[How do I?] Mill An Oblong Thru-slot

karim said:
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)?
Click to expand...
IMO, you are correct. An on size end mill will cut an oversized slot due to tool deflection. I have had good results cutting with a slightly undersized end mill and making a finishing pass along each side. However, the +/- .01" tolerance is fairly loose and depending upon the finish you require , you may be overthinking the problem. I would still use the undersized EM for roughing out the hole. If you used a 5/32" EM, you would have some material for a cleanup pass.

Again, IMO, if you use misting/compressed air or flood coolant, you should be OK for chip evacuation with light cuts.
 
karim said:
...
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
Click to expand...

I find that flipping a part always leads to inaccuracies in the slot - maybe something I'm doing wrong - so I try to cut it from one side. I would do steps 1 and 2 above, then use an extended reach 1/8 carbide end mill and set X and Y stops that would allow me to cut the slot on size. I would conventional cut clockwise, increasing depth of cut by about 0.0625" per pass while inside one of the end holes and keep cutting until I cut through.

Carbide end mills of this length will still flex so you can't take huge cuts but 1/3 - 1/2 the diameter should be okay. They sell extended length end mills in 3 and 4" lengths.

http://www.hawkmold.com/store/p/140.../8-FLUTE-LENGTH-1/2-SHANK-DIAM-1/8-OAL-4.aspx
 
I would redesign the part so the part only has a section thickness of around 3/8"-1/2" in the area of the slot. Or, maybe a series of four thicknesses of plate to give you a 2" thickness? Or make the slot wider, 3/8", to allow larger tooling to be used.
 
That is a TERRIBLY narrow slot. 2" deep? YIKES!!! It would be more easily be cut with a shaper. Do you have one? Even if slotted with a shaper AFTER the ends were pre drilled,cleaning up those ends would be a JOB!!!

Edit: On a SHERLINE MILL? It's not happening. Sorry to be negative,but I don't think you can do it.

another way,IF you have a bandsaw,would be to drill a 3/16" hole,thread a cut 3/16" bandsaw blade through it,re weld or silver solder it,and SAW to the other hole on each side. Clean up by FILING. Even with a bandsaw,clogging of the teeth would be a big problem. Use kerosene or WD40 as a lubricant.

I would not risk a $35.00+shipping end mill in a Sherline mill on that. You'll come up a POORER man!!:)
 
Last edited:
George, a Sherline mill is far more capable than you might think. I have used one for over 25 years and it is capable of doing anything a full sized mill can do, only smaller. I haven't done slots in 2" material but I've done 1-1/2". If he debulks the slot by drilling most of the material out and then cleans up with an end mill, I'm pretty sure he can pull it off.
A Sherline mill or lathe is not a toy just because they are small machines. They are precision machines for smaller work.
 
I'll admit I haven't used a Sherline,but my experiences with an Atlas mill were not that rewarding,and it was a more massive machine. We'll see how he comes out.

Being aluminum and not steel will be a big help.
 
You must log in or register to reply here.
Back
Top