[lcvette]

What I'm posting above is what FSWizard kicks out for specific HSM Machining with Chip Thinning. If rpm is the limiting factor, step over is really the only way to increase MMR. I use HSM with 30% stepover and it works wonderfully with a nice meaty chip and I don't have to run super high spindle rpm, 5-6k is plenty, What your doing is making the mill go faster and cut less. But The step overs you are suggesting are bording on finishing passes.. The same MMR is accomplished with slower feed rates and bigger stepover. Even my cam software wants to run a 30-40% stepover in 6061 aluminum and it is uses Volumill which is one of the leading HSM tool path generators.

Where did you get a .025-.050" stepover from? HSM is all about constant loading not necessarily making the machine move as fast as it can.. Overall efficiency comes from a balance of the two. Not all small machines will be happy whipping around at 100+ipm feedrates. Have you tried more stepover and slower feed rates? A deeper cut avoids rubbing as well, my chips come out nice and thick and the surface finish was excellent, nice steady stream being ejected no issue with rubbing and long tool life, it still takes a nice deep depth of cut this way rarely requiring more then a single plane of machining unless I'm above 3/4" thick material.

I'm just curious why your cuts are so thin? I am guessing you just like to see the machine moving fast maybe? Or touting 100ipm feedrates?

Sent from my XT1080 using Tapatalk

[zero_divide]

Ray,

I have to disargee with you.
Machining aluminum at 10% WOC is a waste of time and should not be done unless there is a tal need for it.

Constant enagagement machining of aluminum at 30% WOC is a new norm in industrial world by now.
You get to make really deep cuts hauling tonns of material and putting more than 15HP load on a single 3 flute carbide endmill.(i have a video of it somewhere on my channel)

It is called HEM - High efficiency Machining. And if your setup allows, you should definately try it.
I use it for everything starting from mike steel to aluminum.

The 10% WOC is reserved for tool steels and hard-to-machine metals.

The main reason HEM works on soft metals so well is because you need very large depth or cut and very fast feed rate to make up for meager 10% WOC. Plus carbide tooling lasts literally months rather way.

IE. I have a video where I am going 300 or so IPM on a Haas pulling almost 16 horsepower at 15000+ RPM with a 3 flute HP carbide endmill. That is with almost 1/8" WOC and 2" DOC IIRC.

Yes, generally it is better to take deep light cuts. But the problem is: you don't often get to make 4x Dia deep cut. Most parts are just 1" deep or so.

On HSMAdvisor try playing with the parameters to see which combination will get you the best MRR.
Then you also have to account reposition time, which with HSM may be half of your total machining time.

Regards.

[petemilligan]

All,

This has been a pleasure. I suspect that a few folk have learned something new about feeds and speeds in a HSM space. I'll look to video the results this weekend & post for further input here (Full time job elsewhere I'm afraid). Fusion seems to be the way to go from what I see. My experience in CAD is much richer than CAM. Fusion is quirky, but deliberately so - it's attempting to add rigor into the design process that would otherwise be overlooked. To be honest, it tests my patience. Comparing BobCAM / Meshcam etc. much more linear & none of that STL bollocks that results in your work piece being made up of triangles.

Thanks all - back soon with results.

Pete