Milling Slots

[HBilly1022]

I've been milling some 1/4" wide slots in 1/4" thick mild steel and I'm trying to figure out the best method. These don't have to be exactly 1/4" wide since they are only for bolts so I have been using a 1/4" center cutting end mill and plunging the slotting. First try I plunged 1/3 depth then cut left to right, at the end of the slot I plunged another 1/3 depth, then reversed direction back to the start. Plunge final depth and then to right again. Second slot I plunged half the depthe and used the same process. Third time I plunged full depth and did it in one pass. I have now dulled 3 HSS end mills. I was running at 1000rpm and using some tap magic brushed on to the steel. According to my feed calculations using a 1/4" 4 flute HSS end mill at 1000rpm and a cut rate of 0.001" per tooth I should be travelling at about 5" / minute. I tried 1/2 that fee rate and found it to be way to fast. I had to slow to a crawl.

Am I doing something wrong? Is there a better way to do this?

I have ordered a 4 flute 1/4" carbide end mill for the next time and hope that will result in faster feeds and longer tool life.


EDIT; forgot to add the pic.

 

[Technical Ted]

Without flood coolant, I run end mills much slower than the feed & speed charts recommend. I usually run ~ 60-80 SFM in steel, especially for roughing/heavier cuts. I've found that feed doesn't dull them up nearly as fast as speed does. Also, the quality of the end mill makes a LOT of difference. If you are using a high quality M42 cobalt end mill you can get away with more speed. A typical chinese end mill, not nearly as fast.

A mister helps if you don't have flood coolant. I use one of these. Even just air blowing on the end mill will help by keeping it cooler and removing the chips as you go.

With HSS, heat kills! Again, heat is caused more by speed than feed.

YMMV,
Ted

 

[bfd]

I like drilling a hole, feed the endmill into the hole and cut the slot.

 

[HBilly1022]

Thanks Ted, next time I will slow the rpms down and give that a try. Might have to look into to a mister now. This hobby just keeps adding up.

Ted, you might recognize the slotted parts. I just added the pic.

 

[Hukshawn]

https://www.ebay.com/itm/Mist-Coola...342838&hash=item33b1cdf15c:g:shQAAOSwB4NWw-7U

I bought one of these a while back. Modified it a bit. Instead of allowing the unit to siphon the lube, I used an old water filter as a pressure vessel filled with lube with a valve on it. Then I have very good control over air pressure and how much coolant is sprayed.
Stock, you need high cfm which sprays too much lube. But modified, it works great at a fraction of the cost of a pro mister.

Here’s the thread I made with that project
http://www.hobby-machinist.com/threads/mist-lube-sprayer.59278/

 

[Terrywerm]

I also prefer to drill a pilot hole, just slightly smaller than the end mill diameter, then follow up with the end mill. Coolant will be a huge help.

Hukshawn posted a thread on making one a coolant mister, and there is another thread with drawings, list of materials, and everything here: http://www.hobby-machinist.com/threads/no-fog-coolant-mister.19957/

 

[EmilioG]

I watched a video where several holes were drilled or center cut (plunged), then running the end mill through.
Less chip packing I suppose.

 

[mikey]

Shawn, I would suggest you use a 2-flute end mill for your slots. I would drill a starter hole, plunge through the hole and lock the quill so you're using the upper part of the end mill, not the cutting end; this is stiffer and will result in less deflection. It would be even better to use a roughing end mill if the finish is acceptable. Calculated speed for a 1/4" end mill cutting full depth is about 1200 rpm with a finishing end mill and a bit higher with a rougher. I would feed by hand so that there is a slight positive resistance to the feed but the cutter should cut freely.

HSS end mills will cut mild steel just fine. Switch to 2-flute end mills to increase chip clearance. Air will help get the chips out and also cool the cut. Coolant is fine but air will work as well or better by reducing recutting of the chips.

 

[Suzuki4evr]

As Mikey said. Use 2fluit slotdrills for that and the more coolent the better. And I recommend depth if cut no more than half the od of mill.So depth of cut for 1/4 inche is 0.125 and I would feed by hand to get the feel of it.

 

[BGHansen]

Drilling is more efficient for removing material than milling. I'd drill a series of slightly undersized holes then cut the slot with a 2-flute end mill. Saves use on your end mill and drill bits are easy to sharpen.

Bruce