Advice on how to do this piece

[Swami]

I dont know anything about machining. I am just stumbling through this with my Sherline 5400 CNC mill.

Here is a picture of a part I make:


Its cut out from 1" bar stock, so you can see its about 4-5" long.

I come in from the side and mill out both sides with "peripheral" milling. So basically every bit of material that is cut away is in the form of a chip (No big hunks)

This takes forever, IMO. It takes 30minutes to do cut this part out, using a 250mm/minute feedrate, taking .20mm cuts.

On the one side where the cutter's diameter is less than the pocket of material I am removing, I have the opportunity to cut a deep channel until is parts away a chunk, I could then come in and clean up the mess.

The problem I find is that digging a channel like that generates a lot of chips, and requires constant babysitting to lubricate and remove chips. This is why I do the peripheral milling. The chips fall out of the way, and it barely needs lube. However, it is hella slow.

Is there a better way?
Thanks,

Swami

[JFettig]

put it in the vice like that, mill off the two ends, drill the holes then flip it up, rezero or use a stop and mill the top part off.

Might I suggest roughing end mills to you? I dont know how good this needs to be or look, but I know that with roughers bigger cuts can be taken.

Jon

[HuFlungDung]

What kind of material are you cutting? What type and diameter of cutter? What horsepower does your machine have?

.2mm depth of cut seems a tad too cautious, a good file would cut faster

[Swami]

Originally Posted by HuFlungDung What kind of material are you cutting? What type and diameter of cutter? What horsepower does your machine have? .2mm depth of cut seems a tad too cautious, a good file would cut faster

I know!

Well, its a 5400 Sherline. The motor is 1/3hp. The material is a softer grade aluminum (Ace Hardware stock). After about 4-5 hours of cut-time the 3/16" HSS cutter I am using is quite a bit less sharp. There is plenty of chatter that I can't seem to get rid of. I have a max RPM of 2800, but it seems to sound best if I run it at around 2000.

I had been doing this part in a vice, with the whole part extending to the left of the vice (meaning it was unsupported). Didn't seem to make any difference in chatter when I clamped it down (both ends) to the table.

I do the .20mm cuts because larger and the whole thing starts to sound pretty bad. The motor doesn't seem to be growning, its the chatter and vibration that makes me want to take a lighter cut.

I have the tiny little machine base (6x12" or so) sitting on 3/4 in board. There are rubber isolation pads between the machine and the board. The board has rubber isopads on it as well, and this just sits on my workbench. Do the iso-pads create a rigidity problem? The idea was to cut-DOWN on vibration, lol.

Thanks everyone,
Swami

[DareBee]

I would be inclined to machine that in 3 steps. Basically from each side facing up to do the necking (or dogbone effect) then from the top for both end steps and the holes. I assume you dont have a toolchanger so you can change tool to a drill and drill holes then change back to milling cutter to start next part. Cant you get a 3/8 or 1/2 end mill in it? Even a 1/4 probably twice as strong. You should be able to run 30 IPM with 4flute cbide at 2000RPM.

[Swami]

Originally Posted by DareBee I would be inclined to machine that in 3 steps. Basically from each side facing up to do the necking (or dogbone effect) then from the top for both end steps and the holes. I assume you dont have a toolchanger so you can change tool to a drill and drill holes then change back to milling cutter to start next part. Cant you get a 3/8 or 1/2 end mill in it? Even a 1/4 probably twice as strong. You should be able to run 30 IPM with 4flute cbide at 2000RPM.

I can use up to a 3/8 mill, I just like the smaller radius thats left by the smaller tool. However, I am open to suggestions and appreciate that you bring this up. I haven't really tried to find out how much faster I can get material off of that with a larger endmill. It might make sense to rough it out with a 3/8 if I can get bigger cuts and then finish it with the smaller one if I desire that radius?

Why would you set it up three times though, rather than letting the whole part get cut from the top? Is there something about not wanting to use the sidewalls of the endmill like that?

Thanks!!
Swami

[HuFlungDung]

Are you using a collet type milling chuck, or a solid endmill holder? An ordinary drill chuck just won't do.

I would also be wondering about how much overhang your tool tip has from the nearest spindle bearing. You've got to keep it short on those small machines. You might check the spindle for free play both endwise, and laterally by applying some hand pressure against it while monitoring for movement with a dial indicator. There will likely be some flex, but there shouldn't be any "click flex", as though a bearing fit was loose, or something similar.

[Ken_Shea]

(boy, I wish a sentence could be written with out using the word I anyway..


Flipping parts while using CNC flips switches off in my brain so I try and avoid and/or limit it whenever possible. Not sure how large your vise opens up but if it is large enough to accommodate the 4-5" that would simplify things. Do all the top machining as necessary and then flip the part on edge and manually remove the resulting corner radius in the notch. This would probably take less time then creating the additional tool paths and work offset setup.

Definitely larger end mill if possible, 4 flute may get you into trouble with flute buggers on that soft aluminum if you do not take serious steps to keep those chips out of the way.

[nervis1]

Have you thought of doing the part manually? From the photo looks like a couple of profiles, holes. Little bit of Dykum, and a center punch, and a good ruler, I'd have that part done in 30 min on my mill drill. Maybe less.

Sometimes for simple stuff I just put my VMC in manual mode and make chips.

[DareBee]

The corner rad is a big reason for flipping as well as the fact that I feel a cutter will rip material out quicker straight on like that.
In a conventional machine it wouldnt even begin to cross my mind to machine that all from the top unless I specifically wanted corner rads. Those corners really put a lot of stress on a cutter as well unless you are contouring a larger rad than the cutter has.

[HuFlungDung]

I wouldn't worry about overstressing the roughing cutter in the corner, after all, the cutter often has to plow full width through the stock somewhere. For finishing, though, I would also try to avoid having the cutter with the same radius as the corner to avoid possible chatter (on a deep wall). In designing the part it is often enough to spec a .2"r corner instead of .1875" which will most likely match the endmill in use. I wonder how many engineers ever give that a thought?

[Swami]

That drawing has caused plenty of confusion for your generous helpers out there. My apologizes. The drawing is not accurate, insofar as I did NOT include the radiuses on the inside corners. Thats why machining it from the top is possible. I don't even want those straight corners as shown. I've been working with it so long, its like I see the radius cuts, sorry!

But apart from that, maybe I just learned something important. When possible, it would be better to have corners with a radius greater than the cutter? This would make sense compared to my observations. There is a great deal of chatter when the cutter is making even minimal cuts at full depth when it meets the "side" of the cut. I suppose some fancy software would make this kind of programming a lot easier. My brain hurts trying to figure out how I am going to write all the g3/g2s (each pass) needed to make sure the cutter is cutting a radius larger than its radius. I could do it, but it doesn't seem fun.

I have it programmed to zig zag along X as it increments slowly in the Y direction. At the X min/max, the cutter isn't as happy is it could be I think. To try to help, I have the last .10mm set to a very low feed as the X hits its min and max. This slows it down a LOT though.

Trying a larger cutter lastnight (3/8) I didn't have long, but I did find that the machine can easily throw much bigger chips (much farther also I might add). I want to write a proper program to test it, but when the cutter was loaded (running in once direction) it didn't seem to mind removing over 1mm in a pass. Quite a bit more than the .20 I was doing. I just have to find out what it thinks of changing direction (load) and how the chatter is. (fingers crossed)