C Axis Wind Up

[metzenwest]

Hi everyone, 

Last week I thrown on a Live tooling lathe with a Y axis. I have never touched a Life tooling lathe let alone a Y axis one.

My first part to make is a simple turn part with 2 mill features. A face contour and a cross contour that requires Y axis moves.

The cross Contour I have figured out and it works perfectly.

The face contour is where the problem is happening, and its post processor related.

Our lathes C axis only excepts C0-C360 for absolute commands, Negative call outs Do not work. To do continuous interpolation an incremental call out of H is needed. H can be positive and negative and can be any reasonable number.

If you command G0 C360. Once you hit 360 degree's its back at Zero degrees.

 

So, he's what my post is doing.

O0000
(PROGRAM NAME - M1808)
(DATE=DD-MM-YY - 18-03-17 TIME=HH:MM - 21:44)
G20
(TOOL - 10 OFFSET - 10)
( 1/4 FLAT FINISH ENDMILL)
G54
N10 T1010
G17 G98
M35
M90
G0 C18.598
G0 X.2461 Y0. Z.5 M8
G97 S2500 M3 P12
Z-.645
G1 Z-.745 F100.
G41 X.3594 C28.771 F1622.17
X.3846 C30.65 F1342.62
X.4071 C33.063 F1723.83
X.4263 C35.869 F2000.
X.4416 C38.958
X.4529 C42.244
X.4597 C45.653

""    ""    ""

X.5415 C351.225 F1199.36
X.5088 C354.993 F1583.7
X.4836 C359.654 F1959.21
X.4676 C5.052 F2000. <=== This will send the C axis backwards 354.602 Degrees. Instead of winding up.
X.462 C10.878
C49.122
X.4659 C54.038

""   ""   ""

X.5947 C86.607 F1836.15
X.5747 C92.413 F1856.88
G40 X.561 C98.569 F1968.89
G0 Z.5
M9
G30 V0.
G30 U0. W0. H0. M5 P12
M30
%

 

I've gone through the post and found this.

#C-axis variables for calculations
one_rev     : 0     #0 = Absolute positioning with wind up, 1 = Start between 0 to 360 closest direction #MU00004
c_axistype  : 2     #1 = C axis winds-up, 2 = C axis signed absolute
                    #3 = index positioning (do not set here, use string)

 

Under machine definition's in Lathe Spindle C Axis I have three options.

Signed Continuous

Signed direction, absolute angle (0-360 deg.)

Shortest direction, absolute angle (0-360.) <=== Current Setting

 

Is there any combo of these settings that will get me what i need? Which is to basically to give me an H incremental move to move the machine into the next 0-360 zone.

I am using the Mplmaster post on X9.

[SlaveCam]

This sounds like an issue for your Mastercam dealer assuming you are on maintenance. However, you could achieve the result by forcing C-axis to output incrementally (use H-letter) and all other axes absolutely. In my post's pfcout and pcout there are lines

if absinc$ = zero, *cabs, !cinc
else, *cinc, !cabs

so to force incremental you have to have

*cinc, !cabs

Test your code thoroughly for side effects!

[Colin Gilchrist]

I would recommend against modifying your post, until you understand the machine a little better. For most Fanuc Lathes, they handle the Face machining with Polar output. Either G12/G13, or G112/G113. (Some are even 12.1/13.1)

You activate this output in the Operation itself, using Misc Integer #4. A setting of '1' is "on".

The +- rotation output of the C-Axis is set in the Machine Definition. Go to the 'Properties of the C-Axis component, and set the option on "continuous positioning" to 0-360 Absolute.

[metzenwest]

I was reading up on G12.1 which I will be testing this week. Mastercam appears to post that out correctly. We are on maintenance for mastercam, but will probably have to bypass our Reseller, the post they gave us was utter junk. MPLmaster was worlds ahead of it.

If i change from ABS to INC, i'm sure it would work, but INC scares me, I can't read it very well.

Like I said I'll keep testing and playing with it.

 

One problem I am having right now is that the post kicks out  I, J, K oh every line there is a arc motion. Well when an I show up under G19, the machine isn't happy. So I need to solve that problem.

 

Thanks for the Reply's guys.