proper application

[Doug G.]

Anybody have input on the best method to profile cut through sheet stainless .130-.25 thick? Would it better to run slow with a ruffer at full depth or take shallower depth cuts but move the cutter faster. There is some dissagrement between machinists in the shop. One side stating the tip will wear out on depth cuts the other stating the full depth method has to run too slow. Any sugestions will be helpful.

[HEAVY METAL]

what size endmill

[Doug G.]

We are using a 3/8 carbide EM to cut out a profile.

[Guest]

I hate to say this but they are actually both right and both wrong depending on the approach taken.

 

I would go around the outside of the .250 plate in 2 depths of cut, 1 in the .130 plate, using a 3/8 4 FL HSS/CO course rougher, then finish in 1 depth of cut with a 4 Flute carbide endmill.

 

You did not state what grade of SST sheet.

 

I'll assume for a minute 303 SST.

 

3/8" rougher about 1500 RPM with a 12 IPM feedrate

which is 150 SFM and a .002 CPT

 

Here's a question, if you did 2 passes at 12 IPM or 6 passes at 36 IPM, which tool path is longer in time?

[JNO]

How are you holding the .130 sheet ?

[Guest SAIPEM]

The problem with sheet material is always lateral tool pressure.

Apply High Speed Machining principles.

Use Contour|Ramp with the smallest tool possible.

Set the ramp depth TOOL_DIA/4.

 

I routinely do the following with 316 and 17-4PH.

 

1/4 DIA 2-FLUTE CARBIDE

6100 RPM 34 IPM

[terry5357]

I personally prefer to ramp thru the part with .00 or so past bottom of part. When the O.D. starts getting dull I drop another .15 in Z and I'm back to fressh endmill, also I would use a 1/4" dia tool. "SAIPEM" is there on speed and feed, a little hotter than I would use but thats just programmer preference (make the tool last a little longer vs. get the part done faster)if you have 100 parts, save the tool, if you have 5 parts get'em done and get'em the hell out of there.......lol.

 

Saipem done much oilfield work, have you:)

[Guest SAIPEM]

quote:

---

Saipem done much oilfield work, have you:)

---

More than I care to remember.

 

Milling sheet material is a losing proposition as far as efficiency goes.

 

It's really a water jet application.

[Doug G.]

Thanks for all the ideas guys. The plates are clamped in a fixture and I prefer the depth cuts method. To me the idea of wear on the tip is the same as wear on the flute. Isn't an edge an edge?

 

I'm trying to improve on the present approach of a full depth 3/8 ruffer at 2ipm, I can take two depth cuts and move 10ipm. Trying to convenct the 2imp guy is the road block.

[Guest SAIPEM]

Doug-

 

You need to keep in mind that wear is not an issue in High Speed Machining techniques.

 

If it was, this technique would not have gained any traction at all.

 

Your chosen method will absolutely wear out the tool faster.

 

Give us an update on how the cut works out for you.

[Guest CNC Apps Guy 1]

I'm an HSM fan so the 2 ipm is wrong IMHO. But seriously, at the end of the day if you both have "sellable" parts, you're both right. It's strictly a preference issue. I've found over the years that there is almost always more than 1 way to skin the cat so to speak.

 

JM2C

[Guest SAIPEM]

Ditto that James.

 

More often than not, the method you can use is limited by the tools at hand.

[PeterM]

Here at Preci we have done a lot of flanged parts in varying stainless grades. For 1/8 or so thick I take 1 rough cut with a 5/16 or 3/8 stub carbide rougher/finisher, 80-100% sfm, .001-.0015 IPT then finish with a 1/4 dia. carbide varible helix finisher, as fast as the finish limitation, we get good tool life and quality with this approach.

 

_____________________

Peter Martin

mcam 3... - x mr2 - mill level 3

Senior Programmer/Milling Supervisor

Preci Mfg.

400 Weaver St. Winooski VT 05468

PH# 802-655-2487 ext. 231

email [email protected]

[Doug G.]

Thanks again guys for the feedback. Here's what we came up with. The 2ipm program was a 29min cycle. The step cut at 10ipm was 13min. We found if we ground a .030 chammfer on the tip of the profile tool it lasted longer and produced less burr. Step cuts was the winner.