Trichordial In 304 Stainless

rokstarr999 · Dec 16, 2016

Trying the Trichordial option on a .750" thick 304 SST flange. I have to slot out a 7" slug out of the center of the flange.

.375 4 FL Pro Max Variable Helix .02CR End Mill

.250 DOC
15% Stepover
.0015 IPT
200 SFM

At these parameters it's an hour run time.

Can I double this with a Trichordial tool path?

Thanks in advance.

CG60 · Dec 16, 2016

Rokstarr
I used a similar approach a few weeks back probably on the very conservative side. My setup was a.500 EM, .750 deep 2300 rpm .016 stepover, full depth of cut. Worked great as I only need to machine .6875rd open slot 2 parts. I used this as a starting point in Feature Cam. Did have to keep the chips cleaned out of the way frequently. I am sure there are some on here that can give better specifics, but I don't get to use this strategy that often. HSM does seem to make endmills last longer. But don't forget it's still 304

GBeaman · Dec 16, 2016

Trochoidal was a great improvement to straight slot milling for me. I use EdgeCam to program these paths around 5 years ago. The evacuation of chips and less then full engagement of the cutter allowed for higher speeds, but more importantly deeper cuts. I say 5 years ago, because the new roughing paths called "waveform" in edgecam are similar to many other highspeed tool paths. They run a constant cutter engagement and do loops in corners to avoid complete tool burial. This tool path has eliminated my need for trochoidal. All of this depends on material shape removal, tool entry and chip evacuation. Your cutting parameters aren't off much. I usually start at a lower SFM for 304 and work up to where I am comfortable. I usually nominally run 1200-1500 RPM with 3/8 EM in 304 120+ SFM.

What software is generating your tool path? If it is in the center, are you drilling a start hole and then entering there? That's what I'd do. Then I'd bury the endmill to .850 deep and flood the crap out of it. If your speeds and feeds are a bit slower it won't matter because you can take 3x the depth of cut. Full depth will allow your chips to evacuate. Of course I'm picturing suspended in a chuck or off the table on blocks. I hope this is helpful. I feel that many others here have better advice, but this is my best stab at answering your question.

apoc_101 · Dec 16, 2016

yea that "waveform" type of toolpath is akin to the HSM "adaptive" toolpaths. they work great and you can push a much greater width of cut (as long as you've got enough flute depth engaged to maintain a consistent tool load).

use a big tool with variable pitch flutes, and go get 'er. the only things limiting your MRR will be workpiece rigidity, spindle horsepower, some other minor variables. unless you're forced to use that 3/8 endmill cause that's no fun. 304 is easy to fly through with the right approach.

Mtndew · Dec 16, 2016

rokstarr999 said:
Trying the Trichordial option on a .750" thick 304 SST flange. I have to slot out a 7" slug out of the center of the flange.

.375 4 FL Pro Max Variable Helix .02CR End Mill

.250 DOC
15% Stepover
.0015 IPT
200 SFM

At these parameters it's an hour run time.

Can I double this with a Trichordial tool path?

Thanks in advance.

Go full depth with your endmill (yes, full depth)

10% stepover
300SFPM
.0025" IPT.

rokstarr999 · Dec 16, 2016

GBeaman said:
Trochoidal was a great improvement to straight slot milling for me. I use EdgeCam to program these paths around 5 years ago. The evacuation of chips and less then full engagement of the cutter allowed for higher speeds, but more importantly deeper cuts. I say 5 years ago, because the new roughing paths called "waveform" in edgecam are similar to many other highspeed tool paths. They run a constant cutter engagement and do loops in corners to avoid complete tool burial. This tool path has eliminated my need for trochoidal. All of this depends on material shape removal, tool entry and chip evacuation. Your cutting parameters aren't off much. I usually start at a lower SFM for 304 and work up to where I am comfortable. I usually nominally run 1200-1500 RPM with 3/8 EM in 304 120+ SFM.

