PDA

View Full Version : Taking the plunge.......

Mangler
08-09-2004, 02:51 AM
Hello.

I've come to possess a CNC Router.
I want to use it for milling face
panels for electrical equipment
out of 0.0625" 5051 AL.

I have a bunch of 2 flute center-
cutting TiAlN 1/16" mills. Since
this is a router type machine no
coolant is possible. Maybe WD40 Y/N?

I am a total beginner. I know that
TiAlN is good if you must go dry.

The tool will be running at approximately
20,000RPM this is uncontrollable at present

How do I calculate the feed rate to keep what
I have happy? How does it change with other
diameter tools?

Thanks for the help.

sandman2234
08-09-2004, 03:14 AM
I don't know about speeds that fast, but war department #40 is good at bridgeport speeds. I would grab a piece of scrap and give it a try. I am sure the feed rate will change as cutter size changes.
David from jax

WJHartson
08-09-2004, 05:30 AM
One thing that you have to do with aluminum and small cutters is to get the chips out of the groove and flutes of the cutter. WD-40 is a good coolent for aluminum. I don't know how 5051 will react, ie build up heat while cutting. If it gets gummy you will have problems getting rid of the chips. I use compressed air to blow the chips out of the way when I mill grooves in aluminum with a 1/8" two flute cutter. I am not turning anywhere the rpm you are.

Hope this helps.

Joe

Samuel
08-09-2004, 11:14 AM
1/16 X 3.1416 = .19635 x(the speed of router, mine is 27,500) = 5,399.6 sfm which is pretty darn fast, correct me if my math is false. wear safety gear and make sure you stand behind a cement wall if you fire it up. mills make for sharp projectiles.

Samuel

DR
08-09-2004, 11:56 AM
Hmmmm,

Samuel,
I think you forgot to divide by 12 to convert the speed to SFM. Makes the speed not quite so bad.

Mangler,
5000 series aluminum may not be the best choice for engraving. IMO, something a little harder would be a better choice. 6061-T6, maybe, it's fairly commonly available. Yes, WD40 will be a great help.

ERBenoit
08-09-2004, 12:03 PM
Since you are using such a small tool and if 5051 is anything like the some of the other 5XXX alloys, it is going to be hard to keep anything happy. Some of the 5XXX alloys machine like cr*p. Some of them are gummy and load the flutes, especially on small cutters. Some of what I have learned is that cutters must be extremely sharp and some sort of lubricant/coolant helps, but does not make a significant difference. Since the some of the 5XXX alloys are soft, they want to displace rather than cut. Not that it cannont be done. I machine 5XXX alloys very infrequently, but when I do, it is usually 5052. It is gummy and does not machine well. I have had very little success using end mills smaller than 1/8" on 5052 regardless of what methods I use and try to change when things go bad. Then again I am not spinning an endmill at 20,000 RPM or machining 5XXX alloys daily either. Those that machine 5XXX alloys on a regular basis must know the tricks.

[This message has been edited by ERBenoit (edited 08-09-2004).]

Artpro
08-09-2004, 12:31 PM
Hi. How about it all you electrical engineer types? If the router motor has brushes, can't the speed be controlled with rheostat or variac? Just asking.
Art

Evan
08-09-2004, 12:42 PM
5051 is a very low silicon alloy. Recommended rpms for a 1/16 end mill is 12000 and up. Recommended SFM is 200 to 600 so you will be in the correct range. Use a lube like WD40.

Info here:

http://www.endmill.com/pages/training/spdfeed.htm

08-09-2004, 12:52 PM
You're engraving by end milling and that is a good application for a focused high velocity air mist at the point of cutter opperation.

Engraving is usually done with single flute cutters and chip clearance isn't nearly the problem.

Mangler
08-09-2004, 01:21 PM
Wow,

WJHartson: I will set up air on the machine.
Samuel: Looks like I do need to divide by 12,(thank you DR), which means;

SFM=(1/16" X 3.1416 X RPM)/12.
=(.0625 X 3.1416 X 20,000)/12
SFM=327 SurfaceFeetPerMinute(?)

Now is this the feed rate, across the material or is this just the lead flute's tangential velocity? If it is the latter how does SFM translate to feed rate?

ERBenoit: Thanks for the heads up on the 5XXX. I was using that because this whole thing is coming from the "sheetmetal" realm. I can go to the local sheetmetal shop and they lop off a chunk, (very convienent), but I think I'm starting to see the writing on the wall.... Sheetmetal fabricators probably want bendy soft stuff that they can break and punch with ease. Making the stuff gummy. Dang!

DR: How much WD40 are we talkin about a drip
every inch cut or ?

Artpro: Yes this is a brushed motor and can be speed controlled, within limits, with a variac (very large) as we are talking about 2.5HP. (I am an EE which is why I need all your help so badly) http://bbs.homeshopmachinist.net//smile.gif More to the point should I run this slower?

Evan: So, I'm not way off on speed, yah! I will leave the variac on the shelf for the moment. What does silicon have to do with it?

Sounds like I should be finding a source for 6061 T6 sheetmetal. I will work on that today.

