[conlimon]

hey all -

i'm a newbie with my Taig 2019 er16 setup from Deepgroove1, and i'm having a bit of trouble getting aluminum to machine nicely. I've been building parts out of acrylic with no trouble, and the machine setup seems good. when i cut aluminum, i feel like some of the chips are getting embedded back into the work, creating a rough looking cut. i guess i'm asking about a starting point for spindle speed, feed speeds, and depth of cuts to get a high quality machined surface. the result i'm having is that when i cut a groove with a square endmill, the sides of the cut are sort of rough. is this normal?

any help would be greatly appreciated. just as a point of reference, i'm using my Taig to build parts for the aircraft that i'm building. my website chronicles the shennanegins here... www.perfectlygoodairplane.net
for any interested. some of my early attempts at using the mill are pictured here:
http://www.perfectlygoodairplane.net...op%20Mill.html


thanks!
cj

[mark c]

Hi CJ
Looking at your pics, It looks like you are cutting dry. With al you need a coolant/oil otherwise it will gall. Use WD 40 if you have nothing else, but you can get a coolant mist system from www.littlemachineshop.com for pretty cheap.
It also looks like you are conventional cutting. To cut the outside of a feature you should go clockwise and on the inside go CCW. This will give a better finish. It's also best to leave .01" on the side and take a finish pass.
That said, a surface speed of 350/450 for a high speed steel end mill is a good starting point, for a 3/8 end mill that is from 3565 to 4583. 1/2 is 2673 to 3437. Depending on the rigidity of the mill (don't know much about Taig) the feedrate will be RPM *.002(+or_)* the number of flutes on the endmill. This can vary widely, but start at .002 and work up or down. For just cutting the outside of a part when the endmill is fully enveloped in the material, I would go no more than 1/3 than the diameter of the tool deep per pass. Depending on the rigidity of the Taig it could be more or less, probably more toward the lesser side.
Hope this helps. It would be a good idea to blow out the cutting area from time to time, but if all you have is a vacuum, then use that.
Let me know if you need more hints and good luck

[warossignol]

If you fly cut try putting a small radius on the bit tip.

[warossignol]

If you fly cut try putting a small radius on the bit tip.

[scubasteve_911]

Hey CJ,

First of all, I'm not a master machinist, but I am a pretty logical person and I have been using the Taig for a few months now.

When we first started out, we used four-flute endmills for cutting into the 6061 aluminum. Big mistake! Stick to 2-flute endmills if you can, the're very good for aluminum. Otherwise, the four flutes can get clugged and chips compact in there, then that's what causes a terrible finish and potentially an endmill break depending on diameter.

I use Mastercam for generating toolpaths and I stick to their recommended spindle speed and feedrates. These can be calculated easily, but I'm too lazy. The rest of the poor finish problems originate from chatter.

Suggested Modifications for you:

1) Use isolation vibration standoffs for the induction motor, available from McMaster-Carr, I forget the part #

2) Bolt that baby down to something big and heavy ( i used a 100lb concrete slab )

3) Use some of that white dryer tubing to make cheap bellows to better protect the leadscrews from chips, or go all out and spend 500$ on proper bellows.. I'm happy with my fairly ugly 5$ solution

Steve

[conlimon]

that is all excellent info - many thanks to those who posted. i'm cutting some stuff this weekend, so i'll give the suggestions a try, and report back!

cj

[mxtras]

At least use an air blast to keep the flutes clear. Direct the air to blast the chip out of the flutes as soon as possible. Of course, this is easier said than done, so multiple nozzles are always helpful. You can make a manifold and use small diameter brake lines or copper tubing to direct the flow and create some flexibility.

One trick to determine speed/feed is to measure the chips coming off the cutter. If they are not coming off the cutter, that's a big problem. Anyway - the thickness should be somewhere around .006" to .007" max for tools smaller than about 3/16" and somewhere around .009" - .010" for larger cutters. These are my guidelines. Always try to use the largest tool the part will allow. The larger diameter will not lolipop as easily since they typically have better flute shape and volume.

Scott

[scubasteve_911]

I think he is already doing something similar by holding a shop vac right onto the workpiece while milling. I like your idea about the tubing, it would be fun to make a shopvac attachment that you can run to a semi-rigid pipe then have directly over the endmill.

