[CROSSHATCH]

All opinions and suggestions are welcome. RAY, thanks for posting in my other thread and I ask this current question because of some other figures I have seen from you in the past.

I am machining some pockets in 6061 Aluminum bar stock. I have a Torus Pro and my current parameters for the machining of the Pocket is an HSM toolpath with a DOC: .36" , WOC: .08", RPM: 6000, IPM: 80-90

This pocket is using a 2 Flute 1/2 .09 Corner Radius Endmill. CR2030.090 | CGS | END MILL

The full DOC sounds pretty good, the ramping into Aluminum screams and squeals


I ask this question because I need my production time to go down. I also ask this question because my machine has bogged down during the cut and well, we all hate; that was one (1) of thirty (30) pockets though, maybe the endmill is wearing?

Am I better off running at these parameters or going to a larger WOC and slowing down my feed or tweaking these settings with different endmills?

Regards,

-Jason

[SCzEngrgGroup]

I would suggest you try some different parameters - you may get a better result with a narrower, deeper, faster cut. My "average" roughing cut, which is not pushing the machine to the limit, is 0.050" WOC, 0.5-0.75 DOC, 110 IPM. At the higher WOC, you may be hitting the torque limit of the spindle. It may actually help you to reduce RPM, to get more torque, as torque drops off with increasing RPM above motor base speed. Also sounds like you're ramp is too aggressive. What ramp angle and feed are you using? I can usually do a helical entry, with 5 degree ramp, at about 70 IPM. A larger helix radius helps a lot with chip clearance.

The practical limit for the Torus Pro is an MMR of about 3.0-3.5. I try to keep down around 2.50-2.75 so I have some margin.

Regards,
Ray L.

[kvom]

Ray's comment about the MMR means that you can try various combinations around the same MMR.

Since drills typically have ta larger MMR than endmills, one idea is to drill the pockets at the entry point so that no ramping is needed.

[CROSSHATCH]

Ray- I ran my code yesterday and the machine did perform very well. The pocket cuts yesterday sounded good and that was at the 90 IPM, .08 WOC and full .36 DOC. I'll play a bit with the RPM today and see what sounds good. At the 6000 RPM, overall the cuts were nice. My Ramp is maybe not aggressive enough, maybe I am rubbing. Only 50 IPM with 2 degree ramp angle. Again, only one pocket squealed and I believe that is due to clamping.

Thanks for the input, doesn't seem like I'm too far off.

Kvom - My biggest problem right now with that and the idea is the tool change. I don't have a PDB and I hate manually changing tools. I would rather leave a tool in a little longer (at the expense of maybe the sound) compared to changing the tool in 15 seconds.

Thanks for the input!

-Jason

[SCzEngrgGroup]

BTW - When it comes to chatter, don't underestimate the impact of the specific tool. I've had what appeared to be virtually identical endmills from different manufacturers, yet one manufacturers tools would chatter horribly, while the others would not chatter at all. Find tools that work for you, and stick with those exact tools. Don't assume all endmills are the same.

Regards,
Ray L.

[CROSSHATCH]

Ray - I agree, I have had good cutters and bad cutters. I'm pretty sure I found some true winners with my latest cutters, especially the one I linked to in my first post and I'm going to stick with them. That cutter does sounds nice and does produce a nice finish at my current parameters. I don't know how much more I can gain from the performance though without something bad happening.

I changed some some things around in the toolpath today so I will report back, however I did not change the parameters of the DOC, WOC or RPM.

Will report back.

-Jason

[keithmcelhinney]

One question: What is your tool stickout? That can really make a huge difference. I don't have great luck with carbide cutters on my machiine. Squeals really bad. It has got better since I retrammed my machine but still I use a cheap 1/2 hss for HSM with great results (thanks Ray). I will have to go back and see what my parameters are though, I can't remember off the top of my head.

-Keith

[CROSSHATCH]

I bought all carbide in the beginning when I got my Torus. Since then, I have switched to HSS for certain tools. All the cutters I used before squealed so badly and sounded terrible. I have since gained more experience in the tooling and use both, but have a better understanding of which tools works for me.

I am trying to use the shortest flute length I can but for the endmill I linked too, as you can see it's quite a long length for only a .36 DOC. However, I had trouble finding a 1/2" cutter with such a large corner radius (.09), I would go to .125" if I could find one. I'm sure a company could make me my tool, but I was looking for a lower cost solution initially.

I don't know, seems rather difficult to find an endmill in that size but I have to deal with the flute length. I must admit though...it does sound good and produced nice chips with a good finish.

Regards,

-Jason

[AUSTINMACHINING]

My typical "safe reliable " speeds in 6061 are .5" doc × .05"woc, 100IPM at 6000 rpm using both carbide and hss 3 flute 1/2" end mills.