[4]

Proper way to cut a Slot

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

oskar

H-M Supporter - Silver Member
H-M Supporter - Silver Member ($10)
Joined
Nov 24, 2013
Messages
211
Likes
77
#1
I want to cut the slot shown on the attached and I’m not sure if it’s ok to plunge slowly straight down in several passes and if the end mill I have is the proper one.

The aluminum bar is 2”x5.5”x0.5” thick, the slot is 4.24” long (should go down to 0.5” deep), the end mill is 2 flute, 0.25” OD, 3/8” shank. I have a piece of pressboard under the bar to avoid damage to the vice,

I have drilled the holes shown in the slot to speed up the milling time; they all are with a 7/32” drill except the 2 in the center are with a 17/64” drill. I was thinking to lower the end mill to a 17/64” hole and then move the axis left / right to complete each pass.

Do you have any suggestions?
 

Attachments

mikey

Active User
H-M Supporter - Gold Member ($25)
Joined
Dec 20, 2012
Messages
4,486
Likes
4,852
#2
I would use a 3/16" roughing end mill but assuming you don't have one and the slot width is not critical then you can use the 1/4" finishing end mill. I would use a 1/8" depth of cut, speed as fast as the mill will run and feed so you feel a slight resistance to the feed as you turn the hand wheel. Repeat as needed.

For slotting, you can feed in either direction; there is no conventional vs climb milling when slotting. I normally start on one end and feed in a consistent direction but that is just preference.

If you can, use air to clear chips and lots of WD40 for lube.
 

T Bredehoft

Active User
H-M Supporter - Gold Member ($25)
Joined
Dec 27, 2014
Messages
2,727
Likes
2,099
#3
MIke is right, don't try to take it all at once. The best rule is to baby your cutter, pretend it's glass and will break at any time. 'Cause it might. And keep the chips out of the slot as best you can. The reason to use a 3/16 cutter to make a 1/4 in slot is that a quarter inch cutter will 'bend' and take out wider than .250.
 

David S

Active User
H-M Supporter - Gold Member ($25)
Joined
Nov 18, 2012
Messages
1,266
Likes
1,018
#4
The other thing to pay attention to is how the work piece is being clamped. Since the vise is camping in the area that you are going to mill straight through, you don't to want it to tighten onto the cutter as you break through or alternately have the workpiece loosen in the vise.

David
 

Cobra

Active User
H-M Supporter - Gold Member ($25)
Joined
Apr 24, 2013
Messages
641
Likes
510
#5
If you cut the slot with a 3/16, you can then move over to each side and climb mill the sides of the slot to improve the finish. If it is important to have .25 round ends on the slot, plunge cut the two ends with your .25 and then use the 3/16 to mill the slot and finish the sides. As stated earlier, take it easy with the depth of cut as you cut the initial slot but drop the mill down to cut the entire depth when you climb mill to finish the slot.
 

oskar

H-M Supporter - Silver Member
H-M Supporter - Silver Member ($10)
Joined
Nov 24, 2013
Messages
211
Likes
77
#6
Thank you all

Sorry David, I don’t understand what you mean. As far as I know the vice holds well and there is no interference with the cutter

Mike I do have a 3/16” shank 4 flute double end endmill with 1/8” OD at each end (total endmill length is 3-1/8”). Perhaps I can use this one? Your tip about the feed direction is excellent because I was wondering about it and now it is all clear.
 

P. Waller

H-M Supporter - Sustaining Member
H-M Platinum Supporter ($50)
Joined
Mar 10, 2018
Messages
643
Likes
426
#7
Place the work on parallels so that the chips drop through, 1/4" will be more then enough.
 

Meta Key

H-M Supporter - Gold Member
H-M Supporter - Gold Member ($25)
Joined
May 4, 2018
Messages
62
Likes
61
#8
As far as I know the vice holds well and there is no interference with the cutter
I'm not David but I think what he is getting at is that the vice is squeezing the part (with considerable force) just where you are removing material. Thus, as the material is removed the remaining stock may bend slightly inward. So, if you make a finishing pass you may find your slot is a little wider in the middle that at each end due to deflection of the material caused by forces imposed by the vice.

Does that make sense? Not sure I'm explaining it very well..

Anyway, looking at the picture you posted earlier I think it would be better to clamp the stock down. Another alternative would be to use two pieces of steel, same length as your stock, between the stock and each vice jaw. That would help distribute the clamping force across the part, including the ends where stock is not being removed.

Maybe the tolerance for the slot width is such that it wouldn't matter. But, if it does matter, I'd clamp it down at each end with the stock raised up on parallels. That totally avoids the possibility of the vice clamping pressure deforming the stock during machining.

