End mills

Discussion about the CNC Shark Pro Plus HD

Moderators: sbk, al wolford

End mills

Postby gpeck » Thu Oct 12, 2017 11:40 am

How good of job will a 1/4" end mill that has a 1" cutting length do on a pocket cut that is 1 1/2" deep, with 1/8 deep cuts and still leave a smooth cut on the side???? Thanks for any info......
gpeck
 
Posts: 158
Joined: Fri Sep 06, 2013 1:35 pm

Re: End mills

Postby Rando » Fri Oct 20, 2017 11:58 pm

What you really want is an "extended length" bit that has a narrower neck by about 0.010. I have some 2fl 1/4" (radiused!) end mills where the flutes are 0.375" tall, and then the shank behind (above) the flutes is cut back that 0.010, out to a total relieved distance of 2.25" inches. This lets me cut a 12mm hole into a solid 2" block of aluminum...on a Shark HD2+. The below picture shows a fully-fluted and an extended-length 1/4 bit from my crib.

Many times, doing that will work okay, but can leave lines if your system isn't very rigid and aligned....need I say more? So yeah, a thin finishing pass with a longer flute-length bit is sometimes needed.

20171020_214057[1].jpg
L-to-R: standard fully-fluted 2-fl 1/4"; 1.5" LBS (overall cut length), 0.375" length of cut (flutes); 2.25" LBS 0.375" LOC.


The first picture, those are the bleu cheese of the steak world, bay bay! Um, okay, yeah....on the left, a traditional full-length fluted bit. In the middle is a bit with the same effective total cut depth, but with only 3/8" cutting. I'll save you the tech talk (this time). Let's just say it's betta. The one on the right, though, that's somebody's good luck charm. That will dig a 2.25" hole in a block of metal just like you, well, programmed it to do that....nevermind. It's a wonderful thing to watch, but dang is it terrifying watching it slowly descend into that block of metal :D.

20171020_214239[1].jpg
Two 1/4" 2Fl end mills. Top one is radiused, bottom one is standard. Love me them curves!


The just-above picture shows two 1/4" end mills. The top one has had the sharp tips ground down to an 0.030" radius. This greatly extends the life of the end mill overall, because even the smallest chip in the sharp teeth of that bottom one can render that $60 bit worthless. So yes, even at a cost of $18 each bit, I have them rounded off, because they last easy an order-of-magnitude longer.

There are many benefits to that LBS-style bit: on a normal fully-fluted bit, the torque, deflection, and on our machines the chances of outright failure of a cut increases linearly as the flute-engagement length increases. By having the flutes only 3/8" tall, the maximum torque is known, and relatively tractable for our machines. Likewise, if the hole is really deep with vertical walls, even with the relieved shank, if the system isn't aligned well, you'll get collisions with the top of the bit way down deep inside. Depending on the situation, it can break the bit, ruin the alignment of the spindle mount, and even pull a part from a vise. Another cool benefit is that internal bottoms have a smooth radius of that amount. The parts are less likely to fracture from that sharp stress-point in the corner, and so are a little stronger. With just 0.030 (effectively 1/32") radius, it doesn't often cause interference issues.

The downside is they are spendy! The ones I get from Swift Tool in Kent, WA, of that style, run in the $65-90 range, EACH. Add on to that the obligatory corner radiusing, and you're looking at a $90-120 1/4" bit.

Hope that provides a little food-for-thought. You can usually find those bits at MSC and Tools Today and such. If you don't find what you need, call Tarik at Swift Tool (253-854-7777) and ask for something in the AC line, like an AC025026WG67S100 (not radiused). Just call. Ignore their web site (https://www.swifttool.com/)...it's an embarrassment, they know. They know CNC grinders and carbide end mills; they don't know web sites.

Regards,

Thom
=====================================================
ThomR.com Creative tools and photographic art
A proud member of the Pacific Northwest CNC Club (now on Facebook)
Rando
 
Posts: 415
Joined: Tue Jan 06, 2015 3:24 pm
Location: Seattle, WA

Re: End mills

Postby Rando » Sat Oct 21, 2017 12:31 am

gpeck wrote:How good of job will a 1/4" end mill that has a 1" cutting length do on a pocket cut that is 1 1/2" deep, with 1/8 deep cuts and still leave a smooth cut on the side???? Thanks for any info......


Now, just to give some more info on the "smooth cut on the side" part....

That's often down to two things: chips in the endmill's flutes. Even tiny chips can cause those lines. But, in wood, the surface final sanding (if any) and the finish often hides those, or they're at least easily removed. There was a recent thread about this; someone suggested a rubber eraser (white or red I don't remember, maybe depends on the wood ;-) ). A dremel-mounted at low RPMs wire wheel would probably make short order of any outward threads.

But, then there's that SECOND thing. And that thing is the sag and deflection in your gantry and spindle/router mount. This is more difficult to get rid of, but in the end comes down to some combination of these solutions:

1) a final finishing pass that's nice and thin, so there's no deflection. In wood probably 0.010-0.020, while in metal I typically do 0.002-0.005" for the final finishing pass. Too thin and the bit will slide instead of cut, making heat and ruining the bit and likely the piece.
2) Sharp bits. Dull bits cause more torque on the whole system. Don't run bits for 40 years and claim they're the same as day one, we all know bits have finite life-spans, and trees eat dirt, which is made of rocks.
3) Cutting in the right direction. Whether it's using climb-milling, or only cutting finishing cuts along the gantry's direction of travel, there are any number of tricks you might find make your machine more happy about not making lines in tall walls. For me, if I'm "pulling" the bit (along the gantry direction of motion), I expect to be able to make much heavier cut, because the bit tends to lift out of the material. But, if I'm "pushing" the bit (going the other way in that same axis), then I know I need to be a lot more careful, since that plunging bit will destroy any dimensional accuracy of a pocket bottom :(.
4) A rigid system. Yeah, I know, there isn't much to go on here. Maybe soon, we'll see.... An aluminum mount plate (Dixie something or other, IIRC) does help, but it doesn't solve the problem entirely. And that problem really comes down to High Density Poly-Ethylene. As in pretty much every piece of HDPE in that gantry and Z-axis system somehow contributes to the deflection. So, it's a reality that has to be dealt with.

All things are possible. Some are just more feasible than others ;-).

Hope that provides a bit help of a vexing problem many of us face in those deep pockets...mainly because we DON'T have deep pockets ;-).

Regards,

Thom
=====================================================
ThomR.com Creative tools and photographic art
A proud member of the Pacific Northwest CNC Club (now on Facebook)
Rando
 
Posts: 415
Joined: Tue Jan 06, 2015 3:24 pm
Location: Seattle, WA


Return to CNC Shark Pro Plus HD

Who is online

Users browsing this forum: No registered users and 1 guest