Need advise for boring a taper

[Captdave]

I have a job that will need to be held in a fixture with 5C collets and need to figure out how to bore the 10* taper to match the collet. I'm running them in a fixture simular to the one I had posted in a earlier post but its not as ridged as I would like and the bolts are leaving undesirable marks on the parts.

I'm going to try making a some split bushings first and see if that will work but if not I would like some advise on how to program the taper. The collets are 1.45 OD on the top and taper down to 1.250" at 10*. I'll be making nuts to screw on the collets from the back side to tighten them.

Thanks, Dave

[glovebox20]

WOW , did anyone say challenge?

I supposed that you don't have a 10* end mill laying around (or purchase) that you could use. Just mill a couple of circles until you get what you want. That would probably the first thing I would try.

If you have the 3d option, you could may try to mill it out with a ball mill perhaps. But this is one feature I never used (current employer doesn't want to buy upgraded software).

There is one more option you could try. First, select a tool (ball Mill preferred). then create a Mill block using lines and arcs. Select "ON" for cutting type. Select a start point on top of your part about the radius away from center point (large dia.) minus cuter dia on "X" put Z start at .020 and Z bottom at "0". Create a new line segment. Move X over to make 10 deg angle match Z move. Change your Z end to chamfer depth + radius of ball mill. Then create a pattern rotate block to rotate the path all the way around until completed your circle.

Here's what it should look like:

I'm going to say a 5C collect has a body Dia 1.250" and a full dia of 1.450 with a 10 deg. angle. I'm going to start on top of the part and mill down. You may want to Rough a few circle pockets first before finishing with the ball mill. Is the 10 deg part of the chamfer .5671 deep? (trig anyone?)

Part zero: Center of part

Block one
Pattern Rotate (Winmax Mill Conversational Part Programing 4-5)
Number: 180 # of time it will repeat blocks
XC: 0" X center
YC: 0" Y center
Start angle: 0 Start at 3 o'clock
Rotate Angle: 2.000 deg Rotate 2 deg (2*180=360 deg.)

Block two
Tool 3/8 ball mill
Cut Type "on"
X start: .5375" ("Full" dia radius minus cutter radius)
Y start: 0"
Z start: 0.02"
Z bottom: 0"
Peck: 0"

Block two. Seg 1
X end: .4044" X start minus "Z end value" to make 10 deg angle match, .5375-.1331=.4044?
Y end: 0"
Z end: -.7546" Depth of chamfer plus radius of ball mill .5671+.1875=.7546
Line Length: Leave Blank
Angle: 180 deg (milling left and down)
Feed: What ever.

Block three
Pattern end.

May want to add something to your tool/part offset to run the program above the part first. The tool path should look like a cone shape with the larger part towards the top of the part. I if the tool path looks right, I would keep adjusting your X start and X end until the chamfer is to size (Hint: use Copy and Change blocks and modify the X dimension to the mill block). Make sure there are NO blend moves enabled or it will probably look funny. The Ball mill should position .02" above the part, mill straight down .02" (to Z0) the mill to the left and down at a 10 deg angle, then rapid back the Retract plane, Rotate path 2 deg. and mill again until you have a complete cone shape circle pocket. Of course, you may want to add pattern locations if you want the do this in more than one spot.

It may not be pretty and probably will be tedious and time consuming, but it might be worth a shot.

Let me know if this works or not.

glovebox20

[Rich Carlstedt]

Am I missing something here ?
I would just get a 3/4 or 1 inch endmill (sturdy) and have it ground with
a 10 degree angle. and use it as is (or whatever angle you need) with circular moves.

Check End Mill suppliers for the forging die Industry, as Die Sinkers use these cutters all the time.

Rich

[Captdave]

Winmax has 3D arc milling built in but I haven't even tried that function LOL. Enco has a 10* tapered mill for around $60.00, since it will be cutting aluminum and I probably will never use it again, I may go that route if the split bushings prove not to be the answer.

[bloke]

How about holding the part in the spindle and programming a line in X/Z to re-create the taper. I did a load of fancy door handles a few years ago using the machine as a vertical lathe.
You just need to program the taper and adjust the X part offset to get the diameter bang on.