Gunsmithing Machinist question

[shadow_sniper]

I am using a bench top, a 2x. I needed to remove a section 1.45 x 2 x 2 of 6061 aluminum. I ended up using a 3/4 end mill and took a bunch of facing cuts about .02 thick. If I took any cuts bigger the machine would shake badly. I had a spindle speed of about 2000. The cuts took about 40 min or so to make. This just seems like a really long time. What am I doing wrong because I need to do this cut one more time on the other side of the part?


I am also about to need to remove a section 11 x 2 x .4. how would you recommend I do this?

 

[wnroscoe]

Re: Machinist question

small machines / small cuts = no chatter and good surface finish

small machines / large cuts = chatter and poor surface finish

With an RPM of 2000 try a feed rate of .007 to .008" per revolution to start with and then finish at .001" per rev. Small machines will take longer when removing large amounts of material. There's nothing you can do except move to a larger machine.

 

[jimmyrjessie]

Re: Machinist question

What is said above is the truth and nothing but the truth! But there is the option of plunge cuting which is a good way to rough out lage amounts of matl.

 

[Long_Action]

Re: Machinist question

the eng mill should be going 500ish rpm. be sure you are spraying some type of oil or coolant on the cutter.... oil works best to keep it from loading up. Maybe try a smaller cutter with a faster feed if the machine is shaking and make sure you are conventional not climb milling.

L_A

 

[triggerguard1]

Re: Machinist question

Drilling is the fastest and most efficient manner of machining there is. Use a twist drill to hog the material out, which will be less stressful on your machine and mill tooling.

Next, formulate a plan to acquire a real manual milling machine. Benchtop models are for plastic and playing.
Don't get me wrong, many people have to resort to their use because of either space, power, or finances, but if you really want to machine something, you'd best have the right tools to begin with.

 

[AJ300MAG]

Re: Machinist question

500rpm for a 3/4" endmill on 6061 aluminum?

I run roughers and finishers at 1500rpm with 30" feedrate for a 3/4" HSS endmill when cutting aluminum...

For the OP, Plunging or drilling to remove the extra stock. Use WD40 as a cutting fluid. A rougher will cut better when removing excess stock, switch to a standard endmill to finish the job.

 

[mark4567]

Re: Machinist question

<div class="ubbcode-block"><div class="ubbcode-header">Originally Posted By: wnroscoe</div><div class="ubbcode-body">small machines / small cuts = no chatter and good surface finish

small machines / large cuts = chatter and poor surface finish

With an RPM of 2000 try a feed rate of .007 to .008" per revolution to start with and then finish at .001" per rev. Small machines will take longer when removing large amounts of material. There's nothing you can do except move to a larger machine. </div></div>

+100 couldn't say it any better!

 

[[email protected]]

Re: Machinist question

If you have a sharp 1/4 inch or 1/2" end mill you might try it- cut the outside with it then go for the center- 6061 is not a real tough alloy like 7075 or even 2024 and you don't mention heat treatment, but this should work better with a smaller machine and even if your metal is -o (soft/annealed) end mills don't usually 'load up' too bad. Check for it and leave an 1/8" till you see if it will work for you- then leave .010 or .020? for a 'finish cut'

If you are pushing the limits of your machine a 1/4" end mill will remove the same amount of metal per minute as a 3/4"-

I Haven't tried enough machine work with a mill to suggest speed or feed so do some trial and error-

 

[Long_Action]

Re: Machinist question

500rpm for a 3/4" endmill on 6061 aluminum?

I run roughers and finishers at 1500rpm with 30" feedrate for a 3/4" HSS endmill when cutting aluminum...

Speed kills your running your cutter way too fast. Is this a cnc or vertical mill? You don't run 3/4" HSS cutters that fast!

 

[300sniper]

Re: Machinist question

i just started playing around with radial chip thinning. the last project i did that had a lot (a lot considering what i normally do) 1018 steel to remove, i used a 1/2" 4 flute coated carbide end mill at a 1" axial depth of cut and .010" radial depth of cut at 2240 rpm and 60 ipm. i removed about 8 lbs of steel in about 40 minutes with a little 1.5 horsepower machine. i don't know how this would work on a manual machine as the feeds are pretty fast but from what i understand, the cutting forces are greatly reduced which i think should help with a small "flexible" machine. you are also working with the entire flute length instead of just wearing out the bottom.

in my opinion, a 3/4" endmill is a bit much for a small machine. i don't think you said what material your endmill was so i can't give an opinion on the speed. i'd probably step down to a 1/2" endmill to lower the cutting forces a bit. maybe try a full flute length depth of cut but small radial depth of cut also. now matter what, a light machine makes light cuts.


edit: i am just a self taught garage hack speaking my experience. don't take anything i say as gospel.

 

[AJ300MAG]

Re: Machinist question

The cutting speed of HSS on aluminum is 300SFPM. Your running about 100SFPM. That's fine for CRS, way to slow for aluminum.

Bridgeport with an airblast mister.

 

[300sniper]

Re: Machinist question

<div class="ubbcode-block"><div class="ubbcode-header">Originally Posted By: AJ300MAG</div><div class="ubbcode-body">The cutting speed of HSS on aluminum is 300SFPM. Your running about 100SFPM. That's fine for CRS, way to slow for aluminum.

Bridgeport with an airblast mister. </div></div>

300 sfm is right for hss in aluminum. i agree with a .75" diameter cutter at 1500 rpm. it actually calcs out to be 1527.8 rpm.

 

[AJ300MAG]

Re: Machinist question

Yep, so just round it off. Could have said 1525rpm, what's a few rpms among friends...

