Need Help!- Programming Tapered spiral milling operation

[mslt1996]

I have a Cincinnati Maxim 630 Horizontal Machining Center with an Acramatic 950 control. I would like to program a tapered spiral milling operation in a bore in absolute. I do not have any programming software, so I need to this manually. Looking for perhaps an Excel program to calculate all of the required information. Can any one help? Thanks. Mark

[mfgbydesign]

How about using AutoCad or similar CAD program, create the finished feature, define the tool, offset the geometry, draw the toolpath, analyse the data, and copy the tool center coordinates into your program.

[fordav11]

you could use helical milling (circular interpolation in X Y Z) or a thread milling function.
I don't know that control but there should be a code for it if you have that functionality
Helical Interpolation is usually an option on Fanuc controls.
Is your cutter tapered also or are you cutting a spiral groove or something else? A bit of info with some sizes might help to visualize it better.

[mslt1996]

The control does not have a canned cycle. You have to use a G02 or G03 circular interpulation code. What I need to know is a method to get the calculated coordinates for X, Y, Z, I, & J. The cutter is straight. I am trying to cut a tapered bore from 6" diameter to 4-1/2" diameter at an angle of 27.5 degrees. Thanks

[angelw]

Originally Posted by mslt1996 The control does not have a canned cycle. You have to use a G02 or G03 circular interpulation code. What I need to know is a method to get the calculated coordinates for X, Y, Z, I, & J. The cutter is straight. I am trying to cut a tapered bore from 6" diameter to 4-1/2" diameter at an angle of 27.5 degrees. Thanks

What Ford is suggesting is that you may have Helical Interpolation as a function of the control. Helical Interpolation is not a canned cycle, you still use G02/G03, but in conjunction with a Z address. If you don't have this feature, and you can quickly determine that cutting some air using a short program including Z address with the circular interpolation command, then you only have three alternatives.

1. Cut a circular path of the appropriate diameter using G02/G02 at a particular Z level, then continue this process by going to a new Z level and cut another circular path with the diameter varied by an amount determined by the 27.5 degree angle and the new Z level. You could use a User Macro program to do this with just a handful of lines.

2. Create a User Macro program to cut the path in short XYZ linear interpolation moves.

3. Use a CAM system to generate an NC program to do the same as 2 above.

Regards,

Bill

[fordav11]

try this as a tester.
this was generated with Vardex Thread Milling Generator (its free) in about 10 seconds.
If this runs you have helical interpolation.
if it throws an alarm you can't do circular interpolation in XYZ (i.e helical interpolation) you can only do circular interpolation in XY


%
O0001
G90 G40 G54
G43 H10 Z2. M3 S2000
G00 X0 Y0
Z0.1
G91 G01 G42 D60 X0.0254 Y0.1330 F0.21
G91 G02 X0.1331 Y-0.1330 Z-0.0028 I0J-0.1330 F0.21
G91 G02 X-0.0465 Y-0.1120 Z-0.0046 I-0.1584 J0.0002 F0.69
G91 G02 X-0.1120 Y-0.0462 Z-0.0046 I-0.1118 J0.1120
G91 G02 X-0.1117 Y0.0465 Z-0.0047 I0.0002 J0.1581
G91 G02 X-0.0462 Y0.1117 Z-0.0046 I0.1118 J0.1116
G91 G02 X0.0464 Y0.1115 Z-0.0046 I0.1578 J-0.0002
G91 G02 X0.1115 Y0.0461 Z-0.0046 I0.1114 J-0.1116
G91 G02 X0.1113 Y-0.0463 Z-0.0047 I-0.0002 J-0.1575
G91 G02 X0.0460 Y-0.1113 Z-0.0046 I-0.1114 J-0.1112
G91 G02 X-0.1330 Y-0.1330 Z-0.0028 I-0.1330 J0
G00 G40 X-0.0243 Y0.1330 Z0
G90 G00 Z8.0000
M5
M30
%

[dak1]

Where do you find the Vardex Thread Milling Generator & does it have an option for producing point to point output for machines without the helical interp option?

[fordav11]

look here. I don't offer support contact Vargus with your questions.
Vardex Thread Turning, Thread Milling & Miniature Threading | TM Gen

[txcncman]

Try this: Spiral Taper G code Creator

I am only going to leave it up a few days.

Yes, I know it needs tweaked a little. Depending on desired step down, I noted that it accumulated error on Z depth of up to 0.0026" for the entire taper length.

[txcncman]

Originally Posted by txcncman Try this: Spiral Taper G code Creator I am only going to leave it up a few days. Yes, I know it needs tweaked a little. Depending on desired step down, I noted that it accumulated error on Z depth of up to 0.0026" for the entire taper length.

I am only leaving this up for a couple of days. After that, it will be available for purchase.

[txcncman]

Originally Posted by txcncman I am only leaving this up for a couple of days. After that, it will be available for purchase.

Originally Posted by txcncman Try this: Spiral Taper G code Creator I am only going to leave it up a few days.

Time is up. I hope this worked well for you. I will be putting up a web page that will make this app available for purchase. Target price will be named there and instruction on how to purchase.