C axis conversion output?

[Dave Loveridge]

I am using a post derived from mplfan, and I am using the c axis conversion G12.1 - G13.1 or as the post used to be G112 and G113. I have been able to work thru most of the problems but I have one problem that I cannot get past.

 

When the tool exits from the cut it outputs the G13.1 and then the next line it does the exit. The problem is on my control I can only use the G40-G41-G42 inside the G12.1

{

N175G1X2.6175C.5348

N180G2X3.235C0.R.6175

N185G13.1<-----Move this line after the G40 line.

N190G1G40X3.3208C346.947F833.53

N195G0Z-2.5

}

 

the only thing I can see is the pmillcca is what creates the G13.1 and the cutpos2 when = to 3 is what causes the output. But I cannot figure out what makes cutpos2 = 3

Code from post below.

 

{

pmillcca #Cross/Face canned cycle code, after

if cutpos2 = three,

[

#Cross/Face canned cycle end code

if abs{cuttype} = two, pbld, n, *sg113, e #Face

else, pbld, n, *sg108, "C0.", e #Cross

result = newfs{11, cabs}

result = newfs{14, cinc}

]

}

 

Any help greatly appreciated

Thanks

Dave

[Steve Biehl - Cimquest Inc]

the secret is the notes in the post.

code:

---

 #Polar interpolation, G112 canned cycle:

# Polar interpolation is active only for face cutting (Right or Left).

# Use the Caxis/Face Contour toolpath. Create geometry for the lead in

# and lead out with the start and end position on the View number 3 tool

# axis. All paths must start and end at the 'C0'location for output to

# be correct. Chain the entire geometry without using Mastercam leads.

# Set mi4 to activate!

---

This is what the mplfan code looks like.

code:

---

 %

O0000

G20

(PROGRAM NAME - T DATE=DD-MM-YY - 11-10-04 TIME=HH:MM - 21:00 )

(TOOL - 1 OFFSET - 1)

( 1/4 FLAT ENDMILL)

G0 T0101

M23

G0 G54 X2.1229 Z.25

C0.

M9

G97 S2139 M52

Z.1

G98 G1 G112

X2.1229 Z0. C0. F6.42

G41 X1.

C-.5

X-1.

C.5

X1.

C0.

G40 X2.1229

G113

G0 Z.25

G28 U0. W0. H0. M55

T0100

M30

%

---

If you need a sample, I can put one on the ftp.

[Don S at Barefoot CNC South]

Dave this is how my post does it.

 

code:

---

 (TOOL - 4 OFFSET - 4)

(FACE CONTOUR HEX 1" FLAT ENDMILL)

G0T0404

M18

G0G54X.7933Z.25

C30.

M8

G97S534M03

Z0.

G98G1G12.1

X.687Z-.54C.1983F6.42

G41C-.1983

X0.C-.3966

X-.687C-.1983

C.1983

X0.C.3966

G40X.687C.1983

G13.1

G0X.7933Z-.29C30.

M9

G00X8.Z8.H0.M05

T0400

M30

---

[Don S at Barefoot CNC South]

I left this off

mi4 = Canned conversion cycle type selection:

# Mill-

# Activates milling axis conversation canned cycles (G107 or G12.1).

# 1 or -1 activates the cycle, the path continues until next entry is

# zero, sign switches (1 to -1) forces g13.1 at null toolchnge, the

# cycle changes or the tool changes.

 

 

But I see I am late

[Dave Loveridge]

I did as the post stated before you put it up, but it still does crazy things. Do you have to draw the geometry to center of the tool and not the edge? If I draw lead in/outs on the path it ends prematurely, and lookahead is turned off. But the other frustrating part is, what if my part does not get milled all the way around, and the post says it must start and end at C0.

What a pain in the butt, I will just stick with using the c axis output, it makes long code but I know it works and I don't have problems with it.

[Post dept]

Dave,

 

Cutpos2 is MP's flag to tell you where you are in the cut. Cutpos2 = 3 is the last point on the surface/chain of the cut. This flag updates itself each time through you post. Cutter comp would generally still be active at this point. I wouldn't even go to that postblock until the end of the tool or mtlchg0. You could also try cutpos2 = 4 (after end of cut). A lot of posts aren't very good at cutter comp and lead-in/outs on polar interp.

 

Brett

 

Brett

[Dave Loveridge]

I will try that,

Thanks

[Allan Brown]

We reworked G12.1 in our Integrex posts. We may have something boiled down and generic for Mazak available that would help - no need for chaining the lead-in.