[davereagan]

Ok guys, I've been watching these trochoidal videos for a while and they bug me. They are amusing to watch, but I think they are designed by CAM guys who get paid by the mile. Eagle understands how to use a Varimill, but I'm not sure anyone else has really seen one take a full diameter depth and width at 30-40 ipm. If you saw it, why would you be interested in .025" passes except on a Sherline? Below is a program to take that 3/4" wide, 1.24" deep slot in 1" hot rolled steel. The parameters are very conservative. I run an endmill for weeks at this rate. I calculate the inches fed to be a total of 8.7, for a total feed time of 17.4 seconds, including a finish pass. Add maybe five seconds for all the rapids and you're still under 25 seconds. Keep in mind, I am running a 1/2" varimill at 3000 rpm. That could easily be boosted to 4000, and feeds could be put to .003" safely. Eagle would do it in one less pass. (I have broken 1/2" endmills taking .75" depth when slotting.) By the way Geoff, your projection length on your holder is atleast 2.5" No matter what machine you run, if you went to a 1.38" gage length, you could push your machine a lot harder and it would be quieter in the same cut. I don't use program line numbers. Datums: X is on the centerline of the slot and Y is at the back of the bar. The tool I would be using is a Hanita Varimill or SGS Z carb, 1/2" diameter, 4 flute, 1-1/4" length of cut. I think any of the variable helix endmills would run this program easily given a solid 40 taper machine.

:G90
M6T9
G0G95 X-.125 Y.3 Z.1 M3S3000 F.0025 H1
G0 Z-.5
G1 Y-1.1
G1 X.125
G1 Y.3
G0 X-.125 Z-1
G1 Y-1.1
G1 X.125
G1 Y.3
G0 X-.125 Z-1.24
G1 Y-1.1
G1 X.125
G1 Y.3
G0 X-.125 Z-1.250 M3S4000 F.002 (FINISH RUN)
G1 Y-1.3
G0 X.125
G1 Y.3
G0 Z.1M2

[Donkey Hotey]

I do not know if MasterCAM has plunge milling; I assume it does.

Thanks guys! :cheers: Man, I love this place and the exchange of information. Yes, I can now confirm that Mastercam X (2005) has plunge milling. I never bothered to look for it until you posted that video. For some reason I kept thinking of plunge milling as something that would swiss-cheese the block but would leave behind the remaining material. I gave it a whirl and sho-nuff, the routine has whatever stepover you want (under the Surface Roughing menu). Plunge mill the material, chase it with a cleanup pass and it's done.

THAT would have been useful for this monster pocketing job I had. I'm going to give that a go next time I have to pocket something.

[Geof]

I was thinking about plunge milling versus trochoidal and realised that Kennametal will push plunge milling because trochoidal is not feasible with an insert mill, while companies making endmills are going to push trochoidal for the opposite reason.

Regarding Varimills I have never had much luck. I have tried them using the speeds and feeds people have suggsted and generally finish up with a two piece cutter.

[BobWarfield]

I was thinking about plunge milling versus trochoidal and realised that Kennametal will push plunge milling because trochoidal is not feasible with an insert mill, while companies making endmills are going to push trochoidal for the opposite reason.

Regarding Varimills I have never had much luck. I have tried them using the speeds and feeds people have suggsted and generally finish up with a two piece cutter.

You can use an indexable endmill for trochoidal and other HSM paths. Here is someone from Seco talking about it, for example:

http://www.mmsonline.com/articles/th...l-milling.aspx

Cheers,

BW

[Donkey Hotey]

In my case, the preference for plunge milling had to do with the part. The parts were clamped shallow in the vise. As such, they wouldn't take really agressive side milling without the possibility of moving. They also had thin webs that would have deflected or permanently bent if I had been pushing into them.

With the plunge milling, it would be pushing the part down into the vise and as advertised, all the load goes into the strongest axis of the machine.

And since when did insert mills not do side milling (trochoidal)? I've got a couple of really nice 3/4", two-insert mills that I use all the time.

[Geof]

Okay, I will qualify my comments.

Trochoidal with very small internal radii is probably less feasible with inserts mills than endmills; I doubt whether you can get a 1/4" diameter insert mill.

What I was getting at is that a company like Kennametal probably has a greater vested interest in pushing plunge milling while a company that is focused mainly on endmills has a vested interest in trochoidal.

The old 'if your only tool is a hammer then all the problems can be fixed by nails' syndrome; or something like that.

Each probably has 'best' applications, but I doubt that either is a panacea. It would be interesting to do a direct comparison on something that could be done either way to see which was the most effective, and to keep davereagan happy we will include Varimill.

By 'most effective' I mean the total cost for finishing the job all the way through including programming time, fixturing/setup time, roughing and finishing and cost of tooling consumed. Also, maybe, factor in a contingency sum because overdoing it with an insert cutter and wiping it out can be more expensive than just shearing an endmill off.

[dertsap]

plunge milling works good in hard to cut materials , and as pointed out parts that dont have a lot of side clamping pressure and face the risk of pulling out due to cutting force , depending upon the material my preference for most plunging would be a large kennametal U drill , well above any plunge mill , the u drill can handle the interupted cut and at the same time can be engaged into the material far more than a typical plunge mill .

insert tools aren't that great for trochoidal cutting mainly because of the depth of cut determines the efficiency , trochoidal cutting has a lot of air cutting time and cutting so much air produces poor results with shallow cuts , I tryed that type of cutting with an insert mill just the other day for a test , trochoidal with the same depth of cut against a typical high speed machining pass took three times the amount of time to remove the same amount of material . I find insert tooling is best at high speeds feeds and conservative cuts and depths , a large amount of material can be removed in an incredible amount of time with minimal load on the tool and machine , also its a case where even at extreme speeds a guy can generally save a tool if it blows an insert with minimal or no damage to the tool

[dertsap]

now you've got me thinking
usually my commons sense doesn't leak out too much but curiosity generally takes over and i choose to ignore my common sense , i was curious as to the torque required to do trochoidal cutting ,I figured it would be fairly minimal because its not a constant torque but spikes , my guinea pig was my homemade router table with a 30,000 rpm router . to be safe i tried a 1/4" depth of cut on aluminum first , i used a 1/2" variable with a .1 loop and a .01 cut at 120 ipm , no problem , so i tried mild steel , i had to slow down to 40 ipm while slotting thru , but the second pass as you can tell mid way thru the video was no problem at 120 ipm , I ran it twice with the same results
I can say that the machine is not normally capable of running anything on steel ( at least thats what I've always thought ) , I think that with the minimal engagement and the interupted cutting the tool doesn't have time to chatter itself to death , so on machines with low torque and less rigidity (boxway vs linear slides) I can see how that type of toolpath is beneficial to machines that aren't designed for hogging

[ame="http://www.youtube.com/watch?v=s1ftb_cA4nE"]YouTube - cutting steel[/ame]

[BobWarfield]

Think about how the cutters are rated for speeds and feeds. They have no idea how you'll use the cutter. They don't come stamped "warning: trochoidal tool paths only." So they have to pick some pretty worst case feeds and speeds to recommend, and try to balance them out against their marketing desire to sell something better than the next guy.

Consider the cutter engagement that happens every time your cutter goes around a corner, or just bulls its way through a slot:



You ramp up to 2x or more engagement, depending on the shape of the corner.

So if you can generate the right toolpaths, your cutters are capable of a lot more performance. The engagement is only one aspect. All that time out in the air to cool off is another.

Cool stuff!

Cheers,

BW