[4]

Using long reach end mills

[3]
[10] Like what you see?
Click here to donate to this forum and upgrade your account!

Jake2465

H-M Supporter - Gold Member
H-M Supporter - Gold Member ($25)
Joined
Dec 27, 2017
Messages
258
Likes
282
#1
In a few weeks I plan to post pictures and also some video of a miniature crankshaft on a 4th axis setup. The most challenging area will be when I will need to do live 4th axis finishing between the counterweights so I can get to the back sides of the connecting rod journals. This will require a 3/8" end mill will a 2-1/4" stick out to reach all the way to the journal.

I thought about just using the same end mill for the whole run so I don't need to change tools. I figured that I could start with something like a .001" chipload and .050" width of cut with a .500" depth of cut. But, I am not really sure because I don't ever really mill with a stick out like that.

I plan to use a solid carbide 4 flute.

Any suggestions?
 

JimDawson

Global Moderator
Staff member
H-M Platinum Supporter ($50)
Joined
Feb 8, 2014
Messages
7,048
Likes
5,246
#2
A 0.500 DOC sounds a bit high, I suspect you will get a lot of chatter. Maybe start out with 0.050 DOC. I've never run that skinny of an end mill with that much stick out. Should be exciting :)
 

Jake2465

H-M Supporter - Gold Member
H-M Supporter - Gold Member ($25)
Joined
Dec 27, 2017
Messages
258
Likes
282
#3
D

Deleted member 473

Guest - Please Register!
Guest - Please Register!
#4
If you don't need to cut with that much flute, get a extended shank carbide end mill.

If you are just cutting the side of a surface, taking full length or .500 at a time should not be a problem with carbide end mill. I've cut some deep slots with 3/8" end mills, not one that deep. Be interested how you make out.
 

Ulma Doctor

Infinitely Curious
H-M Supporter - Gold Member ($25)
Joined
Feb 2, 2013
Messages
0
Likes
17
#5
:nail biter::nail biter::nail biter:

i recently had a brain fart and broke a 1/2" x 3" endmill- i lost track of the DOC in a manual mill and snapped er' clean off :bang head:
i hope you have better luck
 

spumco

Registered
Registered
Joined
Jan 15, 2016
Messages
230
Likes
170
#6
In a few weeks I plan to post pictures and also some video of a miniature crankshaft on a 4th axis setup. The most challenging area will be when I will need to do live 4th axis finishing between the counterweights so I can get to the back sides of the connecting rod journals. This will require a 3/8" end mill will a 2-1/4" stick out to reach all the way to the journal.

I thought about just using the same end mill for the whole run so I don't need to change tools. I figured that I could start with something like a .001" chipload and .050" width of cut with a .500" depth of cut. But, I am not really sure because I don't ever really mill with a stick out like that.

I plan to use a solid carbide 4 flute.

Any suggestions?
Reduced neck endmill is your friend here. They have solid shanks, short flute length, and are way stiffer than a regular long or extra-long endmill. Plenty of vendors sell them these days. Try Amazon - CGC Tools has a pretty good selection and they're really cheap if you're buying the last one in stock. If you don't mind spending money, Harvey Tools has just what you need.

Search for "Necked" or "Neck Relieved" or "Reduced Neck" when you're looking for a tool.

Take light chip loads (0.0015 or so) but don't rub, and 1/2D to 1D DOC, depending on the flute length. Do a 2nd finishing pass because everything flexes - even these things.

Meet your new best friend.
IMG_3432.JPG
 
Last edited:

EmilioG

Active User
H-M Supporter - Gold Member ($25)
Joined
Jul 20, 2014
Messages
1,328
Likes
569
#7
You also have end mills with reinforced, larger shanks. e.g. 3/8" endmill with a 1/2" shank.
Guhring makes some really nice cutters. Guhring RF100 Diver and the new RF100 A 90° for sharp corners., no radius.
 

Jake2465

H-M Supporter - Gold Member
H-M Supporter - Gold Member ($25)
Joined
Dec 27, 2017
Messages
258
Likes
282
#8
Search for "Necked" or "Neck Relieved" or "Reduced Neck" when you're looking for a tool.
Thanks for the tips. The ideal end mill that would work out just dandy for me would be the reduced shank end mill. This way the flutes do not have to span the cut depth of the whole cycle.

Harvey tool sells these and they would be ideal, but look at that price :eek:. The 3/8" one is $130.

http://www.harveytool.com/prod/Squa...255/End-Mills---Square-Reduced-Shank_244.aspx

eBay sells something similar, but the shank is not reduced and the flute length is longer. It is not as optimized for what I want to do, but at one fourth the cost, I will likely try that first.
 

Jake2465

H-M Supporter - Gold Member
H-M Supporter - Gold Member ($25)
Joined
Dec 27, 2017
Messages
258
Likes
282
#9

Jake2465

H-M Supporter - Gold Member
H-M Supporter - Gold Member ($25)
Joined
Dec 27, 2017
Messages
258
Likes
282
#10
You also have end mills with reinforced, larger shanks. e.g. 3/8" endmill with a 1/2" shank.
I wish I could do that. The issue is that those counter weights basically make the end mill have to operate as if it was in a 2" deep pocket. Just having a regular long shank with the same diameter as the flutes will likely cause chip rubbing against the shank and the inner walls.
 

