PDA

View Full Version : Best practice for milling a shape out of stock?



Rtldan
10-18-2013, 02:42 PM
Hello all!
I am new to cnc milling (and this forum!) and I'm using a Taig with gecko 540 drivers.

I have a shape that I would like basically "cut" out of a piece of stock.
My question is, are there any best practices I should be aware of when removing a shape from the center of a piece of stock?

For example, if I wanted to cut a disk out of my flat bar stock, and I'm cutting it in the middle, what prevents the disc from flying out wildly after the cut completes?
And if I am cutting all the way through my bar stock it's most likely up on parallels right?
So do we just let the shape fall from the center of the stock down into the gap created by the parallels?

Sorry for such inexperienced questions. I did try a google search, but finding the right search terms proved difficult.
Thanks for your time!
-Daniel
Portland, Oregon

Rosco-P
10-18-2013, 03:09 PM
How thick is the stock? How complicated is the shape? How accurate must the shape be? Sometimes simple approaches are best. Could it be sawed out and finished by other means? Files, belt sander, bench grinder, die grinder, die filer, etc. Maybe not in your arsenal of tools, but waterjet, plasma cutter, gas axe.

Oops, too fast hitting reply. A disc...., what about a hole saw, rotobroach, fly cutter?

goodscrap
10-18-2013, 03:22 PM
or like my sheet metal bashing mate does, leave at least 3 tiny tabs (about 0.020") to hold the item, then break it out and lightly finish by hand. so if cutting a circle cut most of the depth, but leave the tabs only about 0.030" thick. the number of tabs required depends on the size of what you're cutting out


if you go for a full cut then it might damage the machine/tooling if it wedges through climb milling for example, as said above, other processses might be more suitable

Jaakko Fagerlund
10-18-2013, 03:31 PM
You can expect that the piece will flyout and ruining your cutting tool, sometimes it doesn't happen and sometimes it does, depends on many variables. Best would be to rough out the slot first, so that when finishing the shape the cutting tool doesn't have to cut on both sides of the slot, meaning make the slot wider before finishing. This prevents the flyout tendency somewhat.

I have occasionally milled the shape so that it has a couple of 0.5 mm thick tabs left on it at the bottom, so that it can be just cut or punched off the main stock. Other option is to finish one side of the piece first and attach a clamp to the part and then do the other side. This however will leave lead-in and lead-out marks on the edge of the workpiece in two places.

However, I would question why would you need to mill it so? Can't you just rough out shape from a smaller stock? Or how about milling it to a the upper end of piece and then sawing off the part that held it in the vise?

Or, as I have done many times if the part allows: drill two holes in the workpiece first and then clamp it on two "parallel rings" to your T-nuts. This leaves the whole outer periphery free of clamps, so you can mill all the offending material away. Or if the stock is to be saved, you can clamp the excess stock in two places and then mill the slot, thus separating the workpiece from the stock. Then you can unclamp the excess stock, remove it from the table and do your finishing passes on the workpiece that still sits there attached to the table with those screws.

DR
10-18-2013, 05:32 PM
In milling a disc sometimes I just let it fall and yes, it will sometimes fly out. But, the fly out is not usually any more than just pushing it aside, not flying into your face. Mostly not a good idea, we all do it though. Don't let it drop loose if you're using a fragile cutter (like a tiny end mill, it might get broken).

The best way if possible is clamp a scrap of aluminum or steel in your vise. Drill a hole in your disc material, bolt it down to the scrap in the vise. If I can't put a hold down bolt in a hole in the disc I usually leave .005" or so un-milled through and break the disc out.

macona
10-18-2013, 05:56 PM
Stuck the plate to be milled to another plate with double sided carpet tape. Or super glue it. Cut it out and debond.

lbhsbz
10-18-2013, 06:28 PM
workholding is the hardest part about machine work.

For what you're doing with just CNC mill, I'd start out with material 1/16" thicker than I wanted....I'd rough out the circle from one side leaving it about .040 larger OD than I want, then come in with the same cutter and finish the OD, but don't go all the way through the plate...stop your cut 1/16" before you go through.

