CNC Milling - a "how not to" compendium

[kvom]

Having gotten my new mill (Novakon NM-200) installed and running along with mach3, I decided to make a part. The one I chose was an outer main frame for the ER Westbury side paddle engine that will be my next "big" project. I chose this part since it is fairly complex. That might be the first mistake, as doing a simple part first might be more sensible. Other than that, I learned a few things the "hard way.":

1) Endmills don't like cutting deep slots (i.e., 3xdiameter) in 6061, esp. w/o coolant. (scratch one .25" carbide em)

2) Non-centercutting endmills can't cut slots of any depth unless starting from outside the stock (scratch one .25" HSS endmill)

3) When mounting on sacrificial stock/fixture, make sure that the fixture will fit in your vise, and if it does that any bolts/screws used ton hold it are outside the toolpaths you will need.

4) When making a part with an irregular contour like this one, the stock needs to be mounted on the fixture for the duration. In this case, I had a couple of holes that could be drilled through the stock and fixture for securing with bolts. To do this, the holes need to be reamed and a precise pin pressed into the holes to obtain reliable repositioning. Of course I didn't do this. In then future I plan to use 2-sided tape.

5) Trim the stock as close as possible before mounting to the fixture. In this case, a roughing endmill would have saved me a lot of grief.

While Westbury made his frame pieces from steel, I decided to use 6061 aluminum as I had a piece of scrap that was close to the right size. For the next attempt I'll plan on using steel myself as the swarf is less likely to stick to the endmill flutes.

 

[tmuir]

The lessons that cost you money you always remember.
The first time I used my mill I broke a $25 endmill.
I always spend a moment now to make sure I'm not 'climb' cutting now. :big:

Wish I could afford a CNC mill.

 

[Ed T]

Yeah, bolts are not reliable locators. Dowels or roll pins work well. I've also see tubular pins that the bolts go through if real estate is limited. Be careful with the DST. it can "ooze" in response to lateral loads. For something as critical as the side frames I think you'd be better off with something more rigid and inelastic.

 

[vlmarshall]

Be careful with the DST. it can "ooze" in response to lateral loads.

Too true, taped-down parts can 'squirm' a bit under heavy cutting, if they aren't against a rigid stop of some sort.

 

[shred]

Try superglue as well if you're running coolant-- Double-stick doesn't like that much either.

You can pick up a hole pretty well if you have to move the part for some reason-- 'Blake' style indicators work ok since you've got extra Z to work with as do DTIs and the pointy edgefinders. As long as you know where the hole is supposed to be, you can zap the coordinates right into Mach once you pick it up.

Also think about making aluminum soft jaws for the vise and double-check whatever depths, feeds & speeds your CAD-CAM program spits out. Bobcad loves to try and drive an end mill plunged way in at full SFM and chip load around, no matter what the size and required HP you have if you let it. Some of the Mach wizards don't adhere to tool length offsets too.. I busted a carbide v-bit last night discovering that. :-\

I have a box called 'broken bits'. 90% of it is the result of CNC misadventures.

 

[kvom]

Thanks for the replies.

The frames all have irregular profiles and thus impossible to clamp with vise alone. The inner frames also need raw stock that's ~7"x5"x3/8" with most milled down to 1/8 thickness. The good news is that most of the profile is decorative, with only the drilled hole locations being critical. So my plan is to drill all the holes before any machining, so that any slight wiggle on the tape will not effect anything. That said, I think I will ream the holes after drilling and insert some dowel pins down into the fixture to further stiffen the setup. I don't have any suitable stock material at present, so will work one some other parts in the meantime.

I am also not using any G43 codes as I don't have quickchange tooling. So I'm setting Z height after each tool change. I've used CamBam for the tool paths, and thus all the heights and speeds&feeds are entered manually. I might use BobCad more in the future although the learning curve is longer.

No coolant at present, although I do have a KoolMist setup I got with the manual mill that I've never used. I might give it a try.

 

[starbolin]

I like the idea of inserting dowel pins after drilling but before profiling. Another trick on the thin pieces is to mill the profile not quite to full depth, leaving between 2 and 10 thou depending on the work. Then cut the flashing away after milling.

You're not going to be able to do any kind of pocketing or aluminum without some kind of coolant setup. Worst case mix up some soluable oil and put it in a spray bottle. I've spent many an hour standing in front of a CNC misting a workpiece. Used to do that for so long my hand would cramp up.

CNCs eat up cutters to meet their nutritional requirements. Always start your job with spares. Nothing like stripping the teeth off of your only 1/2" ball end carbide mill ( $45 ) late at night with no chance of buying another till morning and having to spend several hours regrinding the flutes just to get back to the customer's job in time to finish at first light in the AM.