need ideas for 304 SS pockets

[left coast lefty]

I am machining several hundred slots is 304 SS.

They are about 20 inches long, .460 wide by .188 deep,.125 rad in the corners.

Currently I'm using a 3/8 4 fl. Data Flute E/M, ramping in to rough. Getting about 10 or so slots. Despite my warnings, the operator invariably waits too long, and it explodes and leaves a nice gouge on the bottom.

 

I would like to try dynamic mill, but not sure where to start.

 

What size endmill should I use?

What stepover, toolpath radius, speed and feed?

 

I'm currently using dynamic mill on another part, but it takes longer than I would like as the back feedrate doesn't seem to get up to speed in a short distance.

 

Thanks in advance

[Hardmill]

What kind of speeds and feeds are you using.

.188 depth and only 10 slots ?? You should be

getting much better tool life.

Also how aggressive is you ramp toolpath ??

 

 

PEACE

[left coast lefty]

Using 3/8 4 fl. with a .020 cr, 12 ipm at 1700 RPM.

I've actually got it ramping the whole way, so it's going all the way up and back.

[Hardmill]

Id increase my SFM, 166 is way too slow.

Id start @ 250 to 300 minimum, but again

it all depends on your toolpath.

 

Id have the ramp depth @ about .03-.04 on that

contour, with the increased sfm you gonna be

moving much faster.

 

 

PEACE

[Jayson Kramer]

I am figuring the EM is carbide is Tian coated by chance.This helps. I would follow steve and I agree that

166 SFM is to slow and the tool won't last. if it is not coated and sense you are taking full engagement with the tool start about 225 SFM and move up from there. look at starting about .003 FPT.

 

JM2C

[left coast lefty]

Actually I'm getting 20 slots, 2 per part- had a brain cramp earlier.

 

Hardmill, do you mean set ramp depth to .035, set ramp motion to depth, uncheck one way ramping?

 

Jay, do you think I can go full .188 depth at those numbers?

 

Thanks guys, I really appreciate the help!

[Hardmill]

Yeah set the ramp depth.

One way only matters if its an open contour.

Check "make pass at final depth" too.

 

 

PEACE

[left coast lefty]

Thanks Hardmill,

 

I'll give it a shot Monday. This should work with flood coolant, right? What FPT would you suggest with this method?

[Hardmill]

quote:

---

look at starting about .003 FPT.

---

 

 

PEACE

[Dave.L]

I don't have experience with the peel mill cycle, however, others do and they speak of great tool life. However, if you use that cycle be sure to make good size movements. Search the forum for peel mill and you can learn what happened to a Mori with very short stroke.

 

Also, I do have experience with some excellent cutters:

 

Kennametal Harvi II

 

http://www.kennametal.com/e-catalog/Produc...y%3A13232&logo=

 

These tools work awesome.

[taperlength]

Rough and finish tools. So the rougher grenades, the finish tool still cleans up.

[left coast lefty]

So I'm supposed to leave more than .03 on the bottom? It would take at least that to clean up the mess. Anyway, it's just a quick tig fill.

[iowajim62]

In-Process Inspection sheets with Tool Change fields to control the number of parts run per cutter (I would use 8 parts per cutter for this situation) would prevent tool breakage and also provides a tool to calculate costs for future jobs. Also trying tools with larger corner radii can show big improvements in moving the SFM up without torching the tool. The larger radii allow for better chip thinning and putting some of the force back into Z while also making for a tougher tool overall.

jm2c

[mchin-pilot]

Rough with solid carbide feedmills, during ramping the cutting action is on the front of the tool and thats where the feed mill cuts.

[Jayson Kramer]

Is the slot open at the ends if so I would do one pass at say .170 then a finish if you need a really nice floor other wise I would go to depth.

[left coast lefty]

Thanks iowajim, I was thinking that myself. Unfortunately the larger corner radius tool was a special order, and of course they wanted the parts yesterday! We need a Deckel cutter grinder.

[left coast lefty]

The slot is closed, .125 rad in the corners.

[Chris Rizzo]

I'm assuming the end of the tool is wearing first? What about drilling a .440 hole or so, sending the 3/8" endmill to full doc and then peel/dynamic?

 

If you do try something like that, counter-intuitively you might even consider a smaller tool.

 

That's what I've experienced myself, albeit in 4140 at rc 55 or so. But you've got some gummy crummy 304 there.

[left coast lefty]

Chris,

 

The problem I'm having with dynamic pocket is that in a short distance, the back feedrate doesn't get up to speed. I am using dynamic mill on another part, Mastercam says the operation is 12 minutes, but it actually takes 25 minutes.

Could you recommend some speeds/feeds? I was going 73 ipm at 6500 RPM with a .25 E/M in the same 304 SS, with a .045 stepover. Is that too slow?

 

Thanks

[Chris Rizzo]

Those speeds and feeds seem good, sfm is a little hot maybe? If my math is right your chip load is around .0025 with radial thinning. Maybe bump imp a bit if the tool lasts at that rpm. Seems like your right there though. I'd think your time and tool savings from then on will be with the toolpath selection and parameters.

 

I just tried a .460 slot 20 in long, .250 too, with peel mill and dynamic. The peel mill total inches traveled was significantly shorter with identical parameters. Upshot: try your new s&f's with peel mill.

[left coast lefty]

Thanks Chris,

 

I'll give it a shot tomorrow morning. What rounding radius would you suggest?

[Verndog]

quote:

---

Getting about 10 or so slots. Despite my warnings, the operator invariably waits too long, and it explodes and leaves a nice gouge on the bottom.

---

First thing I'd do is add a finish 3/8 data that just cleans up say .020-.03 on floor and .010-.020 on wall. That way even if the operator busts another tool, it wont scrap the part, and walls and floors will look better.

 

Then I'd bump up SPM to around 200-225 (slotting is worst case scenario). Then I'd make damn sure chip evacuation is taking place. Recutting the chips while pocketing will kill tool life faster then anything else.

[Reko]

Left Coast Lefty,

Here is my 2 cents, for what it's worth. I just programmed your slot and my cycle time is 3 minutes 16 seconds complete per slot(in theory, anyway) but I should say I have milled similar things many times.

 

Here is what I did:

 

Rough with a 3/8" Mitsubishi High Feed EM at 8 steps, .023" deep. This tool can plunge so no need for ramping or entry holes. That leaves .004" on the floor and .0425/side.

S2292 F275. = 34 seconds

 

Finish with a 1/4" Z-carb. This EM will last a long time only cutting the small amount of stock that is left and will leave a very good finish.

S4585 F14. = 2 minutes 34 seconds

 

Run BOTH cutters WITHOUT coolant, just AIR.

 

Chances for cutter breakage are minimal.

 

HTH

[Chris Rizzo]

Don't have any real justifications for rounding radius. Except A) it has to be larger than your stepover the larger it is the longer the overall path length. I have found keeping it short (like .01-.015 over stepover) keeps things efficient esp. for narrower pockets/slots. You don't really have much room to utilize mircrolifts and the increased feedrate on loop return. Just keep the tool moving consistent and short (and fast).

 

This is just for roughing, that's where you make (or lose) the money and time. Finishing is always easier, just use a different tool and tweak as needed.

 

Be sure to let us know how everything runs for you!

[Reko]

Never mind. My bad. The Mitsubishi High Feed cutters aren't made any smaller than 5/8".

 

I'm used to the big stuff.