By ForeverGreen
Am I using HSMA incorrectly?
I've been using HSMA for quite awhile now, and it has been really helpful. However, sometimes I come across numbers that make me wonder if I'm using it wrong. I'm machining some aluminum with a Garr A3 endmill (07027). Admittedly, speeds, feeds, and cutting parameters is an area I struggle with, but HSM is suggesting an 11.8% stepover, which seems very low for aluminum, I'm used to running closer to 30% stepover in aluminum. Is that because of the ADOC and stickout? When I put those same numbers into Garr's Technical Advisor, they recommend almost 3x the chipload. Garr's app doesn't suggest RDOC, so I used the 11.8%. Of course, Helical's app gives wildly different numbers again, when I use an identical Helical endmill. But, I'll just focus on the 2 apps for this question.
ForeverGreen
Oops, sent the message before I added the Garr screenshot
Eldar Gerfanov (Admin)
Hello,
When using a purpose-made End Mill (IE. Aluminum-specific endmills and roughers, or so-called high-performance end mills), selecting the HP/Roughing tool type is recommended.
This will give HSMAdvisor a better idea about the tool you are using and give more aggressive cutting conditions.
Tool manufacturers may suggest different starting DOC and WOC values.
It is not very useful to compare the results unless you copy their suggestions into HSMAdvisor and check out how different the suggested speeds and feeds are.
This is in fact how I tune HSMAdvisor with new tools and materials: enter the recommended DOC/WOC/SPEED/FEED, check how much my S% and F% overrides are off, and modify in the database accordingly, so it's closer to 100% for MOST combinations of tools and materials.
MikeHorton
I spoke with a rep at helical a month or so back about their machining advisor calulator and the suggested parameters. I was told that the calculator is a bit "aggresive" with HEM tp's. Was told to drop the sliders 10-15%. I was also informed that 10-20% Ae is their suggested RDOC. He didn't suggest going any wider than that. He said 15% seems to be the sweet spot for them. I'm currently limited by machine capabilites on this current 6061 mold cavity. It's a VF-9 cat 40 machine with a 15k spindle and 500ipm feed cap. I've been running helical emills for the past few molds and I have been maxing both S&F out and adjusting Ae accordingly. If you can get the chips out of the cutters path, let 'er eat. We've had good luck with the helical reduced neck chip breakers also. As far as Garr goes, their HSAL line works great for 6061 also. Have yet to use the A3, a tech informed me they are great for floor machining.
I've had good luck using 90% of F/L for Ap, 5-7 degree ramp with 70-80% od diameter helix woc. These chip breakers do a good job of chip control. I attached a shot of the helical #21822. I try to get under .001 deflection before I activate and RCT or HSM. Try to aim for .0015 deflection with those activated. Garr has a ARC series chip breaker that works well also.