Newbie - Need Feedback on my first CNC Milling attempt

[DominicASP]

I just bought a small three-axis Chinese CNC machine, the 3040Z-DQ. I have no experience with CNC milling or any other machining operations. I am trying to cut a 0.56 in (14.3 mm) by 0.52 in (13.3 mm) rectangular profile through a 1/20 in (1.27 mm) aluminium plate. I am not sure which type of aluminium it is, but it is certainly fairly soft. The machine is controlled by Mach3. I did my initial design in SolidWorks, saved as a DXF, imported the file in CamBam where I tried, with my very limited knowledge, to setup the proper parameters to achieve a nice milling operation, saved everything as a gcode and sent it to Mach3.

My end mill is made of Carbide, 2 Flute 42° Helix with a TiN Coating. It has a Mill Diameter of 1/16 in, a Shank Diameter of 1/8 in, a Length of Cut of 1/8 in with an Overall Length of 1-1/2. I applied a few drops of water-based cutting fluid on my plate just prior to contact. To determine the feedrate and RPM used in CamBam, I used a formula found on this forum. I selected a profile operation with a depth increment of 1/16 in, target depth of 1/16 in, a cut feed rate of 3ipm, plunge feedrate of 1.5ipm, a spindle speed of 2400 rpm and a tool diameter of 1/16 in. The plate was fixed on a wooden plate using screws throughout the operation.

The end result in shown on the attached pictures. My first attempt was obviously not a success and I'm looking to get some feedback and comments to improve the operation and get a way more precise cut. Here are some observations I have noticed during the milling process:
[ul]
[li]I have a large circle at the point of first contact which seems way off the cutting pattern.[/li]
[li]The top horizontal line seems to be fairly straight / parallel to the top surface of the plate and the inside surface finish is close to perfect. This is not the case with the other 3 lines. The cut is way more wavy, not straight and rough on the inside.[/li]
[li]The spindle seemed to have a rough time during the operation. Its speed wasn't constant, it almost completely blocked at some point and jumped a bit.[/li]
[li]The end mill seemed to have been damaged, i.e. lost a bit of TiN coating.[/li]
[li]Chips were not excessive but their evacuation wasn't great.[/li]
[li]I should secure the drop of the profile on my next attempt to prevent damaging my tool.[/li]
[/ul]


I have some questions regarding this operation:
[ul]
[li]Should I use a pocket operation instead of a profile?[/li]
[li]Am I using the proper tool? Would a tool with a finer mill diameter achieve a more precise cut?[/li]
[li]Do my CamBam parameters looks good?[/li]
[li]Could the precision of the CNC machine itself be causing these problems? Can I expect much better with this machine?[/li]
[/ul]

Any additional feedback / comments are obviously more than welcomed.

Thank you all for your precious help!

 

[MikeHalloran]

No photos showed up.

Your description makes it sound like you are cutting a pocket, not a profile; the extraneous circle probably came from a profile macro's start/stop sequence.

A 1/16" diameter end mill will suffer greatly from a 1/8" depth of cut. Maybe .02" per pass would be better.

2400 rpm is not nearly fast enough to make nice chips.
10,000 rpm would be better.
... or, all you've got.
When you are cutting aluminum, you use all the speed you can get, or at least enough to make the chips hit the ceiling.

Use a bigger cutter to get more surface speed. If you can grip a 1/8" shank, use a 1/8" diameter mill. If you want sharper corners, fix them with a file.

If the CNC software doesn't do it for you, use a simple spreadsheet to calculate chip dimensions and metal removal rate, for every cut, and keep track of them so you develop a feel for what's possible.


Mike Halloran
Pembroke Pines, FL, USA

 

[DominicASP]

Sorry for the pictures,

Please check the following links:

http://i58.tinypic.com/25srepk.jpg

http://i62.tinypic.com/10or4w6.jpg

http://i57.tinypic.com/2nuip0g.jpg

http://i62.tinypic.com/12554l1.jpg

http://i61.tinypic.com/2wme1kk.jpg

http://i60.tinypic.com/1jazcp.jpg

http://i58.tinypic.com/96xijb.jpg

 

[MikeHalloran]

You're pushing the tool way too hard.
You probably stalled the XY drive a bit, which would account for the odd shape.

What you do next is coordinate the spindle RPM and the lateral feedrate so that the 'feed per tooth' is .001" or a bit less.



Mike Halloran
Pembroke Pines, FL, USA

 

[BrianE22]

Are you getting aluminum build-up up on your cutting edges? I find I need flood coolant when milling aluminum.

 

[BillPSU]

Typically you should drill a hole in the plate and start in the middle of the hole and arc into the inside of the window. The reason for the arc is to allow the cutter compensation to take effect during the arc in thus not leaving a dimple in the wall of the window. Leave .010" to .030" stock on the inside of the window. Take a second pass and remove the remaining material. Arc out from the window to stop the cutter comp from again dimpling the window. I never used the canned cycle supplied with the machine.

If your machine does not use cutter comp then the arcing process is unnecessary. Simply mill into the window using straight cuts rough it out and then finish cut the window.

Flood coolant would be the best choice but if not available use spray mist to apply coolant and blow the chips out of the cut. Keep your tools as short as possible reducing chatter and cutter deflection.

Bill

 

[JNieman]

When lacking proper coolant or the tooling/enclosures to properly mist and contain the mess, WD40 is a rather sufficient stop-gap solution for aluminum.

There are a few good forums with a host of information. I'm not especially fond of Mach3 but I've used it to get by in some niches and helped get a setup going for others, when that was the most economical choice for their means+needs.

"CNC Zone" I believe is one. "Practical Machinist" has a great slew of help but it is forcibly geared toward the 'professional' situations and if you bring this issue to that forum, your answers will likely be "get a real machine first" and nothing much more. It's a great library/wealth of information to search though. It's just "for the hobbyist" so to speak.

_________________________________________
NX8.0, Solidworks 2014, AutoCAD, Enovia V5

 

[Ebug]

I have not looked at the photos yet, but I will comment on your machining parameters.
A carbide endmill in Aluminum should run anywhere from 800-2000sfm. You are probably going to run out of spindle rpm long before you hit that sfm. Let's work an example using 160sfm.
160sfm
.0625" diameter cutter
2 flute
The formula for RPM is SFM*3.82/diameter.

In your case it works out like this:
160sfm*3.82/.0625(cutter dia) = 9779.2 rpm

The formula for feed rate is RPM*IPT*number of flutes.
I would recommend .0005" IPT(inch per tooth) for your .0625" endmill.

In your case it works out like this:
9779(rpm)*.0005"(chip load)*2(number of flutes) = 9.779IPM(inches per minute)
Round that to 9.78.

For Axial depth of cut I would stick to 1*Diameter of the cutting tool. Make multiple depth cuts until you reach your desired cutting depth.

Much luck,
Rob