circular tool path?

[DG]

I hope somebody can help me with a simple problem. I am cutting a half diameter, say .625 diam , .125 wide with a .01 rad on each side. I am using an A axis rotary. How can I get MC to output simple radius moves of -X- stepovers and 90 to -90 radial moves. Every toolpath I have tried -4 axis rotary, 5axis flow, and 3 axis subs out put long strings of code. I looking for something like;

X-.0625 Z.3125, A90;

F40

A-90

X-.060 F 10

A90

F40

I need to keep the program as small as I can.

I can do this with Powermill but I want to use MCX. Thanks for any help.

[Greg_J]

Hi,

Try going to Arc filter/Tolerances and switch the filter ratio to custom and check Create Arc in XY, XZ and YZ. It changes my tool paths from point to point ot arcs. My program went from 25,000 lines to 5,000 lines, but I am not sure if it will work for 5 axis.

I hope it helps.

 

Greg

[iowajim62]

Try using Contour and turn on Rotary Axis in your operation. You will need to do some setup inside rotary axis to get the desired result.

[DG]

Not quite what i'm looking for ,it still put out many A moves...I am looking for :

 

G54G90G0X0Y0A0

G1X0Y0F75

X-.095A90.0000

Z.260F10

F40

Z.26A-90.0000

X-.090F10

F40

Z.260A90.0000

X-.086F10

F40

A-90.000

X-.081F10

F40

[DG]

"You will need to do some setup inside rotary axis" I'm not sure I follow you? I can get a curve path at a fixed angle and then edit in my rotations..but i really didn't want to do the editing. I have a lot of these programs to edit over to master camX

[Dan@home]

DG, wouldn't you also need the degs per min. feed rate for your rotatory A.

 

I have tried to do this also, only with an arch move (G19) with the A axis move at the same time. The closest I could get was the (Curve 5 axis tool path) using 4th axis. I would get a huge amount of code. instead of maybe a couple of lines, like I wanted.

 

I guess it becomes a spline with a bunch of small lines and A moves, no arcs at all. Herkie jerkie tool path not smooth at all.

 

Had to hand edit it. I would be interested in a solution also.

 

Thanks Dan.

[iowajim62]

Here's pic of rotary setup back in V9.

Diameter is your part diameter.

Here's the code for a Haas. Three cuts in X.

code:

---

 G0G90G54X-.95Y0.A-90.S1069M3

G43H1Z8.5T1

Z8.1

G1Z4.F75.

G41D1X-.45

A90.

G40X-.95

G0Z8.25

X-.85A-90.

Z8.1

G1Z4.

G41D1X-.35

A90.

G40X-.85

G0Z8.25

X-.75A-90.

Z8.1

G1Z4.

G41D1X-.25

A90.

G40X-.75

G0Z8.5

---

[DG]

That's what I'm looking for but I need to do a surface with x step overs. My mcx2 ver doesn't let me unroll the surface? wonder why? that switch is not active. Is it because of the sides? (.010rad)

[DG]

Oh yea, feed rate is not an issue. I can set that to whatever I want.Of course unit per minute is very slow so you have to overfeed if you do it that way. Danbo, I am going to get to the bottom of this one way or another..

[Dan@home]

I guess I am miss understanding your question. You are trying to cut halfway around piece of stock or a D shape in X step overs.

[DG]

Yes, exactly, with just a radial index of 180 degrees each stepover as in the code example I presented or Jim's Haas code. I can not get my rotary axis to do an unroll though.