Would you plunge mill this slot?

[McLaren]

Good morning everyone. I have a .400" diameter 303ss shaft with a slot that runs through it .103" wide by 2.640" long. How would you make it?

 

Right now I am using a 3/32" endmill to rough it out at S8000, F8.0, DOC .033", but it's taking about 4 minutes.

 

I was thinking about plunge milling it but don't have any experience so I'm not sure if that would be the better way to go. Thank you in advance for any and all replies.

[SKIR68]

your sfm is about right but your chip load is way light. I would try 200(sfm) x 3.82/.093=8215 (rpm) 8215(rpm)*.002(chipload)*4 (#of teeth)=65 (IPM). YMMV!!

[spade117]

What cutter path are you currently using?

[Odell]

Ramp back and forth end to end to the bottom and then clean up the outside.

[McLaren]

I'm currently doing a 2d contour ramp. I drilled both ends, and plunge down .033", go across, plunge down another .033", go back across. So on and so forth.

 

Right now I am using a 3/32" endmill to rough it out at S8000, F8.0, DOC .033", but it's taking about 4 minutes.

[K2csq7]

I would not bother with the drill.

[K2csq7]

If your plunging into the drilled ends then going straight across, that is not ramping, that's depth cuts...am I missing something.

Just ramp back and forth.

[McLaren]

It is "Ramp" under contour type, with ramp motion being "Plunge".

 

And eliminating the drill doesn't affect the 4 minute cycle time to rough out the slot, neither does ramping at an angle.

 

Also keep in mind that ramping at an angle makes your depth of cut twice your ramp depth at each end, so I would have to double my cycle time to keep the load on the tool the same. Not really what I was looking to do.

[K2csq7]

Just throwing it out there, I did some slotting with 3/16 end mills, it sounds very similar to what you are looking for. If I can remember correctly I was going a bit more than .900 deep and the slot was almost 2" long. I ran 100's of the parts and the tool wear was nil. I think my ramp depth was .040 (yes .080 at each end I understand), do you have a lot of parts to do? is your tool change time negligable? Do the sides of the slot need a nice finish, I was holding +.004 -0, and it was not a problem. The finish wasn't the best, but it didnt need to be.

[Cad-Camr]

Forget the ramp. Rough drill 1 hole in the center of the slot a little bigger than your End Mill and drop in and 2d contour it. you will save time.

[McLaren]

The slot is .101" +.005" -.000", but I'm using a second 3/32" endmill to take a finish pass so that's fine.

 

Cad-Camr, could you be more specific on how that is going to save me time? Are you talking about taking the entire .400" depth in one shot with a 3/32" endmill?

[McLaren]

And Keith, your .08" deep with a 3/16" seems pretty similar to my .033" deep with a 3/32", so I think I'm in the ballpark with that figure. I was looking more into whether or not plunge milling down the length would be faster.

[MAS58]

I use ramp depth. I changed to plung and it took 1/3 longer then ramping. If you use depth the tool will go down by that depth for the whole contour. No holes needed.

[Mic6]

Slotmill toolpath works great also.

[Cad-Camr]

Maintain your depth cuts. You dont have to ramp. takes too much time. Depth should be aroud 50% of tool Dia and I would use Multi-pass with a .002-.003 thou finish pass. That should reduce your 4 min cut time. Let us know what works best.

[Colin Gilchrist]

I would do it in 4 depth cut passes, using a stub flute 3/32 endmill. Take a look at Harvey Tool. Page 30 of their catalog has a .093 long reach/stub flute. I'm pretty sure you could go 1:1 depth to diameter ratio and be just fine. That would be 4 total depth passes.

 

I'd probably start at 8000 RPM, and 16 IPM. Should cut your roughing time down to a minute per slot. Even if you went 50% of tool diamter per depth pass, it would be about 2 minutes.