What's new
What's new

Slitting Saw Feeds and Speeds Stainless

yorkypoo102

Plastic
Joined
Dec 6, 2022
Looking for some feed and speed advice for using a slitting saw in 304 stainless, general toolpath advice is also of course welcomed.

I have a roughly 10" diameter, 1/4" wall stainless tube that I need to part off into rings using a Haas VF-2. A lathe would be ideal I know, but we dont have one large enough. To prevent the finished rings from flying around I've left some tabs.

Im using a 2.75" OD 1/16"thk 56T HSS slitting saw from Malco saw company (McMaster-Carr) with a vibration dampening 1" arbor. Cutting parameters were 350rpm (252 SFM) and 1.8 inch/min feed. The cut started pretty clean, but by the end of the test the saw was dull and the part was burning. Flood coolant was used, and the tool was basically submerged. I would adjust the rpm or feed up or down by ~20% if it started to get noisy. I've attached images of the tool path and results (note, I did a test pass with a thinner ring to not waste material). Here is an imgur link that has video with sound during the cut.

Looking at the images, it looks like the weld seam caused the failure. While that is a possibility, the burning and noise started a few inches before it. Maybe heat from welding made that area harder, but Ill need to get through it regardless.

I'm gathering quotes for solid carbide and carbide tipped saws now, which sucks as I only really need to make 5-6 passes. Is carbide necessary or is this user error?

Thanks!

1675874665143.png
 

Attachments

  • IMG_1291.JPEG
    IMG_1291.JPEG
    635.1 KB · Views: 29
  • IMG_1294.JPEG
    IMG_1294.JPEG
    729.8 KB · Views: 32
  • IMG_1295.JPEG
    IMG_1295.JPEG
    740.8 KB · Views: 28
  • IMG_1296.JPEG
    IMG_1296.JPEG
    435.9 KB · Views: 27
  • IMG_1297.JPEG
    IMG_1297.JPEG
    754.6 KB · Views: 25
  • IMG_1299.JPEG
    IMG_1299.JPEG
    797.2 KB · Views: 27
It's not a maybe about your weld joint. Expect it to always be harder than surrounding area.

Have learned the lesson about burned up slitting blades a while ago. Too fast or too much depth of cut.
I'm also cranking by hand which is probably the next best way to mess up a blade.

After looking at your second picture I am a little relieved about how my worn out blades look. Just like yours.
The relief is that nothing is wrong with my saw holder. It's not fancy like yours, made it from a solid bar.
 
Last edited:

You should be down around a painful 20-30 SFPM. People tend to run slitting saws way to fast and destroy them instantly because the diameter is larger than the typical end mill. 2.75" saw should be starting at about 30 RPM, if you can do it.
Ouch, painful indeed. I can give it a go, but may be up in the 80-120 SFM with a carbide saw to getthrough that weld. Thanks for the data sheet, I wasnt able to find that.
Would I drop the feed to maintain the feed per tooth, or am I taking to light of a cut here?
It's not a maybe about your weld joint. Expect it to always be harder than surrounding area.

Have learned the lesson about burned up slitting blades a while ago. Too fast or too much depth of cut.
Noted, will likely go with carbide. When you say too much depth of cut, are you talking radially? It is my understanding that full depth is best for chip evacuation. If im running too high of an rpm as Conrad has pointed out, perhaps my feed per tooth is too light.
 
Ouch, painful indeed. I can give it a go, but may be up in the 80-120 SFM with a carbide saw to getthrough that weld. Thanks for the data sheet, I wasnt able to find that.
Would I drop the feed to maintain the feed per tooth, or am I taking to light of a cut here?

Noted, will likely go with carbide. When you say too much depth of cut, are you talking radially? It is my understanding that full depth is best for chip evacuation. If im running too high of an rpm as Conrad has pointed out, perhaps my feed per tooth is too light.
No, just a straight cut.

I stopped using saw blades like this in woodworking a long time ago. Only good for rough cutting. All the good blades are the right grade of carbide.
It should be the same for metal. Unfortunately I have not done enough small slitting stuff to graduate from HSS.

I think you know more about this than I so I will pass the torch.
 
I am also just noticing that the spec sheet says .002-.006" per tooth feed. Can this really be the case for such a high tooth count (56)? 5in/min seems pretty quick for 40 rpm. 1/8" per turn.
I think you know more about this than I so I will pass the torch.
Dangerous assumption to make 😁
 
We used to anneal 303 Se stainless parts by heating them to 2000+ degrees and quenching them in water.
Are you guys certain the weld in 304 is harder? I would have expected softer. That said annealed 304 is more difficult to machine than when it is moderately cold worked.
 
Okay, so likely just running too fast and taking too light of a chip load, which can be solved by slowing rpm. Maybe a HHS will work after all, worth the $30-$40 to find out im sure.

