Getting Rough edges on Taig milling aluminum, please help

[b0gh0s]

Hey guys, I have a Taig CNC mill and am having a bit of trouble with getting some rough edges on the machines edges of the parts I am making.

I am running at 5ipm, about 2K on the head using a 5/32 2flute carbide end mill (.06 doc). I have retuned the mill to ensure no run out and the ways are really smooth, (no wag or run out as far as I can measure).

I am machining parts from .25 inch aluminum, they are small bearing blocks and I am basically taking strips of 1.5inch by .25 inch thick aluminum, milling the bearing seat and then cutting the part out by machining the outline of the part. I am fixing the stock in with some pretty decent vices by taking the strip, laying it flat in the vice (over a piece of wood) and tightening the vice down real well. I am brushing on some lubricant in the begining with an acid brush (tried cutting oil and kerosene on separate occasions).

My edges look really crumby, can you guys suggest some things to look for so I know how to chase this down?

[b0gh0s]

Sorry that is not 5ipm that is a "feed" of 5.

[tomsin22]

What alloy aluminum are you using? Are you taking a finish pass. Make sure you get the chips away from the tool, an oil mister works great. Also if you can get a faster spindle speed my help.

[b0gh0s]

I believe it is standard 6061 aluminum,

I have tried changing the pulley ratio to get a higher head speed, it didn't seem to make much difference just a higher pitched noise when it cut. I just tried cutting another part this morning, I 'misted' wd40 and used a air hose to blow out the chips, I also have a vacuum hose near the head which helps to suck out the chips. None of this made a difference, is it possible to wear a carbide bit out in aluminum? I am making smaller parts with a number of curved surfaces in them, I have probably cut between 30 and 50 parts with this em.

I am not doing any finishing passes, I was hoping to get a fairly even edge cut and then do basic finishing on them (no high shine or anything like that).

The cut edge is coming out with lots of uneven vertical (same direction as em up and down) divots and scratches.

[tomsin22]

Yes it is possible for a carbide endmill to wear. Carbide endmills are more for high spindle speed milling a 5/32 endmill should have a spindle speed around 5k or higher. I would try playing with the feed and maybe less of a doc cut. Also a new endmill may help.

If you are slot milling the part ( you have material on three sides of the endmill) you most likely will get a bad finish becuase the chips get gumbed up in the tool and cause the divots and makes the tool vibrate and you get the vertical lines. You may have to take a .005 - .010 finish pass.

[tomsin22]

How far is your tool sticking out of the collet? This maybe a factor to. The shorter the better

[cncharleydude]

I have got those type of finishes before but its usually from going too fast on my feed and not allowing for any finish passes at a slower feed rate. Normally I will run my RPM at fast as I can with alum. 4000RPM. Also I seem to get better finishes with a 3 or 4 flute endmill and I always climb cut.

[b0gh0s]

Well I took the tool back to J&L and explained what I was doing and they replaced it free of charge. The guy said that it felt kind of dull. I got a few more of the same just in case and went home. I tried a new em and it worked MUCH better, I think I must have just had a bad EM. I am getting a much more reasonable cut now.

This is slot type milling where i do have material on 3 sides of the EM. For these parts I am not really sure of another better way to get the outer edge. I am using RAMS to generate my Gcode and then doing some minor manual tweaking to adjust things.

Couple more questions,

1) Can someone point me to a succinct explanation of how I should figure out doc, feed speed and spindle speed for aluminum based on the EM size?

2) for a part with complex curved edges all the way around it, what are some ideas or suggestions you all might have for securing the material and then cutting the part out if I wanted to avoid slot milling? How can I fixture a part (like a 1x1x.25 alu bearing block with complex curved and straight edges) so that I could do a finishing pass?

3) Any suggestions on how to machine a nice beveled edge all the way around my parts? What would I search for if I was looking for a tool to do that?

[little bubba]

b0gh0s, Trying to step down like that while slotting is going to give you a crappy finish, carbide or not. I'm sure your situation is made even worse by having a smaller unrigid machine.

I'm not sure if your dropping the part out of the bottom or it is still grabbed by the vice? If its still grabbed by the vice, make a finish pass, if its dropping out, rough it down to .220 depth or so, leaving .005 for a finish, then finish to depth, and then run a finish that leaves at least 3 tabs to the original material. A little hand work at the end but it works for a small run.

For a better answer, post a pic, I'm sure you will get all kinds of good help.

For a quick chamfer around the edge to make it look nice, J&L sells micro100 mill drills, 90 degree included angle. They make wonderful chamfering tools and last damn near forever, just don't try and use them as a spotter.

For speed feed and DOC on aluminum, I think more is based on availability of coolant than anything. In general though, from my expierience, 1600 sfm for carbide endmills, 600 for HSS, 3000+ for indexables(with lots of coolant). As for DOC, step over and chip load, they seem to go hand in hand, increase one, decrease the other etc... I have yet to find a good catalog, book or anything that gives accurate info. Expierience, tool life and spindle load will let you know when you are where you need to be, for your particular set up. You will break endmills figuring it out, but at that size they are fairly cheap, though why 5/32? not a straight eighth? More common and cheaper?

[b0gh0s]

5/32 choice was somewhat arbitrary, I have a plethora of 3/32 EMs I get cheap which I use on my router bed for carbon fiber and I had some 5/32s in my random bin of stuff when I started building gcode for the parts I am doing.

Basically, I am dropping the part out of the bottom

What I found by experimentation is that things come out a bit better if when I do DOC at .05, and set the total cut depth for .27 (on quarter inch material).

Basically, the software automagically calculates the passes and I manually edit them (so I have passes at .05, .1, .15, .2, .25, and .27) so that the .25 pass is just another .2 pass, then I punch through and manually sand off the nipple that is left on the one edge of the part.

The only way I can figure to do this is to refixture after I machine the bearing seat so that the part is fixtured to the vice somehow and then machine around the edge. I will post pics in a bit. I like the idea of leaving tabs somehow...

I think I have my Taig pretty well tuned, there is very little runout/play in the table when I checked with a dial indicator, I have the ways pretty tight and they are still smooth. The old EM was really noisy, the new one seems to be quiet as a mouse(comparitively).

[l u k e]

little bubba]b0gh0s, For a quick chamfer around the edge to make it look nice, J&L sells micro100 mill drills, 90 degree included angle. They make wonderful chamfering tools and last damn near forever, just don't try and use them as a spotter.

Why do they not work for use as a spotter?

[titleist]

try using a high helix endmill and moving thru the part a bit faster