CamBam
News:
 
*
Welcome, Guest. Please login or register.
Did you miss your activation email?
December 13, 2017, 07:12:39 am


Login with username, password and session length


Pages: [1]
  Print  
Author Topic: Milling slots in 14 ga. aluminum panel  (Read 481 times)
airnocker
Wookie
****
Offline Offline

Posts: 368


View Profile
« on: October 12, 2017, 00:03:17 am »

I'm preparing to mill some 1/8" slots in a small equipment box aluminum panel.  Hammond Mfg. only states the aluminum panel is 14 gauge (.070").  Here's the pdf of the small enclosure.  The three 3" x .125" slots will be milled on the sloped front face for slide potentiometers.  Photo attached of my "hold-down" method.

My question is: what type of aluminum is typically used for these kinds of aluminum panels? Or is it of not much importance for this application?

I intend to use a 2-flute 1/8" end mill.  I have two types, a generic HSS bit and a GARR Tool Carbide shown here: https://www.garrtool.com/pages/tooldetaillogin.jsp?edp=41017%20&series=620MA_640MA

Ain't never done no aluminum on my DIY machine, but I think it's worth a try.  I will only be using Y-axis motion during the slot milling.  My thought is to only do light DOCs in the range of .05-.010 as time-on-task is not an issue with feeds in the 20 IPM range.  I'd like to use ivory soap (the old solid type) as a lubricant or WD-40 in moderation.

I appreciate any thoughts on this. 


* 1456CE3BKBU.pdf (217.03 KB - downloaded 7 times.)

* 20171011_152155_001.jpg (2838.88 KB, 5312x2988 - viewed 56 times.)
Logged

airnocker

Everything depends on everything else
lloydsp
CNC Jedi
*****
Offline Offline

Posts: 7209



View Profile
« Reply #1 on: October 12, 2017, 00:10:17 am »

Such boxes are usually 6061 sheet, and perfectly-machinable... but you need LOTS of liquid coolant to prevent metal from adhering to and building-up on the cutter.  Do NOT cut it dry with 'normal' cutters, because it's a sticky, gummy, adhesive alloy.

Lloyd
Logged

"Pyro for Fun and Profit for More Than Fifty Years"
airnocker
Wookie
****
Offline Offline

Posts: 368


View Profile
« Reply #2 on: October 12, 2017, 02:15:09 am »

Thanks Lloyd
Logged

airnocker

Everything depends on everything else
chuckeroo
Wookie
****
Offline Offline

Posts: 353


View Profile
« Reply #3 on: October 12, 2017, 10:36:21 am »

Believe or not iv'e have good luck with compressed air using a pancake compressor.pointed the nozzle directly at the bit while cutting and followed it around.the first thing i noticed is that the temperature of the compressed air was a lot cooler than i anticipated. Now i do live 30 miles away from the gulf of mexico so humidity level is always high , thus keeping the water droplets in the compressed air. wonder if that's what cools down the air?
Logged
lloydsp
CNC Jedi
*****
Offline Offline

Posts: 7209



View Profile
« Reply #4 on: October 12, 2017, 12:08:27 pm »

Chuck,
If your compressor has any cooling fins in the 'hot air' circuit between compressor and tank, and/or if the air has any significant residence time in the tank before you dispense it, and/or if you have relatively long lines between the compressor and nozzle, then --

What you're experiencing is 'expansion cooling'.  That's a pretty-normal artifact of compressed air systems that have the correct amount of heat dissipation for the newly-compressed air.  It's just like a refrigerator.

The air heats significantly upon being compressed.  If it were immediately released, expansion of the still-HOT air would come back out of the circuit at roughly the same temperature as it went in.  But if that hot, compressed air is first cooled to ambient before it is released, then expansion cooling results in a much lower temp than ambient.

It probably has little to do with moisture content.  Et al, moisture disturbs the efficiency of that process.

That said, I've never found air-jet (alone) to prevent adhesion of 6061 to cutter edges.  Some water mist containing a lubricant has always been necessary, for me.

Lloyd
Logged

"Pyro for Fun and Profit for More Than Fifty Years"
jk
Storm Trooper
***
Offline Offline

Posts: 215


View Profile
« Reply #5 on: October 12, 2017, 12:42:45 pm »

From my limited experience with alu you'll be fine with the wd-40 and small DOC (say, 0.6mm). Use the fswizard online to calc your feed & speed (derate feed by 20% for some margin). Most likely you'll want to drill holes for lead-in to avoid plunges. If time is not an issue, you may predrill the whole slots ) 

I suggest a little modification to your fixture. Install your wood block on the table. Set the orgin in cnc control. Mill the recess 0.070'' deep for your sheet so it fit there. Screw/clamp the sheet now. Run the alu program from the same orign. This way your sheet will lay flat and be registered against the side of the recess with rotation prevented.
Logged
lloydsp
CNC Jedi
*****
Offline Offline

Posts: 7209



View Profile
« Reply #6 on: October 12, 2017, 13:56:32 pm »

"Most likely you'll want to drill holes for lead-in to avoid plunges. If time is not an issue, you may predrill the whole slots..."