Attachments

EmilioG

Active User
H-M Supporter - Gold Member ($25)
Joined
Jul 20, 2014
Messages
1,328
Likes
569
#11
I refer to these: guh0615550a.jpg
 

mksj

Active User
H-M Supporter - Gold Member ($25)
Joined
Jun 12, 2014
Messages
1,862
Likes
2,273
#12
I believe you would want to look at extended neck, if searching eBay you need to check the box include description when looking under end mills. All those listed below the shank is the same size or smaller than the cutting end, probably want a 3Fl or 4Fl which should have less chatter. Carbide will be stiffer.
Some examples:
https://www.ebay.com/itm/Harvey-Too...1-4-x3-8-x1-4-3FL-Qty-3-43600964/352143694645
https://www.ebay.com/itm/Metal-Remo...3-4F-Carbide-End-Mills-QTY-2-USA/351517302764
https://www.ebay.com/itm/MICRO-100-GLR-375-4-Carb-End-Mill-3-8-In-4FL-CC-Uncoated/272781657829
https://www.ebay.com/itm/WIDIA-HANI...-Mill-3-8-Dia-1-1-2-Cut-G3830867/272817321308
https://www.ebay.com/itm/WIDIA-HANITA-TM4V0510004S-Sq-End-Mill-3-8-Dia-7-8-Cut-G3829981/282621799529
 

projectnut

Active Member
Registered
Joined
Apr 14, 2014
Messages
448
Likes
299
#13
Have you considered taking a standard diameter end mill and reducing the shank yourself. I've done it on HSS end mills on several occasions. I fixture the end mill in a spin indexer, then put the spin indexer on the magnetic chuck of the surface grinder. Don't know if it will work for a carbide end mill, but it's a simple straight forward procedure on a HSS one.
 
D

Deleted member 473

Guest - Please Register!
Guest - Please Register!
#14
Don't go with the reduced shank end mill. That will snap off in a heart beat!

Do what projectnut is saying, take a extended reach end mill and just grind down a few thousandths above the cutting flutes. Just enought the clear the part. Then chuck on it as close as you can without hitting the work piece for best results.
 

spumco

Registered
Registered
Joined
Jan 15, 2016
Messages
230
Likes
170
#15
https://www.amazon.com/dp/B0080CKM26/ref=twister_B009TYM47A?_encoding=UTF8&psc=1

If you grind the flutes down for clearance, they're just as weak and prone to flexing & chatter. The solid shank, reduced neck versions are significantly more rigid. If you keep your WOC shallow, the neck doesn't rub on the pocket wall.

And get a radius end - your crank pin journal will be happier with a small fillet at the pin to counterweight point. Shafts don't like sharp corners at section changes - they snap at the high-stress points.
 

jbolt

Active User
H-M Platinum Supporter ($50)
Joined
Dec 3, 2013
Messages
1,460
Likes
1,406
#16
Look at Maritool for reduced shank end mills. About $70 for a 4 flute carbide end mill.

I totally disagree with 4gsr about them snapping in a heartbeat. They are much more rigid that an standard extended end mill. I started using then for deep work about 6 months ago and they are fantastic for rigidity and finish for deep work.
 

Karl_T

H-M Supporter - Sustaining Member
H-M Platinum Supporter ($50)
Joined
Oct 14, 2014
Messages
1,021
Likes
429
#17
Just thinking outside the box...

Have you considered doing all the work in a lathe with a four jaw chuck? I've seen many a crank built this way.
 

Jake2465

H-M Supporter - Gold Member
H-M Supporter - Gold Member ($25)
Joined
Dec 27, 2017
Messages
258
Likes
282
#18
Just thinking outside the box...

Have you considered doing all the work in a lathe with a four jaw chuck? I've seen many a crank built this way.
I think for making a one off, that would not be a bad way to go. But, the actual reason I want my mill to it is merely to test my 4th axis. I figure if the mill can get through the quarter million lines of code that it will take to machine that crank, then I should have a pretty reliable setup.

So, the crank you see in the pictures is a totally made up, I can just get rid of the counterweights and then I can use a standard length end mill and still be able to run the 4th axis through it's paces.
 

Karl_T

H-M Supporter - Sustaining Member
H-M Platinum Supporter ($50)
Joined
Oct 14, 2014
Messages
1,021
Likes
429
#19
Yep, that's going to be a complex milling job. The coding for that would be way over my pay grade.

I do think I'd consider this approach. Ruff each throw out from the right and left side. One block of code for the left, mirror for the right. repeat for the next cylinder. This code would not be horribly complex. Then clean up the last few thou and do the bearings in a lathe.


Just more outside the box suggestions. Trying to avoid all the problems too long an endmill causes.
 
Last edited:

Jake2465

H-M Supporter - Gold Member
H-M Supporter - Gold Member ($25)
Joined
Dec 27, 2017
Messages
258
Likes
282
#20
Yep, that's going to be a complex milling job. The coding for that would be way over my pay grade.

I do think I'd consider this approach. Ruff each throw out from the right and left side. One block of code for the left, mirror for the right. repeat for the next cylinder. This code would not be horribly complex. Then clean up the last few thou and do the bearings in a lathe.


Just more outside the box suggestions. Trying to avoid all the problems too long an endmill causes.
That's good insight.
 

Karl_T

H-M Supporter - Sustaining Member
H-M Platinum Supporter ($50)
Joined
Oct 14, 2014
Messages
1,021
Likes
429
#21
dunno why, but I keep thinking how I would make five or ten cranks using a lathe to do the finish work. If I am just being a pain in the behind, ignore me.

Using both a mill with six index points and a lathe with four different centers causes real setup issues. Especially if you want to be accurate AND quick.

My solution would be a fixture for each end. Assuming 3 cylinder, the throws are 120 degrees apart. (Fours cylinder is actually easier cause you got two pairs 180 degrees apart) I quickly modeled a concept of what the fixture would be for three cylinders. Mount one of these on each end of your raw stock. The center hole is for locating in the index head on the mill, use the three outer holes to locate for indexing.

Next turn between centers in the lathe. Center holes do the mains. outer holes do the cylinder rod bearings Capture.JPG .
 
[6]
[5] [7]
Top