[tazman2221]

what is the best way to pick-up and chase threads? i have no instruction manual to do it but have used the manual thread program in the centurion 7t controller. i have been picking up the thread every single time i want to make a pass. it seems like there should be a way to only pick-up the thread one time and be able to make adjustments to remove material in several passes. is there a good way to chase threads? thanks

[Robert Zmigro]

Do not attempt this on a CNC machine. The setup time involved would be more than your boss/foreman would care to put up with! It is also a very dangerous proposition. Your boss came to you for your expertise. Tell him you would be glad to do the job on a conventional lathe.

[r44astro]

or you could buy a manual thread chaser. Depending on the application.

Bill

[jpawelk]

what is the best way to pick-up and chase threads? i have no instruction manual to do it but have used the manual thread program in the centurion 7t controller. i have been picking up the thread every single time i want to make a pass. it seems like there should be a way to only pick-up the thread one time and be able to make adjustments to remove material in several passes. is there a good way to chase threads? thanks

In order to achieve multiple pass thread chasing, the lathe must have the spindle orient option. Once you have the spindle orient option you can contact me for the program that is used to thread chase on the CNC machine. It is possible and the program works very well. Setup time is about 1-2 minutes.

[tazman2221]

the centurion 7t controller allows me to stop the lathe, position my tool in the thread groove, tell it the vitals, hit go and it retracts, moves out, and runs through the threads at the same depth that i initially placed my tool. it works ok but i have to reset the tool in the thread 10+ consecutive times to finish the job. i inquired to milltronics about the orient feature. the company i work for replaced our manual lathes with cnc because it didn't like rotating equipment exposed so we have to deal with that kind of logic! machine guarding gets carried away sometimes. thanks for the help.

[r44astro]

I do not know is these are insinde or outside thread if out side the manaual thread chaser might be a good choice, not sure how many have to do, but outher than buying mnul chaser, the reply is probaly the best best choice, reguardless using a covention lathe is the best choice but still it can be a recipe for diasaster if not done correctly and you will ruin what you already have. What id is make a pass with the tool not touching and check at diferrent places (depending on the length) to see I am properly set up.
I have only done American threads not any metric so maybe this changes some things not sure ... GOOD LUCK I out side threads a manual chaser is a good choice, if inside and not very deep a manual thread chaser is also a good choice

bill

[r44astro]

Excuse the spelling on my last post its early and not enough coffee I was refering to the second post as a very good approach..

bill

[Farmers Machine]

Are you chasing a thread that is to tight where 1 or 2 passes would fix it or cutting a thread to lengthen It?
either way it is a walk through candy land on a Milltronics control.let me know and i will explain what and how to do it.
The Farmer.

[tazman2221]

we do quite a bit of repair and rework. sometimes the threads are too tight by .010 p.d. or more. we sometimes have to lengthen the threads on a bolt.

[jpawelk]

we do quite a bit of repair and rework. sometimes the threads are too tight by .010 p.d. or more. we sometimes have to lengthen the threads on a bolt.

And with the program that I sent you, you will be able to do all of the above.

[Farmers Machine]

To extend the length of a thread, there is some information that you have too gather before you write your program, and from my sample, I am going to extend the length of threads on a 3/4" bolt with 10 threads per inch. I want too thread at 300 rpm.

Will assume your lathe does not have spindle orient.Write a program with a tool change with feed rate .1 and 300 rpm. Change display screen to error and run the program. Record what the average following error is in the Z axis. On my lathe it's about .008". Put your bolt in the chuck and change your screen do the diagnostics page. Rotate the chuck until the spindle marker is highlighted on the screen. Use some type of device to mark the chuck and the sheetmetal behind it as a reference point. Go to hand wheel mode and move the center of the threading tool to the bottom of the 5th full thread. We want to teach G54 here at minus .508". Now, 5 threads and the following error in the Z axis. Record the depth that the point of the threading tool is in the bottom of the good thread.

Now write a program #1 with tool change for the threading tool #3 and 300 rpm. Next event call program #2 and loop it ten times.

Now lets write program #2. Pick threading, cycle #1, start point at 1" diameter, Z .2 for two full threads at .1 per revolution. Thread depth = .750 . End in Z @ -4.00. Answer questions for taper and start angle to suit your needs. When this one single pass is complete, the machine will rapid it back to X1 Z.2, now do a position move to X.994 and fill out misc. page on the bottom line G50X1.0 , G50 is an incrimental work shift. Now the tool is at .996 but the machine still thinks it's at 1". When the next threading cycle runs, it will cut 0.003 from each side. This will put the tool at .744". Figure the depth from the bottom of the thread that you recorded from your set up to double check that 10 passes at .006 will put you where you need to be.

Go to RUN menu and select program #1. Hit cycle start and then turn the spindle speed override knob to 0. The threading tool will rapid to the start point but will not go further b/c the chuck is not turning. Very carefully, start to rotate the chuck in the direction that it would normally run and when the encoder marker lines up, it will start to carry the threading tool across the part. Visually verify that the center of the threading tool is in the center of the thread. DO NOT BACK UP OR ROCK THE CHUCK because the carriage will continue to move and you will be out of time. Turn the spindle speed override to 10% and the chuck should start and the tool should make it's first pass following the existing thread and then skimming the bolt till it gets to Z-4. If everything looks good too you, and you are in time, then advance spindle speed to full speed and let it finish the part. Mike the threads or test with a nut to verify the fit. Either add more passes in program #1 or change offset on the wear page.

The main thing is, to be in time when you teach the tool and know what your trailing error is so that you don't split a thread.

[tazman2221]

In order to achieve multiple pass thread chasing, the lathe must have the spindle orient option. Once you have the spindle orient option you can contact me for the program that is used to thread chase on the CNC machine. It is possible and the program works very well. Setup time is about 1-2 minutes.



we installed the program and it does everything we need to chase and/or lengthen an existing thread. thanks to all that have helped me get this figured out. i appreciate your time and knowledge!

[FabricioP10]

I’m trying to chase a taper thread in a box connection?..what’s the best method?im on a doosan with Fanuc Controls cnc lathe