[How do I?] Mill An Oblong Thru-slot

K

karim

Registered
Registered
Joined
May 4, 2016
Messages
80
I need to mill a slot like this:

oblong thru-slot

oblong thru-slot


The slot should travel all the way through the part, as perpendicular as I can manage, with size tolerances of ±0.01". The part isn't actually cube-shaped... I just didn't bother to draw the whole part, just the slot.

Material: Aluminum
Depth: 2"
Slot Width: 3/16"
Slot Length: 5/16"

Should point out that I'm doing this on a Sherline 2000 mill.

I'm thinking:
  1. Drill the two end holes undersize
  2. Ream holes to 3/16"
  3. run a 1/8" end-mill between the centers along both edges
  4. Flip part and repeat step 3
Am I on the right track? I'm a little worried about verticality (caused by drill imprecision/wandering), hence the drill/ream operation.
Also wondering about the potential for the end mill to "buck" in the slot. I've never used an end mill "trapped" like this at depth. Will a 1/16" clearance between the trailing edge and the opposite surface be enough?

All input welcome.
 
Last edited:
You will not likely find an end mill that diameter with a 2" depth of cut, that is 16 diameters.

MSC has a 1/8 x 1 1/2 depth, you would have to do it from each side 1"+ deep. A WEDM would make short, expensive work of that at a closer tolerance.
 
Yeah, I figured I'd have to do both sides. Somehow failed to include that in the steps above.

EDM is waaaayyyyyyyyyy outside of my budget envelope ;)
 
your plans sounds kinda like how i'd go at it!, with an exception,
i'd go a step further and drill out as much slot material as possible- then clean out with the endmill
just be prepared to take a lot of light cuts and buy a couple extra endmills if you have luck anything like mine ;)
 
Another thought....
Use a stop on one side, too, so that you can locate from the same side (parallel to the slot centerline) when you flip it to get as close as possible.
 
dulltool17 said:
Another thought....
Use a stop on one side, too, so that you can locate from the same side (parallel to the slot centerline) when you flip it to get as close as possible.
Click to expand...

That's a good idea, but the problem lies in what I didn't tell you ;), which is that the part in question is not symmetrical on any axis (and the slot is off-center) so I think the best thing I can do when I flip it is to keep the same face against the fixed vise jaw (which will keep me lined up on the Y-axis). I'll have to locate to the part edge and then advance along X the known distance to the first center.
 
I would use the end holes themselves for registration. Machine the top side completely and flip the part, put a 3/16" pin in the chuck, and move the inverted part until the pin drops easily into the end hole. Check the second hole and shim the part if necessary to align. A rotary table or vice with a swivel base would simplify the procedure. You could use an edge finder or wiggler to locate the hole as well.
 
Am I correct in my thinking that its an absolutely terrible idea to run a 3/16" end mill (effectively standard milling AND climb milling at the same time) through the slot?

And do you guys think that 1/16" is enough clearance for chip evac (i.e.: a 1/8" end mill in a 3/16" slot)?
 
I might plunge cut that one, one of the few instances I would plunge with an end mill. Drill an undersized pilot hole, then plunge with an on-size end mill. Step over about 0.005 and plunge again. Lots of coolant, and keep the hole cleaned out.

I would use an endmill something like this one.
http://www.harveytool.com/ToolTechInfo.aspx?ToolNumber=35512
 
You must log in or register to reply here.
Back
Top