Posting G13's

[Rob @ Target Machine]

Does any one have any tricks up their sleeves to get G13's out of Mcam Mpmaster post? My solution so far is to use custom drill cycle 9 to post subprogram calls(prog # is passed through peck1)variable. I write the G13's manually into a sub. I know I could use another custom cycle to post simple G13 routines, but I need something more like this:

 

00216 (CC35542.216..SP)

(.060 EM-.1016 FEEDTHRU)

G90

Z.01

G1Z-.012F3.

G13I.0702D26F3.

G13I.0702D26F4.

G1Z-.057F3.

G13I.0503D27F3.

G1Z-.067

G13I.0507D27F3.

G13I.0507D27F4.

G1Z-.012F20.

G13I.0702D26F5.

G0Z.05

M99

 

Any ides would be appreciated.

[Guest]

What you are trying to accomlish is NOT a Mastercam function. It is a shorthand machine coding method.

 

AFAIK, the way you are attempting it, a custom drill cycle, is the way this needs to be done.

[Rob @ Target Machine]

That's right, but I have altered mill.txt to name my new cycles(which I will code later).I am still deciding how to label the custom parameters for each new cycle.

 

My main problem right now is passing these custom 1-10 parameters to my post. What variables are used? eg. as peck1 is for 1st peck - what variable represents custom drill parameters 1-10?

 

Any examples of a custom drill cycle out there ?

[Guest]

drl_prm1$ - drl_prm10$

 

are the custom drill paramter variables

 

quote:

---

Any examples of a custom drill cycle out there ?

---

Do a search on Custom Drill cycles there is a TON of information on the forum

[Rob @ Target Machine]

Thanks. So can I use them in a canned cycle directly? Like#

#***************

# Subprogram Call

# ***************

#

ifdrillcyc=8,

[

sub_prg_call=drl_parm1$

pcan1,pbld,n,strcantext,e

pbld,n,"M98",*sub_prg_call,e

]

 

isn't the $ for mcx?

I am using 9.1 at work and X2mr2 at home

[Craig-B]

Here are some from V9.

http://www.emastercam.com/cgi-bin/ultimate...ic;f=1;t=012485

[Josh T™]

It'd be nice if the circle mill toolpath could output G13s. Maybe wishful thinking.

[crazy^millman]

Here is something I did a few years back.

 

Linky

 

 

Linky defined better

 

 

HTH

[Rob @ Target Machine]

Ok I've set up cycle defs and custom parms in mill9.txt and have some luck getting G13's posted just fine as custom 10 - 15. I would like to force a subprogram call as in custom 9 of Mpmaster post and send my drill code to the sub I called. How do I make a sub from my custom cycle?

[crazy^millman]

The subout$ varaible comes into mind. I would look to the handing of the sub methods and use that logic to construct what you are after. May have to buffer some information. I would think using the program number and NCI name would be best with a mi trigger, but the door is really wide open to do what you want, just depends on how far you are needing or wanting to go with things.

 

HTH

[Tim Johnson]

The variable subout determines which channel you want your posted data in (4 channels).

 

quote:

---

I would like to force a subprogram call as in custom 9 of Mpmaster post and send my drill code to the sub I called. How do I make a sub from my custom cycle?

---

You're asking about two seperate processes. Since You're using G13 I'm assuming the subprogram is inside of your control and I'll guess a Fanuc Control. To transfer your drl_prm1 - drl_prm10 to the sub you'll first need to transfer the MC variables to the Fanuc local variables (#1 - #33) the the call the G13 bringing in the variables.

 

I don't have a macro call in my drill cycles and I don't have a Fanuc manual to look at for the Variable letters (some letters will be missing) but it would probably look similar to this;

 

code:

---

      if drillcyc = 9, # G13 Macro cycle

[

pbld, n, pdrlxy, e

pbld, n, refht, e

pbld, n, "G13", "A", drl_prm1, "B", drl_prm2, "C", drl_prm3, "D", drl_prm4,

"E", drl_prm5, "F", drl_prm6, "G", drl_prm7, "H", drl_prm8, "I", drl_prm9,

"I", drl_prm10, e

pcom_movea

]

---

I see that you have Z changes in your cycle and apparently your G13 program won't handle that. If this is an added cycle I would make the G13 program handle them. If this is a machine tool cycle you will be needing much more to this drill cycle.

