What ends mills should I buy?

[CamSec]

Hi Everyone,

I ordered a Deepgroove1 mill earlier in the week so that I can try out different designs for the product I`m working on. I`ll be milling wax to start with, but the goal is to make aluminum molds. The mill comes with a 1/8 & 3/16 inch end mill, but I`m thinking I need a ball end for my design, would something like the one below be a good choice?

http://www.amazon.com/gp/product/B003CP0SRA/ref=ox_sc_act_title_1?ie=UTF8&m=ATVPDKIKX0DER]Amazon.com: Niagara Cutter CB430 Carbide End Mill, General Purpose, TiAlN Coated, 4 Flutes, Ball End, 1" Cutting Length, 1/16" Cutting Diameter: Industrial & Scientific

To get a better idea of what it would look like I did a single pass simulation in FreeMill with a 1/16" ball end and the detail looked acceptable, but the outer curves had visible stepping. (Yes, I need to look at more CAM software). The bottom of the mold will be 1" deep, and it will need to be smooth and flat. The interior pockets do not have to be perfectly square, my CAD software just doesn't like filleting them. Dimensions of the part are 143x67x25.5mm

[cameraguy]

you probably want to get a couple different sizes of tool so you can do roughing, so that you don't have to try to cut that much material out with a 1/16" ballnose. stepover would be painfully small to get a flat bottom with that bit.
you may also want to look into 2-flute or even single flute mills, or even profile mills. the taig spindle doesn't spin fast enough for a 4-flute for that. it doesn't even spin fast enough for a 2-flute that diameter really, but you can make due.

if you consistently cut with micro endmills, you may want to consider going to a water-cooled vfd spindle to get the rpm's up to what tools that small of diameter like.

[dlaery]

I would get 2 flutes, solid carbide, no coating.

[CamSec]

Thanks for the advice! I noticed that with the 2 flute version, the cutting length is 1/4" vs 1", will that cause me problems if I have to mill parts deeper than 1/4"?

[cameraguy]

i will guarantee there is a misprint/typo in there. you will never see a cutting tool like that with a cutting length of 16 times the tool diameter. wouldn't be nearly strong enough to function.

you are not going to be able to come close to removing that much material (better than a dozen cubic inches or so) of material with a 1/16 in. ballnose. nor would you be able to cut an inch deep pass into aluminum with it anyway. you are talking about passes removing only likely hundredths of inches at a time with something that small. it would be like excavating a basement with a teaspoon. you need heavier tools to start. think of it like a sculptor would start shaping a large block of rough stone - you don't start the project with the fine sandpaper!

there are dozens of cutting strategies for that part, for example you might really want to use something more like a 1/4" or 3/8" diameter mill to hog out the rough shape and a smooth bottom in there, followed by a smaller mill to clean up and to cut the small details and small radius transitions. You may even use three tools.

it sounds like you are curious and just starting out with both machining and toolpathing strategies. i would suggest reading up on how to best determine feeds and speeds on different materials and spend some time practicing with a variety of cheap tooling on scrap materials to learn the basics of what each tool is capable of before you try to attempt complex toolpathing - it is far too easy to have the computer ask a tool to do things physically impossible!

[awetmore]

I don't see how you are going to do the deep square edges on that piece. Even a 1/16" end mill is going to leave you with a 1/32" radius on the corners. Can you redesign your part to have a inside corner radiuses instead of a square edge?

It looks like you plan on using a ball end mill based on the radiused bottom edge? That will take a very long time to make a flat bottom because you'll need to have a very small step over. Switching tools to a flat bottomed end mill will save you a lot of time.

How deep are the holes for your mounting screws? You'll probably want to do those with a drill, plunging an end mill (without interpolation) usually results in fairly imprecise holes, and your holes aren't very large.

This is a fairly tricky part for a first project.

I primarily use 2 flute 1/8", 3/16", and 1/4" end mills from Atrax on my Taig. Enco sells them for reasonable prices.

1/16" end mills will typically have a 1/8" depth of cut.

[CamSec]

Thanks for the feedback! As long the PCBs fit the case I`m not that fussed about the interior corners. The screw holes are for threaded inserts (3.3mm diameter, 5mm deep), so hopefully that will be OK. Of course they`ll be islands rather than holes when I convert this into a mold, I`m sure that will be fun.

