[roundman]

Hi everyone this is my first new thread and I always like this section. I wanted to know how to cut a higbee on an ID thread on a hass SL10? Is it possible and how would I do that?
Thanks

[WOLOG]

What type of thread are you cutting? 60 deg. V, Acme, stub acme?

I normally use a grooving tool that is a little wider than the width of a single thread form.

Copy your threading cycle, move the z start position back 1/2 pitch, slow Rpm's to 200-300 rpms, use M24, and adjust z length accordingly. Sometimes you have to adjust the z start position a little so you don't cut into the next thread. If this is not clear, I can post an example.

[roundman]

It is a standard 60 degree but on occasion we also do acme threads but so far there has been no callout for a higbee on that. I would appreciate it if you would post an example for me.

Thankyou
Roundman

[WOLOG]

I'll get you an example in the morning.

[WOLOG]

Take a look the z positions and rpms. That is about all it takes to do a thread clip for and ID or OD thread. Depending on the width of the thread and grooving tool, you may have to move the z start point of the clipping tool accordingly.

Maybe I can video it for you if I can find the time.


10 PITCH STUB ACME LAYDOWN)
G54
G00 G53 X0 Z-22.
G50 S3000
M42
T404
G00 G97 S200 M03
X1.31 Z0.1 M08
M24
G76 X1.04 Z-0.625 K0.045 D0.0111 F0.1
G00 X1.31 Z0.1579
M09
G00 G53 X0 Z-22.
M01


N11

(ISCAR PENTA CUT)
(THREAD CLIP)
G54
G00 G53 X0 Z-22.
G50 S3000
M42
T1111
G00 G97 S100 M03 (1/2 rpm of threading cycle)
X1.31 Z0.15 M08 (z start +1/2 pitch)
M24 (thread chamfer off)
G76 X1.04 Z-0.125 K0.035 D0.0111 F0.1
G00 X1.31 Z0.1579
M09
G00 G53 X0 Z-22.
M01

[roundman]

Wolog,

Thanks for the info I will plug these numbers in to my machine and see what I get. If you find the video sometime that would be interesting to watch. I have seen Mazaks use a sancronized type of cut for Higbees but so far no one that I have met seems to have done this on a Haas lathe.

[Donkey Hotey]

You've got the lathe programming manual, right? Take a look at G32 threading. From what I've read, it does not automate the multiple thread depth passes (you have to program each depth cut) but, it doesn't lose synchronization either. That should make it work for you. You program a thread, with any combination of X and Z moves, and it will cut the thread for you.

The example in the book shows a tapered thread, going to a straight thread, then into another taper. If it can cut that, it should be able to cut a higbee.

[DonutSlayer]

I do a lot of higbee's, you have to get the front edge of the groove tool in the same spot as the tip of the threading tool by adjusting the start point, and thread it usually about 1/2 to 1 pitch deep depending on the starting chamfer of the thread, and you can use only 2 or 3 cut's for the higbee , and remember a lot of machines wont allow you to change the RPM from the threading tool, I know none of ours do, we have to higbee at the same RPM or you have a lot harder time getting a match.

[roundman]

I have other projects first but I will try it this week. Thanks

[WOLOG]

As far as changing RPM's, you are supposed to be able to change rpm's if the thread start is in increments of the thread pitch. I have done this quite a bit on the TL-2 and a few times on the SL-30. If the thread is almost to depth and I get chatter, I won't change the rpm's just in case. If I am not close to depth, I will change the rpms with no problems.

The reason that I always change the Rpm's to do a thread clip is because I can get a better pull out on the starting thread. The x retract speed is far too slow to do it at higher RPM's. It takes a little playing with but it works fine. Practice on a scrap piece.

[Radian Racing]

3 weeks with my TL1 and being raw on CNC now all I know is that I really know nothing.

However I have scrapped the IPS and the VQC options just scrambled my machines control (Haas apparently will release a new software to cure that problem). But took the advice of the old hands here and spent hours on the actual G-Code and yep I am getting it right. Actually enjoying it and have made now 100 studs 3/4UNF with 20mm Knurl at pitch 1.5mm into EN19 steel and there was pain and late night learning but I got it right and the machine is absolutely accurate.

Would love to have had more RPM available. When parting off I can hear the speed is too low right at the last 4mm of cutting.

If only we could have 3000RPM on these machines.

Anyway please tell my what is a Higby thread?

And I note M24 in your code that is Chamfer off on threading. Is this important on internal threading. Need to know since next job is internal threading.

I am so glad for this forum, with such expertise available to read. Thank you so much.

[roundman]

It is where about 1/2 of the starting end of a od or id thread is basically flattened. The point of the thread is eliminated to allow I believe ease of starting the threaded item and to lessen the chances of boogering up the threaded parts. No sharp point very nice. Used in Oil feild parts often.

[swain]

I have never done it to any specification....but its basically a 45 degree chamfer before threading to prevent crossthreading for anything that is taken apart and put together alot.

Pretty much commom practice for me on any thread done on the cnc lathe unless it is a real short thread...no room for it...ect.

In some cases I have chamfered the start and finish of the thread both inside and outside threads....mostly outside.

S

[roundman]

The beginning of the v thread is from > to \_/ for about .05 into the pitch turn or so on the plug gage. After the .050 or so flat it comes to the full point again. Wish me luck.

[roundman]

I used WOLOG's suggestion and after messing up one thread and rereading his instructions it did a good Higbee. I appreciate the help very much. I showed it to the programmer and he did not jump for joy like I felt like doing when it turned out. (I always get that way when I try something new and it works good) He just said cool and asked me what I did so I showed him the tool I used and that was as far as we got he was called off to do something for the shop boss. I will look at the other suggestion offered soon. Thanks.