 

[ 10-12-2008, 12:06 PM: Message edited by: Tim Johnson ]

[gcode]

quote:

---

Since You're using G13 I'm assuming the subprogram is inside of your control and I'll guess a Fanuc Control.

---

G13 is a Haas circle milling cycle

Postion the tool at XY centerline and Z depth

the G13 line contains the radius and feedrate

I think you can also defined stepover and a finish passes. G13 is a CCW cicle mill (climb cut)

and G12 is clockwise.

[Rob @ Target Machine]

I was thinking about something like this:

 

if drillcyc = 10, # G13 - Standard Feedthru

[

psub_call_s

psub_st_s

pbld, n, pdrlxy, e # depths and radii are in drl_prm 1-10

pbld, n, refht, e # feedrates and ccomp assignment are in mi 3-8

pbld, n, "G1 Z", drl_prm1, "F", mi3, e #

pbld, n, "G13", "I", drl_prm2, "F", mi4, "D", mi5, e # solder well depth

pbld, n, "G13", "I", drl_prm2, "F", mi4, "D", mi5, e # spring pass

pbld, n, "G1 Z", drl_prm3, "F", mi3, e

pbld, n, "G13", "I", drl_prm4, "F", mi6, "D", mi7 e # rough @1/2 depth

pbld, n, "G1 Z", drl_prm5, "F", mi3, e

pbld, n, "G13", "I", drl_prm4, "F", mi6, "D", mi7 e # rough at finish depth

pbld, n, "G13", "I", drl_prm5, "F", mi6, "D", mi7, e # finish feedthru diameter

pbld, n, "G13", "I", drl_prm5, "F", mi6, "D", mi7, e # spring pass

pbld, n, "G1 Z", drl_prm1, "F", mi8, e

pbld, n, "G13", "I", drl_prm2, "F", mi4, "D", mi5 e # cut burr at solder well depth

pbld, n, refht, e

psub_end_s

pcom_movea

]

 

 

I,m using Mpmaster v9.1post. The concept of how to code a custom drill cycle is getting clearer to me, but how

do I push code into a sub, and return???

 

The additional point part is no prob.

 

Am I even in the ballpark???

 

[ 10-13-2008, 11:02 AM: Message edited by: mastercamguru ]

[Rob @ Target Machine]

Hoping to get close to this:

 

sub:

 

00216 (CC35542.216..SP)

(.060 EM-.1016 FEEDTHRU)

G90

Z.01

G1Z-.012F3.

G13I.0702D26F3.

G13I.0702D26F4.

G1Z-.057F3.

G13I.0503D27F3.

G1Z-.067

G13I.0507D27F3.

G13I.0507D27F4.

G1Z-.012F20.

G13I.0702D26F5.

G0Z.05

M99

[Rob @ Target Machine]

This is what I came up with :

pdrlcst #Custom drill cycles 8 - 19 (user option)

#Use this postblock to customize drilling cycles 8 - 19

#

# custom vars ****************************************

fmt Z 15 depth_1

fmt Z 15 depth_2

fmt Z 15 depth_3

fmt Z 15 depth_4

fmt I 15 rad_1

fmt I 15 rad_2

fmt I 15 rad_3

fmt I 15 rad_4

fmt F 15 plunge_fr

fmt F 15 rough_fr

fmt F 15 finish_fr

fmt D 15 comp_1

fmt D 15 comp_2

fmt D 15 comp_3

fmt Z 15 clear_hgt

fmt Z 15 feed_hgt

#

depth_1 = drl_prm1 # depths and radii are in drl_prm 1-8

rad_1 = drl_prm2

depth_2 = drl_prm3

rad_2 = drl_prm4

depth_3 = drl_prm5

rad_3 = drl_prm6

depth_4 = drl_prm7

rad_4 = drl_prm8

#

#

plunge_fr = mr1 # feedrates are in ------- mr 1-3

rough_fr = mr2

finish_fr = mr3

#

#

comp_1 = mi3 # cutter comps are in ---- mi 3-5

comp_2 = mi4

comp_3 = mi5

#

#

clear_hgt = refht_a

feed_hgt = refht_i

# *******************************************************

#

pdrlcommonb

if drillcyc = 8,

[

sub_prg_call = peck1

pbld, n, "M98", *sub_prg_call, e

]

