Need Help!- how do I get a smooth finish

[dingo0722]

I am working on some H13 tool steel and seem to have trouble getting a consistent surface finish with out scalloping and tooling marks. What parameters would you recommend for a finishing pass, cut depth, step over and end mill style.


Thanks

Dan

[Cmailco]

Any more information you could add about the particular machining operation would be helpful; ie, side milling, facing, etc.. What's the material condition?

[dingo0722]

Im just doing a pocketing program into some annealed H13. I have been using a 4 flute 3/8 carbide and started with a 50% stepover. I could feel each step with my finger. I reduced the stepover from 50% to 25% to 12%. Scalping is reduced but still not smooth enough. I was finishing the cut at a 0.1” depth of cut. Could this be a tooling issue? I also noticed that when the tool cuts a full diameter pass, that depth is slightly lower than the rest of the pocketing sequence. Not sure if its because the tool is loaded differently than the rest of the program

[christinandavid]

Sounds like a rigidity issue. Obviously something is flexing with increased load - I would rough the pocket floor to within 0.01" and finish with a fresh cutter.

If you still get mismatch on your stepover it could be a squareness issue between the head and the bed.

DP

[dingo0722]

I check the squareness tomorrow with a dial indicator on the spindle. I have one that goes down to 0.0001 which should be more than sufficient


I wonder about ridgidity. It is a huge machine.

[ad64075]

H13 suits itself extremely well with high-speed, dry milling with a corner-radius tool. On a 3/8" solid carbide TiAlN coating, 2-flute, steep helix, a .03 - .06 radius works very well, 80% step over on effective cutting diameter, 9,000 rpm (yes, 885 sfm), .030 - .035 depth of cut and 120 ipm, leave .01 - .012 for floor finish at 60 ipm. Do not use liquid coolant! Air will be required for chip evacuation, and at this metal removal rate, the heat will dissipate with the chips. Fullerton makes a teriffic "Z" series tool for this application. I know these parameters sound extreme, but it you have a machine that can process smoothly at these speeds, I promise you can not beat the finish you will get. Another point to keep in mind when programming is how the tool exits the pocket. If you go directly from a feed line (G1, G2, G3, etc.) to a rapid (G0) move, your tool WILL leave a swirl in the bottom of the pocket! It is very important to clear the floor of a pocket with a fed move prior to rapiding to the clearance plane.

I have worked for a very large, international extrusion die company for most of my adult life, and aluminum extrusion tooling in made exclusively from H13. I have incredible amounts of knowledge regarding machining the material, and as compared to all other forms of steel, H13 remains one of my favorite to cut.

Good luck!

[Cmailco]

First off, never cut with a 50% overlap; you're starting the cut at the thickest portion of the chip, exerting the highest shock loads on the cutter in doing so. Shoot for 65-70% of the cutter width for general pocketing unless using a hi-feed mill, then use whatever the manufacturer recommends.

If you're driving the tool in a CAM package with tool engagement angle parameters, it's another ball-game entirely.

All that aside, have you checked TIR on this particular holder? What about the spindle bearings? Any noticeable change in indicator movement when applying pressure to the spindle?

A 3/8 tool is pretty small for any noticeable scalloping due to perpendicularity but I'd suspect you'll find out once you check it.