CJ,

I forgot to mention you can buy high-helix endmills especially made for aluminum, but they're too much money for my blood.. If you check out an ebay store called Discount Machine Shop, he sells 8% cobalt endmills (either 2 or 4 flute) with a 3/8" shank and various cutting tool diameters for dirt cheap. I buy all my stuff from him, $3.50$ is hard to beat for an endmill

Steve

[mxtras]

I really don't think a vacuum is going to provide enough pressure to blast the chip from the flute of a rotating cutter. My suggestion was to use the force of the air blast to clear the flute - not to simply clear the path of chips. The chips tend to want to stick to the flute right at the cutting edge. As the cutter rotates, the next cut on that flute welds the sheared aluminum to the previous chip and the cycle continues until you have a spinning aluminum lolipop.

Using an air blast should be a second choice to flood or mist coolant for aluminum but it is effective for small diameter tools. Air volume is not critical - a directed pressure stream is the key.

Scott

[scubasteve_911]

Ahhhh, I gotcha, I didn't think air would provide adequate pressure because if a chip gets compressed on there, it takes a hell of a lot of force to get it off.

Steve

[mxtras]

That it does. If it is stuck on there that well, your feed/speed is way off.

With good chipload, the chips will pretty much fly off like they do milling any other material (well, almost). Over a short period of time, there will be build up on the face of the flute when cutting dry.

Like I said - measure the chip thickness. Just as when drilling, focus on making a good chip and treat the cut as a byproduct rather than the other way around.

Scott

[ZipSnipe]

Mxtras makes a good point. However you didn,t say if you were face milling or pocket milling. With face milling a carbide face cutter(if they have one for a Taig) is the way to go(and you could use it dry). For pocket milling flood coolant is the preferred way to go or at least use the blast of air. We mill lots of aluminum where I work and those are the two methods we use.

[txcowdog]

Hey Steve,

Thanks for the referral to Discount Machine Shop.

[Geof]

It is close to impossible to consistently get a good finish on aluminum without some coolant or lubricant. One cheap and easily obtainable lubricant you can use is automatic transmission fluid; just brush it on down the path you will cut, even a small amount will prevent the chip welding to the tool.

[scubasteve_911]

Hey Steve,

Thanks for the referral to Discount Machine Shop.

No Problems! When you're a poor engineering student like myself, you just have a nack for smelling out the best values

Steve

P.S.- Discount Machine Shop is actually a company called Shars at www.shars.com , but they offer pretty much everything that is listed online at Shars at a discounted price on Ebay. To place an order, I give ebay links in an ebay with quantities. If there is something in the catalog that isn't on ebay, I can order it this way from them via a part number. I have been very happy with their stuff and won't go anywhere else. I ordered a 31$ screwless vice and I was astounded by its quality.. Maybe because I am new to machining, but I couldn't believe that I cannot see the seam where the vice closes, even under very good lighting...

[bnocturnal]

hey all -

i'm a newbie with my Taig 2019 er16 setup from Deepgroove1,

Hello,

I was wondering if this is the setup you purchased: http://cgi.ebay.com/ws/eBayISAPI.dll...ksid=p3907.m29

And are you happy with it? I saw one other post on here that was not happy with Deepgroove1, but they seem to have a really good price on the Taig.

Thanks,
Dave

[fredhh47]

Here is a trick I use when I need to lubricate the cutter on my milling machine. It can get a little messy, but works well enough that I haven't invested in a dedicated mist sprayer. Put an acid brush in a can of dark cutting oil and have it sitting near your machine. When the cutter gets into the cut, take the oiled-up brush in one hand and an air hose in the other. Put the bristles of the brush into the air stream while aiming the air stream at the cutter. Voila', a do-it-yourself mist spray. This really works very well when flycutting or face milling, but also is fine for slot milling. If this fails, buy a cheap mist spray unit and some water-soluble coolant and mix it very thin. I use about one to two ounces of WS concentrate to a gallon of SOFT or de-ionized water (like for steam irons). My hard water makes a goopy mess and the crap doesn't dispense well. P.S. when using the dark oil, be warned that it smokes and stinks. Open a window or a door for ventilation.
Fred

[Jacksonqin0305]

Hi,this is Jackson, mechanical manufacturing engineer with extensive field knowledge and work experience and my factory located in the world manufacture base center Dongguan/Shenzhen,China,
we offer Lathe and Milling/sheet metal fab/parts stamping service, any new works,
Just contact me,[email protected] / whatsapp+86 13532883201 skype bailong0305,thanks