[dneisler]

Ok, I love my Tormach, but so far I have only cut, acetel and 6061, and 7075 aluminum. So, not i need to mill some 1/2" 304 SS.

1. What tool to use, I was looking at some 1/2" 5 Flute Carbide endmills from MSC, but not sure that is the best to use, suggestions?
2. What feeds and speeds to start with. I am not 100% used my gwizard much and do not trust it 100% yet. I can make it say a large variations of F&S.
3. I have a C/T tapping head from tormach, and never used it, I would to tap some M10x1.25 holes in this SS. How would I code that in HSMWorks Express?


Suggestions?

[zero_divide]

Choise of tooling depends on what you want to do with it.
If side milling a 5 flute will be ok i guess.

I would suggest a coated variable flute 3 or 4 flute endmill for general machining.
Try to not do any slotting.
Use coolant with high concentration.
Aim at ideal chipload, reduce the depth of cut if load is too much.

My FSWizard suggests 200 sfm and 0.002 ipt chipload
At slotting depth of 1/8".

[dneisler]

I will be doing a outside profile, and inside pocket that is pre-drilled. I realy have no idea, I just saw that 5 flute increased the feedrate, so I am open to any suggestions.

[zero_divide]

I will be doing a outside profile, and inside pocket that is pre-drilled. I realy have no idea, I just saw that 5 flute increased the feedrate, so I am open to any suggestions.

5 flute is a really bad idea on stainless unless you are making very light profiling cuts maybe up to 15% radial.
I would go with 4 flutes

[RussMachine]

Ditch the 5-Flute, and go with 4-Flute, Coated Carbide.
Use coolant, and feed it as fast as your machine can handle, DON'T Feed too slow as Stainless likes to work-harden.
I'd feed it at a minimum of .004 (.001 per flute). Then Bump it up as you can.
If you plan on tapping, Tormach recommends long-hand programming instead of using G84, as the machine doesn't support rigid-tapping.
I just tapped some 1/4-20 blind holes with the ER20 T/C head, and it worked like a charm.

[sperman]

You will probably find that GWizard recommends F&S that are faster than the machine can handle. At least that has been my experience. It's not a HP problem, but a rigidity problem.

[fizzissist]

Get yourself some Dataflute carbide endmills, 3 flute, run them at about 300SFM to start, and follow the mfg's recommendations for feed. Contrary to other suggestions here, run it dry with a good air blast (for chip clearing) for longest tool life.
Run the tap wet, and use a GOOD tap, not some cheapo from Harbor Frate. OSG and Emuge make some great taps for 304, and Emuge's tech support has been awesome for me. (try 180 blind 0-80 holes in 304SS for fun)

I've run a lot of 304SS (dual cert) and it's no big deal. It will work harden, so you have to be more aggressive and not let the tool dwell. Rigidity is also an issue, and I don't know anything about your setups, or your Tormach.

There are some other great endmills for this material, but I tend to like these..I also recommend the .010-.030 radius'd edges, both for finish and for edge integrity.
http://www.dataflute.com/catalogs/dataflute/DFSSI.pdf

[Steve Seebold]

I hate 304 stainless steel. I would rather machine inconel or titanium than 304. At least with those, you know what you're up against. I have cut 304 in a real CNC in the past, and it has to be the most unpredictable material I have ever cut. You can cut 10 pieces off the same bar, and every one will machine different.

I found that carbide doesn't work that well on 304. I had better luck with 4 flute cobalt end mills.

[fizzissist]

I hate 304 stainless steel. I would rather machine inconel or titanium than 304. At least with those, you know what you're up against. I have cut 304 in a real CNC in the past, and it has to be the most unpredictable material I have ever cut. You can cut 10 pieces off the same bar, and every one will machine different.

I found that carbide doesn't work that well on 304. I had better luck with 4 flute cobalt end mills.

Well, I've machined thousands of parts out of 304SS, on "real" CNCs.... And I'm here to tell ya that if carbide doesn't work for you, you're using the wrong carbide, you're programming it wrong, or your machine isn't rigid. Never mind the quality of the material you've procured.

Most of the parts I've made have been on a Fadal 4020 or a Mazak SQT 250M, but I've also run it on a Haas VF3, VF5, and cam type automatic screw machines.


Everything is 304, and the tapped holes in the gas cell on top are blind 0-80's

[MichaelHenry]

And I'm here to tell ya that if carbide doesn't work for you, you're using the wrong carbide, you're programming it wrong, or your machine isn't rigid. Never mind the quality of the material you've procured.

What carbide tooling do you recommend for 304SS on a machine the size of the Tormach?

Mike

[Just Me]

All Carbide tools are not the same...for SS use a 37* helix... 6061 uses a 45* helix...A cornerround of .02 will last longer for roughing than a square corner...this is the part of the tool that breaks down first...Use a 3 flute tool for pocketing & slotting....use a 5-6 flute tool for profiling...Also don't use a 1" flute if your olny machining 3/8 deep...

[fizzissist]

What carbide tooling do you recommend for 304SS on a machine the size of the Tormach?

