Milling a pocket in Aluminum or Steel with clean sharp edges

[mikey]

Thanks for the reply.

I'm trying not to go too crazy with it as I cant afford a set of roughing and high helix end mills. So I'm really trying to find the main problem here just to get to a point where a simple slot looks reasonably presentable. I concur that these end mills may be just too poor a quality and stepping up to a better set might be required or maybe finishing passes.

Actually, you're going to find that you can't afford not to use roughers. They will cut 20% faster and last 3 times longer than finishing end mills. They do all the hard work and allow you to save your finishing end mills for finish cuts.

The other thing to consider is what tool holder you're using. The more run out your holder has, the poorer your tool life, finish and accuracy is going to be.

The cheapest way to mill is to buy good tool holders (ER collets work well), good roughing end mills and high quality finishing end mills. Yeah, might not make economic sense until you actually use them and find they last much longer than junk.

 

[Boswell]

lack of compressed air is a big problem for milling slots in aluminum. Either using a mister or just an air gun, clearing the cut chips out of the hole is necessary for a good surface finish. While I have never tried this, perhaps you can build in a bunch of pause and retract actions into the gcode to give you a chance to remove the cut chips from the slot. Also taking more cuts at a shallower depth, will take longer but make clearing chips easier. Let us know how it goes. Oh yea, one more thing, accept the poor finish from the mill and then clean up the surface of the cut with sand paper. Let us know what you try and how it works.

 

[macardoso]

If compressed air isn't available, I'm a fan of gas duster cans for office use and WD-40 (just enough to keep the cutter wet, don't flood it).

 

[ThinWoodsman]

You don't need "a set" of roughing and finish end mills. Depending on the size of your machine and the size of the work you do, you can get a 3/8 or a 1/2 roughing end mill and use it for everything, If the slot is 1/4" as described, then get a 3/16.

I've had a couple of projects recently that entailed milling 1" to 2" deep pockets in unknown (mild) steel. Some things I learned:

* non-roughing HSS end mills dull quickly, especially when cutting on both sides and buried in chips
* start with a driled hole, then plunge-cut the largest hole you can get away with, then work with a rougher from the outside of the pocket to the inside, and use a standard end mill for the last pass of 0.005 or so
* when using the rougher, stop periodically to remove chips - forget compressed air, flood coolant, and all that unless you're in a hurry
* for deep holes, you may need to rough out twice: once at half-depth, once at full-depth
* finish the slot in one pass that will generate as few chips as possible, using low-pressure air (aka a turkey baster or bellows) to clear the chips

 

[KMoffett]

Another feed/speed calculator option (free): Calculator

 

[Mercedes107]

Well some good news today. I went back today with a what looked to be an unused end mill from the same low cost set I purchased on e-bay. It did look sharper both before and after the job was complete. Based on the comments I got in this thread I used a 3/16 end mill at 50% over speed from that recommended by the little machine shop calculator. Which came out to a recommendation of 4 IPM, so I used 6 IPM for the 2 flute 3/16" Cobalt end mill at 2400 RPM. I did the first pass right down the center of the path by telling the software it was actually a 0.25" endmill. That allowed be to evaluate the first pass only as I performed the task previously without vacuuming chips and with only WD-40. So the only variables that changed from yesterday were the diameter, feed speed and a change from CRC thread cutting spay foam to WD-40. I purposely did not vacuum for this first pass as I wanted to compare the results to yesterdays. The results are shown in pictures 4 and 5 before and after vacuuming the chips. While there is still quite and edge, it is a significant improvement over yesterdays results. In fact its good enough for most of the work I do after debur.

Now to see the effect on making closer passes and climb milling verses conventional milling. I reset the too software to a 0.2" diameter for the inside path and 0.3" diameter for the outside path, this ended up being 0.006" to 0.007" away from the final dimension. These passes were performed going around in the same direction, producing climb milling on the inside edge and conventional milling on the outside edge. The final passes were with the tool set at 0.1875" and 0.3125". Once again producing climb on the inside an conventional milling on the outside. The results of that were a definite reduction in the burrs but essentially no perceptible change between the climb and conventional edges

So my conclusions are as follows:
90% of my problems were due to a dull end mill
possibly better performance may be obtainable with higher quality end mills if needed
Better performance is defiantly achievable by making the last pass thin.
Difference between climb milling and conventional milling was not evident in this case

Other things to consider:
The suggested use of roughing and hi helix finishing end mills now becomes more practical with a CNC machine since I can now easily cut a 1" radius with a 1/4" end mill. Hell I can get rid on my boring bars and holder. Now 1 or 2 roughing end mill and high helix end mills goes a long way. So I will put some of those on my shopping list.

Many Thanks for all the help.

Next project will be CNC on steel.

 

[Mercedes107]

If compressed air isn't available, I'm a fan of gas duster cans for office use and WD-40 (just enough to keep the cutter wet, don't flood it).

I'm thinking of putting a propeller on the tool holder.

 

[macardoso]

My personal preference for aluminum cutting is YG1 branded "ALU-POWER" endmills. They are widely available on Amazon and eBay for easy purchasing. They are 3 fluted with polished edges and gullets for great chip evacuation. I have a 3/8" one that I have used for almost 2 years with no perceptible wear. Can't help you if you crash the machine and break it but they aren't too expensive for middle of the road carbide endmills. I would not use this on steel.

I'd try a 1/4" one, preferably with a short flute length (more rigid). You'll find it to leave a fairly mirror finish on walls if you keep it lightly lubricated while cutting.

LINK HERE

 

[Mercedes107]

My personal preference for aluminum cutting is YG1 branded "ALU-POWER" endmills. They are widely available on Amazon and eBay for easy purchasing. They are 3 fluted with polished edges and gullets for great chip evacuation. I have a 3/8" one that I have used for almost 2 years with no perceptible wear. Can't help you if you crash the machine and break it but they aren't too expensive for middle of the road carbide endmills. I would not use this on steel.

I'd try a 1/4" one, preferably with a short flute length (more rigid). You'll find it to leave a fairly mirror finish on walls if you keep it lightly lubricated while cutting.

LINK HERE

Thanks
They do look good.
Next challenge will be steel. I will be using carbide for that.

 

[macardoso]

Yikes! That looks like a complicated part! What is it for?