Then flip the plate over, and mill 1/16" off of the backside of the circle...it'll fall out with minimal burrs when you're done.

Now, if I had more equipment at my disposal, I'd rough cut the circle on my bandsaw, clamp it down to an undersized block on my rotary table with 2 clamps positioned on one side. Machine as much as the OD as you can without hitting the clamps, then move one clamp at a time to the other side of the part, then machine the rest of the OD.

Rtldan
10-18-2013, 06:46 PM
Hello all!
Thanks for your suggestions!
Yes, I can see how a disc shape might be more easily cut out with other methods.
The disc shape was actually just an example for clarity. Sorry about that!

My actual shape is a bit more complex than a disc. It's actually a one off prototype for a cell phone case. The stock wouldn't actually need to be much larger or thicker than the profile of the case, however, I'm attempting to essentially make an open "ring" or "bumper" for this particular prototype, which means there won't be any material in the center of the profile (back or front) to which I could attach work holdings. It's essentially just the contour.

My original idea was to make a fixture that was essentially a negative of the part with clearance for the endmill so that I could cut the profile. At this time the work piece could be held in the center with screws or something. Then using the fixtures clearance again, mill the center out and basically let the outer bumper ring drop off of the screwed down center piece of stock. I suppose it might be possible to use some double sided tape, or even very small clamping on the corner of the bumper after the profile has been cut. I've also got some cam screw low profile workholdings that might be of use...
Any reason this is not a decent idea?

Again, thanks so much for your help. This adventure into CNC Milling is one wild ride and I appreciate the support of the community for newbies like myself!
-Daniel

JEZX
10-18-2013, 06:56 PM
i made a bunch of aluminum bars for parallels ,i put them under the center of my work and cut 95% of the depth away then cut 1/2 way around on one side 100+% depth , the put a hold down to the center and cut the other half .
ive made lots of parts which i just cut 99% of the depth and pop the part out and file off the last 1%.

it also helps if you make 2 full alternating paths for the cut , stepping .01 + from one cut to to the finished cut .clime the inside cut and the outside cut . so if you are cutting a 1'' circle cut 1.01 away for ever other pass .

bobw53
10-18-2013, 08:05 PM
There really is no "best" way to drop something out of a plate.

Best way has already been said, start thick, then flip and face.

Leaving tabs is good thing, especially if you are dropping your finished part, actually with tabs, you aren't dropping it. I'd say that leaving a small bit all the
way around is just about the same thing. Works best when the plate is attached to a plate of some sort.

You can completely drop it, but it won't be finished, since there is nothing holding it. I only completely drop something when I really don't care or the drop out
is a hole in the part I want to keep. To keep from breaking endmills, you need to break it out where the endmill is really only constrained on one side, in a pocket
or a hole. This can require some experimentation.

Better methods when your stock is already to thickness... If you have holes, do those first, then bolt it down.
Also, machine only part of the profile, then grab that part of the profile in soft jaws and machine the rest.

I'm sure you are trying to get this done in one operation, but occasionally, multiple operations can result in a quicker, and more stable process.

Dave S.
10-18-2013, 08:53 PM
As Bob above said. Do any interior work first and then use cap screws into prethreaded holes in you base plate. You can also use servo screws if you are using a wood base plate. Here is an example of the latter.

Dave

http://i132.photobucket.com/albums/q3/Dave_Sohlstrom/000_0646_zps46ccb63e.jpg (http://s132.photobucket.com/user/Dave_Sohlstrom/media/000_0646_zps46ccb63e.jpg.html)

Rtldan
10-20-2013, 05:58 PM
Hi again everyone!
Thanks for the detailed explanations and various ideas on how best to accomplish this sort of thing.
I think I have a lot better idea on how to go about setting up my job.
Special thanks to Dave S. for the picture which was extremely helpful. I hadn't considered using cap head screws with washers. Pretty great idea, will have to try that one.

Looking forward to learning more from all the fine people on the HSM forums - and maybe someday contributing too!
Many thanks again,
-Daniel