Post Help

[mtnflyr]

Hi All,

I'm looking for post help for a Kitamurea with Fanuc 16IMB control.

 

The program needs to have G05.1Q0 followed on the next line by G05.1Q1, at the top of the program.

I've added the this (See below) to my post from mpmaster but I'm missing something.

The G05.1 lines are not posting.

 

Please help...

 

#added on 09/14/09 for Kitamura

 

plast

last_op_id = op_id$

last_cuttype = cuttype

last_rotary_type = rotary_type$

last_tlplnno = tlplnno$

last_mr1 = mr1$

last_mr2 = mr2$

 

phsm1_on #High speed functions before G43

if opcode$ = 3 | opcode$ = 16,

[

mr1$ = 0

mr2$ = 0

]

if mr1$ = 1 & mr1_flg <> 1, #Advanced Preview (look-ahead) control - G08 P1

[

pbld, n$, "G08", "P1", e$

mr1_flg = 1

]

if mr1$ = 2, #AI-NANO 2, AI(nano)CC output (Artificial Intelligence Contour Control) - G05.1 Q1

[

pbld, n$, *sg49, e$ #Must be in G49 and remain before G43

if ipr_type > 1, ipr_type = 0 #Must be in G94

pbld, n$, sgfeed, e$

pbld, n$, "G05.1", "Q1", [if mr2$, "R", no_spc$, *mr2$], e$ #Mr2 gives accel/decel value/coefficient, usually R or P

mr1_flg = 2

]

# HPCC is working when called before G43.4 on Fanuc 31i

# if mr1$ = 3 & mr1_flg <> 3, #AI-HPCC and AI-nanoHPCC (High Precision Contour Control) - G5 P10000

# [

# if ipr_type > 1, ipr_type = 0 #Must be in G94

# pbld, n$, sgfeed, e$

# pbld, n$, "G05", "P10000", [if mr2$, "R", no_spc$, *mr2$], e$

# #pbld, n$, "G05.1", "Q2", e$ #auto arc filtering

# mr1_flg = 3

# ]

 

phsm2_on #High speed functions after G43

if opcode$ = 3 | opcode$ = 16,

[

mr1$ = 0

mr2$ = 0

]

# HPCC is working when called before G43.4 on Fanuc 31i, see phsm_1 above

if mr1$ = 3 & mr1_flg <> 3, #AI-HPCC and AI-nanoHPCC (High Precision Contour Control) - G5 P10000

[

if ipr_type > 1, ipr_type = 0 #Must be in G94

pbld, n$, sgfeed, e$

pbld, n$, "G05", "P10000", [if mr2$, "R", no_spc$, *mr2$], e$

#pbld, n$, "G05.1", "Q2", e$ #auto arc filtering

mr1_flg = 3

]

if mr1$ = 4 & mr1_flg <> 4, #Mazak Geometry Compensation/Accuracy G61.1, Mazak High Speed Machining Mode - G05 P2

[

pbld, n$, sgfeed, e$ #Mazak can be in G94 or G95 but it must be called before G05 P2

if mr2$, pbld, n$, "G61.1", ",K", no_spc$, *mr2$, e$ #Mr2 gives accel/decel value/coefficient, K

else, pbld, n$, "G61.1", e$

pbld, n$, "G05", "P2", e$

mr1_flg = 4

!convert_rpd$ #Mazak Fusion requires high feed motion only, comment out for Matrix

convert_rpd$ = one #Mazak Fusion requires high feed motion only, comment out for Matrix

]

 

phsm_off #High speed functions off

if mr1_flg = 1, #Advanced Preview (look-ahead) control - G08 P1

[

pbld, n$, "G08", "P0", e$

mr1_flg = 0

]

if mr1_flg = 2, #AI-NANO 2, AI(nano)CC output (Artificial Intelligence Contour Control) - G05.1 Q1

[

pbld, n$, "G05.1", "Q0", e$

mr1_flg = 0

]

if mr1_flg = 3, #AI-HPCC and AI-nanoHPCC (High Precision Contour Control) - G5 P10000

[

#pbld, n$, "G05.1", "Q0", e$ #auto arc filtering

pbld, n$, "G05", "P0", e$

mr1_flg = 0

]

if mr1_flg = 4, #Mazak Geometry Compensation/Accuracy G61.1, Mazak High Speed Machining Mode - G05 P2

[

pbld, n$, "G05", "P0", e$

pbld, n$, "G64", e$

mr1_flg = 0

convert_rpd$ = prv_convert_rpd$ #Mazak Fusion requires high feed motion only, comment out for Matrix

]

[mtnflyr]

I posted this progrgam with the mpmaster post and the G05.1 lines are still not posting. Is there something in the config that needs set to pick up the info correctly?

[Ron Branch @ 5th Axis]

What is the toolpath you are using for your 1st operation? If you notice that post is using operations as limit to posting out these commands then you might have the wrong operation type and that is what is limiting it from outputting the code you are looking for.

 

Just a thought.

 

HTH

[Tony35]

do you have MR1 checked on with a value of 2

[mtnflyr]

I've made a rest program doing a contour cut which mills the profile and I have a tappping cycle which needed to have G84.2.

 

quote:

---

do you have MR1 checked on with a value of 2

---

I have changed mr1$ = 0 to mr1$ = 2. Is this what you're refering to? If so that didn't help.

