
Ox
 
I thought it decreased it by 5deg?



When I cut some of the larger pitch threads I set my first line P in the 2 line G76 cycle like this P020555. Doesn't that give you a indeed angle 55deg?

I believe if you set your control to use the 1 line G76 cycle you have more angles to use but I agree with what you're saying it does seem like a downgrade for the 2 line cycle.

My bitch is the way you have to do multiple lead threads by shifting the Z start instead just a freaking variable. Lol....

Brent

Hello Brent,
By specifying an angle less than the included angle of the Threading Insert, material on the trailing flank of the Thread will be cut. For example, A0 will take an equal amount on the Leading and Trailing flank.

On controls that use FS16 Standard Format (two Block Format), FS15 Format (one Block Format) can be selected via parameter. One Block Format allows the angle in the G76 cycle to be specified in 1deg increments for 0 to 120degs.

To the OP
I agree with OX, a thread of the diameter and length you specified will give you grief threading with a single point tool. However, from a programming point of view and although HAAS make no mention of it in their manual, you may be able to compensate for the flex by using the Continuous Threading function using G32. This is a function available on Fanuc Controls and as the HAAS mimic most of the Fanuc function, this also may be available with the HAAS.

If the function is available, I would rough the thread using the G76 cycle and then finish using the G32 Continuous Threading function.

Regards,

Bill
 
I thought it decreased it by 5deg?



When I cut some of the larger pitch threads I set my first line P in the 2 line G76 cycle like this P020555. Doesn't that give you a indeed angle 55deg?

I believe if you set your control to use the 1 line G76 cycle you have more angles to use but I agree with what you're saying it does seem like a downgrade for the 2 line cycle.

My bitch is the way you have to do multiple lead threads by shifting the Z start instead just a freaking variable. Lol....

Brent

Using a 55deg infeed with a 60deg insert causes the trailing edge to cut a little bit on each pass. For clarity, 0deg infeed is straight plunge in where it cuts equally on both edges of the insert.

I think...

Ah, Bill got in first while I was AFK :)
 
Well Shit!

All this time I thought I was trying to make things better but in reality making things worse. :wall:

Thanks Fellas!

Brent
 








 
Back
Top