if drillcyc = 9, # G13 - Standard Feedthru

[

#psub_call_s

#psub_st_s

pbld, n, feed_hgt,

pbld, n, "G1", depth_1, plunge_fr, e

pbld, n, "G13", rad_1, rough_fr, comp_1, e # solder well depth

pbld, n, "G13", rad_1, finish_fr, comp_1, e # spring pass

pbld, n, "G1", depth_2, plunge_fr, e

pbld, n, "G13", rad_2, rough_fr, comp_2, e # rough @1/2 depth

pbld, n, "G1", depth_3, plunge_fr, e

pbld, n, "G13", rad_2, rough_fr, comp_2, e # rough at finish depth

pbld, n, "G13", rad_3, finish_fr, comp_2, e # finish feedthru diameter

pbld, n, "G13", rad_3, finish_fr, comp_2, e # spring pass

pbld, n, "G1", depth_1,finish_fr, e

pbld, n, "G13", rad_1, finish_fr, comp_1, e # cut burr at solder well depth

pbld, n, clear_hgt, e

#psub_end_s

]

pcom_movea

 

pdrlcst_2 #Custom drill cycles 8 - 19, additional points (user option)

#Use this postblock to customize drilling cycles 8 - 19

pdrlcommonb

if drillcyc = 8,

[

sub_prg_call = peck1

pcan1, pbld, n, pxout, pyout, strcantext, e

pbld, n, "M98", *sub_prg_call, e

]

if drillcyc = 9, # G13 - Standard Feedthru Additional Points

[

pcan1, pbld, n, pxout, pyout, strcantext, e

]

pcom_movea

 

Post crashed and reported duplicate pdrlcommonb and posted a few G13's, two place decimals for feedrates, and a long line of G1's and G13's without any x-y moves. Not as easy as it looks. LOL

[Rob @ Target Machine]

Ok my format statements are wrong, thats why only 2 place decimals. I know I have the concept, but what am I missing ?

[crazy^millman]

You can not define your variables inside of the pdrlcst that is a post section. You need to define them outside of that either before the drilling cycles are called. I think this is casing some of your trouble. Look at the second link you will see how I handled this.

 

HTH

[Rob @ Target Machine]

Can't find any links.

[Rob @ Target Machine]

Ok found in my email thanks. I'll move them up in the post & lets see what happens.

[Toby-Axis]

I forgot about these but they work. Got them straight from the Bridgeport guy for a Fanuc 0i-MC barely a year old.

 

I hope this can help at least a little.

 

O9013(G13 CCW CUTTING)

(OIM & 18MC CONTROL)

#25=#4

#7=#7+13000

#1=#[#7]

IF[#6EQ#0]GOTO1

#6=#6-#1

N1#2=#4-#1

#3=#2/2

#4=#2*2

IF[#6NE#0]GOTO10

IF[#18EQ#0]GOTO5

IF[#25LE#1]GOTO3333

IF[#18GE#2]GOTO4444

#11=#18-#3

#12=#11*#11

#13=#3*#3

#14=#13-#12

#10=SQRT[#14]

#15=#2-#18

#16=#9*3

G91G94

G3X#18Y-#10R#3F#16

X#15Y#10R#3F#9

X-#4R#2

X#4R#2

X-#15Y#10R#3

X-#18Y-#10R#3F#16

GOTO100

N5

IF[#25LE#1]GOTO3333

G91G94

G3X#2R#3

X-#4R#2

X#4R#2

X-#2R#3

GOTO100

N10

IF[#17GE[#1*2]]GOTO5555

IF[#25LT#1]GOTO6666

G91G94

#18=#17/2

#19=#6/2

G3X#2R#3F#9

G3X-#4R#2

X#4R#2

DO1

#4=#17+#4

#2=#4/2

IF[[#4-#30]GE#6]GOTO20

G3X-#4R#2

#30=#2

#4=#17+#4

#2=#4/2

IF[[#4-#30]GE#6]GOTO30

X#4R#2

#30=#2

END1

N20#2=#2-#18

#4=#4-#17

#20=#6-#2

#4=#4+#20

#2=#4/2

G3X-#4R#2

G3I#6

G3X#6R#19

GOTO100

N30#2=#2-#18

#4=#4-#18

#20=#6-#2

#4=#4+#20

#2=#4/2

G3X#4R#2

G3I-#6

G3X-#6R#19

N100G1G90

N3333#3000=5(END MILL TOO LARGE)

