Results 1 to 20 of 22
Thread: Cutting a arc on manual mill
04-08-2010, 09:55 PM #1
Cutting a arc on manual mill
Need to cut an arc on a manual BP has a DRO (non programable) Apx a 3" radius arc. Is it best to scribe the arc and attempt to follow it manually and then clean up with a sanding wheel or use the Dro to help take a series of cuts. Just learning so any help with setting up the DRO to do an arc would be appreciated.
04-08-2010, 10:32 PM #2
Well before CNC everthing was either round or square . sorry
04-08-2010, 10:38 PM #3
No rotary table?
04-08-2010, 11:00 PM #4
yeah, rotary table, gotta be, otherwise you don't need the BP to begin with.
It's not etch-a-sketch.
04-08-2010, 11:33 PM #5
Rotary table, but if you don't have that, it depends on the number of parts, tolerance, and whether this is a "get it done, no matter how" job, or a "time is money" job.
If time is not an issue, you can use a large diameter endmill (i'd go 1" or so) and essentially make a 1000-hole bolt circle. Then just plunge at each of these points. Depending on how closely spaced each plunge is, the finish can be quite good. The drawback, of course, is it takes forever.
I used a similar method to cut a very accurate coarse helix on my bridgeport without a helix attachment for my dividing head.
04-09-2010, 01:22 AM #6
Hard to know without actually seeing what you are making. Another way of doing it is with a boring head set to the correct radius and take a serious of cut intil you are to size.
04-09-2010, 02:04 AM #7
If you are reasonably math and computer literate its not that difficult to use a spreadsheet to compute a set of co-ordinates for plunge cuts using an end mill in a similar manner to the 1000 hole bolt circle suggestion from Halcohead. I have a feeling that there is a free program or spreadsheet macro out there to do this (from Marv Klotz?? maybe) which will start from any set of co-ordinates so you don't have to re-set the DRO. Print-out large and cross off each pair as you go. If your settings are fine enough to get a decently smooth curve you won't see if you miss one of a pair or miss a step. One error can usually be cleaned out but make several and you could be in real bother. As I found out on a job with plenty of work already invested!
Harder if you don't have circular arcs. My DRO does circle arcs but when I needed a varying non circular arc curve I ended up rough plotting the thing in Cricketgraph, curve fitting to get an equation and evaluating that in a spreadsheet to get enough points to make a smooth curve. Tedious.
Good start for a smooth is increments about 1/20 th of the cutter diameter and cutter less than half the arc radius. Larger increments are fine if you can get in to clean it up. As I recall things there is little gain from going smaller.
04-09-2010, 04:52 AM #8
You can make a table of values easily in a spreadsheet program. The table of values is how CNC got started.
You don't state desired accuracy, or if the shape is through. If it is a through shape, finish it with a file. If its not a through shape, think about making it one by overlaying the part with the arc on the base material.
04-09-2010, 05:16 AM #9
It seems a swivel base vise, just clamped down between the 1,000 pts and 1,000 plunges, would do a decent job.
Might take a little fiddling around to get the right radius set in also, but it would work.
04-09-2010, 06:15 AM #10
Take two square pieces of steel big enough to lay your workpiece on and a hard dowel pin. Drill one hole through the center of both piece, tight enough for an interference fit. Ream one plate to make a sliding fit. Press the pin into the interference fit. Bolt the piece with the pin in it (pin up) to your table and indicate it to center the pin under the spindle, and note your coordinates. Bolt your workpiece to the other plate with countersunk screws from the bottom, with the part located with the arc the appropriate distance from the dowel pin center. Use spacers if you want to preserve this "fixture". In a place that does not interfere, bolt a long handle (e.g. several feet, long enough so that it can't make a complete revolution without hitting the mill frame) to the top plate. Apply grease between the plates and assemble. Fix a small diameter (for safety) endmill in the spindle. MAKE SURE YOUR ENDMILL HELIX/SPINDLE DIRECTION PUSHES THE PART DOWN, NOT UP. Move the table so that the desired radius (include half the endmill diameter in your calc) is achieved. Standing outside the radius of the end of the handle, turn the machine on. Remaining clear of the handle, you should be able to slowly swivel the part to cut your arc.
Or, for a a couple hundred bucks buy a used rotab on ebay.
Note the small diameter end mill (it will take longer with a less-nice finish, but the small diameter imparts a lower torque on the part from the machine spindle), long handle (high torque on part by operator, operator standing outside the radius of handle) and helix direction (machine does not spontaneously disassemble your fixture). You could drill and ream extra holes around the circumference and drop pins in them as you progress to limit uncontrolled travel of your system, or you could use a sleeve with a countersunk bolt instead of a dowel to ensure the top plate is held down.
