Novice to milling aluminum, questions about small precision milling

New to CNC milling aluminum.
Really basic questions.

Will a square and round end mill plunge cut the same, or is one cleaner/ faster?
Do they have similar too lifetime?

Milling a pilot hole for m5 threading (thread mill).
How big should the pilot hole be, or where can I look it up?

Same question with machine tap, m5.
Where can I learn hot to do a machine tap with blind hole?
What type of tool(s) can be used with an m5 tap in a blind hole?
(I have only done hand taps)

I want to mill a number of thru holes in a 3/4" bar (20mm), and it seems most end mills wont cut that deep.
Holes vary from 1.8mm to 6.4mm (about 1/16" to 1/4").
Suggestions?

Do square end mills cut on edges as well as end? I see the fluted part as "length of cut", but I'm
not sure if that means the fluted edge also cuts, or if the length is how deep chip removal works.

To avoid tool changes, I was planning to use a smaller diameter square end mill, like 4mm, and circle it to make a 6mm hole.
I assume thats no different than grooving with an end mill. Is it better to do shallow circles, or plunge full depth and do a slow circle?
or does it matter?

I find "SFM" as a "speed" limit, like 350 sfm for aluminum.
My desktop mill goes to 11,000 rpm. The sfm to rpm computation I saw for aluminum
gives much higher speed for small diameter end mills, like 1mm and 2mm than
my mill can go. Is running slower rpm ok as long as i run slower feed?

Where can I learn about milling small deep holes in aluminum?
Sizes like 6mm by 18mm deep, m5 threaded by 7mm deep, 1.8mm by 11mm deep.

Yep, pretty novice questions...

If anyone can answer 1 or 2 or more, thanks!

newbee

Not sure what you mean by round end mill, ball end mill maybe? A bull nose end mill with a corner radius would probably plunge the best and give you the best tool life.

As far as what size hole to drill for taps or threading. Look up metric tap drill charts. Or pick up a Machinery's Handbook(very useful). One tip for figuring out holes for metric taps is subtract the tap size by the threads for the drill to use. ex: m10x1.5 tap would use a 8.5mm drill(10-1.5=8.5)

Why mill holes thru in the 3/4" bar instead of drilling them? Drilling them is way more cost effective.

End mills cut on the edge of the flutes but they will also cut on the bottom of it if you are plunging or ramping.
Length of cut tells you how much material you can remove if you are at full depth of cut.

If you are pocketing out with a smaller end mill it is better to ramp the end mill into the part rather than plunge. Typically ramping the depth at 10% of the cutter diameter.

Not sure what you mean about speed limit. Running slower rpm is fine just remember to adjust your feed accordingly. Say your spinning at 10000 rpm on a 1 flute cutter going 10ipm, if you slowed it down to 5000 your feed would then be 5 ipm. Your feed is staying constant at .001" per tooth.

Is there a technical school by you to take some classes to get more proficient? I have found practicalmachinist.com has alot more members and way more useful information.

Hope this helps.

That helps a great deal. I have nothing more precise than a drill press, and a cnc desktop on the way.
So i dont even know what i dont know. For example, can my little mach3 milling machine also handle drill bits? I assume not.

Yes I meant ball end mill. Glad i asked, since neither of my guesses was right.

I need a blind hole threaded m5, then a perfectly centered thru hole either from same or opposite side, which is 2mm diameter.
Its for 3d print head and abs filament. There are many precision holes, and all must register with other parts.
I assume I will only get that precision with CNC, and multiple tool passes without moving work piece.

Other holes have similar issue, 2 diameters to deal with insulators and screw diameter, etc.

yes, you answered my question on speed. I was worried of the recommended speed was 20,000 i could not use it at 10,000 at all.
Slower feed makes sense.

Thanks again.

