CNC Turning threads in B-16 material

Having a hard time getting a good finish, it seems that the insert is tearing more than just cutting.

Using 22 ER N 60 Insert, Grade VC905 This is what we have tried..

200 RPM @ .01 DOC, that broke the insert..

250 RPM @ .005 DOC, that chipped the leading edge of the insert..

Any info/suggestions that anyone could give would be greatly appreciated.

Thanks..

Reply to
tnik
Loading thread data ...

The lowest cutting speed I could find for a carbide insert in free machining brass is 550 sfpm. You haven't mentioned the diameter of your part, but I'm going to guess you need to crank up the rpm. Broken inserts are often a sign of too slow. Not to be confused with burnt, though. That means too fast, but you probably figured that out without me pointing it out. ;-)

Later,

Charlie

Reply to
Charlie Gary

B-16 as in bolt material "A193 Grade B16"?

How (exactly) did you program it?

(What cycle are you using and what are the corresponding parameter settings? For instance see this chart

formatting link
) (What angle pull out at end of thread are you using (parameter setting or code?)

Oil or Water? If water what coolant and what concentration?

200-250 RPM seems quite low, what size thread?

At your .01 DOC setting how many thread passes was it making?

Is there a thread relief?

Tom

Reply to
brewertr

Yep

Not sure.. I'll have to ask.. I run the mills ;)

-- It's G97

Coolant, its blue cool S2420 - 3-5 on the refracto

M42 x 4.5

alot is what I was told.. guess the DOC keeps changing as it gets down to the root.

No there isn't...

They were able too get a good finish, now they can't get any life out of the insert, running at - 500 RPM @ .01 / .002 min, .001 finish

Reply to
tnik

May want to check that again.

We/I need to know the EXACT threading cycle they are using. Can you copy and post the code or send it via email?

If that means 4% you should be OK since that is on the high side of the manufacturers recommendation. For threading you usually want to stay on the high side.

500 RPM is where I would start.

Should be around 19 passes, 22 if the material seems hard. And I would caution against too little an in-feed amount for this materiel and such a course thread.

Then you HAVE to make sure the tool is FEEDING out rather than rapid out, I would recommend 45 degrees. This can be set by parameter and/or G-Code depends upon machine and controller.

In my experience a light DOC for this course a thread on this type of material has a tendency to rub the insert rather than cut. If a spring pass is needed for a better finish then limit it to one.

Not many programs will generate G-Code for Alternating Flank Infeed. It is probably the best method for your thread but most people don't use it because it takes longer to program and more than likely it has to be done manually.

Vargus has a GREAT FREE THREADING PROGRAM you should download it. It will generate the passes for you.

formatting link
This is what it generated for your passes

P1 0.0140 inch Z1 0.0022 inch P2 0.0116 inch Z2 -0.0045 inch P3 0.0106 inch Z3 0.0016 inch P4 0.0081 inch Z4 -0.0031 inch P5 0.0069 inch Z5 0.0009 inch P6 0.0060 inch Z6 -0.0026 inch P7 0.0055 inch Z7 0.0006 inch P8 0.0050 inch Z8 -0.0023 inch P9 0.0047 inch Z9 0.0004 inch P10 0.0044 inch Z10 -0.0021 inch P11 0.0042 inch Z11 0.0003 inch P12 0.0040 inch Z12 -0.0020 inch P13 0.0038 inch Z13 0.0002 inch P14 0.0036 inch Z14 -0.0019 inch P15 0.0035 inch Z15 0.0001 inch P16 0.0034 inch Z16 -0.0019 inch P17 0.0033 inch Z17 0.0000 inch P18 0.0032 inch Z18 -0.0018 inch P19 0.0031 inch Z19 0 inch

Total 0.1087 inch (profile height) Infeed value is radius.

P1 0.356 mm Z1 0.059 mm P2 0.294 mm Z2 -0.111 mm P3 0.270 mm Z3 0.045 mm P4 0.207 mm Z4 -0.075 mm P5 0.174 mm Z5 0.025 mm P6 0.154 mm Z6 -0.064 mm P7 0.139 mm Z7 0.016 mm P8 0.128 mm Z8 -0.058 mm P9 0.119 mm Z9 0.011 mm P10 0.112 mm Z10 -0.054 mm P11 0.106 mm Z11 0.007 mm P12 0.100 mm Z12 -0.051 mm P13 0.096 mm Z13 0.004 mm P14 0.092 mm Z14 -0.049 mm P15 0.089 mm Z15 0.002 mm P16 0.085 mm Z16 -0.047 mm P17 0.083 mm Z17 0.001 mm P18 0.080 mm Z18 -0.045 mm P19 0.078 mm Z19 0 mm

So if you give a copy of the CNC Program We/I can make specific recommendations and may even edit your code and send it back to you.

Tom

Reply to
brewertr

PolyTech Forum website is not affiliated with any of the manufacturers or service providers discussed here. All logos and trade names are the property of their respective owners.