-----------------------
That's not necessary, and uses up a lot of time you could be better spending on other things.  Use the "spiral leadin" feature with zero degrees for the 'spiral angle', and it will do the slots progressively from the surface-down, very nicely.

Lloyd
Logged

"Pyro for Fun and Profit for More Than Fifty Years"
EddyCurrent
CNC Jedi
*****
Offline Offline

Posts: 3256



View Profile
« Reply #7 on: October 12, 2017, 14:38:40 pm »

A lot of the carbide cutters I use for wood do not have cutting edges that extend across the whole diameter of the tool at the end,  there is a gap in the middle, that's why I always use a lead-in move.
Logged
Garyhlucas
CNC Jedi
*****
Offline Offline

Posts: 1029


View Profile
« Reply #8 on: October 12, 2017, 15:18:57 pm »

Apply the WD40 or soapy water with a brush so you can push the chips away at the same time. Makes much less mess than air blowoff.

My experience with electrical back panels is that they are not 6061 but more likely 3003 based on how they drill and tap.

If you weld material to the end mill just toss it in some caustic, sodium hydroxide, lye, which are different names for the same thing. The aluminum will be gone in no time and no damage to the end mill.
Logged

Gary H. Lucas

Have you read my blog?
 http://a-little-business.blogspot.com/
lloydsp
CNC Jedi
*****
Offline Offline

Posts: 7209



View Profile
« Reply #9 on: October 12, 2017, 15:33:23 pm »

Gary,
I got the impression he was working with a small 'project box', like Bud Boxes.  They usually are (if not 6061) a VERY 'sticky' alloy that just loves to weld to dry cutters.  I may have been just 'assuming', since I see the same effect with 6061, which is ubiquitous.

Lloyd
Logged

"Pyro for Fun and Profit for More Than Fifty Years"
airnocker
Wookie
****
Offline Offline

Posts: 368


View Profile
« Reply #10 on: October 12, 2017, 16:13:39 pm »


I suggest a little modification to your fixture. Install your wood block on the table. Set the orgin in cnc control. Mill the recess 0.070'' deep for your sheet so it fit there. Screw/clamp the sheet now. Run the alu program from the same orign. This way your sheet will lay flat and be registered against the side of the recess with rotation prevented.

Thanks JK, I considered recessing the wood block to address any potential rotation.  But that seemed time consuming, so I opted to located the four hold-down screws accurately so their shafts are tangent to the sides of the panel on both sides producing the same effect.

I found this F&S calculator for 6061 Al, so I will first try the spiral lead-in move with RPM ~ 8550, DOC= .01" and FR=17IPM with a single flute bit.

I'm going to have to loose the cardboard strips beneath the screwheads though since once they get soggy with oil they will be useless.  They are intended to protect the finish of the panel, so I'll come up with something else more moisture proof.

Thanks everyone!


* 6061 Alum Feed Rate Calculator.jpg (202.76 KB, 525x758 - viewed 20 times.)
Logged

airnocker

Everything depends on everything else
robertk925
CNC Ewok
*
Offline Offline

Posts: 12


View Profile
« Reply #11 on: October 12, 2017, 17:00:54 pm »

If the sheetmetal is bent then it is most likely either 3003 or 5052. We use 5052 for all of our clients' chassis designs. It is typically stamped and not machined. 5052 is very sticky and difficult to mill, so air/WD40/coolant is a must.
Logged
Garyhlucas
CNC Jedi
*****
Offline Offline

Posts: 1029


View Profile
« Reply #12 on: October 12, 2017, 23:09:35 pm »

Yes,
6061 does not bend well, you see stress marks on the outside of the bend.
Logged

Gary H. Lucas

Have you read my blog?
 http://a-little-business.blogspot.com/
lloydsp
CNC Jedi
*****
Offline Offline

Posts: 7209



View Profile
« Reply #13 on: October 12, 2017, 23:19:36 pm »

Hmmm... Gary, I'm going to have to try some 'square bends' on my brake with 6061.  I almost _always_ use a small radius (only by habit) on bends when building chassis.  Maybe that's why I didn't notice the 'stress marks'.

Lloyd
Logged

"Pyro for Fun and Profit for More Than Fifty Years"
Pages: [1]
  Print  
 
Jump to:  

Powered by MySQL Powered by PHP Powered by SMF 1.1.19 | SMF © 2013, Simple Machines

Valid XHTML 1.0! Valid CSS! Dilber MC Theme by HarzeM
Page created in 0.143 seconds with 18 queries.

Copyright © 2008 HexRay Ltd. | Sitemap