This makes sense. I copied the slitting feeds and speed for 304 off of another post, but Im now realizing he never stated his tool material. It was most likely carbide, and being that all of the other tooling I use on a regular basis is carbide the high SFM didnt jump off the page at me like it should've. Chalk it up to inexperience.

I'll try the recipe from the pdf you sent and report back when I've made a cut.

Thanks everyone!
 
Actually, while I'm at it. is high or low tooth count better for stainless? I can adjust for a consistant feed/tooth regardless, but I'm sure theres a right and wrong.
 
Actually, while I'm at it. is high or low tooth count better for stainless? I can adjust for a consistant feed/tooth regardless, but I'm sure theres a right and wrong.
I'd shoot for a "middle" tooth count, which in this case might be 6 - 8 per peripheral inch. Not fine like a jeweler's blade, or coarse like an Al cutter. Shoot for engagement such that two or three teeth are always in the cut, max of four (these are my guesses, someone like CB would have better insight).

Chip flushing is critical, if you don't think you can be sure of constant coolant impingement then err on the side of coarser teeth and slower feed.
 
I am thinking that slotting from the outside would lessen tooth contact and loading of the teeth with chips. If you have to go carbide contact Southern Carbide, they used to sell direct, I think they still do.
One other thing to look at would be https://watkinssaw.com/ cutters. They have angled edges for production cut off use on lathes.
 
Last edited:
AFAIK, heat doesn't harden 300-series stainless, only cold working does. Also makes it magnetic!
It might be a case of "non-L" 3xx having enough free carbon to precipitate out as chromium-carbide after welding. Or something...

Edit: here's a link to the phenomena:

 
Last edited:
I can't help with the slitting saw parameters. But why not just band saw off the ring, clamp it, and clean it up? Or sub it out to someone with a lathe? I thought maybe it was something special of a material, but that looks like shop rolled flat bar welded into a tube. It would be grossly wasteful of material, but a 10" ring laser or waterjet cut from from plate at the end of the day seems like it would be cheaper and easier...?

sendcutsend.com has online parts designer. 10" OD / 9.5" / 1/4" thick ring is $95.22 qty 1. $57.20 qty 10. going to 1/2" thick is $205.90 qty 1 and $123.54 qty 10.
 
I can't help with the slitting saw parameters. But why not just band saw off the ring, clamp it, and clean it up? Or sub it out to someone with a lathe? I thought maybe it was something special of a material, but that looks like shop rolled flat bar welded into a tube. It would be grossly wasteful of material, but a 10" ring laser or waterjet cut from from plate at the end of the day seems like it would be cheaper and easier...?

sendcutsend.com has online parts designer. 10" OD / 9.5" / 1/4" thick ring is $95.22 qty 1. $57.20 qty 10. going to 1/2" thick is $205.90 qty 1 and $123.54 qty 10.
Water jetting was my first idea too. We're making a handfull of these rings, and they have lips on them so they can be re-stacked concentrically to make a tube of varying and precice length, so each ring will be different length to give us some variability (like weight plates being added to a barbell).

The diameter of the stack is important, so we will be machining the OD of multiple rings before parting them to ensure they're the same. After theyre all parted we can flip and do the backside machining without changing the OD.

We could do it on a lathe, but we would have to do it externally and money is pretty tight. Im also worried about them using a 3-4 jaw on this. We have 8 clamps on it currenlty and can already see some deflection in the part if not secured carefully.

As for the cost, since the rings cant be nested for water jetting, the cost went up pretty steeply with a lot of waste. Also they'll be around 3/4" thick in some cases. We had the tube rolled and welded for $90 and can get all the parts out of it.
 
Going back to the weld. The hypodermic tubing that I cut is also welded tubing. Hypo tubing is cold worked inside and out in multiple operations of annealing and cold working after it is welded. I have never seen any evidence of 2 materials in the millions of cuts that we have made. On the OP's example I would expect a different hardness on the weld, and that the process was controlled well enough that the material in the weld was the same as the rest of the tube.

Original post said the cutter burned up before getting to the weld.

Milland mentioned chip flushing, I to think that is very important with any sawing operation on stainless.
 
I've got a new saw, 3" OD HSS with a lower tooth count (30) because it was the only one available for same day pickup. I'll test again with a lower rpm and report back.
I've also adjusted the tool path to cut on the outside as per FredC's advice. As a researcher, changing multiple variables hurts a little but hey, as long as it works. Going with .002" per tooth as per this data sheet, still seems heavy but I dont have a lot of HSS experience.
1675970310914.png
 
Try and have as many teeth as possible engated in the cut. The last diagram above is non-ideal. You want to have the saw just barely clearing the inside of the cut. You want slow then you think, and faster feed than you think. Slow feed means you will be work-hardening the material while cutting it.
 
You can control how many teeth are engaged at one time by changing the how far the cutter penetrates your tube. My suggestion for the outside was thinking you had too many teeth engaged at a time and they were loading up with chips. With the 30 tooth cutter you could get hammering if there are not always three teeth cutting at a time.
 








 
Back
Top