Has anyone had success machining 304 stainless steel on their MR1?
I tried recently but encountered heavy vibration that forced me to stop the job. I’m wondering if this material is too tough for the MR1, or if I just need the right tooling and cutting strategy.
Any advice on recommended end mills, feeds, and speeds would be greatly appreciated.
Thanks!
Contact Richardbeck83 on this forum or Facebook. I think he has experience with Stainless steel on his MR1.
What coolant are you using? What speeds/feeds? What cutter? Any coating on the cutter? Depth of cut? Stepover? Etc…
The cutting parameters worked fairly well for me, but was able to tweak them on some coated endmills with a few more flutes.
Hi Jellis,
I used the Fusion Cool 2240 flood coolant with the Langmuir-supplied 1/2-inch, 4-flute, non-ferrous cutter. I ran it with a 1mm depth of cut and a 2mm step-over.
The cutter started to turn red, and the vibration was pretty concerning.
Let me know if you need any other information.
Thanks!
Safe to assume you’re just facing? What speeds and feeds are you using?
I’ve found because of the MR-1 limitations a 5 flute with a AlTiN coating worked best for me.
t looks like the other picture didn’t go through, so I’ve added it here. We were facing the part down about 1mm with a 30% step-over using a 4-flute ferrous end mill. I can see the end mill was glowing red, which is a bad sign, and the sound was horrible.
When you machine stainless steel, does your MR-1 vibrate noticeably? I assume you’re using an end mill specifically for stainless steel. Could you send me any modifications you made to your stainless steel preset? I’d like to try it again with a different bit.
I was tweaking mine at the controls but I believe my starting point was 2500 RPM and 20 ipm. Keep in mind, some people say less is more, but sometimes more is more.
Your depth of cut and stepover look fine.
Yes, there was some noticeable vibration early on. But once everything was dialed in it lightened up.
Yeah, the 5 flute AlTiN coated endmill was meant for harder metals like a stainless.
Ive done lots of 304 and its very tricky. Thats not necessarily an MR1 thing, but just how it fights you in general.
First, if you see sparks, youve already hardened the part by rubbing. The horsepower and rigidity issues with small mills make 304 a pain. “303, shes for me. 304, shes a whore”. Max out the coolant, right at the tip of the endmill. Try reducing the depth of cut but INCREASING the chip load. If you traverse across the part more quickly while cutting larger, thinner chips, you can keep more heat out and get a good finish. The problem there is horsepower, so you have to do some practice cuts on scrap. Ive trashed lots of non-coated endmills playing with 304. Also, some other folks here might be able to speak to this better than I, but 304 wildly varies. I bought some pieces from some rando on eBay and it cut totally differently than a piece I got from McMaster. Then I got a piece of known 304 from a local vendor and it cut differently from both. So, thats 2 sources that can be trusted, one that might not br. Im no expert and Im sure I made changes to each cut, but the differences were obvious between the 3, even though they were all “304”.
Also, to reiterate, if you see consistent sparks, your feeds and speeds are off or you have already hardened the material from rubbing. I bet after the first 2 or 3 seconds of sparking, you can see the wear on your endmill with the naked eye. Expect some loud squealing, thats the nature of the material. I cant cut stainless without hearing protection.
I was never able to get very aggressive with 304 on my mill. I ended up doing lighter depths of cut with a higher step over to save machine time. Any time I tried loading up the tool I got some vibration and I kept worrying I’d stall the spindle. Having stalled it once before with a Woodruff cutter, I learned then that the machine will keep trying to feed even if the spindle drive kicks off.
Thanks, all!
I will give this another try using your suggestions above.
The problem I think you might run into is that you need to take a good size chip at a low SFM. I have had problems with the MR-1 having the needed HP at 1500 rpms. If your cut is too shallow with SS it will work harden and then shit goes bad at and exponential rate. You’ll prolly stall the spindle if you try to run the needed feeds and speeds for 304 if you’re using a 1/2" endmill. So I would recommend going to a smaller endmill.
Try this endmill with the feeds and speeds recommended by Hass Tooling.
1/4" Dia. Carbide End Mill, 6 Flute, Hyb. AlCrN Coated, 1/4" Smooth Shank x 3/4" LOC, 0.03" Radius, HEPM
It has a variable pitch to reduce vibration, the coating needed to cut ss, and extra flutes to make up for the lost time due to using a 1/4" endmill.
It also has chip breakers which will help the chips stack up slower in your machine. It looks like you need around .050" step over with .0023" to .0027" Chip load. They claim this coating will allow up to 700 sfm. I wouldn’t do that but I would at least get the spindle up around 4k rpm. Use full flood coolant.
Also is says you can run .05" step over at .75 deep. If you are going to take a shallow cut make sure you take the full .0027" chip load.
The worse thing you can do with SS is take shallow cuts with slow feeds and high rpms.
I have run this endmill in mild steel even though it’s rated for SS. I removed 15 pounds of steel with 1 of these 1/4" endmill and it was still kicking ass and taking names. I also used this endmill to cut the laser cut edge of some steel which normally destroys endmills.
This.
Granted my machining experience is from a Tormach 1100, and I’ve slept since then, but stainless is counterintuitive. You need to take a deeper depth of cut for a given pass to get underneath the work hardened outer layer from the previous pass. You need to use FLOOD coolant and it is highly beneficial to run carbide with a slick coating like TiN or TiCN. It also helps to have a spindle with significant rigidity, which I know the MR1 doesn’t have the best, so that you can plunge harder (deeper cuts) into the work.
Shallow cuts and/or high RPM= work hardening, and once you’ve started, your tool will dull and it’s over (for the most part). If you see sparks, HIT THE ESTOP.
I always kept a 1/2" (which I know is asking too much from the MR1) rougher that was a 4 flute, TiN coated at the ready for heavy cut rate jobs and stainless. For the MR1, find a good 1/4" or 3/8" 4 or 5 variable pitch flute rougher, and spend some money on a good workhorse tool. Once you get the speeds n feeds down (and relax the clench when you realize they actually work), they’ll run almost forever, esp on aluminum.
Thanks so much for this information, I’m placing the order for the endmill and will try it!
yeah, I double checked the math with my feeds and speeds app and it’s showing that you would need 2.4hp to run a 1/2" endmill in 304ss. So if you go with a 1/4" endmill you’ll have plenty of hp to increase the chip load.
Thank you! Which app do you use for this sort of thing if you don’t mind me asking?
Thank you! Which app do you use for this sort of thing if you don’t mind me asking?
I use this app when I’m not sure where to start. It’s not perfect but it’s a great starting point. FSWizard: Speeds and Feeds They have a mobile app as well.
Haas says to run their end mill a lot more aggressive than the FS wizard does. So there is still risk and using your best judgment. I like the hp calculation that FS wizard has. That is just math that is pretty settled. It does it for you. I’ve stalled the MR-1 spindle enough times that I don’t bother with anything over 3/8" unless I need to bore a large hole 2" + deep. lol
once you buy from Haas Tooling you can leave a review of the product you purchased and they will send you a $50.00 coupon you can use on your next order. If you buy over $100.00 shipping is free. haha I ended up getting a bunch of those endmills using my coupon and free shipping. It ended up being less than $10.00 each. 
Awesome! This is helpful, thanks for all the info!
Keep us posted on results too!
