What's new
What's new

High Feed roughing on dual contact 30 taper

Mike RzMachine

Cast Iron
Joined
Feb 4, 2007
Location
Utah
I'm going to be cutting some 4140 steel fixtures on my dual contact 10k robodrill and need to reach about 2.8" deep with a 1/2" diameter endmill for a good bit of the cutting. I thought this would be a good opportunity to try high feed roughing, high RDOC and short ADOC. I'd like to find an effective, low risk approach for roughing larger (still small, shoebox and smaller) steel parts on this machine.

I was comparing high efficiency (100% ADOC, ~15% RDOC, 6 flute Helical .5 Dia x 1.25L) to high feed (4% ADOC, 65% RDOC Helical .5 dia 5 flute high feed mill) using adaptive roughing and wanted to get some feedback from those with experience on 30 taper machines. It looks like HEM comes out about 20% faster for machine time. This isn't an issue as this particular fixture is a once in a while job.

Does the HFM approach do better for chatter in deep features (stiffer tool shank) or lower risk of pull stud failure (primarily upward axial force)? Can anyone share experience on 30 taper high feed roughing?

Thanks,
Mike
 
This is a timely question for me too. I am generally interested in looking at high feed milling for roughing small steel parts on my 30 taper machine too. My application is not so deep though.

One thing I can't figure out is why those little high feed mills are so expensive. It doesn't look like there is much to them. Lakeshore Carbide's high feed mills are the cheapest I've seen but I can't speak for how well they work.
 
I'm not an expert on small taper machines, but I like the thinking of trying to stay with axial loads to lessen stress on the pullstud.

Another thing to consider is chip transport and removal from the machine. Either method will make a lot of chips, so which can be handled better - tons of needles (large axial, small radial), or smaller 6/9's (low axial, high radial)?

At least, this is how I think it'll work out...
 
I think you can get better tool life out of dynamic milling vs HFM. You're using the whole flute length, so the wear is distributed over more carbide. I haven't tried going that deep, but I get five hours of life with a 1/2" sticking out 1.5" in grade 5 Ti.
 
While a 40 taper is the smallest machine I have I can tell you I use both strategies every day. A high feed mill is going to push the tool holder up into the spindle, an endmill is going to try to pull it out. That said the high feed cutter is going to care less about how rigid your connection is and is not even a close comparison of how far you can reach. I have a 5/8" inserted high feed mill with around 5" reach that works great. The biggest issue is chip evacuation on closed pockets, TSC is the hot ticket there, air blast second and flood coolant coming in a distant third.

I've found most of the time high feed is much faster for true 3d parts and if its prismatic I tend to go the trochoidal route provided I don't have to reach far.
 
How about tool life with high feed mills? Seems like that little bit of cutting edge is really working hard.

I get the best life with Kyocera which ironically is the cheapest ones I have. I've never compared material removed to insert/endmill cost as tooling cost is minimal for me and there is lower hanging fruit to go after :D

Not that it matters but chips from a feed mill are much nicer to handle than needles from an endmill
 
I bought a Sumitomo inserted high feed mill. It IS slower overall than if I ran a rougher. However I decided the trade off of being slower was better than the cost of purchasing a rougher with comparable reach.

Can you run a tool larger than 1/2” or is that the max diameter?
 
Even if I am going to use an endmill to clear a closed pocket I still poke a hole with a feedmill. They can helix in way faster than an endmill and I would venture to say quicker than a drill. 3/4" tool, 1.25" hole with a 1 degree helix at 200 ipm makes a pretty fast hole in steel.
 
I wouldn't recommend it because I always try to give very conservative feeds and speeds, but one of my good customers that is also local to me uses this on 4140 at 900 sfpm. With flood coolant. All adaptive programming. But his parts are only 1-1/8 thick. Almost 3" deep with a 1/2 shank tool on a BT30 taper is a big task. I am not saying it cannot be done, but is tricky.

Variable Flute End Mills With Chip Breaker - Made in USA - MariTool
 
I would go with both hem and hfm. I would do the first inch (maybe more, depending what the part looks like) with a 3/8" end mill 5 flute, 1" LOC, full depth with about .020" stepover at around 300 IPM. Switch to a high feed tool for the deeper stuff. If you need to do any finishing, switch to a neck style reach tool 1/2" or 3/8" Diameter (could also deep rough with this) depending on any corners you have to get into. I always prefer to use a smaller tool and interpolate corners. If you bury a cutter in a corner, that is where you will have issues.

