What CAM systems incorporate Chip Thinning into their feedrate calculations?

[BluishInventor]

Why do you care so much about how thick the chip is?

Feed per rev/flute, not chip thickness, is going to determine scallop height and resulting surface roughness.

Same feed rate with .005" finish pass or with .02" finish pass should produce similar finishes. Chip thickness will be much different. Why bother with chip thickness nonsense?

Two things, let's consider a 0.005 finish pass:
- Seeing what the actual thickness would be at any given feed/speed combination. Knowing that, I could apply a specific final thickness to a variety of tools/sizes/speeds and adjusting the feed to match a known good value.

- Getting insight into cutting pressure and deflection. A thicker chip could mean I would need a spring pass because of cutter deflection. Or I could find optimal chip thicknesses for certain diameters that give me the results I want.

Sure, I could look at overall FPT and just use that. But I still don't know what the actual chip thickness really is. Do I need to know? Not really. Would I benefit from the extra information? IMO yes.

 

[Mike RzMachine]

About 10 or so years ago, the local Iscar rep (shout out to Clay East) was very good and showed me the Iscar HEM library on MasterCam. We were machining 15-5 H900 with air blast 1" deep on a Brother 30 taper. We picked a 3/8" 5 flute from the library, and the HEM feeds and speeds came up with 14,500 rpm and 650 IPM at 5% stepover full depth. I laughed and Clay said go for it. It ran great with great tool life too. Made a mountain of chips.

getting a bit away from the cam chip thinning discussion on this question. How does the small radial margin allow much higher SFM for a given tool coating in harder materials? All of the tool charts i've used recommend a surface speed well below 300 sfm for hardened stainless, with the exception of guhring nano-Si. Iscar only shows up to 300 sfm for the solid carbide endmill series i found on their website.

any advise on how to related practically allowable surface speed with small radial engagement? that would be a huge time saver for me, assuming I can maintain reasonable tool life.

Thanks,
Mike

 

[mhajicek]

getting a bit away from the cam chip thinning discussion on this question. How does the small radial margin allow much higher SFM for a given tool coating in harder materials? All of the tool charts i've used recommend a surface speed well below 300 sfm for hardened stainless, with the exception of guhring nano-Si. Iscar only shows up to 300 sfm for the solid carbide endmill series i found on their website.

any advise on how to related practically allowable surface speed with small radial engagement? that would be a huge time saver for me, assuming I can maintain reasonable tool life.

Thanks,
Mike

If the cutter's flute is engaged in the work for 90 degrees of it's rotation, it's heating up for 25% of the time, and cooling down for 75% of the time. Take less engagement, and those proportions change, perhaps to 10% heating and 90% cooling, or 5% heating and 95% cooling. That results in a lower temperature in the cut. So you can speed up until the heat gets back to the same point it was at with the high engagement. With the spindle speed increased, by perhaps several times what you were using for the heavy engagement, now you increase the feedrate until the chipload is the same as it was before, and now you're really cooking along, but the stress on the cutter is the same per unit time as it was originally.

 

[007Rob]

getting a bit away from the cam chip thinning discussion on this question. How does the small radial margin allow much higher SFM for a given tool coating in harder materials? All of the tool charts i've used recommend a surface speed well below 300 sfm for hardened stainless, with the exception of guhring nano-Si. Iscar only shows up to 300 sfm for the solid carbide endmill series i found on their website.

any advise on how to related practically allowable surface speed with small radial engagement? that would be a huge time saver for me, assuming I can maintain reasonable tool life.

Thanks,
Mike

The answer to this is pretty much the reason why modern HSM/volumill/adaptive/whatever else you want to call it toolpaths are so great.

Essentially, with smaller stepover HSM cuts each flute on the endmill spends less time in the cut generating heat compared to the amount of time it spends not in the cut cooling off. This lets you run higher speeds. And because of the chip-thinning effect of smaller stepovers, you can increase the table feedrate while still maintaining the same chip thickness at the tool as well.

Unfortunately a lot of the tool companies catalogs don't really show what you can get away with using HSM techniques but some of the better feed and speed calculators will take this into account


EDIT: looks like I was too slow typing this up I think the fellow above did a better job explaining this effect

 

[Mike RzMachine]

Thanks! both explanations are very helpful. I've typically made up some time with hsm paths due to longer axial engagement, but datasheet sfm. This will be hugely helpful.

 

[mhajicek]

I use HSMAdvisor, and the Helical Machining Advisor Pro, for calculating cutting parameters. It's very interesting how the recommended parameters change when you alter the depth and stepover.

 

[BROTHERFRANK]

getting a bit away from the cam chip thinning discussion on this question. How does the small radial margin allow much higher SFM for a given tool coating in harder materials? All of the tool charts i've used recommend a surface speed well below 300 sfm for hardened stainless, with the exception of guhring nano-Si. Iscar only shows up to 300 sfm for the solid carbide endmill series i found on their website.

any advise on how to related practically allowable surface speed with small radial engagement? that would be a huge time saver for me, assuming I can maintain reasonable tool life.

Thanks,
Mike

Very good point and also well explained by several members.

 

[aldepoalo]

BobCAD-CAM does with it's adaptive feed rates. Here is a breakdown for calculations and concepts https://bobcad.com/in-depth-guide-for-adaptive-high-speed-machining-using-cnc-software/

 

[Chris59]

CAMWorks has something similar for VoluMill, I'm assuming any CAM that licenses VoluMill has the same thing, I don't ever use it, I have occasionally selected the parameters to see what it calculates and sometimes they seem a little ridiculous. I try to stick with what I know works well, I've used Helical's Machining Advisor a couple times.

View attachment 347243

I use it all the time. Seriously. Try it. Cutting 17-4 and Titanium. Saves a lot of time as well as tool life. I often have to slow it down just because the mill isn't capable of going that fast.

 

[Bigdawg]

I thought that was the entire point of dynamic tool paths, that they keep the load on the tool that same throughout the cut (Or as close as possible) by taking small circular cuts.

 

[mhajicek]

I thought that was the entire point of dynamic tool paths, that they keep the load on the tool that same throughout the cut (Or as close as possible) by taking small circular cuts.

They (try to) maintain constant cutter engagement, but not necessarily chip thickness. Of course if you have constant engagement, the chip thickness with remain mostly constant. Mastercam used to have a filter that would adjust feedrate to maintain constant chip thickness when engagement varies, but after the dynamic paths with constant engagement came out everyone stopped using it.

 

[paels]

Esprit does chip thinning in profitmilling toolpaths.

What is ESPRIT ProfitMilling? | ESPRITCAM

Want to up your tool life and reduce cycle time by up to 70%? ESPRIT’s ProfitMilling cycle can help. New pocketing strategies, improved chip evacuation, and an optimized initial channel width all work together to bring your throughput to new levels. ProfitMilling is available in all of ESPRIT’s...

www.espritcam.com

 

[Job Shopper TN]

This kind of stuff is Solidcam’s entire schtick, pretty much, at least within th iMachining tool paths. It gives you a starting point given the material, tool and parameters, with a slider to adjust aggressiveness, and the ability to tweak it further if desired.