[curiosity22]

Hey G'day people,

Chip loads, I've been trying to get my head around this but its not making sense. I understand depending on how many flutes the size of the cutter how wood chips need to be cleared. What I'm not understanding is the math behind it.

I've had a look at various manufacturers of end mills and some do and others font specs on their tools. ie chip load feed speed etc.

Say I have a single flute end mill 6mm, how do you work out what the chip load should be? or is this something only the manufacturer can give you?

We have a speed and feed we are comfortable with load up the 6mm single flute and for whatever reason we now need to use a 2 flute.

The speed and feed are going to change based on the chipload? how does the calculation for the chipload work?

Or am I beating my head for nothing? Is knowing the math behind chipload really important in which case I want to learn how to go about the calculation. Or do I go back to my coffee and just worry about speed and feed.

I hope you guys understand what I'm asking.

Cheers,
Steve

[Sterob]

I'm not expert, but my understanding is that one is trying to achieve a particular 'chip load' when calculating feeds and speeds.
Everything revolves around that. Changing from the 2 flute cutter to a 3 flute cutter means the feed and/or speed of the tool will need to change in order to maiantain the chip load.

Chip load important as too fast and your tool will bend and break......too slow the the tool will 'rub' and overheat.....

With Aluminium it appears to be more important as the chip size helps with removing heat from the tool and job.

You need to use 2 formulas. Sutton has a good explanation. ( I'm at work so don't have access to that info.)

Its a bit tricky to get your head around if your not a 'machinist', like me. I'm into electrons....

[curiosity22]

I'm not expert, but my understanding is that one is trying to achieve a particular 'chip load' when calculating feeds and speeds.
Everything revolves around that. Changing from the 2 flute cutter to a 3 flute cutter means the feed and/or speed of the tool will need to change in order to maiantain the chip load.

Chip load important as too fast and your tool will bend and break......too slow the the tool will 'rub' and overheat.....

With Aluminium it appears to be more important as the chip size helps with removing heat from the tool and job.

You need to use 2 formulas. Sutton has a good explanation. ( I'm at work so don't have access to that info.)

Its a bit tricky to get your head around if your not a 'machinist', like me. I'm into electrons....

Hey Sterob,

Thanks for the input, Ill have a google for Sutton and see what that reveals for me.

Well you seem to have a better understanding than I..

Cheers,
Steve

[peteeng]

Hi C22 - Chipload is the size of the chip that the cutter is trying to take. Say 0.5mm or 0.1mm depends on feeds and speeds as you know...

So its simply the feedrate in units/min divided by the rotational speed in rpm so the units are the same. ( mm/min ) / (revs per min) gives mm/rev this is the distance moved forward for each rev and its tooth (if single tooth tool) . If you have more cutting edges then the distance is smaller. So divide the chip size by the no of teeth on the tool.

The tool makers do lots of tests and publish guidelines for the chip load. Then there's the surface speed which is more to do with tool wear then performance. All of this tries to maximise the material removal rate (MMR) so the job gets done asap with as little wear on machines and tools as possible.

https://cimquest-inc.com/what-is-chip-load/

High Speed Machining takes this further and uses the full tool depth to do the cut. This reduces the bending moment on the tool so the tool is stiffer yet can cut more material if the machine has the power and rigidity to cope. Some CAM systems will calculate MMR for each setting and the path time. Then you can make decisions based on MMR.

So a single flute 6mm tool. Say you have a feed of 2000mm/min and a spindle speed of 10,000 rpm then the tooth progresses 2000/10000= 0.2mm each rev so the chip size or chip load is 0.2mm

https://www.cutter-shop.com/informat...oad-chart.html

Looking at this table for plywood and a 1/4" cutter they say use a CL=0.3mm so the 0.2mm is too small. So either feed faster or slow the tool down. So if we speed up feed mm/min = rpmxCL = 10,000x0.3= 3000mm/min so increase from 2000 to 3000mm/min. Once you have a good CL for your machine and material and tools you can scale up and down to suit the job and maintain the CL. Cheers Peter

[curiosity22]

Hey Peter G'day,

Thank you for the links and explanation, I think I can work with that. I get the gist of it.

I was looking at it totally different.

Thank you very much thats given me the right path to follow.

Cheers,
Steve

[RCaffin]

All this assumes that your spindle has sufficient power and sufficient rigidity. If you are working with a router, as you seem to be, then these are NOT guaranteed. In which case, you may have to reduce the chip load.

1-flute, 2 or 3 or 4 ... Since each flute makes a cut, going from 1-flute to 2-flute might mean you can feed twice as fast. Maybe, if you have the spindle power. But the clearance space for the chips goes down as the number of flutes goes up. Typically, a 4-flute cutter is more rigid than a 1-flute, but it has a lot less clearance.

For wood, with a carbide cutter and in a commercial environment, one usually tries to keep the RPM up.

Cheers

[machinehop5]

...one more thing that always helps to know/understand is SFPM of the material being cut/machined.
https://en.wikipedia.org/wiki/Surface_feet_per_minute

[curiosity22]

...one more thing that always helps to know/understand is SFPM of the material being cut/machined.
https://en.wikipedia.org/wiki/Surface_feet_per_minute

Thank you for the link, added to my favorites.

Cheers,
Steve

[FastFarmer]

I made a video on this a while ago for hobby machines - https://youtu.be/XW3k96KilNk

Once you have your feed rate (Vf), a good rule is Vf -30% for ramping, Vf - 70% for plunging, and Vf - 85% for full depth slot (I say 75% in the video, but it's a bit agressive).

[curiosity22]

Hey G'day,

thank you for taking the time to put this up. Have it bookmarked.

Cheers,
Steve


Once you have your feed rate (Vf), a good rule is Vf -30% for ramping, Vf - 70% for plunging, and Vf - 85% for full depth slot (I say 75% in the video, but it's a bit agressive).[/QUOTE]

[FastFarmer]

No problem Steve. Hope it helps.

BTW Always use adaptive strategies and run your cutter at full Vf with 25% of width (optimum load) at depth = to width of cutter... and you'll be cutting chips like a pro in no time.

Unfortunately for most hobby guys the only viable option with such tool paths is Fusion 360. However if you use it, then in the tool settings once you put your rpm, tooth load and number of teeth in, it will calculate the Vf for you (same as I did manually). Then you just need to set the ramping and plunge rates as I suggest.

Oh, and always check the optimum load and depth settings in the tool path you create. Fusion makes some not quite right assumptions sometimes.

[curiosity22]

No problem Steve. Hope it helps.

BTW Always use adaptive strategies and run your cutter at full Vf with 25% of width (optimum load) at depth = to width of cutter... and you'll be cutting chips like a pro in no time.

Unfortunately for most hobby guys the only viable option with such tool paths is Fusion 360. However if you use it, then in the tool settings once you put your rpm, tooth load and number of teeth in, it will calculate the Vf for you (same as I did manually). Then you just need to set the ramping and plunge rates as I suggest.

Oh, and always check the optimum load and depth settings in the tool path you create. Fusion makes some not quite right assumptions sometimes.

Fastfarmer G'day,

Thank you again, excellent video. I learned a lot. I did not know that about Fusion 360. I have it loaded and every so often I tinker with it. Creature of habit using software I'm more familiar with. But I may just start using it if only for the Vf calculations, whats the worst that can happen. I've penciled in your notes and added to my documents I call "things to remember" I reference it a lot.

Cheers,
Steve