04-09-2010, 07:19 AM #11
I've used circular interpolation to cut arcs on milling machnes ever since I learned it was possible in 1966. You have to calculate a tool path and that requires a little trigonometry. The tool path is nothing more than the radius (arc) you wish to cut plus (or minus) the cutter radius. Cutting an arc via circular interpolation is the same thing as drilling a bolt circle only there's lots more steps.
A spreadsheet takes a lot of the donkeywork out of the calculation and believe me it's worth learning to use a simple spreadsheet program just for circular interpolation and bolt circles.
Or you can do it manually:
Select a cutter and determine its radius. Add the cutter radius to the work radius if the arc is convex or subtract it if the arc is to be concave. That's the radius of the tool path. Next select the number of steps that results in overlapping cuts. This leaves a scalloped edge whose little crests are called "cusps". The larger the cutter radius and the smaller the step the smaller the cusps you have to later dress off.
Plunge cutting with a flat ended endmill causes large circular cutting forces; enough to shift the part unless it is firmly clamped. An endmill ground with a drill point will do the job with less strain on the machine. I'd size the endmill according to the material and the stiffness and condition of the machine. I have a Bridgeport clone. A 3/8" endmill plunged straight into aluminum is about the limit for plunge cutting from the solid.
The formula for each cutter position (offset) is X = Sine of the step angle to the axis times the tool path radius. Y = Cosine of the step angle times the tool path radius. Next position is 2 times the Sine... next step 3 times... and so on for the length of the arc. Remember that you multiply the step angle by the step number BEFORE you take the Sine or Cosine from the trig table.
If calculating by hand you make up a table of four columns listing step number, step angle, X offet, and Y offset. A spreadsheet will print this automatically. I clip the offset list to a piece of plywood and use a 6" scale to track my steps.
Locate the center of the radius and set a 0,0 on your DRO. Dial in the first set of offsets, lock the axes, and plunge. Proceed from step to step until the radius (arc) is complete.
You may wish to bulk out the waste with a slightly undersized cutter then finish with the on-sized. Sounds like a hassle and it is but after a few sessions the process becomes almost automatic. I have to be careful. I'm a little dyslexic and tend reverse pairs of adjacent numbers. If you have any quirks like this you will soon to be careful.
If you do a good job dressing off the cusps the radius will be clean and smooth as if fully machned.
04-09-2010, 09:10 AM #12
I have done this sort of thing a number of times, including other than circular curves. I made a series of involute cutters from flat stock to cut large Plexiglas models of tiny gears to check the mesh. I first roughed the shape to remove material, then programmed my Hewlett Packard 9100 calculator ( the one I am named for ) with the involute formula, incrementing a small angle with each repeat of the program. Then it was just a matter of setting the initial X & Y, hitting the continue button, setting the new X & Y, repeat until total boredom or finished part, whichever occurs first. This is what a CNC machine does, without the human in the loop. I stoned the scallops out. I did not use plunge cuts, but was careful to make the movements in the same order every time, X first, then Y, or the opposite. Remember to make the setting that will move the cutter away from the work first. Otherwise, the actual cuts will be the setting for one axis and the previous setting for the other axis. I used the largest cutter that would fit in the radius to minimize scalloping.
Note to Bosley- I have also used the method you describe with good results, but almost any cutter you find will lift the work because they are designed to lift the chips out of the cut. You just need to make the setup rigid. Again, I used large cutters and used the appropriate axis to feed the part over in small increments until I got the pivot point to the center of the desired radius. Of course, that approach would not work for a radius of more than 180 degrees.
04-09-2010, 10:19 AM #13
Both the bolt slot arc and the upper arc on this shop built clapper box (on this shaper) were done using the above described methods. Neither required perfect scallop free finish, so no spread sheet was made an it did not take so long. Just trig and knowing what to do with it. There is also no DRO on the mill used.
04-09-2010, 01:23 PM #14
04-09-2010, 02:51 PM #15
cuttin an arc on manual mill
HELLO TO ALL,
i think you might find this in PATS LINKS.
there is some information for cutting a large
raduis on a mill. don't know if this is what you
are looking for, but if you have never been to this
website, it is worth looking at.
04-09-2010, 03:07 PM #16
04-09-2010, 03:50 PM #17
Another option, should you have one, woud be a Volstro rotary head or a big Milwaukee rotary head mill. Zero on the center of the arc, run the spindle out to the 3" radius and do it to it. I found a Milwaukee rotary in a scrapyard, but somebody had already cut the knee off the column with a torch.
04-10-2010, 02:54 AM #18
04-10-2010, 06:15 AM #19
Pat's Big List Of Metalwork Links
04-10-2010, 06:26 AM #20
cutting an arc on manual mill
HELLO TO ALL,
when you go to PATS LINKS, you will have
to scroll down to HINTS, AND HOW TO, in
order to get to the part that says cutting a
large radius on a mill.
you may spend time on this website, because
it is overwhelming!