Dan,
I was really talking you up a few weeks ago in South Carolina at a shop that was looking to purchase their first Swiss Lathe. I hope they purchase one from you guys as I know you personally could help them tremendously so they can compete at even a higher level. I contacted George and gave him the shop info.
I'm assuming it's on a Tsugami Swiss?
To summarize all of those parameters for those tools in that material at that Hardness, I would suggest to target the coating. Eifeler-Lafer out of St.Charles IL (go see them while setting up at IMTS) has a coating called Sistral. It was developed for hard milling & turning processes. It can handle more heat, something like 30% more than TiALN and can handle the shock that the hard materials can send back to the cutting edge fracturing most coatings.
formatting link
there is contact info on this site but the Sistral is so new I see now that it's not on there. Talk to them and they brochures they can send you on it.
The material composition leads you into how difficult this material will be to machine it. 17% Chromium-7% Nickel and some Manganese and Silicon, used in many "Spring Type" applications besides medical and aerospace. So it's going to twist and bend before letting go of any chips while you try to defeat it with your tooling. But let's take each tool and see what can be improved slightly.
On the 1" Endmill. I would assume the inserts are the more accurate Ground not Molded inserts ? Something that has a tolerance class of E or C. Like a molded insert would say APMT and the ground insert would be APCT refer to this link
formatting link
these inserts are ground to repeat and locate in the pocket more accurately and since they are ground to size they will slice through the material better too. In this instance the sharper tool would be great for slicing through the nickel and manganese. The hard coating will be good for the Chrome and Silicon, heat resistant and abrasion resistant respectively. If you are on a Swiss, I prefer to use a higher Helix (50 degree helix) 5 or 6 flute endmill so as flute # 1 is coming out of the cut, flute # 2 is in or nearly in the cut. This helps since in most Swiss machines the guide bushing is not clamped on the bar stock such as a vise would be holding a part in a mill, thus you are milling with a loose vise. So if the next flute is in the cut as the previous flute is exiting the cut, the tool doesn't take the shock of loading the material agains the side of the guide bushing once again. Most Insertable endmills will not kick the insert at that high of a simulated helix. I would look at possibly an Iscar Multi- Master screw-on tip endmill. They have them in larger diameters with multi flute, High Helix options. Talk to eifeler about putting the Sistral on it. Your current tool is running 200SFM at .003 Chipload which I would say is good safe place to start at with SFM but might be a bit too much on the chipload for the multimaster. Are the chips sticking to the insert at all? Have you ran this portion of the program dry ? Sometimes letting ALL of the heat go out with the chip is the way to go instead of trying to cool it while it's cutting.
For the 5/16" and 1/4" endmills, the 200 SFM again sounds fair to start at. I would make sure these endmills are made for the Mold Industry. That is, for Hard Milling applications. I have found that if the failure mode of a tool is that the material is work-hardening and the dull edge produces more rubbing action than preferred to the expected cutting action, then it's going to fail very soon after this point in time. However, if the substrate and coatings are designed for Hard Milling, even the hardness of the material won't contribute to the tool's failure as the tool is designed to cut in materials upto
70Rc. YG-1, OSG, Mitsubishi are just a few that produce these endmills.In essence you eliminated your failure mode.
On another note, and this applies to most all applications using ER collets. Look at the back of the collet and see how much of the actual diameter that is supposed to gripping the shank of the tool is actually counterbored which reduces the length that the shank is being held onto. See
formatting link
to see an example of this. Techniks is simply the brand I use to illustrate the concept. There are other brands such as Nikken that offer the same concept. But this idea gives you more gripping power, the tool runs more accurately UNDER LOAD WHILE CUTTING not simply when you are putting an indicator on it during setup. More tool life can be expected as well as nicer surface finishes.
For the Key Cutter, If possible get a Helical Fluted design. We have them made near us for the medical applications, wrap it in Sistral again. I don't know what you're doing with it but I assume some type of undercut? Sometimes these tools are used to reach further into the part. If you are using a Harvey Tool or Internal Tool Key Cutter ask them to give you slightly more "dish" on the faces than the norm angle. This will give more clearance so if the tool moves a bit while cutting it doesn't immediately rub on the large face of the tool.
Seems to me that 200SFM is your safe zone. Stick with it. But to make the claim of raising the heat range to 700SFM is a big jump. Anytime I see 17% Chrome, 7% Nickel, my range of SFM is narrowed to +/- 50 SFM, not 500SFM. Turning is all about being sure the center line is adjusted according to where the chipbreaker is working the best due to the Depth of Cut and Feedrate. Tool Nose Radius amount comes into play also. Make sure your Depth of Cut is more than 1/2 of the Tool Nose Radius to stabilize it in the cut. On a Swiss you can get by with taking less due to the rigidity of the turning concept on a Swiss with the tool being in the cut right at the guide bushing. But don't be bashful to adjust your centerline up or down after you establish the depth of cut and feedrate that is giving you a good chip deformation. Again, Sharp Chipbreaker, Hard Turning Grade, Ground Insert would be the way I would go.
For the cutoff Tool, even as much as I love the Iscar Do-Grip system, try the NTK cutoff that has the serrations. You can find it here
formatting link
On any cutoff due to these 3 things, width of the tool, the amount of feedrate and hardness/toughness of the material, there will be some downward or undercenter movement. (If the tool is upside down, yes it's going up but it's still undercenter) . The Iscar Do-Grip is either a self grip or a screw down design. Either pocket can fatigue quickly in an interrupted cut. The NTK Serrated style locks the insert nicely. Chances of this insert going behind center is slim. They lap the cutting edges so they are sharp plus they are in the 3mm width range so it should be sturdy enough to help with the interruption.
Horn has some new Swiss tools coming out at IMTS that are coolant induced and use standard ISO inserts. This may be helpful to concentrate oil flow into the true cutting zone.
After you get a satisfactory part off, try bumping the tools up something like 2-3% each in feed and speed until you see a difference( either good or bad) and if a tool begins to fail, back it off a bit. But don't stop the other tools yet. I think you will find out the 200 SFM range for turning will be safe because of the total amount of heat generated in this continous cutting action. However, with the endmills you will go up higher since you inheritly are breaking up the heat with each flute taking a cut.
I hope this is what you are choosing to run at IMTS. I would like to see it run.
Take Care Dan and keep up the great work out there in the field helping people be competitive. You are a true asset to American Manufacturing today.
JR