My shopping list is now:
"http://www.amazon.com/gp/product/B003BIEP2M/ref=ox_sc_act_title_4?ie=UTF8&m=ATVPDKIKX0DER"]Amazon.com: Niagara Cutter C230 Carbide End Mill, General Purpose, Uncoated (Bright), 2 Flutes, Square End, 1-1/8" Cutting Length, 1/4" Cutting Diameter: Industrial & Scientific

http://www.amazon.com/gp/product/B003CYKGOG/ref=ox_sc_act_title_6?ie=UTF8&m=ATVPDKIKX0DER]Amazon.com: Niagara Cutter CB230 Carbide End Mill, General Purpose, Uncoated (Bright), 2 Flutes, Ball End, 1" Cutting Length, 1/8" Cutting Diameter: Industrial & Scientific

http://www.amazon.com/gp/product/B003BIEOWS/ref=ox_sc_act_title_7?ie=UTF8&m=ATVPDKIKX0DER]Amazon.com: Niagara Cutter C230 Carbide End Mill, General Purpose, Uncoated (Bright), 2 Flutes, Square End, 1" Cutting Length, 1/8" Cutting Diameter: Industrial & Scientific

http://www.amazon.com/gp/product/B003CP0SRA/ref=ox_sc_act_title_5?ie=UTF8&m=ATVPDKIKX0DER]Amazon.com: Niagara Cutter CB430 Carbide End Mill, General Purpose, TiAlN Coated, 4 Flutes, Ball End, 1" Cutting Length, 1/16" Cutting Diameter: Industrial & Scientific

I checked the specs and when they say cutting length, they mean depth of cut. I hope.

Will the 4 flute one work for cutting wax? If not I found these long reach 3 flute Harvey mills. I`m looking at 4890 for the 1mm battery contact inserts.
Harvey Tool - Long Reach, Stub Flute - Carbide Miniature Square End Mills - Amorphous Diamond Miniature End Mills

Received the Taig mill and a box of machinable wax to practice on, should receive the motors and Gecko controller on Friday.

[Jim1245]

I use the 1/4" 2-flute ball end cutters designed for aluminum from LakeshoreCarbide.com to cut aluminum molds on my Taig. They are expensive but don't seem to wear out.

[CamSec]

Received the box with the Gecko controller and stepper motors, but I think one of them is bad, whatever axis I connect it to is 10 times louder and very rough compared to the others. I removed the suspect stepper from all the coupling bits and it vibrates in my hand if I jog it at 100% speed in Mach 3, and doesn't move at all at 5% speed. It does the same if I plug it into a different port on the Gecko. Is this something I can fix, or do I need a new motor?

[CamSec]

Had a quick reply back from Paul at deepgroove1, they have a new guy soldering the wires on the DB 9 connector. I should be able to fix the cold solder joint pretty easily.

[CamSec]

Thanks to schmutzig's config file, I now have EMC working, and I`m trying out MeshCAM, which seems pretty decent. I screwed up the tool change though, EMC confused me by not letting me jog the Z axis up to change tools, so I had to stop the program, jog it, then re-run it from the tool change, and I think I got the Z offset wrong. Whats the best way of changing tools while keeping the Z offset zeroed?

I`ll attach a photo of my 2nd attempt. The roughing pass was with the 1/8" end mill, 2nd pass with the 1/16" ball end. There was supposed to be a 1mm pencil pass but I wanted to figure out tool changing first.

[awetmore]

Whats the best way of changing tools while keeping the Z offset zeroed?

This is the tool change macro for CamBam that I use with EMC2:

<ToolChange>M09
{$spindle(off)}
G53 G0 Z0
{$comment} T{$tool.index} : {$tool.diameter} @ {$s} rpm {$endcomment}
T{$tool.index} M6
G43 H{$tool.index}
M03 {$s} {$spindlecw}
{$clearance}
M08
</ToolChange>^M

G53 is a direct move, so it raises the Z to the top of it's travel. The final {$clearance} usually translates to a G0 Z0.25, which will move back the tool using the offset table to be 0.25" off of the surface.

I've never used MeshCam and don't know if there is a similar set of post processor macros that are used to tailor the output for your specific system.