helical toolpath with cutter comp active

[HEAVY METAL]

I can't figure a way to create a toolpath to follow a helix I have drawn with cutter comp active. the helix is 2.7 mm pitch wraped around 560 degs. I can only get a correct toolpath when compensation is set to off. so everytime I want to bump the cutter in or out i have to create new helix geometry. Is there a way to accomplish this that I am not seeing?

thanks heavy

[htm01]

i do threads that are 1 turn captured on the ends and i just do a circle and add the z in edit

[robh]

I believe you need a line in order to activate G41 or G42. I don't think it can be done on an arc move at least not on any of our machines.HTH

[htm01]

it won't do cc because its a 3d spline.i just add 1/4 turn of Z to each 1/4 of the circle.

 

this is 1 turn 8TPI

 

( 1/2 #108THREAD CUTTER TOOL - 4 DIA. OFF. - 4 LEN. - 4 DIA. - .5 )

T4 M6

G0 G90 G55 X0. Y.1865 S1200 M3

G43 H4 Z.2

M8

G1 Z-.569 F10.

G41 D4 Y.3865 F6.

G3 X-.3865 Y0. I0. J-.3865 Z-.5274

X0. Y-.3865 I.3865 J0. Z-4858

X.3865 Y0. I0. J.3865 Z-.4442

X0. Y.3865 I-.3865 J0. Z-.4026

G1 G40 Y.1865

[ATG]

Can't you use transform tool path after the initial path. Just tell it which direction to move and how much, and how many steps

[HEAVY METAL]

I'm hoping to find a way to do it inside of mastercam with no edits

[ATG]

Thats what I'm talking about....

[Midwest]

have ya tried contour ramp.....use a circle.....don't need a spline....... with cutter comp..........works 4 me.

[mcpgmr]

Heavy, Is this a thread your trying to mill? Like midwest said, Use contour/ramp and turn wear comp on. you might have to tweak the % of tool to lead in by so you don't hit the other side of the hole if it's an internal feature. I do this all the time. I use like 20% of the tool dia. with it set to tangent and maybe a 5% radial lead in and it works fine. HTH!

[gcode]

Have you tried using thread mill?

you can force the toolpath to start in the center,

define the pitch and lead in/lead out and it will

post a helix if your machine df and post are set up correctly

[bogusmill]

I cut helixes using contour with cutter comp on all the time as well as using thread mill and one thing I've found out is I never get a good path if infinate look ahead is checked.

[Don M]

quote:

---

Have you tried using thread mill?

you can force the toolpath to start in the center,

define the pitch and lead in/lead out and it will

post a helix if your machine df and post are set up correctly

---

This is how I do it also.

It works great.

[David Colin]

'Thread mill' is the only way to go with cc if you need to machine from bottom to top. Drawback, lead-in are not powerful...

[Tinny]

With regards to the helix toolpath with control, try start at centre and set start angle and arc sweep to zero. This gives you a G1 G41 to apply cutter comp, but no arc approach. As long as you start above the material it will be fine.

 

Works for me.

[sew]

uncheck infinte look ahead.

 

should work sweet.