Helical interpolation is the way to go.
You can use a smaller dia. em, and make the hole exactly the size that you want.
Drill the thru hole 1st so that the chips from the 2nd tool can fall through, 2nd mill the blind hole for the tap with any size em you have smaller than the hole using helical interpolation.
IMO that is the best way to make a hole the exact dia. you want if you do not have a tool the size you need.
As for speeds and feeds.. carbide can run at 1100 sfm easy just use some type of coolant or your chips will melt to the cutter.
Feed rate of 120 IPM is fine too.
Sample code below:

N0101 (TOOL=1 PASS=1)
(EM .1875 4F)
( FINISH SIDE SIDE1)
G0 G54 G90 G40 G80 G49
G91 G30 Z0.
G30 X0.0 Y0.0
G0 G90
T1M06
S12000 M3
G0 X0.0062 Y0. T1
G43 H1 Z1.1 M8
Z0.1
G1 G17 Z0.01 F120.0
G41 X-0.008 Y0.0142 D01
G3 X-0.0223 Y0. R0.0142
G3 X0. Y-0.0223 Z0.0039 R0.0223 F32.13
G3 X0.0223 Y0. Z-0.0022 R0.0223
G3 X0. Y0.0223 Z-0.0084 R0.0223
G3 X-0.0223 Y0. Z-0.0145 R0.0223
G3 X0. Y-0.0223 Z-0.0206 R0.0223
G3 X0.0223 Y0. Z-0.0267 R0.0223
G3 X0. Y0.0223 Z-0.0328 R0.0223
G3 X-0.0223 Y0. Z-0.039 R0.0223
G3 X0. Y-0.0223 Z-0.0451 R0.0223
G3 X0.0223 Y0. Z-0.0512 R0.0223

This is using a 0.1875 3FLT dia. em with a spiral of 0.025 per rev.
Use this until you reach your Z depth.
Now you don't have to run this fast of rpm and feed rate but you can use cutter comp and that will make it easy to size your hole.



Good Luck! :cheers:




Attachment 220118

You generally want to drill holes with a drill bit, not an end mill. While there are center-cutting endmills, they don't drill as effectively as a real drill bit. You can also use drill-point endmills, if you really don't like changing tools. You can enlarge the holes with a regular side-cutting endmill once you've got them drilled. But if these are large holes that have to be exactly round (any backlash in your mill and they won't be), you're probably going to want to drill them first, then enlarge the holes to less than the full dimension with an endmill, then use a boring bar to get the finished dimension. A reamer can also work, if they're small holes where the boring tool won't fit.

Andrew Werby
www.computersculpture.com

For the precision holes i would just drill and ream. If you use a 135deg split point drill your location should be fine assuming your machine is accurate enough. Boring is great for getting holes to size and for location of holes but it does take longer than just drilling and reaming.

The through holes are 1.8mm at the smallest, 0.75 inches of aluminum.

I have found lots of drills that say they work with cnc, usually HSS.

Are the RPM's for drilling a 1.8mm bit different than a 1.8mm end mill?

Any concerns about the drill wandering off center as it goes through?

Quote:

---

Originally Posted by mrbl11

The through holes are 1.8mm at the smallest, 0.75 inches of aluminum.

I have found lots of drills that say they work with cnc, usually HSS.

[That should be able to drill aluminum.]

Are the RPM's for drilling a 1.8mm bit different than a 1.8mm end mill?

[A little; you want to go about as fast as your spindle will spin for a bit that small.]

Any concerns about the drill wandering off center as it goes through?

---

[Yes; to minimize that, start with a center-drill to mark the holes so it doesn't skid off at the start. Use a short drill rather than a long one. Do a peck-drill cycle to clear chips. And to get a 1.8 mm hole, use a drill bit that's smaller than that and ream to make up the difference. ]

Andrew Werby
www.computersculpture.com

the sfm remains the same assuming you are using a hss end mill. As awerby says spot drill the hole first then peck drill at 1xdiameter increments. a good rule of thumb for picking out drills for reamed holes is using a drill that is 97% the diameter of the reamer. ream at half the speed twice the feed. If you are using a 135deg split point you might be able to get by without spotting but i spot just to be safe. My favorite drills are from precision twist drill company

Why do you need to mill the holes? If you are threading them, just get the matching tap and drill; and drill the holes.

wow, I read the thread. I can't believe this is even an issue. I'm with mrquacker. spot, drill, C-sink (maybe?), and SEND THE TAP IN! I don't see it. I have to free up the machine, there's more work behind this job.

2 flute center cutting for aluminum to prevent clogging. Carbide if you can afford it but ms works fine as well.

Sent from my GT-N8013 using Tapatalk