ISCAR Slitting mill feed suggestions wanted

Hi, I use one of these at my job.

https://www.iscar.com/eCatalog/item.aspx?cat=2300686&fnum=381&mapp=BO&app=0&GFSTYP=M&isoD=1



The tool is new. It's with ic908 inserts.

https://www.iscar.com/eCatalog/Grade.aspx?grade=IC908&item=6095389&fnum=229&mapp=BO&app=0

I can't find any feed recommendations. I need feeds for soft steel and austenitic stainless. Yes, we've used these a lot, and I do know what we normally use which would be 400rpm or 500rpm, F150mm/m or F300mm/m depending on the load. However I think there's room for optimizing.

Any suggestions welcome, also milling strategies.

So we have those in quite a few widths and diameters and one thing I found is that they like feed. You don't want to baby it.

I would start at 180M/Min on steel and bang the feed to 0.1/tooth (this is conservative). So on your 125mm that equates to about 460RPM and about 370mm/min. Then see what the chip looks like, you do have a thin blade at 3mm and they are crazy expensive so you don't want to blow it up but that is a decent start point.

Don't have too much experience slitting stainless but on IC908 I am guessing that the M/min would be roughly 80.... but feed similar to 0.1/tooth

NAST555 said:

So we have those in quite a few widths and diameters and one thing I found is that they like feed. You don't want to baby it.

I would start at 180M/Min on steel and bang the feed to 0.1/tooth (this is conservative). So on your 125mm that equates to about 460RPM and about 370mm/min. Then see what the chip looks like, you do have a thin blade at 3mm and they are crazy expensive so you don't want to blow it up but that is a decent start point.

Click to expand...

Thanks for a good reply. I have the 3mm and the 6mm variants. What I did for the last job was I set it to 200M/Min (2172, soft steel) (510rpm) and took the recommendation for HSS slitters (0.04/tooth) and doubled it (.08), ending at F325.

It worked fine. I tried F400, that worked fine too. As you said tho these are expensive and I don't want to run into trouble caused by my poor experience. You'd use these values regardless of width of cut? I cut 20mm with this, max is 34. Our shop's programs have that feed at F150 (i.e. for max width), which would be, as you call, excessively babying it. (Also mostly S400.)

What I have found is that it likes full slotting rather than side cutting. so If you need to side cut maybe try to work it out that you can full slot as much as possible...

If you mean depth of slot your only issue is getting the chips out of the cut, it is why I suggested to run it hard to get it out of the cut as quickly as possible. I run a 5mm one like yours dry at 0.12FZ at 150mm/min and it kicks butt.

NAST555 said:

What I have found is that it likes full slotting rather than side cutting. so If you need to side cut maybe try to work it out that you can full slot as much as possible...

If you mean depth of slot your only issue is getting the chips out of the cut, it is why I suggested to run it hard to get it out of the cut as quickly as possible. I run a 5mm one like yours dry at 0.12FZ at 150mm/min and it kicks butt.

Click to expand...

Thank you, that's exactly what I was looking for, and matched my instinct for what would be right. I don't want prolonged tool engagements. If you cut fast enough the workpiece won't have time to get angry at you.

(Yes I meant depth of slot.)