What software is generating your tool path? If it is in the center, are you drilling a start hole and then entering there? That's what I'd do. Then I'd bury the endmill to .850 deep and flood the crap out of it. If your speeds and feeds are a bit slower it won't matter because you can take 3x the depth of cut. Full depth will allow your chips to evacuate. Of course I'm picturing suspended in a chuck or off the table on blocks. I hope this is helpful. I feel that many others here have better advice, but this is my best stab at answering your question.

I'm using Feature Cam and yes I started with a .515 drilled hole. I think I'm starting to get it. The Trichord increases your depth of cut and not so much your SFM.

rokstarr999 · Dec 16, 2016

Mtndew said:
Go full depth with your endmill (yes, full depth)
10% stepover
300SFPM
.0025" IPT.

This will be fun. Will give it a try, thank you.

Matt@RFR · Dec 16, 2016

rokstarr999 said:
I'm using Feature Cam and yes I started with a .515 drilled hole. I think I'm starting to get it. The Trichord increases your depth of cut and not so much your SFM.

No, it allows you to increase everything but stepover, which decreases to somewhere around 8-12%. Here's a video of us in 304 at 600 SFM, no air blast. Don't wuss out or you'll never learn what is possible. Worst case scenario... you break a $30 endmill. That's cheap knowledge.

Imco HSM in 34, Haas VF-2ss - YouTube

And by the way, it's spelled trochoidal. Most people here call it HSM, or High Speed Machining.

GBeaman · Dec 16, 2016

Just to clarify. As far as I know there is no reason to run dry in stainless. The more coolant the merrier. I also think that the 600sfm video is set up at much less then 10-12% step over.

Another benefit of using full depth of endmill is that I you get much more use out of one endmill as you were going to bury .25 deep and kill the first 1/4" of flute. Now you can kill the whole length and remove at least 3x the material.

Atomkinder · Dec 16, 2016

Another vote for HSM toolpaths. We run 1000SFM or more on mild steel (with a 1/2" EM), 10% stepover, around .0055/flute and tool life is great. We do very little stainless so not much HSM experience there but it's the first thing I turn to.

CG60 · Dec 16, 2016

Matt@RFR said:
No, it allows you to increase everything but stepover, which decreases to somewhere around 8-12%. Here's a video of us in 304 at 600 SFM, no air blast. Don't wuss out or you'll never learn what is possible. Worst case scenario... you break a $30 endmill. That's cheap knowledge.

Imco HSM in 34, Haas VF-2ss - YouTube

And by the way, it's spelled trochoidal. Most people here call it HSM, or High Speed Machining.

Matt
I like your setup in the video. I knew there was a lot to be gained with these techniques. Doesn't appear that you are having any problems with the material sticking or welding to the endmill. I will have to apply some of this next stainless job. Thanks for sharing.

XD341 · Dec 16, 2016

GBeaman said:
Just to clarify. As far as I know there is no reason to run dry in stainless. The more coolant the merrier. I also think that the 600sfm video is set up at much less then 10-12% step over.

Another benefit of using full depth of endmill is that I you get much more use out of one endmill as you were going to bury .25 deep and kill the first 1/4" of flute. Now you can kill the whole length and remove at least 3x the material.

Wha?! Yes run dry, use an air blast if possible not for cooling reasons just to remove swarf. I even run indexable tools dry in SS, thermal shock is a killer of the harder grades of carbide that typically run in stainless applications. Get it hot and leave it hot.

As for solid carbide...look at Niagara. Some of the 5 and 6 flute stuff in stainless is so much better than everyone else it's actually hard to believe.

GBeaman · Dec 16, 2016

Wha?! Yes run dry, use an air blast if possible not for cooling reasons just to remove swarf. I even run indexable tools dry in SS, thermal shock is a killer of the harder grades of carbide that typically run in stainless applications. Get it hot and leave it hot.

Okay, great. I thought the video was dry to highlight the tool path. I learned something new. I usually do when I am here.
I was always afraid of chip welding and work hardening the material. Never have tried to cut 304 dry on purpose.

Sorry if I confused the thread.