Mike

It's not the "size" per se. It's horsepower, spindle speed, rigidity, and available feed rates that determine the size of the tools.
You want to engineer the tooling so that it is operating within its best parameters in terms of SFM and feed that the machine is capable of.

ie... you can use a 1" endmill if you don't have the RPM capability to make the SFM recommendations, but you don't want to spend $100 on a tool.
You'd like to use a 1/4" endmill and save money, but you can't get the RPMs high enough....
Sucks to be a machinist, don't it?

Small shop guys also want to use a single tool for everything. As Just Me points out, there's different geometry for different materials and applications, along with different coatings. Long past are the days when a handfull of 883 carbide in your box would do just fine.

[Spinnetti]

All, that said, the practical approach is to look at the tools you have on hand or are willing to buy, and optimize feed and speed for the material you are cutting.... I think G-Wizard gives mostly decent starting points, but always end up tweaking from there. All this assumes the basics are covered.. keep your holders, cutters etc short as possible to keep bending moments down and hold the work well....

[MichaelHenry]

All Carbide tools are not the same...for SS use a 37* helix... 6061 uses a 45* helix...A cornerround of .02 will last longer for roughing than a square corner...this is the part of the tool that breaks down first...Use a 3 flute tool for pocketing & slotting....use a 5-6 flute tool for profiling...Also don't use a 1" flute if your olny machining 3/8 deep...

What about coatings for SS304 - are there any to definitely get or others to stay away from?

Fizz - I've no problem buying tooling specific to the material or the task, just a little fuzzy on what's best/good for SS. For end mills, who is a good vendor? I usually buy from Mari Tool, Lakeshore Carbide, or McMaster-Carr.

[dneisler]

I don't have any tooling other than stuff for Alum so I will be buying all new. Here is what I am thinking for tooling and F&S take from Gwizard Conservative side. Please, I am open to suggestions. I would like to not break any $40 end mills.

Lake Shore Carbide - 1/4" 90 Deg Single End Carbide Spot Drill
* CenterDrill - .2 DOC 1.0 IPM 2050 RPM

PTD - Stubb Drill, Carbide 5.5mm
* Drill - .6 DOC 2.0 IPM 2800 RPM

PTD - Stubb Drill, Carbide 1/2
* Drill - .6 DOC 2.0 IPM 1300 RPM

Lake Shore Carbide - 1/2 - 4 Flute End Mill - Corner RAdius .015 - ALTIN
* HSM 2D Adaptive - Outside Countor - .52 DOC .05 WOC 6.0 IPM 1750 RPM
* Profile - Outside Contour Finish - .52 DOC .01 WOC 6.0 IPM 1750 RPM
* Pocket Pre Drilled Entry - Inside Pocket - .05 DOC .5 WOC 4.5 IPM 2100 RPM

[LSM]

You start running out of hp on a .500 em in 304, and the brand you chose makes a difference.
I used to buy the cheap carbide tools they would chip real fast, went to the guhring firex variable helix for stainless,
they cut faster and last much longer.
stick with a 3/8 or 5/16 they are cheaper and it keeps the machine happier.
304 will eat tooling though.

[zero_divide]

I don't have any tooling other than stuff for Alum so I will be buying all new. Here is what I am thinking for tooling and F&S take from Gwizard Conservative side. Please, I am open to suggestions. I would like to not break any $40 end mills.

Lake Shore Carbide - 1/4" 90 Deg Single End Carbide Spot Drill
* CenterDrill - .2 DOC 1.0 IPM 2050 RPM

PTD - Stubb Drill, Carbide 5.5mm
* Drill - .6 DOC 2.0 IPM 2800 RPM

PTD - Stubb Drill, Carbide 1/2
* Drill - .6 DOC 2.0 IPM 1300 RPM

Lake Shore Carbide - 1/2 - 4 Flute End Mill - Corner RAdius .015 - ALTIN
* HSM 2D Adaptive - Outside Countor - .52 DOC .05 WOC 6.0 IPM 1750 RPM
* Profile - Outside Contour Finish - .52 DOC .01 WOC 6.0 IPM 1750 RPM
* Pocket Pre Drilled Entry - Inside Pocket - .05 DOC .5 WOC 4.5 IPM 2100 RPM

Here are some screenshots i made for some of your tooling*.
Imo your calc is too light on the feedrate.
Sfm for drillig seems a it high to me and feed is a little low.
For HSM milling your feed is way too low.
Same thing with slotting. Chipload is very low.

Anyway please do run the parts and tell us how it went!

Attachment 218102Attachment 218104
Attachment 218106Attachment 218108

[dneisler]

Well this was with g wizard at its most conservative setting

Sent from my SM-N900V using Tapatalk

[zero_divide]

Well this was with g wizard at its most conservative setting

Sent from my SM-N900V using Tapatalk

The problem with it is that there is a "gas pedal" that controls both cutting speed and feedrate at the same time.
It is easy for newbies, but say you want to just reduce cutting speed and leave chipload alone?

Too light of a feedrate will cause rubbing. Could work in aluminum, but in SS it will be a disaster. Trust me.
For your case taking such light cuts you will be fine just leaving chipload untouched, but reducing cutting speed by 25%.... Just in case.

Make sure you have some sort of coolant going at least for drilling.