What's new
What's new

Rule of thumb for the smallest / largest End to use on a part?

mtags

Plastic
Joined
Jan 9, 2018
Hello!

I'm curious to know if there is a rule of thumb out there for quickly determining what the smallest and/or largest End Mill would be to reasonably use on a part? I'd like to use some combination of the part's dimensions (Height, Width, Length) to scale. I've heard 50% of the Mid part dimension before, but that isn't great for High Aspect ratio parts.

For instance:
Part 1: 10cm * 50cm * 25cm part would have a min tool size of _____? A Max tool size of _____?
Part 2: 10cm * 100cm * 10cm part would have a min tool size of _____? A Max tool size of _____?
Part 3: 10cm * 10cm * 10cm part would have a min tool size of _____? A Max tool size of _____?

Part 3 likely isn't going to use a 10cm End Mill. Part 2 isn't going to use a 0.1cm End Mill.


I'm assuming there aren't any micro features on the part and the features are normally sized / proportioned vs. the part in question.
 
Has nothing at all to do with the part's outside dimensions. I make small parts with large endmills, and have to use tiny endmills on some large parts. Some parts I use half a dozen different endmill sizes.

Regards.

Mike
 
Dimensions (pocket radii etc.) can determine size.

If you're trying to maximize metal removal, speeds, feeds, and the maximum HP of your machine are some determining factors.
 
I don't disagree with the comments for the smaller tool. However, what about the larger one. There is some large tool used to bulk remove the excess stock in areas where corner fillets, etc aren't limiting. How do you typically set that larger Mill size?
 
For me the machine used would be more important than the parts size, as well as stickout, rigidity, nearby geometry, etc. 1/2" dia endmills are the goto tool for some shops, we often apply a 2" shellmill everywhere we reasonably can, and range up to 5" and down to 1/8", sometimes on the same part. This is where experience pays off.
 
Way too many factors to utilize a rule of thumb. Experience is key here.
The only advice I can give you is you generally use the biggest tool for the job,but then again even that doesn't apply 50% of the time.
 
Yet another tradeoff is high speed milling (smaller end mills running very fast) vs. conventional lower speed milling (largest end mill - maybe a face mill - you can run at conventional speed and feed, up to limit of machine rigidity, hp, etc.).
 
Hello!

I'm curious to know if there is a rule of thumb out there for quickly determining what the smallest and/or largest End Mill would be to reasonably use on a part? I'd like to use some combination of the part's dimensions (Height, Width, Length) to scale. I've heard 50% of the Mid part dimension before, but that isn't great for High Aspect ratio parts.

For instance:
Part 1: 10cm * 50cm * 25cm part would have a min tool size of _____? A Max tool size of _____?
Part 2: 10cm * 100cm * 10cm part would have a min tool size of _____? A Max tool size of _____?
Part 3: 10cm * 10cm * 10cm part would have a min tool size of _____? A Max tool size of _____?

Part 3 likely isn't going to use a 10cm End Mill. Part 2 isn't going to use a 0.1cm End Mill.


I'm assuming there aren't any micro features on the part and the features are normally sized / proportioned vs. the part in question.

.
got to do with
1) can you hold the part
2) what is vibration limit of part in vise, fixture, chuck, clamps
3) what is tool in tool holder limit
4) what is depth and width of cut needed
5) what is maximum radius if have to leave a corner radius
.
many many times when you go to facemill of 50 to 150mm dia you can increase chip load or feed per tooth for example from
.05 mm to .40 mm per tooth cause the big thick insert on big
facemill can take a lot more feed at higher rpm (2x to 3x sfpm) too and can
take a lot more depth or width of cut
.
so if 100 mm facemill goes 1500 mm per minute feed dont matter if it over hangs part if it run 200 to 400% faster feed if it does it in one pass.
.
and facemills with proper inserts can leave a mirror finish of course thats often better than grinding. that is 10x to 100x faster and often more mirror like
.
facemills of 2" dia(50mm) often can take 10hp and 4" dia(100mm) can often take 20hp or more. basically there is a ratio to motor hp and cubic area turned into chips and the power conversion efficiency goes up with thicker chips. if i take a big plate 1 meter by 2 meter and 10mm thick and shear it into 2 each 1by1 meter plates it takes less power per hour than if i convert 1by1meter of 10mm plate into .05 thick chips. thicker chips have better power efficiency ratio
.
and not many end mills leave a mirror finish, off hand i cannot think of any
.
facemill literally can create a big pile of chips 10x to 100x faster AND might be 10" or 250mm long (or much longer)or gage length from spindle face. usually as tool and tool holder length increases to reach all the part facemill is much much faster
.
even if using a end mill a 2.0" or 50mm roughing end mill can plough through 40mm wide by 40 mm deep in one pass where as a much smaller one would have to take many more passes. hard to describe but see it everyday
.
and if you need a 50mm dia and a 250mm flute length how you going to cut the 250mm depth of cut (even if width of cut low) with a 10mm dia end mill in one pass
 