[Tony35]

this is how i have our kitamura 4XiF setup

no i meant in the operation i have all our defaults set to MR1=3

is this what you trying to do

 

AI NANO

%

O0000 (TKTK)

(KITAMURA 4XiF)

(MCX FILE - TONY FORGOT TO SAVE)

(DATE - SEP-14-2009)

(PROGRAMMER - )

(REV LEVEL )

N1G0G17G20G40G80G90

N6G91G28Z0.

N11M28 (CHIP CONVEYER ON)

(3/4 SUNAMI VARIMILL IN THRU COOLANT HOLDER - 900 SFM TOOL - 13 DIA. OFF. - 13 LEN. - 13 DIA. - .75)

N16(TEST G5 Q1)

N21T13M6

N26M50 (CHIP FLUSH ON)

N31S4584M3

N36G0G17G90G54X-.8678Y1.2918

N41G40G80G49

N46G990 Q1.F128.35

N51G05.1Q1

N56G43H13Z3.

N61Z.1

N66G94G1Z-1.F100.

N71G41D13Y1.1418F128.35

N76G3X-.7178Y.9919I.15J0.

N81G1X.7151Y.9918

N86G2X1.0901Y.6169I0.J-.375

N91G1Y-.7097

N96G2X.7151Y-1.0846I-.375J0.

N101G1X-.7178Y-1.0847

N106G2X-1.0928Y-.7097I0.J.375

N111G1Y.6168

N116G2X-.7178Y.9919I.375J0.

N121G3X-.5678Y1.1419I0.J.15

N126G1G40Y1.2918

N131G0Z3.

N136G05.1Q0

N141G990 Q0.

N146G91G28Z0.

N151G28Y0.

N156M29

N161M30

%

 

HPCC

 

%

O0000 (TKTK)

(KITAMURA 4XiF)

(MCX FILE - TONY FORGOT TO SAVE)

(DATE - SEP-14-2009)

(PROGRAMMER - )

(REV LEVEL )

N1G0G17G20G40G80G90

N6G91G28Z0.

N11M28 (CHIP CONVEYER ON)

(3/4 SUNAMI VARIMILL IN THRU COOLANT HOLDER - 900 SFM TOOL - 13 DIA. OFF. - 13 LEN. - 13 DIA. - .75)

N16(TEST G5 Q1)

N21T13M6

N26M50 (CHIP FLUSH ON)

N31S4584M3

N36G0G17G90G54X-.8678Y1.2918

N41G43H13Z3.

N46G94

N51G5P10000

N56Z.1

N61G1Z-1.F100.

N66G41D13Y1.1418F128.35

N71G3X-.7178Y.9919I.15J0.

N76G1X.7151Y.9918

N81G2X1.0901Y.6169I0.J-.375

N86G1Y-.7097

N91G2X.7151Y-1.0846I-.375J0.

N96G1X-.7178Y-1.0847

N101G2X-1.0928Y-.7097I0.J.375

N106G1Y.6168

N111G2X-.7178Y.9919I.375J0.

N116G3X-.5678Y1.1419I0.J.15

N121G1G40Y1.2918

N126G0Z3.

N131G5P0

N136G91G28Z0.

N141G28Y0.

N146M29

N151M30

%

[mtnflyr]

I've just started at this company today. They have been using Gibbscam. I need to duplicate how their programs post or as a reasonably close to that as possible in Mastercam.

This is an example of how the programs are posted here.

 

N1G17G40G80G49

N2G05.1Q0

N3G05.1Q1

N4G54

N5T1

N6M6

( OPERATION 1: HOLES )

( MILL C'BORE .256 X .118 DEEP )

( TOOL 1: .125 COUNTERSINK )

( CS#1 - XY PLANE )

N7T002

N8S6000M3

N9G90G0X.0044Y0.

N10G43Z1.H1

N11M8

N12Z.1

N13G82G99X.0044Y0.Z-.0625R.1P200F30.

N14G80

N15M9

N16G91G28Z0.

N17M5

N18M1

 

Every tool starts with the lines:

G17G40G80G49

G05.1Q0

G05.1Q1

[Ron Branch @ Verisurf]

Well that is very off. What do those codes do for that machine? I would just hard code it for now if it is a requirement, but would research what they do since it seems like they are turning it on and off with those 2 lines. Also if memory serves me correct you are not suppose to use it for drilling cycles and that would include tapping.

 

HTH

[Ron Branch @ Verisurf]

DOUBLE POST !@#$$#$@%#@@$!

 

HTH

[Tony35]

im confused why they would have it setup like that...bad gibbs cam post maybe

look in the kitamura book it will tell you how G5 Q1 works and when the machine will just shut it off (drilling/tapping/toolchange/etc)i dont know why you would make sure it is off just to turn it on

 

i ran into a similar problem here with edgecam they wanted the code just like so out of MC i told them you got more BS in the program then is needed

here is what it should look like they fought it in the beginning but now they are use to it change can be a hard pill to swallow

 

if they are dead set on it hard code it like ron said

 

good luck

[mtnflyr]

Agreed. It probably doesn't need to post as the example shows. It would be more effecient if it only turned on when needed.

I don't think they'll have a problem if it isn't exactly like the Gibbs programs as long as it works. So far none of the test programs I've posted is putting in the code anywhere. Does the command only come up with certain kinds of contour cuts or should it post with any contour cut?

[Tony35]

i have mine set for any milling HPCC will be on

[Mr. Wizzard]

Not sure what to do in the post, not an expert. For a quick fix, can you use Toolpath -> Manual Entry, then just type it in where you want it so it posts every time?