Need help programming an acme thread...

[Edster]

I've got a progamming problem, I'm making a 3" .5" Pitch 1.0" lead (double start) left handed bastard thread, I mean ACME thread I've never programmed a double start thread or left handed thread or acme thread, so it's nice to get them all at once. Anyway I've got it programmed using the g32 threading cycle. I'm rapiding to clearance of x3.5, z-7.5, feeding to depth of first cut, G32 Z.5 F1. Q0. Then rapid to x clearance then back to z-7.5 then feed to first depth of cut again, then G32 Z.5 F1. Q180000. for the second start.

The problem is the thread is deep and I have to take small passes, a lot of small passes. The double start multiplies the passes x2, so my program is huge. I'm also feeding straight in. I'd like to program with a 14deg infeed angle and a G76 threading cycle but I'm not exactly sure how. Any help would be appreciated.

[Eurisko]

Sounds like fun.

The 14 degree infeed isn't a problem, just multiply the cumulative depth of cut by Tan(14) to get the Z offset for each starting position.

If each pass has a depth of cut of .010, the Z start position is offset +.0025 before each pass.

start position (X,Z) (single start threading, left-hand)
pass 1: X+2.980 Z-7.5000
pass 2: X+2.960 Z-7.4975
pass 3: X+2.940 Z-7.4950
...
pass n: (X=+3.000-.020n) (Z=-7.5025+.0025n)

I'm not familiar with Haas programming, but the program size could be greatly reduced by using a Do ... While or For ... Next loop.
Just initialize the X and Z start variables, and add a constant value after each pass.

Use another variable to keep track of the number of passes. Loop until done.

I never cared much for canned cycles. What fun is THAT???

[makrskr]

G00 xclearance Z-7.5
G76 Xfinish root dia Z.5 A14. D depth of first pass K height of thread F.5
G00 Z-7.75
G76 Xfinish root dia Z.5 A14. D depth of first pass K height of thread F.5

[Edster]

So,

Major dia is 2.9875
Minor is 2.4563
Thread height is .2656

G00 X3.1
Z-7.5
G76 X2.4563 Z.5 A14. D.005 K.2656 F1.0 Q0.
G00Z-7.5
G76 X2.4563 Z.5 A14. D.005 K.2656 F1.0 Q180000.
G0 X3.1 Z.5

How do you specify the number of cuts?

How do you specify the number of spring passes?

How does it determine the depth of cut? It says depth of first cut, does that mean it will take .005 each pass?

What is the difference between a P2 double edge cutting, cutting ammount constant, and P4 double edge cutting cutting depth constant?

[Geof]

Originally Posted by Edster So, Major dia is 2.9875 Minor is 2.4563 Thread height is .2656 G00 X3.1 Z-7.5 G76 X2.4563 Z.5 A14. D.005 K.2656 F1.0 Q0. G00Z-7.5 G76 X2.4563 Z.5 A14. D.005 K.2656 F1.0 Q180000. G0 X3.1 Z.5 How do you specify the number of cuts? How do you specify the number of spring passes? How does it determine the depth of cut? It says depth of first cut, does that mean it will take .005 each pass? What is the difference between a P2 double edge cutting, cutting ammount constant, and P4 double edge cutting cutting depth constant?

Dig out your manual or go to the Haas website and find the lathe manual. It describes the G76 routine. D is the depth of the first pass and then it uses a formula to calculate the depth of the following passes which gets smaller and smaller. There is a Setting to make sure it never goes below a certain depth.

[Edster]

Thanks for the replies, I experimented for the better part of a day and figured out what all the settings and P1-P4's did. I always wondered how to alternate sides of the threading tool

[Edster]

The test piece is done and I'm working on the actual part. The 416SS is tough for the TL-1 to cut. I wish it had a gearbox.

Here is a pic if anyone is interested.

http://www.ewwenterpriseinc.com/images/ACME1.JPG

http://www.ewwenterpriseinc.com/images/ACME2.JPG

[Geof]

Originally Posted by Edster The test piece is done and I'm working on the actual part. The 416SS is tough for the TL-1 to cut. I wish it had a gearbox....

Yes, when you need a slow spindle speed you are also running the motor at a speed at which it has low efficiency and loses torque.

I took the covers off and had a look with the idea of fabricating a reduction drive.

There is an encoder drive off the spindle and what I thought would be possible would be to put in a layshaft with a pulley the same size as the spindle pulley.

Then transfer the encoder drive to the layshaft and have a separate drive going from the layshaft to the spindle with a choice between direct drive or a two to one reduction.

When the machine is running on the reduction drive the spindle would be turning at half the speed the controller is reading so you would have to double all your spindle speed commands and at the same time halve all your feed commands.

The problem I foresee with this is that the backlash from the reduction drive belt would be affecting the encoder. This would make rigid tapping impossible but should not affect threading.

An alternate way would be to make a two speed encoder drive from the spindle. When driving the spindle at a two to one reduction the encoder would be driven by a one to two drive. This should solve the backlash problem.

The reason I would change the encoder drive is because the controller sets the motor speed by the frequency it supplies and if you simply put in a different drive belt ratio the speed from the encoder would not match what the controller was expecting so it would give a spindle following error.

I will be getting a TL2 later this summer with the full enclosure and higher spindle speed option. Once it is out of warranty I might play around a bit and see if these ideas work.

[HuFlungDung]

Nice job, Edster. Good luck on the real one. 416 is very nice to machine though. What kind of tooling are you using? Laydown threading tools would be the best, with angle shims to get the clearance that you need on the insert. Such animals are available.

I would recommend that you have a 'centered pass' in between every cut on alternate thread flanks. It makes quite a difference when the tool is only cutting on one edge at a time. The least of my worries, if I was working a difficult job, would be debating whether I must write out a longhand program that would cut exactly the way I envisioned, or whether I would settle for a general purpose macro that was less than exactly what I wanted.