What's new
What's new

would this be a candidate for High Speed machining?

Torch or plasma cut the big chunks off first? Bandsaw is possible as well.
I considered it because I can probe off the OD or the c-bore, if only we had a halfway decent saw.

I've never seen High Speed machining before and I thought it'd be the simplest solution to this so I may try to convince them to buy some new tooling and try it out. I did ask the programmer and he said he thinks the workpiece needs to be more rigid, so I asked here.
 
I considered it because I can probe off the OD or the c-bore, if only we had a halfway decent saw.

I've never seen High Speed machining before and I thought it'd be the simplest solution to this so I may try to convince them to buy some new tooling and try it out. I did ask the programmer and he said he thinks the workpiece needs to be more rigid, so I asked here.
I think you're good for workpiece rigidity.
 
Yep. Send it.
But use a good end mill with a corner rad.
Sandvik Duramill WK-II-LX-50750-R030
530SFPM
.0075ipt
Full depth
5%stepover.

If you're unsure, just take in 2 depth cuts.
I do have a question about your feeds and speeds.
Is 530 considered HSM?

At .0075 chipload with the 5 flute that's only like 20 IPM and I'm used to seeing like 400 IPM whenever I see HSM mentioned and machines not being able to run the spindle or read ahead fast enough. And the High Speed Machining "Solomon Curve" where there's a tipping point where cutting temperature unintuitively begins to decrease once you get past a certain speed increasing tool life (like over 3000 SFPM.) My machince tops out at 6000 rpm, so I'd almost be able to get 1200 SFPM
 
Last edited:
I do have a question about your feeds and speeds.
Is 530 considered HSM?

At .0075 chipload with the 5 flute that's only like 20 IPM and I'm used to seeing like 400 IPM whenever I see HSM mentioned and machines not being able to run the spindle or read ahead fast enough. And the High Speed Machining "Solomon Curve" where there's a tipping point where cutting temperature unintuitively begins to decrease once you get past a certain speed increasing tool life (like over 3000 SFPM.) My machince tops out at 6000 rpm, so I'd almost be able to get 1200 SFPM
When adjusted for chip thinning 0.0075ipt at 530sfm is 232ipm assuming a 5% radial engagement on a 3/4dia tool.
 
When adjusted for chip thinning 0.0075ipt at 530sfm is 232ipm assuming a 5% radial engagement on a 3/4dia tool.
Oh yeah I was using 530 rpm. At 2699 rpm it's 101 IPM at .0075 IPT, then 231 IPM after accounting for chip thinning.

That's more like it. I'm still curious about running 2000+ sfpm, but my machine can't anyways
 
Yes, HSM with an endmill is the way to go on this. Two depth passes.

The ideal cutter would be a 3/4" necked tool with a 3" LOC and 1.5" flute length, 0.031 corner rad, 5-flute variable pitch with chip breakers, CrN-based PVD coating.

With the right parameters optimized for a balance of MRR and longevity, I'd expect at least 300 minutes in the cut. Pushing the parameters to favor longevity over MRR, 1000+ minutes in the cut.

DM me if you want me to make this tool for you.
 
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.

Another option that works well for this kind of part, assuming your machine (50 taper mandatory) and your fixturing is up to the task, is a long edge (porcupine) inserted cutter. Like a Sandvik 390/490 long edge. Very high MRR, very good cost efficiency.

The kind of MRR you are talking about per part is not conducive to solid carbide, unless you like spending money for fun.
 
It's only 4130 its not like its going to turn into diamonds. Having 90% less material to remove would be a net positive.

It would be too hard for my liking. I do a lot of parts that used to be flame cut 4130 plate. I pay extra now to have them saw cut. Easier on endmills, easier on the machine, don't have to be near the machine to make sure there isn't going to be a tool failure etc etc. That's just me YMMV
 
It would be too hard for my liking. I do a lot of parts that used to be flame cut 4130 plate. I pay extra now to have them saw cut. Easier on endmills, easier on the machine, don't have to be near the machine to make sure there isn't going to be a tool failure etc etc. That's just me YMMV
Fair enough, I usually don't scoff until it's over 52ish hrc. I usually don't mill flame cut stock, I usually have it laser cut and the HAZ isn't too bad on that.

The OP would need a pretty decent vertical saw if he were to cut the outside profile. It's going to be slow too, unless my vertical blades just suck but cutting 2.5" thick steel on my (vertical) saw would take all day without burning a blade up. Horizontal would be a different story but then you can't cut the actual profile, just lopping off chunks.
 
If you're unsure, just take in 2 depth cuts.

Another option that works well for this kind of part, assuming your machine (50 taper mandatory) and your fixturing is up to the task, is a long edge (porcupine) inserted cutter. Like a Sandvik 390/490 long edge. Very high MRR, very good cost efficiency.

The kind of MRR you are talking about per part is not conducive to solid carbide, unless you like spending money for fun.
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
 








 
Back
Top