What's new
What's new

would this be a candidate for High Speed machining?

Looking at the part and its fixturing, it doesn't seem like the most rigid situation with that stem holding the big wide top, so yeah, a heavy-action cut from an inserted tool is possibly going to be a problem.

I still think commodity 1/2" endmills zipping around at 200-250 IPM is the way to go. 8-10 in^3/min, low impact cut, cheap tooling.

Regards.

Mike
100% agree that with op's existing fixturing it's absolutely a non-starter.

Nonetheless, I have done a LOT of heavy removal parts in 4xx0 steels with 50 taper machines, and as much as I love adaptive paths/high speed roughing, I have never, not once, produced a shorter cycle time on this kind of part with that strategy.

Adaptive roughing is great for pockets and lighter spindles. For 2.5" thick pieces of 15" bar with >50% material removal, there are no endmills cheap enough to make it worthwhile compared to big cuts with indexables.

But for sure, op would have to improve his fixturing.
 
I did a lot of this kind of thing in a past life.

The easiest way to deal with the brim on high feed is to switch to conventional cutting for the last few passes, the tool is much less inclined to grab the edge that way
Conventional cut on the last pass was the first thing I tried last time I ran the part because it seemed like conventional would push the edge of the brim down as it cut rather than catching the raised edge first with climb, but it didn't help. It did leave a much better finish and reduced spindle loads because with climb cutting it sweeps the cut chip between the toolholder and the wall smashing .030" of material back onto the part.
 

Attachments

  • Snapchat-1375376532.jpg
    Snapchat-1375376532.jpg
    163.6 KB · Views: 26
Conventional cut on the last pass was the first thing I tried last time I ran the part because it seemed like conventional would push the edge of the brim down as it cut rather than catching the raised edge first with climb, but it didn't help. It did leave a much better finish and reduced spindle loads because with climb cutting it sweeps the cut chip between the toolholder and the wall smashing .030" of material back onto the part.

You can avoid recutting of the chips either by flooding with very strong coolant nozzles or run air. Assuming you have enough air compressor capacity
 
15" OD and 2.5" thick 4130 226 HBW, most of it gets machined off. They've always went with High Feed, but once there's about .200" left in Z, the brim (like a hat) starts flexing down away from the feed mill and starts breaking inserts.
Have you considered a dual approach? High feed down to 1/2" thickness and then use a 5/8" endmill to remove the rest using light but fast radial cuts.
 
Conventional cut on the last pass was the first thing I tried last time I ran the part because it seemed like conventional would push the edge of the brim down as it cut rather than catching the raised edge first with climb, but it didn't help. It did leave a much better finish and reduced spindle loads because with climb cutting it sweeps the cut chip between the toolholder and the wall smashing .030" of material back onto the part.

I have to say I have never had walls that look as nasty as that. What kind of high feed tool are you using?
 
You can avoid recutting of the chips either by flooding with very strong coolant nozzles or run air. Assuming you have enough air compressor capacity
I do flood coolant. It's not a recut chip. The chip is still attached to the base material when it gets smashed between the part and the tool. Climb cutting starts from the OD and peels the chip towards the inner wall. Conventional starts cutting from the inner wall so you get the shiny finish you see in the pic.
I have to say I have never had walls that look as nasty as that. What kind of high feed tool are you using?
Same thing. This is the chips being swept between the wall and the tool body. Has no effect on tool life, but it's probably unecessary wear on the spindle which we've had rebuilt twice this year (twice because mazak's guy did a shit job the first time.) Conventional cutting doesn't have this particular issue. But it's a 5 insert 3" sumitomo MSX feedmill with wdmt1406zdtr-h inserts, at .050 doc, maybe 90% stepover, .048 ipt and 500 sfpm.
Have you considered a dual approach? High feed down to 1/2" thickness and then use a 5/8" endmill to remove the rest using light but fast radial cuts.
I have. I considered taking the last .3-.4 with a square shoulder inserted mill. But HSM was something I wanted to see. But I'm not the programmer anyways and they don't like improving the process. I've brought them features that were way out of tolerance and show them the proof in the code, but they scoff and say "look at the simulation, that looks about right" or "We've always done it this way. How is QC even going to check that feature." So I generally use the programmer's code as a guide. If it works, cool. But normally I end up rewriting everything by hand to make features on size, rewrite all features cut with the same tool to center of tolerance, add fillets and chamfers, remove toolmarks, improve workholding, improve tool life and cycle time, etc. I can't write HSM by hand though so I was considering bringing it up once more.
 
Last edited:
High feed cutters will not like super thin sections below due to the axial pressure.
High feed cutters run at their high feed rate can not make nice walls due to the crazy chip load on the side.
Slower feed to make a wall and the bottom end is not happy and will die due to rubbing.
These facts are inherent in all high feed milling cutter designs.
 
Last edited:
. Climb cutting starts from the OD and peels the chip towards the inner wall. Conventional starts cutting from the inner wall so you get the shiny finish you see in the pic.

It's maybe a fair assumption we might already know that.
 
I have. I considered taking the last .3-.4 with a square shoulder inserted mill. But HSM was something I wanted to see. But I'm not the programmer anyways and they don't like improving the process. I've brought them features that were way out of tolerance and show them the proof in the code, but they scoff and say "look at the simulation, that looks about right" or "We've always done it this way. How is QC even going to check that feature." So I generally use the programmer's code as a guide. If it works, cool. But normally I end up rewriting everything by hand to make features on size, rewrite all features cut with the same tool to center of tolerance, add fillets and chamfers, remove toolmarks, improve workholding, improve tool life and cycle time, etc. I can't write HSM by hand though so I was considering bringing it up once more.

Are your managers ok with your programmers not doing their job?

I can't imagine they'd be thrilled if they knew this was happening...
 
But normally I end up rewriting everything by hand to make features on size,
Fuck that.
If the programmer can't do their job, it's not on you to fix the program.
If the boss truly won't make changes to efficiency, then it's time to find another job.
The worst thing you can do is re-write the program that you're given, because if the code crashes the machine and/or a valuable part.... it's 100% your fault.
 








 
Back
Top