316 STAINLESS

[Fig sign]

Doun with your speed .dO NOT BE AFRAID TO DRASTICALLY DOUNRATE YOUR RPM

[Thee Dragracer1951]

The last EM to go away work hardened the material where it broke the EM. I have slowed down to 60sfm and .0013ipt and .05 doc 30% radial. That seems to work but I'll be here all day doing one pocket

Sigh....

[Colin Gilchrist]

Jim,

 

If you are using any of the standard pocketing routines in Mastercam (parallel spiral?) you will not be maintaining your step over amount when the endmill cuts into the corners of your pocket. You need a different pocketing stragety.

 

I would switch to the High Speed pocket method, Use a step down of .2-.25, Set your stepover in X,Y to 20% radial engagement.

 

In the High Speed dialog box, turn off Trochodial cutting, Then set your toolpath corner rounding radius to about .25

Check out the cutter motion when you do this. It will eliminate the sharp corners in your pocketing toolpath. I suspect these corners are the root of all your problems.

 

At 30% step over the angle of engagement on your cutter is 70.529 degrees. When the cutter goes into one of your pocket corners, the engagement angle changes to 160.529 degrees, which is basically like doing a full slot cut. You need to maintain more of a constant angle of engagement in the way you step your tool over.

 

As a bonus, by going with a deeper step down, you use more of the flutes of your endmill which should gain you some tool life as well.

 

If you can upload a file on the FTP site with just the pocket geometry, I'll take a look at it when I'm off the clock and write you a sample toolpath.

 

HTH,

[Colin Gilchrist]

Note that if you use the High Speed pocket method, you will need to do some re-machining in the corners of the pocket if the corner radius is less than .5 (.25 cutter radius + .25 toolpath corner rounding radius).

 

Good Luck.

[Thee Dragracer1951]

The Geometry I have is 2d. I am NOT above building a model. The HS pocketing routine is a surfacing routine. I certainly see your pooint though. As an aside...would a morf pocket be better then the parallel spiral w/ cleanup?

Grasping at straws here...

But I am going to get on doing up a model

Thanks

[Colin Gilchrist]

Jim,

 

There is a High Speed step over method available in 2D pocketing. That is what I'm talking about. I use the "High Speed" step over method for every single 2D pocket I cut. It works great and all you need is wireframe.

 

HTH,

[Colin Gilchrist]

I would stay away from Morph spiral. It isn't very efficient.

[Thee Dragracer1951]

I'm on it Colin.

I'm going to do a model as well.

[Colin Gilchrist]

I'll do a little example and email it your way.

 

[Bowfisherman]

Are you sure it's not innconnel?

[Kevangel]

This probably isn't the answer..but have you tried some "cobalt high speed drills and endmills" (new ones!! that have never touched metal)sometimes carbide just is not sharp enough for ampco 21, and that "mold steel" that you don't need to vent because air can escape thru it, don't remember its name...twice large shops have given me hot jobs and furnished carbide because wierd steels are soooo tough and I used cobalt high speed cause it pops right thru it, but its got to be BRAND new.. (they look at me in bewilderment when I return their carbide unused and tell them it cuts pretty decent)

[3R!< W3NG3R]

For drilling stainless, I use nothing but OSG EX-SUS-GOLD.

 

As for material, there is a tolerance that it is made to, so once it could be at one extreme, and the next time you do the job, speeds and feeds will not work the same. Drives me nuts too.

[Tim Johnson]

quote:

---

The inconsistancy is diffrent "Heat" or "Lot" numbers. There is a 316L spec for that type of stainless usually found in bar stock that is "free machining" and would not give you the trouble you currently have. Perhaps annealing is an option?

---

316L does not mean "free machining". In fact IMO it's tougher to machine than 316 or 316H. The L is for low carbon. It's designed mainly for welding. During the welding process the carbon will rise to the material surface and decrease the corrosion resistance. With 316L there is less carbon to get to the surface. Because of the low carbon 316L will also work harden more easily so you want to decrease your speeds/feeds. I will usually run the speeds/speeds at 75% of what the tool manufacturer recommends. I will usually cut my drilling pecks up to 1/2.

[Scott Garrison@Weiler Engineering]

We run 316L all day here (pharamceutical machines).

 

We run 35sfm with regular high-speed tools. We found carbide just doesn't stand up to the abrasivity of stainless. Have you ever thought of rough drilling out this pocket? Drilling is the most effective way to remove material since you have optimum tool rigigity.

 

Also, certs don't mean a thing! That's for the company to be able to shift blame if there is ever a lawsuit. There can be a drastic difference between lots. We see it all the time.

 

Also, the low carbon is also for cleanliness, we send our parts out to be passivated which is a process that eats carbon on the surface.

 

I would definetely slow your RPM's down either way.

 

Good luck.

 

Scott

[Thee Dragracer1951]

Just to add a little closure to this saga, I got through the job. Delivered them. Played absolute H3LL getting paid for the job. Found the customer had 17 judgements against them, I sent them to collections and recovered 75% of the bill.

Ain't this fun? Now...who wants to step up and start a machine shop?

But on a more positive note, My little Sharp box way machine runs this stuff just fine when I get the speeds and feeds right.

Thanks for the help.

[pkrogman1]

You can run a M.A. Ford 178 series tool profiling @ 2292 rpm and 37ipm with 20% radial and 100% axial. For a Full depth slot ues the 177 series tool @ 21 ipm

[GoetzInd]

I would have also tried something other than an ER32. Something with more contact. E.g. Heat shrink, hydro, power mill chuck or even a nice stub EM holder. I don't think your utilizing the ridgitity of the box ways with the ER. Although SFM and toolpath would probably make the biggest difference if your break'n tools.

 

Mike

[Guest]

jim,

would you be interested in sharing the name of the company? e-mail would work. am in your area and would be good not to perpetuate dead beats.

 

doug

[MACHINEMASTERG]

we cut 316l all the time also we find that high speed milling works best for us ..light deepth of cut at higher feed rates ..tialn coated carbide maybe .015 deep at 50 to 75 ipm

[Thee Dragracer1951]

Email sent Doug

[Colin Gilchrist]

Hey Jim,

 

Did you ever try the 2D High Speed pocketing method?

[Thee Dragracer1951]

I did Colin, Worked well. But I'm not making those parts any longer.

[Mike @ BC-MFG]

Try using a Titex drill with tfl coating. they work great. Or you could go carbide in which I'd suggest an SGS hipercarb.

[Thee Dragracer1951]

I used an AME cobalt inserted spade drill and when I called the tech folks there, the numbers were absolutely spot on. Drills started going 250 / 300 holes. They told me to peck it which made zero sense to me but, I did any way and that cured my drilling issues.