[vonnieda]

Hi all,

I have a Taig 2016 CNC conversion that I bought last year and have been trying to teach myself to use it. I am a complete beginner to machining in general but I like to learn and have done a lot of reading and a lot of experimenting.

I'm having some troubles with the mill that make me wonder if I am just trying to do things it's not meant to do. I have a project I've been working on for a long time that requires me to mill out several pockets from a 4" x 4" x 0.50" bar of aluminum. I actually bought the mill specifically to make this part.

The short version is that I have never been able to successfully cut this part without breaking something. I'm not sure if I am trying to cut too fast, or too deep or what. I added flood coolant to the mill, which just barely works, but does seem to help.

What I'm looking for in this post is some experiences of people with a similar setup. Are you able to cut aluminum with no problems? What size tools do you use? What feeds and speeds? Do you use coolant? How deep do you cut per pass?

As a guideline, I am trying to cut pockets as deep as .475" in .50" 6061 aluminum.

I'm trying to decide if all this trouble would be better spent scraping together some money and buying a bigger mill

[escott76]

What kind of end mill (flutes and material), how fast, what DOC are you currently using? You should be able to cut this material with your mill, it's most likely not understanding the methods for getting there.
Leaving .025 in larger areas is gonna provide it's own challenges, just be aware that if you don't hold stuff down or use the wrong feeds and speeds, ripping through may be an issue.

[vonnieda]

What kind of end mill (flutes and material), how fast, what DOC are you currently using? You should be able to cut this material with your mill, it's most likely not understanding the methods for getting there.
Leaving .025 in larger areas is gonna provide it's own challenges, just be aware that if you don't hold stuff down or use the wrong feeds and speeds, ripping through may be an issue.

These are a lot of the questions I am asking for help with

End mills are 2 flute, solid carbide. The main one I am trying to use is 1/4". How fast and DOC are things I am looking for guidance on. I've tried a bunch of different mixtures. I can do things pretty well if I take like 0.050 DOC but it'll take till the end of eternity to make a part.

The info I am looking for is; for people who have and use Taig micro mills, what feeds and speeds are you using with 6061 aluminum? I'm trying to get a guideline so I can figure out if I am just doing things wrong or if I am pushing the limits of the machine.

Thanks,
Jason

[escott76]

These are a lot of the questions I am asking for help with

End mills are 2 flute, solid carbide. The main one I am trying to use is 1/4". How fast and DOC are things I am looking for guidance on. I've tried a bunch of different mixtures. I can do things pretty well if I take like 0.050 DOC but it'll take till the end of eternity to make a part.

The info I am looking for is; for people who have and use Taig micro mills, what feeds and speeds are you using with 6061 aluminum? I'm trying to get a guideline so I can figure out if I am just doing things wrong or if I am pushing the limits of the machine.

Thanks,
Jason

"The end of eternity" is a little over the top and dramatic. I prefer to deal with numbers like the actual cycle time, actual DOC, and feed rates.
You say you "break things every time", but won't say what feed rates you are using, or speeds. If you are looking for someone to just give you an answer and get it to work, it's gonna be a long road. Why not start by defining where you are, and then things can be suggested that would help you zero in. Breaking things every time (what things?) is not good, and does not have to happen.
First off, .050 on a .250 end mill is 1/5 the diameter, which is not too shabby for a small mill to push. I do that on my homebuilt mill and am happy, and my parts take a lot less time than until the end of eternity. You combine a smaller DOC with reasonable speed and feed, and you have a passable metal removal rate for the size machine you are talking about. Your mill only has so much rigidity and so much horsepower.

[jalessi]

Vonnieda,

How many of these parts do you need to make?

Jeff...

[vonnieda]

"The end of eternity" is a little over the top and dramatic. I prefer to deal with numbers like the actual cycle time, actual DOC, and feed rates.
You say you "break things every time", but won't say what feed rates you are using, or speeds. If you are looking for someone to just give you an answer and get it to work, it's gonna be a long road. Why not start by defining where you are, and then things can be suggested that would help you zero in. Breaking things every time (what things?) is not good, and does not have to happen.
First off, .050 on a .250 end mill is 1/5 the diameter, which is not too shabby for a small mill to push. I do that on my homebuilt mill and am happy, and my parts take a lot less time than until the end of eternity. You combine a smaller DOC with reasonable speed and feed, and you have a passable metal removal rate for the size machine you are talking about. Your mill only has so much rigidity and so much horsepower.

For speed I have been mostly using either 7500 RPM or 10,000 RPM. The information I have read has said that for small end mills like this you need high RPM to get a good chip. Additionally, my CAM software generally tries to set the speed to 12k or higher, and 10k is as high as the mill will go.

For feed, I have just been shooting in the dark. My CAM software shows 24 IPM. I have tried that and variously: broken end mills, stalled the motor, pulled the work out of the clamps.

I think that probably the main issue I am having is DOC. You say .050 is reasonable; I'll try that and try increasing my feed to see if I can get a reasonable cycle time.

Thanks for the help,
Jason

[vonnieda]

Vonnieda,

How many of these parts do you need to make?

Jeff...

Right now I am just prototyping. I don't really *need* to make any of them, it's just hobby stuff. If I come up with something that works I'll probably make 10 or 20 of this particular part in it's lifetime. I'm not dealing with production times or anything like that.

Thanks,
Jason

[jalessi]

Vonnieda,

Two parts took six hours to machine.