Todays chores;
Procure a PC load up Win2000.
Find source of 6061 T6.

Thanks everyone.

Mangler
08-09-2004, 01:24 PM
Forest Addy: We cross posted Ha!
"Mist", hmmmmm, what be this mist you refer to?

Samuel
08-09-2004, 02:03 PM
Good god! 12! sulk sulk

Mangler
08-09-2004, 02:21 PM
Samuel: You get partial credit!!

Evan
08-09-2004, 02:31 PM
The more silicon in the alloy the lower the SFM should be used. Silicon is abrasive and will cause fast cutter wear above certain speeds. Look at the chart in the link I supplied for information on feed speeds. That is calculated as chip load per tooth, in other words how much cut each flute should take. In the case of a 1/16" endmill in 5051 the suggested chip load is .0002 to .0005 per tooth. For a two flute mill at 20,000 rpm then the feed rate for a chip load of .0005" would be 20 inches per minute (20,000 x .0005 x 2).

[This message has been edited by Evan (edited 08-09-2004).]

Mangler
08-09-2004, 03:24 PM
Evan: Thanks for te clear explaination. Ah the s i t e! I looked for hours.. Google failed me badly. Great site much thanks.

Lee
08-09-2004, 10:10 PM
If you can rub candle wax on the part where it will be cut, this will help to keep the bit from clogging up on ya. It depends on how much you are cutting and the speed as to how hot the bit will get. I route .063 aluminum in a trim router with a 2 fluted flush trim bit and only use wax as a lube. I actually cut 3/8" slots in it this way. I tried WD40, but it wouldn't stop the bit from clogging. (I may not have used enough) I just rub the wax along the path I will cut and it melts as I get to it. Very little wax left on the part to clean off afterward. I have a router speed controller and tried it being slowed down. It didn't work as well. It may work better if I went faster than 20,000 rpm with it. http://bbs.homeshopmachinist.net//wink.gif Hope this rambling helps.

------------------
Lee

Mangler
08-10-2004, 02:48 AM
Lee: Great idea. The wax method sounds a lot easier to implement then a DW40 drip of some sort.

Evan: Looking at that site...

Let me see if I have this right.

1) Looking at the table: AL material 1/16" gives a chip load of .0002-.0005 and an RPM of 12,222 or faster.

2) Using the formula
InchesPerRevolution = Chip load X No.Flutes
Using .0004", and 2 flutes
IPR=.0004" X 2 = .0008"

3) Next I use the formula
InchesPerMinute(FEED RATE) = RPM X IPR
or IPM = 20,000 X .0008" = 16 InchesPerMin

Is this correct?

Thanks

Evan
08-10-2004, 10:40 AM
Yep, that's right. BTW, beeswax works the best.

spope14
08-10-2004, 12:01 PM
Speeds and feeds are correct as noted above.

I also use this formula

SFPM x 4 divided by the cutter diameter in decimal inch. This formula is about +/- 3 to 5% of the "12 and pi" formula.

As for a coolant - I use "edgelube", which is available through MSC, and has a lower melt point - which allows for better penetration to the cutting edges, and better chip removal, and better (more even)spread than beeswax, and leaves less residue (thus easier to remove). Cheaper as well, and less is used. I have used beeswax though, and like it, so whatever you do with "solid lubes" is good. Heck, used a "yankee candle" once in a pinch, the part smelled like apples.....

You can also use kerosene in engraving, or I also use "Tap magic". the surface tension tends to hold the coolant into place on the edges of the part, strange as it seems.

[This message has been edited by spope14 (edited 08-10-2004).]

Mangler
08-10-2004, 12:37 PM
Evan: Thanks for the confirmation and the bee's wax point, I was wondering, as I have bee's wax for archery,(string making), already.

spope14: That formula apppears to avoid the chip load value which seems kinda nebulous to me.

Let me walk thru your method:

SF(P)M=(1/16" X 3.1416 X RPM)/12.
=(.0625 X 3.1416 X 20,000)/12
SFM=327 SurfaceInchesPerMinute

IPM(FEEDRATE) = (SFPM X 4)/DIA.(CUTTER)
IPM = (327 X 4)/.0625
IPM = 20,928 inches per minute.....

ummmmmmmm. That's ummm 20 Miles per Hour!!!

I seem to be "run into the ditch" here..

Apples? Does that mean I can get different candles and get a fake strawberry smell too? http://bbs.homeshopmachinist.net//smile.gif

I will get my hands on the edgelube.

Thanks for the help.

Artpro
08-10-2004, 01:30 PM
Mangler. In the '60s I was fabricating sheet metal parts for the electronics trade. Front panels which were to be engraved, were always/usually made of 6061-T6 alloy, both for engraving purposes as well as providing better anodizing finish. As was mentioned, 5000 series allows are softer, so they punch and form easier. Go with 6061 for engraving and save yourself some grief.
Art

Mangler
08-10-2004, 02:19 PM
Artpro: Okay. I just ordered 2 sheets of 6061-T6 out of Mcmaster-Carr. Done!