Here is a Titanium part I roughed and finished with a neck style 5 flute 3/8" end mill hanging out about 3". Gage length was about 5.5" with holder. Dual Contact spindle Brother. roughed at 3500 rpm, .018 step over and 150 IPM. Ran great. Did this as a test to see what I could do with this set up. Steel could run faster.

Titanium long reach.jpg

Titanium long reach fin part.jpg
 
Thanks for the feedback. I don't generally have a lot of deep roughing but often enough that I've fought with chatter and poor tool life using long roughers on my old machine. I also had great experience with a 3/16" Guhring 3192 series. Its a hard mill in between HEM and HFM and cuts a flat bottom like a bullnose. Brother Frank, that's great advice on roughing down as far as possible with a short high flute count HEM approach.

Frank Mari, I'd like your thoughts on a range of .5-1x Dia flute length reduced shank endmills for roughing and finishing for lighter machines like mine.

Mike
 
HFM are great for deep pockets and sketchy setups and are very reliable, but I've found them to be generally slower (MRR) than HSM on the parts and materials I've done.

I find HFM to give excellent life. I run Seco inserted high feed mills and the Seco/Niagara solid carbide. I've roughed a lot of hardened 4140 (41-44HRc) with a single 1/8" high feed. It is still razor sharp. You have so large of a radius that they seem to be very resistant to wear and chipping? I'm not a tool geometry designer!
 
I'll chime in with our experience. First off, we have a Mikron with a HSK 30 Step-Tec spindle. There is no way it will do any sort of reliable HEM with a 1/2" endmill, it's just not rigid enough, it will however do HFM with 3/8 and maybe 1/2" endmills fairly well. I will say that in every instance HEM is faster than HFM, but nowhere near as reliable. The HEM toolpaths and horrible for long hangouts and shaky setups. HEM toolpaths create an incredible amount of side pressure, I have actually spun an HSK 63 holder in our Fidia spindle because it does not use the drive lugs, and that was in aluminum when I was giving her nuts. On our Hermle I must be very carefull using them because I work mostly with magnet workholding, those toolpaths will twist the workpiece if they are not really blocked in properly. I will take a HFM toolpath anyday, I run allot of unattended time and even rough hard S-7 with long overhangs lights out, it's just much saver and more reliable. Saving 20% overnite doesn't help shit if you come into a mess in the morning. Not only that, the guys that love the HEM toolpaths, question for you, when your into a long cut and you can see the endmill is getting dull and it's questionable if it will make it, how do you restart your program after setting a new tool?
 
question for you, when your into a long cut and you can see the endmill is getting dull and it's questionable if it will make it, how do you restart your program after setting a new tool?

On our Okuma mills it's simple, note the line number that you stop the program at, set new tool, restart at that line number or a few before, cycle start.
 
I'll chime in with our experience. First off, we have a Mikron with a HSK 30 Step-Tec spindle. There is no way it will do any sort of reliable HEM with a 1/2" endmill, it's just not rigid enough, it will however do HFM with 3/8 and maybe 1/2" endmills fairly well. I will say that in every instance HEM is faster than HFM, but nowhere near as reliable. The HEM toolpaths and horrible for long hangouts and shaky setups. HEM toolpaths create an incredible amount of side pressure, I have actually spun an HSK 63 holder in our Fidia spindle because it does not use the drive lugs, and that was in aluminum when I was giving her nuts. On our Hermle I must be very carefull using them because I work mostly with magnet workholding, those toolpaths will twist the workpiece if they are not really blocked in properly. I will take a HFM toolpath anyday, I run allot of unattended time and even rough hard S-7 with long overhangs lights out, it's just much saver and more reliable. Saving 20% overnite doesn't help shit if you come into a mess in the morning. Not only that, the guys that love the HEM toolpaths, question for you, when your into a long cut and you can see the endmill is getting dull and it's questionable if it will make it, how do you restart your program after setting a new tool?

In 3d surfacing paths (and maybe more, been a long time) you can set a tool life in Mastercam, either by minutes or inches in the cut and it will stop and retract in Z and put an M00 stop to check the tool.
 








 
Back
Top