N4444#3000=6(RAPID MOVE TOO LARGE)

N5555#3000=7(STEP OVER TOO LARGE)

N6666#3000=8(ENTRY ARC TOO SMALL)

%

[Rob @ Target Machine]

Ok better got x-y output back, but some missing code from pdrlcst routine pdrlcst_2 is ok though.(assuming I can get sub to post), but I'll need to get G13 routine working first. This is what I'm getting now:

T1 M06 (.060 EM)

(MIN - Z0.)

G00 G90 G54 X-1.1158 Y-.5451 S6000 M08

G91 G43 H1 Z0. M03

G92 Z.05 M08

G90

G1 Z-.012 F1.5

G13 I.0703 F3. D28.

G13 F5.

G1 Z-.057

G13 I.0503 D29.

G1 Z-.067

G13

G13 I.0508

G13

G1

G13

X-1.0158

Y-.4451

X-2.2743 Y-.3918

I changed fmt statements as follows:

# custom vars ****************************************

fmt Z 2 depth_1

fmt Z 2 depth_2

fmt Z 2 depth_3

fmt Z 2 depth_4

fmt I 12 rad_1

fmt I 12 rad_2

fmt I 12 rad_3

fmt I 12 rad_4

fmt F 15 plunge_fr

fmt F 15 rough_fr

fmt F 15 finish_fr

fmt D 15 comp_1

fmt D 15 comp_2

fmt D 15 comp_3

fmt Z 2 clear_hgt

fmt Z 2 feed_hgt

I moved them up to where I can see others at beginning of post section. Something tells me I might be assigning a a drl_prm value to a variable that has not yet been defined. That would not end well. I'll move the variable assignments down to right before the drill cycle section.

[Rob @ Target Machine]

Axis ---I wish I had macro B.

 

This is a yasnac I80 control on a Matsuura mc510-vf. The G13's were an option for the control, but no macros that I am aware of. The control ignores any line beginning with #. I'm just trying to define a few cutom drill cycles to output the G13'3 so I don't have to make manual edits so often.

[Rob @ Target Machine]

Thanks Crazy Millman.

I got all the G13 code posting fine. Couple bugs with clearance and feed planes, but 95% better. I forgot to use *. Now if I can take that routine and make it post as a sub, then I'll have won this battle.

[Rob @ Target Machine]

T1 M06 (.060 EM)

(MIN - Z0.)

G00 G90 G54 X-1.1158 Y-.5451 S6000 M08

G91 G43 H1 Z0. M03

G92 Z.05 M08

G90

Z0. G1 Z-.012 F1.5

G13 I.0703 F3. D28.

G13 I.0703 F5. D28.

G1 Z-.057 F1.5

G13 I.0503 F3. D29.

G1 Z-.067 F1.5

G13 I.0503 F3. D29.

G13 I.0508 F5. D29.

G13 I.0508 F5. D29.

G1 Z-.012 F5.

G13 I.0703 F5. D28.

Z0.

X-1.0158

Y-.4451

X-2.2743 Y-.3918

[crazy^millman]

Like I said you are making this a lot harder than it has to be. I use to do this with a Mi trigger in my post. I would use the NCI name and program number to assign my sub program number. I then used a mi trigger in the pheader and psof part fo the post that took the standard header and then made it a sub header and the same with the M30 by using the trigger it made it a M99 instead of a M30. Then in an operation you choose you can then use a Mr to assign the main program with the sub program number you want. You can even do a manual unit and just call it if you want everything coming out of Mastercam. Keep it simple has always been my rule.

 

HTH