Meta Key
 

David S

Active User
H-M Supporter - Gold Member ($25)
Joined
Nov 18, 2012
Messages
1,266
Likes
1,018
#9
Thank you all

Sorry David, I don’t understand what you mean. As far as I know the vice holds well and there is no interference with the cutter

Mike I do have a 3/16” shank 4 flute double end endmill with 1/8” OD at each end (total endmill length is 3-1/8”). Perhaps I can use this one? Your tip about the feed direction is excellent because I was wondering about it and now it is all clear.
Hi , What I mean is that your vice jaws are fairly narrow and are gripping the solid work piece in the middle. My concern might be is that as you cut through to the bottom the work piece is no longer solid and may squeeze in a bit, and perhaps come loose.

David
 

oskar

H-M Supporter - Silver Member
H-M Supporter - Silver Member ($10)
Joined
Nov 24, 2013
Messages
211
Likes
77
#10
Now I get it David and you have a point

The bar is 1/2” thick and I don’t think it will be squeezed by the vise however I will try to see if I can use clamps to hold it down because the parallels under it sound a good idea too. In any case the tolerance of the slot is not critical
 

WarrenP

Active Member
Registered
Joined
Feb 25, 2018
Messages
128
Likes
27
#11
The aluminum bar is 2”x5.5”x0.5” thick, the slot is 4.24” long (should go down to 0.5” deep)

Are you saying your piece of work is .5 inches thick and your going to make a slot .5 inches deep? Wouldnt that mean you are cutting it in half? If so then they will come apart as someone else said, correct? Maybe you are just saying it can go up to a .5 inch depth but your not going that deep?
 

oskar

H-M Supporter - Silver Member
H-M Supporter - Silver Member ($10)
Joined
Nov 24, 2013
Messages
211
Likes
77
#12
Are you saying your piece of work is .5 inches thick and your going to make a slot .5 inches deep? Wouldnt that mean you are cutting it in half? If so then they will come apart as someone else said, correct? Maybe you are just saying it can go up to a .5 inch depth but your not going that deep?
Perhaps I’m missing something which is normal for a beginner but the bar is 5.5” long and the slot will be 4.25” long so there is enough material on the ends to keep the bar together. It’s true that the slot will go right thru to the bottom

You may overlook the fact that my vice is a Taig mini vice and there is no way I can put enough force on it to squeeze the 1/2” thick aluminum because if I tight it too much the 1/4” threads on the vice screw will strip. It would have been a different story if I had one of these expensive precision vices with the big handle and screw
 

Video_man

Active User
Registered
Joined
Nov 9, 2011
Messages
138
Likes
59
#13
Recently made such a slot, I clamped the work in a t-slot groove on the mill table. I milled a clamping flat on one end to locate the work in case it needed to be removed and replaced, and to prevent it from turning while working. I used a 3/16 mill to hog out most of the material then switched to the 1/4 inch mill to finish the slot, which I've found to help keep the bit from wandering a little wide. Worked fine.
 

oskar

H-M Supporter - Silver Member
H-M Supporter - Silver Member ($10)
Joined
Nov 24, 2013
Messages
211
Likes
77
#14
I would use a 3/16" roughing end mill but assuming you don't have one and the slot width is not critical then you can use the 1/4" finishing end mill. I would use a 1/8" depth of cut, speed as fast as the mill will run and feed so you feel a slight resistance to the feed as you turn the hand wheel. Repeat as needed.

For slotting, you can feed in either direction; there is no conventional vs climb milling when slotting. I normally start on one end and feed in a consistent direction but that is just preference.

If you can, use air to clear chips and lots of WD40 for lube.
Regarding what you said Mike about “…speed as fast as the mill will run…” my question pertains to the belt between the motor and headstock.

In my setup I have the Taig ER16 Headstock along with a Sherline 90VDC VS motor and both have the Sherline 10000RPM pulleys which allow 2 belt positions and I wonder how long the small belt will last at high speeds.
 

mikey

Active User
H-M Supporter - Gold Member ($25)
Joined
Dec 20, 2012
Messages
4,486
Likes
4,852
#15
Didn't know you had a high speed spindle. For a slotting operation with an axial depth of cut of 1/2 the cutter diameter, cutting speed is about 375 SFM; this gives you an RPM of about 5730. With a high speed spindle, I assume you have a tach so just dial it in and adjust speed and feed to your liking.
 

oskar

H-M Supporter - Silver Member
H-M Supporter - Silver Member ($10)
Joined
Nov 24, 2013
Messages
211
Likes
77
#16
I understand and thanks for your time Mike

Nicolas
 

MrWhoopee

H-M Supporter - Silver Member
H-M Supporter - Silver Member ($10)
Joined
Jan 20, 2018
Messages
532
Likes
347
#17
Are the jaws on the vise wider than 4.25? If not, then once the roughing cut is done, the stock will move in the vise and you will not be able to hold it without collapsing the slot.
 

oskar

H-M Supporter - Silver Member
H-M Supporter - Silver Member ($10)
Joined
Nov 24, 2013
Messages
211
Likes
77
#18
The vice jaws are only 2” wide and I finished the slot without collapsing the aluminum bar. Honestly I just can’t see why some believe the 1/2” thick bar could have collapse by cutting a 3/16” slot in the center. Anyway the job is done and perhaps I was lucky?
 
[6]
[5] [7]
Top