Attachments

  • ShinyMilling_cropped.jpg
    ShinyMilling_cropped.jpg
    17.9 KB · Views: 51
Use the biggest Tool you can, until you need a smaller Tool.

R


Thanks Rob, brilliant! :crazy:

I'm giving a hard time, but ya, what he said...

Sometimes toolchange capacity is a problem, so maybe cut out the 1" and rough with a 1/2". etc...

edit: +1 for attracting tom's attn... ;)
 
Thanks Rob, brilliant! :crazy:

I'm giving a hard time, but ya, what he said...

Sometimes toolchange capacity is a problem, so maybe cut out the 1" and rough with a 1/2". etc...

edit: +1 for attracting tom's attn... ;)

.
obviously it depends on parts being made and your machine. many horizontal cnc you need longer tools in longer tool holders to reach.
.
if you got to remove 1/2 ton of material on a 10 ton part normally you aint going to do that with a 1/2" dia end mill
.
a cube if 300mm by 300mm by 300mm steel about 480 lbs or easily over 200kg usually not going to be using a 10mm end mill on it
 

Attachments

  • EndmillsLong.JPG
    EndmillsLong.JPG
    74 KB · Views: 86
you want to use 5hp you usually need 25mm dia end mill thats not too long
.
even 50mm dia hss roughing corncob end mill chewing through 40mm wide AND deep in one pass going to need a lot of hp like 5-10hp
.
often tool size is based on how much material it can convert to chips in a minute that is how much hp it can take without breaking. or rather how much cutting forces it can take. obviously if cutter is experiencing 200kg (or more) of force trying to bend it, a long 12mm dia end mill going to have a problem
.
when length to dia ratio is over 3x that is 10mm dia and 30mm length can take so much but 10mm dia and 60mm length will bend 2x2x2 or 8x more. if 90mm long its 3x3x3 or 27x more bending
.
the cube of length to dia change is one of the laws of the universe
 
That's the way that I have always looked at it. The features to be cut have a lot more influence on the size of the tool than the overall size of the part.

On the large end, you should have some cutters, facing cutters that can flatten a large dimension at one pass. This will save time as using a 1/2" end mill to face a 6" wide by 20" long slab of metal is a total waste of time. Facing cutters in the 2" to 4" diameter range are fairly common. There is some advantage to using a cutter that is bigger than the width of your part as it can finish the flattening pass faster due to the arc that the leading edge of that cutter is creating. But that advantage starts to become less with a diameter somewhere around 1.5 times the width of the part. This assumes good tram.

For things like slots, many will choose a cutter that is around 75 to 90 percent of the slot width. Down the middle to rough it out and then clean up the two sides with two final passes.

For pockets a rough cutting tool may make the hogging out process faster and easier and then a tool change to produce the final size and features like the corner radii. On the other hand, for a small pocket just doing the whole job with the final cutter may be more efficient.



Has nothing at all to do with the part's outside dimensions. I make small parts with large endmills, and have to use tiny endmills on some large parts. Some parts I use half a dozen different endmill sizes.

Regards.

Mike
 
even contouring around a small part. even if small part is only 1.5 or 2" tall if 1" dia end mill does contour at 10 to 20 inch per minute in one pass
.
and 2" dia carbide insert mill does it at 25 to 50 inch per minute in one pass cause
1) more rigid can take cutting forces more easily
2) carbide inserts usually run faster sfpm or faster rpm often 200% faster
3) bigger thicker carbide inserts can take higher feeds often 200 to 1000% more
.
so even if contouring and width of cut is less than 0.2" and depth of cut is 2" the bigger mill will chew through it in one pass much much faster usually.
.
bottom line small dia mill 10-20 ipm feed
bigger carbide insert mill 25-50 ipm feed
.
bigger is faster usually even contouring
.
only time you cannot go faster with bigger mill is slotting. obviously if slot is 1" wide you cannot use a mill bigger than 1" dia
 








 
Back
Top