Need Help!- conical machining

[Shibumi]

1. How does one program a conical cut (depression into the material?
What tool does the job best so the stepping is minimized?

2. How are parts typically held in place while the final cuts are made to separate them from the stock they are being cut from? Especially if the parts are small?

[vlmarshall]

Originally Posted by Shibumi 1. How does one program a conical cut (depression into the material? What tool does the job best so the stepping is minimized?

I suppose that depends on the cut you need to make, and the machine you're cutting it with. Can you cut it with a ballmill and a tapered reamer?

Tapered ballnose endmills are available, and can be custom ground.

A progressive series of G13's could do the job for you...

Originally Posted by Shibumi 2. How are parts typically held in place while the final cuts are made to separate them from the stock they are being cut from? Especially if the parts are small?

I often stick material to the mill table with doublesided tape... but only for parts that I can cut without coolant.

Clamp the stock to the table with several strips of tape under it.
Profile your parts, but not to full depth, leaving enough material to hold them in place while you do whatever other features your parts have.

When this setup is finished, light cuts around the parts will seperate them from the stock without tossing them across the shop.


Alternatively, if the stock is thicker than the finished parts, leave them together while machining, seperate them later with a bandsaw, and skim off the excess material from the back side in a vise.

That's the fun thing about this trade/hobby; there's a million ways to do anything, you just have to find what works for you/your equipment/your products.

[stevo1]

We use to do a lot of parts that required OD and ID conical step milling. We wrote 2 macros to do this. So if your machine can handle macro programming then this is pretty quick to set up. We used a 3” shell mill with .06 radius tips. You cannot take a pick in the Z larger than your radius. I know there is better ways to do this. Once we started out sourcing this product the shop that was doing them used the High Feed tooling and would rip the material off in about 1/3 of the time. Set your main macro up like this.

O0001(main program)
G65P8011A()C()I()K()D()E()F()H()M()Q()R()S()T()U()X()Y()Z()
M30

Variable definition fill in the data below into the () in the main program:
A=cone angle
C=tool tip radius
I=ramp in radius(“I” must be specified before “K”
K=feature position top or bottom of part 0 or minus the part thickness this will work with H value (this will be the height at which you will specify the diameter to cut to in the H value)
D=tool radius
E=exit plane
F=feed/min
H=feature diameter at “K”position
M=coolant code
Q=pick size in Z
R=reference plane
S=speed (RPM)
T=tool number
U=next tool (pre call)
X=center position
Y=center position
Z=final cutting depth

O8011(OD conical milling macro
#30=#17*TAN[#1]
IF[#18EQ#6]THEN#18=#3-#3*TAN[#1/2]
IF[#6EQ#0]THEN#6=#18
#32=#11/2-[#18-#6]*TAN[#1]-#3+#3*TAN[45-#1/2]+#7
IF[#4EQ#0]THEN#4=#7
G90G17G0X[#32+#4+#24]Y[#4+#25]M3S#19
Z[#18+#17]M#13
N1G0X[#32+#4+#24]Y[#4+#25]
#33=[#32+#7]/#32
IF[#18LT#26]THEN#18=#26
G1Z#18F[#9*#33]
G3X[#32+#24]Y#25R#4
G02X[#24-#32]Y#25R#32
G02X[#32+#24]Y#25R#32
G03X[#32+#4+#24]Y[#25-#4]R#4F[#9*3*#33]
#32=#32+#30
#18=#18-#17
IF[[#18+#17]GT#26]GOTO1
M9
G0Z#8M5
M99

Let me know if you want me to post the ID conical step milling program.

Stevo