[Pysiek]

Please forgive me if this is inappropriate thread here
I have a small part to mill. I will use my CNC X2 LMS mill. The material I will use is 6061 3/8" thk aluminum. The part will be cut out out of 3.5" x 2.5" scrap.
What feed , spindle speed and cut depth should I use for each pass? I will use 3/8" flute with two teeth.

[txcncman]

Get a copy of Machinery's Handbook and learn to use it.

Assuming uncoated carbide, I would start with 450 SFM. So, now let's learn to do the math on that. SFM is Surface Feet per Minute. Your end mill is measured in inches. So, you have to do a conversion.

RPM = (SFM X 12") / (d X PI)
RPM = (450 X 12) / (0.375 X 3.1415)
RPM = 5400 / 1.1781
RPM = 4584

Now for feed rate. I would start with 0.004" per tooth. More math:

Feed = RPM X Feed per tooth X Number of teeth
Feed = 4584 X 0.004 X 2
Feed = 36.67 IPM

For depth of cut, I usually start with what I call 50/40. 50% of diameter for Axle and 40% of diameter Radial Depth of Cut (DOC). So, 0.1875" for the axle DOC and 0.150" for radial DOC.

Most of this information is in Machinery's Handbook. Examples of the math are in Machinery's Handbook.

[Pysiek]

txcncman thank you for your reply. My machine can only go 2500 RPM. So if I want to run it on 2500 RPM I have to pick 250 SFM?
Why you choose .004"? Is there a definition or some kind of table?

[txcncman]

txcncman thank you for your reply. My machine can only go 2500 RPM. So if I want to run it on 2500 RPM I have to pick 250 SFM?
Why you choose .004"? Is there a definition or some kind of table?

If the RPM calculation gives you a number higher than the limits of your machine, you have to use the limit of your machine for RPM. So, the calculation gave 4584. You will use 2500. This changes the feed rate calculation:

Feed = 2500 X 0.004 X 2
Feed = 20 IPM

I choose 0.004" because you are machining aluminum and not steel or stainless steel.

Tables are in Machinery's Handbook along with descriptions and explanations of machining operations.

[Pysiek]

One more question. Where did you get the 450 SFM from?
And the tool is HSS

[hoss2006]

Physiek, here's a HSS Feed and Speed chart, go with no more than .002 chip load for the X2, carbide could run higher.
http://www.endmill.com/pages/trainin...nd%20Mills.pdf
Also here's a nice Speed and feed calc.
Milling Calculators
The best would be Bob's GWizard.
GWizard: A CNC Machinist's Calculator for Feeds and Speeds
Hoss

[txcncman]

One more question. Where did you get the 450 SFM from?
And the tool is HSS

I got 450 out of my head. The actual low end of the scale is 500. Here is a chart from Machinery's Handbook for your use:

[Pysiek]

Thanks Hoss. I have seen your website also and I have a question for you. What kind of vise did you use on your X2? The current vise that I have purchased from LMS extends over the table and because of that I'm limited with the travel. Do you know anything about some kind of small vise? The current one I have is : http://lmscnc.com/1699 . When I mount it on the table I can't turn it around because the mounting bolts are sticking out.

[hoss2006]

I had a 3 inch LMS vise on my X2 but some folks squeeze a 4 on theirs. More ideas here.
http://www.cnczone.com/forums/bencht...t_vise_do.html
Hoss

[txcncman]

I want to emphasize that the recommended speeds and feeds you get from Machinery's Handbook, a tool vendor, or any other source are just that, a recommendation. You can think of it as a starting point. What actually works best on your machine, with your material, with your tool, with your tool holder, with your work holding, machining your part feature may be different than the recommendation. This is where years of experience comes into play. And this is where I can grab a number like 450 out of my head.

As much science as there is in machining, there is still a lot of art involved. Craftsmanship. Artisanship. Even the way the sunlight is shining through a window at a certain angle can make a difference on how something machines from one day to the next. Make lots of sacrifices to the machining gods to help offset all these variable.

[Pysiek]

Guys I set up the machine as:
Feed 20IPM
RPM 2500
depth of cut .1875
tool dia .375
2 teeth

When I start to cut the whole machine start shaking and go out of adjustment. I need to retighten everything after it's done. And also do a terrible job machining.

[Starleper1]

Do yourself a favor and get a subscription to Gwizard. You won't be sorry. There are many additional conditions to look at other then the basics you find on a feeds and speeds chart. Those charts are to get you in the ballpark.

One particular setting you will need to account for with having a smaller machine, is the hp/weight ratio, which the Gwizard can calculate.

[SuperFlyLoser]

Guys I set up the machine as:
Feed 20IPM
RPM 2500
depth of cut .1875
tool dia .375
2 teeth

When I start to cut the whole machine start shaking and go out of adjustment. I need to retighten everything after it's done. And also do a terrible job machining.

I used the info you gave and put them into the speeds and feeds link that Hoss sent to you. HERE and it gave me 10 IPM

Then I put the same parameters in Gwizard and got between 9 and 13 IPM (2 lowest Conservative settings). So how did you get 20 IPM?

SFL

[Pysiek]

I'm sorry. Before I used the bit with 4 teeth that's why. But I have tried the 10 IPM and still same thing.
I have asked a CNC guy at my work and he told me that if my tool is cutting the part with whole dia then I should go with 6 IPM and only .030-.060 deep cut

[steamboatmodel]

I'm sorry. Before I used the bit with 4 teeth that's why. But I have tried the 10 IPM and still same thing.
I have asked a CNC guy at my work and he told me that if my tool is cutting the part with whole dia then I should go with 6 IPM and only .030-.060 deep cut

Unless you have to you should limit your cuts to 1/3 of the tool Dia.
Regards,
Gerald.

[Pysiek]

I might use a smaller bit about 1/4" or 1/8" dia.

[Kingjamez]

txcncman gave you terrible advice competely overlooking the fact that your are using an X2. Try a 1/4" endmill and a 0.05" DOC and watch the machine perform a lot better.

[mrcodewiz]

I had the best luck with 3 or 4 flute 1/4 to 7/16 end mills on the X2 but I normally cut at a max depth of .1 inch with the 3/8. I think I ran around 13 to 15 IPM.

If you haven't already, make sure all the gibs are tight as well.


edited to add: I also have the belt conversion so I was probably running higher than 2500 RPM. IMO, The belt drive is the best thing you can possibly do to an X2.

[Pysiek]

I also have the belt conversion so I was probably running higher than 2500 RPM. IMO, The belt drive is the best thing you can possibly do to an X2.

My X2 comes with belt conversion. There is no gears.

[Pysiek]

txcncman gave you terrible advice competely overlooking the fact that your are using an X2. Try a 1/4" endmill and a 0.05" DOC and watch the machine perform a lot better.

That what my CNC guy told me to do because the X2 is only 0.62HP