What's new
What's new

What CAM systems incorporate Chip Thinning into their feedrate calculations?

BluishInventor

Aluminum
Joined
Jul 7, 2020
One thing that's bugged me over the years is that I have yet to see a CAM system incorporate Chip Thinning into their Feed/Speed parameter settings. Is there an explanation to why that is?

It seems like a concept that's been around a very long time and adding to that, high speed or dynamic tool paths could utilize it in all situations with a stepover less than 50%. Realistically, any toolpath with less than 50% stepover could use it.
 

Mtndew

Diamond
Joined
Jun 7, 2012
Location
Michigan
Is there an explanation to why that is?
Yes.
There isn't any defined parameters that everyone uses when it comes to HEM. You might use 10% stepover and a certain SFM and feedrate for a 1/2" diameter end mill in 8620 material and the person next door uses something completely different with almost identical results.
 

goooose

Hot Rolled
Joined
Nov 14, 2007
Location
canada
Yes.
There isn't any defined parameters that everyone uses when it comes to HEM. You might use 10% stepover and a certain SFM and feedrate for a 1/2" diameter end mill in 8620 material and the person next door uses something completely different with almost identical results.

There are defined parameters. Chip thinning is just a calculation using your defined chip load and stepover. The feed is increased depending on the step over to maintain the defined chip thickness.

Now, the calculation for SFM and and increase in feed beyond that RCTF is another story. Yes, most will use an external calculator or their own flavor but Mastercam has Iscar HEM built in that can be used. It still has a bit of dialing in to see what setting works for you and your machine.
 

BROTHERFRANK

Stainless
Joined
Dec 20, 2013
Location
SoCal
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.
There are defined parameters. Chip thinning is just a calculation using your defined chip load and stepover. The feed is increased depending on the step over to maintain the defined chip thickness.

Now, the calculation for SFM and and increase in feed beyond that RCTF is another story. Yes, most will use an external calculator or their own flavor but Mastercam has Iscar HEM built in that can be used. It still has a bit of dialing in to see what setting works for you and your machine.
 

gregormarwick

Diamond
Joined
Feb 7, 2007
Location
Aberdeen, UK
Featurecam (presumably also PowerMill) has a function for calculating/optimising cutting data for it's "Vortex" adaptive toolpaths.

I almost never use it, favouring HSM Advisor instead.
 

Mtndew

Diamond
Joined
Jun 7, 2012
Location
Michigan
There are defined parameters.

Let me rephrase that, there isn't 1 single speed-feed-d.o.c. that everyone runs their end mills at. We all run things differently.
Like you said, "it needs a bit of dialing in to see what setting works for you".
My point was there isn't 1 hard and fast rule that works for everyone. ;)
 

BluishInventor

Aluminum
Joined
Jul 7, 2020
Let me rephrase that, there isn't 1 single speed-feed-d.o.c. that everyone runs their end mills at. We all run things differently.
Like you said, "it needs a bit of dialing in to see what setting works for you".
My point was there isn't 1 hard and fast rule that works for everyone. ;)

Yeah, that's a definite given. I just think it would be nice to know what my effective chipload is at on any tool and any operation. Not just the standard FPT at full radial engagement.

Like, what's my effective chipload on a finish pass where I'm only taking .005" off the wall? Let me break out my RCTF to find out!
 

barbter

Diamond
Joined
Oct 27, 2007
Location
On Tour...
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.

That's blown me away - totally lost for words.
I'd be running a 12mm 5flute at 12% stepover and 3metres/min on a #40 with coolant.
 

goooose

Hot Rolled
Joined
Nov 14, 2007
Location
canada
I just think it would be nice to know what my effective chipload is at on any tool and any operation. Not just the standard FPT at full radial engagement.
Like, what's my effective chipload on a finish pass where I'm only taking .005" off the wall? Let me break out my RCTF to find out!

Why would you care about chip thinning on a finish cut?
Chip load also has no benefit on a conventional pocketing op that may have varying engagements throughout the toolpath, specifically when hitting corners.
The RCTF in Mastercam is just a check box. Set you desired chipload, set your stepover, it increases feed to maintain the chipload you put in.

Mntdew, op asked about chip thinning. That is a straight calculation, no user feel input required.

Anyone interested, this is the calculation...
chip-thinning-formula-2.png


CT = desired chip thickness
D = diameter
Rdoc = radial depth of cut
IPT = adjusted feedrate

How to Combat Chip Thinning - In The Loupe
 

thesidetalker

Hot Rolled
Joined
Jan 11, 2015
Location
Bay Area, CA
Yeah, that's a definite given. I just think it would be nice to know what my effective chipload is at on any tool and any operation. Not just the standard FPT at full radial engagement.