[ame="http://www.youtube.com/watch?v=oSDUaDG_Gfo&feature=related"]YouTube - LARGE MOUNT[/ame]

[vonnieda]

Vonnieda,

This part took six hours to machine.

Jeff,

Thanks a ton for posting this. Very informative video! Sounds like I just need a dose of patience

Also, your setup is very inspiring! Give me a lot of ideas for upgrading my work space.

Thanks,
Jason

[jalessi]

Jason,


We have a few Taig mills at our shop however the one in the You Tube video is not one of ours.

It belongs to: Peter Zicha

http://www.cnczone.com/forums/showth...468#post582468


Jeff...

[mike_mccue]

I'm a milling beginner as well... but I've worked with power tooling most of my life... so I tend to work in a tools comfort zone.

This part required 2-1/2 hours machine time:



1/4" thick 6061 stock
1/8" end mill
6000 rpm
0.06" DOC
2.0"/min feed

I haven't experimented with higher speeds because this seems to work well.

best regards,
mike

[wwendorf]

I don't use a taig, but here are some numbers that I think should work OK for you.

Try .50" DOC, 12" IPM, 3400RPM. I can cut using this same numbers with a .1" DOC on my Syil X3, so, with a Taig which is less rigid, those numbers "should" work OK.

Wade

[jalessi]

I don't use a taig, but here are some numbers that I think should work OK for you.

Try .50" DOC, 12" IPM, 3400RPM. I can cut using this same numbers with a .1" DOC on my Syil X3, so, with a Taig which is less rigid, those numbers "should" work OK.

Wade

Wade

I believe you meant .050" DOC.

Jeff...

[wwendorf]

Yup, you'd be right on that. .050" DOC. What can I say -- FINGER FUMBLE!

<grin>

Wade

[awerby]

and ramp up the speed as I gained confidence. Realize that the first part of the cut is the hardest. Even if you've got a center-cutting endmill (if you don't, that would account for some breakage) it's difficult for them to plunge straight into a piece of metal. The more sophisticated CAM programs "ramp" into a cut, moving across as well as down until they're at the right depth, and then start cutting. You can also make things easier by drilling a strategic hole where the pocket starts; this eliminates the plunge problem.

Also, the start of your pocket is the most difficult for the machine, as the cutter has to cut on both sides, and remove its full width. This has to go a lot slower than the subsequent cuts in a pocket, where you're only cutting on one side of the tool and removing only a fraction of the tool's width in material. Remember to program for the ramp and slower initial speeds at each successive level, since this problem repeats itself each time you plunge into the material. So while 12"/min will probably work fine after the first rectangle of the pocket is cut (in an "outside in" routine), you'll want to slow it down to around 2 IPM for that first critical bit.

Andrew Werby
www.computersculpture.com

[mike_mccue]

Andrew that is a helpful explanation.

I've been scratching my head when I see suggestions of 12ipm. It just didn't seem like my mill could do that. It makes more sense now that I consider going slow, as you describe, at the start.

best regards,
mike

[escott76]

Andrew that is a helpful explanation.

I've been scratching my head when I see suggestions of 12ipm. It just didn't seem like my mill could do that. It makes more sense now that I consider going slow, as you describe, at the start.

best regards,
mike

With the mill I built (similar spindle limitation) I regularly cut 6061 at .040 DOC and from 15-20 ipm. For Al on a small mill I will try to go with HSS optimized for aluminum cutting in the diameter you are talking about. Less prone to chipping with the rigidity (or lack thereof) of a smaller mill.
Spinning too fast and NOT feeding fast enough is gonna rub in the cut and cause lots of issues. You will have an optimum chip load for the end mill, and a reasonable SFPM. Although your CAM program may recommend higher RPMS that is also because it thinks you have the horsepower to keep spinning the cutter, and the table power to push at speed through material. Since you don't have those, you need to back off one to within the limits that you have and the other will follow.
Coolant always helps, but you have to stay within the power that you have available. Make the belt slip or the motor stall, and you have problems.

[SCzEngrgGroup]

Unless you like wearing out your tools in a hurry, maintaining proper chipload is *the* most important thing. For a 1/4" tool, you want to be around 0.001"/tooth. How fast and how deep you can feed is determined by how much spindle power you have, and how rigid the machine is. In this case, you're rather challenged in both. You want to be at about 400 SFPM in aluminum, which for a 1/4" tool would mean about 5000 RPM, with a feed rate of about 10-12 IPM. I'd guess a Taig probably won't do that at 0.050" DOC, so your best bet is to reduce DOC and aim for those numbers. Using carbide tools on such a small machine is a complete waste of money. There is absolutely no advantage.

Regards,
Ray L.

[vonnieda]

Unless you like wearing out your tools in a hurry, maintaining proper chipload is *the* most important thing. For a 1/4" tool, you want to be around 0.001"/tooth. How fast and how deep you can feed is determined by how much spindle power you have, and how rigid the machine is. In this case, you're rather challenged in both. You want to be at about 400 SFPM in aluminum, which for a 1/4" tool would mean about 5000 RPM, with a feed rate of about 10-12 IPM. I'd guess a Taig probably won't do that at 0.050" DOC, so your best bet is to reduce DOC and aim for those numbers. Using carbide tools on such a small machine is a complete waste of money. There is absolutely no advantage.

Regards,
Ray L.

Chipload is one of the things I have had the hardest time with. I don't understand the concept well. Is there a site, or something, that has a good explanation for the beginner? I mean, do I actually pull chips out of my swarf and measure them to determine how I am doing?

[jalessi]

http://www.akhurstcnc.com/chipload.htm