Hazzert · Dec 16, 2016

The only time I have experience any significant chip welding is with indexables finishing the floor of pockets relying on air blast alone . I'll normally turn on coolant for the finishing pass or at the very least smear some cutting oil on the surface.

robstah · Dec 16, 2016

GBeaman said:
Okay, great. I thought the video was dry to highlight the tool path. I learned something new. I usually do when I am here.
I was always afraid of chip welding and work hardening the material. Never have tried to cut 304 dry on purpose.

Sorry if I confused the thread.

With all the money you will save with this technique, I would invest in a MQL setup and ditch coolant completely.

apoc_101 · Dec 16, 2016

don't even necessarily need MQL unit if you or your machinist is attending the cutting operations, air blast clears the chips and excess heat, and operator hand-sprays some excellent fluid on the too/cut zone in the finish bottom faces or other trouble areas. for steel and stainless I'd recommend Unist 2210EP... there isn't a better fluid in my experience.

Good way to try out MQL if you're not convinced. Unist will even send you a free bottle to try it yourself. (ask for their aluminum product too, it's fantastic!)

Matt@RFR · Dec 16, 2016

GBeaman said:
Okay, great. I thought the video was dry to highlight the tool path. I learned something new. I usually do when I am here.
I was always afraid of chip welding and work hardening the material. Never have tried to cut 304 dry on purpose.

We cut dry on purpose, but it has very little to do with material and nearly all to do with SFM. This is from knowledge gained here, not by trial and error, but anything below 500 SFM on steels uses coolant, anything above is dry. The theory being that carbide does not like heating / cooling cycles and can crack from it, and coolant at 500 SFM and above can create those cycles every time a flute comes out of the cut and is hit with relatively cold coolant. Obviously 500 SFM is a massive generalization, but without the time to actually test these things, it has worked very well for us.

Chip welding and work hardening in this scenario is only going to come from either SFM being too high, chip load being too low or both. This is assuming good chip evacuation, of course. For these tool paths to work, you can't be afraid of your equipment, and you can't be afraid to break stuff while learning. Yeah you can rip around at 1,000 SFM, but if your chip load is too small, your tool won't last for shit. I've had to back off SFM on some things because the feedrates required for good chip loads were not doable with my current control. With better motion control, I could up the SFM back to where I wanted it.

rokstarr999 · Jan 18, 2017

Atomkinder said:
Another vote for HSM toolpaths. We run 1000SFM or more on mild steel (with a 1/2" EM), 10% stepover, around .0055/flute and tool life is great. We do very little stainless so not much HSM experience there but it's the first thing I turn to.

Im assuming SFM affects chip load. I can't run faster than 7500rpm so 1000 SFM is out of my reach. How would you adjust chip load for a reduction in SFM?

Thank You

Finegrain · Jan 18, 2017

As I was recently taught

.003-.005" chipload, but that's with the small radial engagement chip thinning accounted for. A straight .005" chipload toolpath with low (5-10%) stepover will only be ~.0015" real chipload. Select the chip-thinning option in your CAM (RCTF in Mastercam) to get the right actual chipload.

Your 7,500 RPM is good for 982 SFM with a 1/2" EM, but I'd try 600-800 SFM first. You may find that your control won't give an accurate toolpath once you account for the chip thinning -- 7500 x .015" (estimate based on .005" actual chipload) x 4 flutes would be 450 IPM, pretty brisk.

Regards.

Mike

mkd · Jan 18, 2017

slotting-out a 7" slug???

I vote sanvik High feed cutter. You know, the ones that screw onto a shank.

a 3/8" could be a little pricey to start, but it can be programmed with a simple ramp @200IPM conservatively, and it won't brinel your ball screws.

Trichordial In 304 Stainless

Aluminum

Aluminum

Hot Rolled

Hot Rolled

Diamond

Aluminum

Aluminum

Titanium

Hot Rolled

Titanium

Aluminum

Hot Rolled

Hot Rolled

Stainless

Aluminum

Hot Rolled

Titanium

Aluminum

Diamond

Stainless

Similar threads