Like, what's my effective chipload on a finish pass where I'm only taking .005" off the wall? Let me break out my RCTF to find out!

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?
 

CarbideBob

Diamond
Joined
Jan 14, 2007
Location
Flushing/Flint, Michigan
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?


Seems like mixing apples and oranges since you add in scallop height.
The first CAM I used that took this in account was MasterCam 8... That a long time ago and one had to go the other optimization screen.
I do remember it spitting out just plain scary feedrates and I did not want to hit the green button.
This matters and it is well know that many more carbide tools die from lack of feed or chip than those that die from moving too fast.
I'll tell a customer to up the feed rate by three or six because of the thin and things wrong in chip formation...... They look at me like a crazy fool.
Dad had a similar problem telling people to turn off the coolant and go faster with carbide. This seemed so wrong to everyone.

Chip thickness on a mill and lathe different. Lead angle and tool radius? How does that change things?
A lathe has one thick number, a mill does not.
How does a high feed milling cutter work at huge feedrates?
So confusing and how can a normal machinists who makes parts understand this which just seems to be weird and some kind of "Black Magic"?
Bob
 

BROTHERFRANK

Stainless
Joined
Dec 20, 2013
Location
SoCal
That's blown me away - totally lost for words.
I'd be running a 12mm 5flute at 12% stepover and 3metres/min on a #40 with coolant.

This video is of a 15-5 H900 part also. Spindle was 10k max rpm so couldn't run the 14500 on this one. Similar depth and stepover. 3/8" 5 flute end mill.
https://youtu.be/G8byzRQPn9s

I guess it would help to include the link
 
Last edited:

Marvel

Aluminum
Joined
Jan 14, 2019
Location
Minnesota
Featurecam (presumably also PowerMill) has a function for calculating/optimising cutting data for it's "Vortex" adaptive toolpaths.

I almost never use it, favouring HSM Advisor instead.

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.

Untitled.jpg
 

CarbideBob

Diamond
Joined
Jan 14, 2007
Location
Flushing/Flint, Michigan
....
Chip load also has no benefit on a conventional pocketing op that may have varying engagements throughout the toolpath, specifically when hitting corners.
,,,,
Inside corners....oh my. Now we are a lot of arc in contact .
I think most have seen squeal like a little bitch on the inside corners while fine everywhere else.

Weird to me is that so many do not bother to take a caliper and measure the thickness of a produced chip.
It tells not only the chip thinning basics but also the chip compression ratio which measures cutting efficiency and helps dial in tool geometry/prep and/or surface footage that shears nicely in a given material being cut.

Add in the heat per tooth taken for a light step vs full cut and it is all so confusing.
At what point down on chip load are you rubbing and burnishing vs shearing?
Bob
 

5 axis Fidia guy

Stainless
Joined
Aug 17, 2006
Location
Wisconsin
Powermill has the chip thinning option in their options, along with calculating the correct RPM's using the actual WORKING DIA, aka, ball endmills taking light cuts.
 

thesidetalker

Hot Rolled
Joined
Jan 11, 2015
Location
Bay Area, CA
Seems like mixing apples and oranges since you add in scallop height.

Alright Bob, he specifically mentioned questioning chip thickness for finishing passes in the post I quoted. Where did I go wrong?

Are you going to tell me a .005" finish pass and .02" finish pass programmed at a feedrate to produce the same chip thickness will have equal surface finishes? Obviously the .005" cut will have a much higher feedrate to produce the same chip thickness. But you're saying it doesn't matter and the finish will be equal?


And endmills don't produce scallops? Ok
 

thesidetalker

Hot Rolled
Joined
Jan 11, 2015
Location
Bay Area, CA
Powermill has the chip thinning option in their options, along with calculating the correct RPM's using the actual WORKING DIA, aka, ball endmills taking light cuts.

That's a nice feature to have for tools like ball/tapered endmills, chamfermills, c-sinks, etc where the cutting diameter can vary depending where the tool is angled or positioned.
 

DMF_TomB

Diamond
Joined
Dec 13, 2008
Location
Rochester, NY, USA
obviously high feed rates cnc does not follow programmed path as accurately. over 100 ipm feed many
cnc are easily over .0010" following the programmed path and .003" error not unheard off
.
many try increasing feed til it gets noisy, but i have seen where over .007" was needed to finish
the part where roughing was so aggressive
 








 
Top