Help with 1/32 ball end mill cutting aluminum

[Jeff Gomes]

Hi All:

Please bear with me if my questions seem elementary.  I am climbing several different learning curves simultaneously.

I keep breaking 1/32 inch mills (http://www.pocketnc.com/carbide-ball-long-reach/132nd-ball-long-reach-stub-flute) even though I am trying to follow the Harvey Tool feeds and speeds recommendations and also extrapolate from the PocketNC feeds and speeds tutorial.  The project is aluminum molds for injection molding of some rather intricate little parts that need that level of detail.  I am trying to rough with 3D Adaptives (rest machining a progression of 1/8 flat, 1/8 ball, 1/16 flat, 1/16 ball, 3/64 flat, 3/64 ball, 1/32 flat, 1/32 ball), followed by a 1/32 ball Scallop to finish.  I have yet to have a 1/32 ball mill survive the 3D Adaptive operation.  This is getting really expensive and frustrating.

Question 1:

Would anyone be so kind as to share a Fusion 360 CAM recipe that works with these mills on 6061 aluminum?

Question 2:

Is there a more durable 1/32 ball mill that I should try?  I started with these because I am a neophyte and they are what is sold on the PocketNC site.  However, they are longer than necessary for the molds I am working on at this time, and it seems intuitive that the extra length probably makes them easier to break.

Thanks.

~ Jeff

[Pocket NC]

Pocket NC

Hi Jeff,

Before running any more parts, can you share your F3d of the part you are trying to run?  If not, can you send it direct to us at in...@pocketnc.com  Its hard to know what the issue is without having a look at the tool paths.

Thanks,

Matt

[Jeff Gomes]

Sure.  It says it won't export to f3d because the design has referenced components.  So here is the link to it shared online:   http://a360.co/2mmrxjb

[Jeff Gomes]

Here are a couple of screen shots of what I'm trying to make.

[Pocket NC]

Pocket NC 

Hi Jeff,  I am not sure why you are having tool issues. I looked at your tool paths and don't see anything crazy happening.  You will most likely need to watch the tool as it cuts to see where its having problems.  If tool length is the problem, you could go with the following tool from harvey http://www.harveytool.com/ToolTechInfo.aspx?ToolNumber=27831 as it is cheaper and shorter. We would have to custom order it but the lead time is short.  Cheaper yet,  In the FR4 section, we have a brand of endmills that is super cost effective,  with a .031 ball endmill, have a look to see if it will work. http://www.pocketnc.com/fr4-machine-shield-1/fr4-endmills

-Matt

[Jeff Gomes]

Matt:

In a way I'm glad you didn't see anything crazy.  But in another way, I was hoping there was some simple fix that I was overlooking.  I guess the only choice is more trial and error with even more conservative paths.  I will take a look at the endmills you mentioned.

Thanks.

~ Jeff

[Randy Kopf]

Jeff:

My initial thoughts looking at your mold pictures and considering the initial tool your using and the machine I am not too surprised you would be having trouble. The first problem your having is that the spindle really can't run any where fast enough on the Pocket NC for that type of work with such a small cutter. SFPM on 6061 is like 1000-1500 SFPM

The formula for RPM is 

SFPM * 4 / CUTTER DIA = 

1000 * 4 /  0.03125 = 128,000 RPM yet the Pocket NC only runs at 10,000

This doesn't mean you can cut. It just means you really have to do some compensation.

First your feed rate must be decreased. And you chip load must also decrease from a normal calculation.

Second your relieved part of your tool should be no more than what will cut your part.

If your cavity is only 1/8" deep then the total tool tip should be just a little more than that.

What I see from the initial cutter is 1/32 diameter that is probably 3/8" long. that is before you hit the 1/8" diameter shank. It's just too fragile for any real cutting.

So find the shortest tool to do the job, run the spindle at max rpm, and do super light depths of cuts like maybe 0.001"-0.003" (Axial depth of cut) and very light step overs like 0.003"  (Radial step over)

Well that's my initial thoughts. 

[Randy Kopf]

Jeff:

Try to do as much work initially with the largest diameter tool possible.

Use the smaller diameter tools as needed. 

I am really pressed for time until next week but I could put together a strategy that likely will work.  I am a journeyman mold maker and have been making molds for 35 years. And I have the Pocket NC. 

If what your were cutting was plastic or wax you likely would not be challenged but with Aluminum you will be very challenged without a decent cut strategy that machines the mold in a progression of roughing, semi rough, semi finish then finish tool paths.

Randy

[Jeff Gomes]

Randy:

Thank you for your help.  Finally yesterday I managed to finish one half of the mold without breaking anything.  I had arrived at almost exactly what you just suggested, with miniscule axial and radial engagement.

It is nice to feel that I am on the right track at last.  I really appreciate the time you and Matt took to look at my challenges.

~ Jeff

[diego Garcia]

Hey jeff,

If its alright it be awesome to see the molds and how they turned out, maybe a even a video of how the pocketnc cuts, and how your clamping it be a great visual reference.

best of luck

best regards

Diego

[Jeff Gomes]

Diego:

If and when I ever get a set of injection molded parts out of this lengthy and exacting process, I plan to document the entire workflow for my colleagues.  I will be happy to share most of that here.  Unfortunately at the moment, my PocketNC is on its way back to Montana for repairs.  So my forward progress is paused.

However, I can describe my basic approach now.  I chose a mold size of 3 x 3.5 inches as something that should fit on the PocketNC with clearance around the edges equivalent to at least the diameter of the largest tools I was likely to be using.  Rather than attempt to make a vise to hold something that would fill most of the b-table, I decided on an acrylic fixture that can be bolted down to it with consistent positioning, and to which in turn I can bolt my mold blanks once their corners are drilled and counterbored.  Of course I need another setup for drilling those corners and also the holes in the main fixture.  So I 3D-printed another fixture for that job.

A major goal in all of this has been to allow for metal-safe mold modifications by being able to anchor a mold in a repeatable position.  If I can come within 1 or 2 thousandths of an inch of putting it exactly where it was when it was first cut, I hope that will be close enough for most of the molds I plan to make.

~ Jeff