LinkBack URL
About LinkBacks
I actually just ordered that same mill from them this morning.
I will try it out tonight and let you know how it goes.
| | |
I've started working on a homemade paintgun, its going to be built much like a normal one, and so far I've been using the AR-15 Lower Receiver as a guide...
I'm just worried about absolutely massive milling times when I go to make one of these things, I understand small machine, small tools, long milling times, but I'm hoping to avoid the 20 hour marathon fate that my current tools are looking at...
I'm right now milling a 1/4x version of the receiver as a test, 1/4" 3-flute square end mill for the initial roughing then followed by 1/8" 2 flute ball to finish the profile... Currently my tool path is looking at 5 hours to completely run, and thats one side, got to flip it over and do the other half, another 5 hours in profiling I"m sure....
Would a 4 flute 1/2" carbide be pushing it for the Taig?
[edit]
Had a look around McMaster, I'm considering this one so far: Part# 8829A82
[/edit]
I actually just ordered that same mill from them this morning.
I will try it out tonight and let you know how it goes.
Looking forward to your review, especially the feeds/speeds/doc/finishOriginally Posted by 5artist5
I only had a few min to play with it last night. I decided that to give the new cutter a fair test I should do a nice job tramming first. I spent most of the time I had doing that so I didn't have a lot of time to test different setups.
I had the belt set on the second fastest speed.
I can tell you this, the face milling that I did was great! It left a great finish. I did notice that It didn't seem to want to go as deep as 3/16 cutter I had been using, but obviously it steps over much farther.
I also made a few side milling passes but I was not very impressed with them. I am hoping that the speed of feed was just off. As I said, i didnt get to spend much time with it.
I am going to play with it more tonight though, I'll post some pics if you are interested?
well, i did some more tests and i still didnt getgood side milling out of it.
the face milling is really nice though. It can remove a lot of material also.
Unfortunatly I was careless and I didnt clamp the work well enough and the cutter ended up digging in. It sucked the work peice out of the vice and threw it across the room! In the mean time 2 out of three of the fluts are ruined :-( So there goes that 40 dollar cutter.
Oh ouch, sorry to hear about that! What was the deal with the side milling? Come out fuzzy or something?
With an endmill of the type that you just brokeit should leave a very nice finish. I am sure it is just a speed and feed issue. I would say that that mill is probably too much for a Taig to push, not the least of the problems being belt slip when using the side of a cutter that large.
I would consider maximizing the speeds and feeds using the smaller cutters, say up to 3/8". The fastest I can cut on my Taig was 10 ipm, but that was as fast as the machine would go without stalling.
Mike
Warning: DIY CNC may cause extreme hair loss due to you pulling your hair out.
yeah, im going to try out a 1/4" 2 flute uncoated one like this 26865A33
That way im only out 15 bucks if it blows up! I need to get some hold downs too, there are a lot of shapes that the vice isnt good at holding tight enough.
A 3/8" 2 flute should be fine. Get good quality un-coated carbide (OSG, Niagara, etc...). That's what I use on the Sherline. A Taig is a beefier machine, it should handle it no problem.
I run either a 3/8" .025" DOC at 8IPM
or
.02" DOC at 10IPM
in 6061T6. About 70% step over for both.
Any more and the finish starts to suffer (I think from column flex)
A Taig should be able to handle at least 3/8" EM .035" DOC at 10 IPM. If it can't the limiting factor is the electronics, not the machine.
Good luck.
Use roughing end mills. You can get them pretty cheap out of Enco's Hot Deals catalog. I have some M-42 Cobalt ones made in Spain that cut excellent on my Taig. If I remember correctly (haven't been running my Taig much lately) I could go about 5k RPM at 15-20 IPM and 0.100" DOC, full width cut. You just have to lay on the coolant (flood or mist) to remove the heat and keep it all lubricated nicely.
Also see this link to my website to see a Taig mill out an AR-15 lower. That'll give you a good plan of attack and if you have any questions on the setup/machining feel free to ask. Also, its very important to tram your mill correctly before machining a large part like the lower else you'll have accuracy problems.
Holy crap, thanks for the link!
So far I've been running a 1/4" carbide (SGS) at 0.035" DOC at 21 IPM dry... Up until recently, without air either...
Any opinions on high/fast helix (aka 60 degrees) tools? Opinions on TiN coatings as well? I don't imagine my little Taig can push a tool to the point where the coating becomes useful.
I've found that coatings mostly help when running dry or with minimal lubrication. The roughers I use have a TiAlN coating which supposedly lets you run dry, but not at the speeds/feeds we run. Those cutters are made to take a massive chip load (which aids in putting the heat all in the chip and not the work) which keeps materials like aluminum from getting gummy and galling onto the cutter.
When running roughers (or any other cutters) as of lately I've just been giving it a squirt of WD-40 every once in a while and brush the chips out of any the way of the cutter to keep them from being re-cut. I used to run flood coolant quite a bit, but the Taig is just not made for flood coolant and it eventually caused some scarring of the X axis dovetails from chips getting flushed in there. If I were to use my Taig more (I mostly use the Fadal or Bridgeports at work now) I'd probably invest in a mist setup to keep the temps down and clear out the chips as well as providing the necessary little bit of lubrication.
The issue with our Taigs is that they are not beefy enough to load up the cutters to the proper chip load. This results in lots of friction at the cutting edge which results in a lot of heat buildup which can cause bad things to happen in soft, low softening point metals like aluminum.
If it helps any, I try to use solid carbide tooling for nearly all of my cutters. I've found Atrax tooling to work quite well in a lot of machining applications on my Taig (they're also about the same price as US made HSS cutters if you get them through Enco's Hot Deals magazine). Carbide will minimize deflection of the cutter (less broken cutters, better surface finish) and will last a lot longer than HSS cutters.
Oh, the other problem with underfeeding the cutter that I forgot to mention was that they will dull quicker due to higher cutting speed that we usually end up running (which also results in more effective cuts per tooth per tool path) and the cutting edge not being able to bite off enough to get past the heat affected work hardened zone (only applies to steels, stainless steels and some other exotics, not so much with aluminum).
I noticed a huge tool life improvement, cut quality improvement, feedrate and DOC improvement when I switched from (quality US made, mind you) HSS cutters to (cheap end US made) carbide cutters. Luckily for us the tooling is so small that the price difference is nearly negligible. I've also had good luck with Cobalt tooling (roughers, drill-mills, etc.).
FWIW, I plan on doing some more AR-15 lowers someday, but this time on the Fadal at work so I don't have to sit there in the basement for who knows how many hours on end.
Posting Permissions
| | |