 

[CDiPrecision]

Re: Machinist question

I run 1/2" Carbide 3 flute EM at 10,000 RPM, 200 IPM 1/4 inch depth of cut.. works good and leaves a decent finish..I slow the feed rate for plunging, but its all on for XY moves..

 

[Glen Seekins]

Re: Machinist question

For your smaller machine you can still get it done. I would saw cut as much as possible first. I would use a 1/2" em, full RPM and make it cut with about 25% stepover. Its important that you are climb cutting. Pick your stepover go at least 1/2" deep and see what it will do. If you still have power go deeper, but do not go wider with your cut. By doing this, it is called radial chip thinning and you wont use as much horsepower

 

[JWArmory]

Re: Machinist question

I use a handy dandy little equation.

3.82 x SFM / D = RPM where:

SFM is surface feed (taken from about any tool catalog based on the tool type and material, redline tools has a good one I use a lot)

D is diameter of the tool.

 

[txlimey]

Re: Machinist question

Like CDiPrecision said people who are machining Aluminum all day use carbide/PCD tooling running on high speed spindles.
I have personally seen both Magnetic Bearing and Air Bearing Spindles used for machining Aluminum. These were running a 40-60,000rpm, and up to 60hp in size. They were removing 1200 cubic inches per minute, with mirror like finish.

 

[Glen Seekins]

Re: Machinist question

We use only carbide, high end tooling and with the robodrill we have 24000 RPM. it is scary fast

 

[shadow_sniper]

Re: Machinist question

So what should I be doing conventional or climb milling?

 

[Long_Action]

Re: Machinist question

If your using a small machining center I would drop your cutter size down to a 1/2" Try taking small passes conventional milling with a good feed rate. Maybe .050 deep...Does your machining center have a power feed? I would keep your rpm's around 1000 with a 1/2" carbide endmill(spray the cutter dorn with oil). post a pic of the machine and give me a good idea how thick and tall the ways and lead screws are. Crazy things can be done with larger mills and or cnc equipment but I have seen many cnc machines have new lead screws, shear pins, and spindles installed due to beating on the machine. With a benchtop machine I suggest only climb milling on your last final pass to leave a good surface finish.

 

[Sean the Nailer]

Re: Machinist question

<div class="ubbcode-block"><div class="ubbcode-header">Originally Posted By: jwarmory</div><div class="ubbcode-body">I use a handy dandy little equation.

3.82 x SFM / D = RPM where:

SFM is surface feed (taken from about any tool catalog based on the tool type and material, redline tools has a good one I use a lot)

D is diameter of the tool. </div></div>

Uh, as I remember, that CS*4/D formula is specifically for HSS (High Speed Steel) tooling. When you get into carbides, and ceramics, and that gamut then the values change. Near exponentially.

 

[Glen Seekins]

Re: Machinist question

climb cut, light stepover and as deep as you can go power wise. Y

you will also get more life out of your tool becuase you are using more cutting edge. When you cut with just the end in light cuts you wear out the first .1" becuase it has to cut all of the material.

make sure your table isnt sloppy loose or it will grab and jump on you. I lightly close the table lock

WD40 will work as lube. You wont be able to flood it to keep it cool, so a little bit of WD will keep the aluminum from sticking to your tool.

 

[AJ300MAG]

Re: Machinist question

I've found the formula works fine. What you see is higher SFPM values. For plain jane carbide 600SFPM works on aluminum. Get into coated carbide and 1000SFPM+ isn't unrealistic. Diamond tooling is a whole nother world...

 

[bignada]

Re: Machinist question

What about using a 32 tooth hacksaw blade?

why mill the entire area? If you have a xy axis table, do your square with the endmill and your small block of material drops out at the end. Think of this as a block test for milling machines....

6061 cuts easily with a decent hacksaw. Could also use a hole saw and then even out your corners on the mill.

Always a way...

 

[triggerguard1]

Re: Machinist question

You need to conventional mill for roughing, regardless of the tooling used on nearly any machine except a CNC. Even a very good knee mill is not rigid enough to withstand the abuse. While it may take a while to destroy your machine, make no mistake, you will destroy it given time.

In the world of efficent machining, climb milling is king. Better tool life, tighter tolerances, better finishes, and faster feed rates, but it is at home on rigid CNC machines only.

Reserve a climb milling cut for the last final finish pass on a manual piece of equipment.

To determine your rpms, you first must determine what your SFM is based on material to be cut, tool to be used, and fixturing method.

Take the SFM and plug into this equation...

Surface Feet/diam. of toolx3.82= Tool RPM.

That equation is good for all tools and materials, it simply needs to change based on the recommended SFM for the materials cut and tool used.

As a for instance, If I'm cutting 1018 mild steel on a CNC milling machine, I'm roughing with a 3/8" endmill at 800SFM. My chip load will be .0035 per tooth....Here's my real numbers based on a 4flute endmill.

800SFM/.375=2,133.3333333x3.82=8149RPM

.0035 x 4 flutes=.014 (This is the feed per revolution)

.014 x 8149=114.086 inches per minute

Knowing those numbers, you would plug 8000 rpm and 110 IPM into the machine and have it all nice and rounded off.

If you're like me, my spindle maxes out at 7500, so keeping with the same chip load, I would end up with 105IPM.



An easy way to think about SFM is like a roll of toilet paper, the closer you get to the middle of the roll, the more revolutions are made to pull the same amount of paper off the roll.
With the same SFM, a smaller tool runs at a higher RPM than a larger tool.