Mangler
08-10-2004, 02:22 PM
spope14: Hey I am looking at MSC web site they list 279 different cutting fluids...None are called "edgelube" or seem to refer to that... Any chance you can get the name, or part number, or ?

Thanks yet again.

Evan
08-10-2004, 02:26 PM
Look for Tapmatic Edge Lube (not edgelube). You should be OK with the feeds as above on the 6061. Although it is a harder alloy it still only has a max of 0.8% silicon.

Don't know about MSC but KBC has it. Part# 1-444-43200

Personally I use Cut-Ease, basically the same thing.

[This message has been edited by Evan (edited 08-10-2004).]

Mangler
08-11-2004, 02:14 PM
Evan: Thanks for the leads I have procured LPS Tapmatic Stick from Mcmaster-Carr, (I usually get my stuff from them UPS ground in one day)

spope14: What am I doing wrong with your formula?

Mangler
08-16-2004, 01:17 PM
IT WORKED!!!

I just wanted to thank you guys
for the great help. Yesterday I
cut my first panel out. Course I
had the wrong setting so the router
cut the inside path around and panel
and the outside paths around the holes
in the panel but once I figured out that
things went very smoothly, except for
that one embarrassing Z ref that was
about an inch lower than it should've
been.

So anyway, I have my panels a day early.

Thanks again.

Evan
08-16-2004, 01:25 PM

Mangler
08-16-2004, 09:39 PM
Evan....Hmmm I have pictures...but..
How do I post them? I don't have any kind
of site to stick them on then provide a link
to. Any suggestion?

L Webb
08-16-2004, 10:06 PM
Use www.photobucket.com (http://www.photobucket.com)

Les

spope14
08-17-2004, 10:06 AM
Must admit mistakes when you make them. I was thinking RPMS of the cutter needing to be found method. BUT - RPM's were already known. I worked out the other formulas above my initial post just for fun (and for teaching ideas), but got carried away with the solution of RPM's.

As for the "candles", I tend to experiment in my job a bit. The idea is this, you use what you can in a pinch. Most scented candles have a high "oils" content, and a low melting point, which releases the scent. Rub your hand on a regular "birthday cake" or regular table candlestick (unscented), and even dig a fingernail into it. The regular candles are slightly to moderately brittle. Do the same on a scented candle, especially one in a jar or something. Much more "oily" and soft. They also tend to leave a residue on your skin that will be slick when you rub fingers together, where a normal candle will not as well.

I once turned a job of 50 aluminum racing hood pins for a racing "R&D" guy using those crazy candles, for the edgelube was out, and the job was a "must have yesterday" job.

Just mentioned to illustrate a bit of a point. I have those "apple candles" all over my house.

Heck, even used "Edge shaving gel" once as a fly cutting lube and a tapping compound for tapping aluminum, and used simple green in concentrate as a lube for engraving just a month back. Stinks being out in the boonies, a bit poor, and having to improvise for those good paying jobs that were "needed yesterday". makes you think however, and you tend to think of these crazy things even when you have everything.

Worked well enough for the job at hand, but would rather use the real things like Edge Lube, Acculube (which is also good - Acculube paste, just got an 8 ounce sample of the blue paste, love it).

[This message has been edited by spope14 (edited 08-17-2004).]

Mangler
08-24-2004, 02:25 AM
Hello everyone, I have made it over my time hurtle and finished my project in time for the "Dog and Pony" show. The original idea was to have a shop do the panels but they all quoted lots of money for low quantity and 3 weeks turn. Since this is an on going problem I decided to give this solution a try. It's worked great!

This first photo is a bonus(grin) photo to warm you up. I snapped this shot on a trawler delivery in Puget Sound.
http://img.photobucket.com/albums/v461/kcress/Standing_By.jpg

This is the machine I just acquired from K2cnc.
http://img.photobucket.com/albums/v461/kcress/TheMachine.jpg
http://img.photobucket.com/albums/v461/kcress/TheMachine2.jpg
http://img.photobucket.com/albums/v461/kcress/Try4a.jpg
http://img.photobucket.com/albums/v461/kcress/Try4b.jpg
http://img.photobucket.com/albums/v461/kcress/Try4c.jpg
http://img.photobucket.com/albums/v461/kcress/Try4Finish.jpg
http://img.photobucket.com/albums/v461/kcress/EdgeLube.jpg

The point of the router was to make this metal box and lid(not shown).
These were cut out of 5051 22gauge 0.024"
I'm using Carbide TiAlN Center Cutting mills 0.0625" in dia. I tried using several 0.031" mills on this 22 gauge stuff but they snapped faster then I could tear ten dollar bills in half. So I changed to programs and ran with the larger mill.
http://img.photobucket.com/albums/v461/kcress/BackofPanel.jpg

And this front panel. I routered. Out of 6061-T5 0.0625" thick.
http://img.photobucket.com/albums/v461/kcress/FrontofPanel.jpg

Evan
08-24-2004, 10:46 AM
Ain't it nice when things work http://bbs.homeshopmachinist.net//smile.gif