Toolpath and tool recomend for 15-5

[kunfuzed]

What's a good tool and toolpath for pulling 15-5 off in a core roughing situation? We're burning up our 1 1/4 Iscar T490 inserts (IC830). Right now were at .150" DOC @ 200 - 400 SFM with and without coolant.

 

Thanks!

[MIL-TFP-41]

Mitsubishi AJX cutter rips through the stuff. I run in both 15-5 & 17-4 at 350~400SFPM & about .03 CPT (chip per tooth) & .05~.06 DOC. VP15TF grade of insert.

[kunfuzed]

Haas VF-5 cat 50 5k spindle BTW.

[jeff]

Hanita Varimill

[Ron Branch @ Verisurf]

Look at their High feed inserts we are using them in 15-5 right now on some applications and seeing very good tool where. What H condition is the material?

[cobra95kev]

Feedmills might not be the best in a core roughing type cut unless you have enough excess stock to take at least 75% stepover.

 

I would check out the new iscar chatter free endmills with a Volumill/Dynamic toolpath type.

Large stepdowns and small stepovers.

 

Hard to say which would be better without seeing the part and stock.

[kunfuzed]

H1025

[kunfuzed]

Here's a rough idea.

 

I'm not stuck on core roughing, just seemed like a good description.

 

Thanks so far guys!

 

[Ron Branch @ Verisurf]

I would contour cut that all day long making sure to keep my step over to 60 to 70% of the cutter step over. Surface finish Contour would work good here. Then where you have excess make the chains you need to then highfeed it. I could have that part roughed with a highfeed cutter in 1025 condition less that 10 minutes no problem. We run our highfeed cutters at 220 sfm with .035 to .04 per tooth feed which on our 2" highfeed cutter is 500 rpms and 80 imp with .05 depths of cut. We turn the corners ever 5 parts. We were taking on some parts 3 hours to rough that we are now taking 32 to 40 minutes. Tooling got cheaper and we gained tons of free time by doing a lot of this material with highfeed cutters.

 

HTH

[cincy k]

If your setup isn't ideal you may want to try a button cutter from someone like sandvik. R300 cutter. Gives you a bit more flexibility than a high feed with some of the same benefits when used properly. When we were roughing this material we typically cut it dry and gained tremendous tool life. Only resaon to rough it wet is where there are thin cross sections where a slight amount of heat may deform or effect your base material.

[Ron Branch @ Verisurf]

cincy we do these types of part dry as well when highfeeding. Any coolant and forget about tool life. It is cool seeing pop corn chips coming off of 15-5 when you are feeding it at 80 to 125 ipm with a high feed cutter.