Threading 316L

[RoboElvis]

Hi all, I was hoping to hear your opinion on a threading issue we have here...

We are cutting external 3/4"-14 NGT threads into 316L from bar stock.

The code used for this is a G71, w/ 500 RPM.

The tool is a Sandvik top-lok 60 degree insert.

The program was initially set like this:

N0603 G71 X 0.9828 Z -1.50 I -0.0355 H 0.0928 D 0.0448 U 0.0024 B 60 F 1 J 14 M22 M73 M33

Note the first cut (D) at .0448 deep and the final (U) at .0024.

One tooling engineer said no cut should be more than .012 even if it's just the point of the threading tool. Another said the program is fine as the chip load decreases as the tool cuts deeper with each pass.

Who's right? I just want the stupid inserts to last more than 5 pieces.

[g-codeguy]

First your spindle speed is too low. We run at S1400 in the same material with Seco CP500 lay-down. You might be able to run even faster with the Sandvik insert. Second I think your D value is a bit large. Start at D.03 and experiment from there. The regular Okuma programmer used D.016, but I consider that too light for this coarse a thread. I normally stick with U.006 for 316 SS. Need to keep material from work-hardening.

I prefer M32M75 with B around 50, but I am more use to Fanuc controls.

EDIT: You can alway increase the H value and keep the D value a little bigger in order to keep the number of passes down. That way the first cut isn't as heavy yet the number of passes doesn't increase as much as they do when you drop the D value.

[g-codeguy]

Mr. Elvis. How did you make out?

[RoboElvis]

We're working through some burr issues right now. Waiting on tooling for an unrelated portion of the part.

I did, however, talk to our journeyman machining who swears by taking only .001 per pass. The issue is root control in the thread. The tool has a .003 - .005 nose radius and once the radius goes, the part is scrapped. They all take light cuts so as to not load the tool tip too much.

[g-codeguy]

Thanks for the update. I appreciate it.

[Daleb]

With that course of thread & that material you are not going to get very many parts per tip. All the insert companies will tell you will, but you won't. To keep your thread profile I use two cutters. One to rough the thread and the other to finish the thread. If you do this method make sure you leave enough material for the finish insert to clean up the entire thread. I'm suprised with taking that light of cuts (.001) that with this material it isn't work hardening. The thread insert I have found to have the most luck with is Vardex.

[RoboElvis]

I never thought about running a second tool. I run a spring pass with the first tool to clean anything up in the thread. Would i come in with something that has a larger nose radius so that the finish path tool has a little more material to cut, but not load the whole tool?

That's something i'll try in the future. We've got customers yelling for this part and i need to just get stuff out the door.

[g-codeguy]

Originally Posted by RoboElvis I never thought about running a second tool. I run a spring pass with the first tool to clean anything up in the thread. Would i come in with something that has a larger nose radius so that the finish path tool has a little more material to cut, but not load the whole tool? That's something i'll try in the future. We've got customers yelling for this part and i need to just get stuff out the door.

No. Leave .010/.015 per side for the 2nd tool. Use the same type of insert so the dimension from the side of the insert to the center of the radius are the same for both rough and finish.

[Daleb]

g-codeguy is correct in that you need enough material to clean up the entire profile, but I have used the same insert or one with more radius to rough with. If your part has an undercut or your customer does not care about the way the last thread looks you can use a G92 or G32 threading program if it is in the control on your machine. That is a line by line in X-Axis. Your Sandvik catalog should have how much each pass should be. I've had success using G92 sometimes instead of G71 (my control uses G76).

[joem5825]

I am new to milling and need help choosing my first machine. I would like manuel mill now but convert it to cnc later i am looking at the grizzly G0484 http://www.grizzly.com/products/9-x-...th-Stand/G0484

[RoboElvis]

UPDATE:
I've gone with the same coding as before but with D.018 and U.0008. I still run a spring pass to clean up a first thread burr issue. We're on 40+ pieces with the same insert and it looks great.

Now if i can find an insert that will survive turning down the hex bar stock...

Thanks, guys

[SQT18MS]

One word for you TUNGALOY

If you guys have access to tungaloy in the States you should realy try tungaloy.

Used this in turning 4x4" forged duplex whit the best of luck.

The insert were CNMG 120412 and in the roughening prosess i used special tooø holders to use the 100degree angle on the same CMNG inserts.