post

[rasmond]

Using mastercam ver 9.0,Mpfan post,after post always got this nc code :

N3 G0 G90 G54 X391.485 Y-82.407 A0.S2464M3

N4 G43 H1 Z5.M8

How did this A0 come from & how to remove this,

 

If I used the mpsubrep post it gave this correct post that I want:

 

N1 T1 M06 (FACEMILL DIA 125)

N2 (MAX | Z5.)

N3 (MIN | Z-.5)

N4 G00 G90 G54 X237. Y-42. S700 M03

N5 G43 H1 Z5. M08

Without the A0

 

Pls Help

[chris m]

Change the answer to numbered question 164 to 'no' and change your rotary axis settings to reflect the fact that you do not have a 4th axis

 

# --------------------------------------------------------------------------

# Rotary Axis Settings

# --------------------------------------------------------------------------

vmc : 1 #0 = Horizontal Machine, 1 = Vertical Mill

rot_on_x : 0 #Default Rotary Axis Orientation, See ques. 164.

#0 = Off, 1 = About X, 2 = About Y, 3 = About Z

 

C

 

[ 01-02-2004, 12:04 PM: Message edited by: chris m ]

[Paul Decelles]

Set this switch to 0

 

code:

---

rot_on_x : 1 #Default Rotary Axis Orientation, See ques. 164.

#0 = Off, 1 = About X, 2 = About Y, 3 = About Z

---

[chris m]

Is there an echo in here; or what?

 

How's the new job, Paul?

 

As if you're really gonna say ' actually, it sucks...' on this website

[rasmond]

Thank you very much , all the Expert down here, I really appreciated , Solved my problem. If not got to post & edit the nc files to removed the A0, very tedious if I ,ve 20 tools. using fanauc system, they cannot read T1 M6 there will be an alarms, only have to edit it to

T1 OR T1

M6 M06

 

Thank You , If U can Teach me , How to Change it to T1 NEXT LINE M06. WOULD BE REALLY appreciated.

[chris m]

Change this:

 

if stagetool >= zero, pbld, n, *t, "M6", e

 

to this:

 

if stagetool >= zero, # Toolchange altered to 2 lines (cdm)

[

pbld, n, *t, e

pbld, n, "M06", e

]

 

in the start-of-file [psof] subroutine

 

and then change this:

 

pbld, n, *t, "M6", e

 

to this:

 

pbld, n, *t, e

pbld, n, "M6", e

 

in the toolchange [ptlchg] subroutine

 

C

 

[ 01-02-2004, 12:45 PM: Message edited by: chris m ]

[rasmond]

I can get the ist tool

T1

M06

But the next tool will be after I follow your step Changing the mpfan post.

T2

T2M06

 

thanks.

[chris m]

You probably have the *t on both lines

 

C

[rasmond]

This is the ist one correct can change to

T1

M06

pcom_moveb

c_mmlt #Multiple tool subprogram call

ptoolcomment

comment

pcan

if stagetool >= zero,

[

pbld, n, *t, e

pbld, n, "M06", e

]

pindex

if mi1 > one, absinc = zero

pcan1, pbld, n, *sgcode, *sgabsinc, pwcs, pfxout, pfyout,

pfcout, *speed, *spindle, pgear,

 

The 2nd tool cannot , below is the pst text tat I alter for the second line which gave me the

T2

T2M06

 

Thank you again for your quick response, & now s'pore time is 3.38 am, everybody is still asleep. wat is the time your place.

 

Thousand apology for bordering you , still waiting for your reply, if not cannot sleep until the problem solved.

[Jack Mitchell]

quote:

---

As if you're really gonna say ' actually, it sucks...' on this website

---

Love ya Chris - you make my day.

 

 

Regards, Jack

[chris m]

Sorry, I am not understanding your last response about the T2 problem. My ptlchg sub looks like this:

 

ptlchg #Tool change

pcuttype

toolchng = one

ptoolcomment #Moved up from below (cdm)

comment #Moved up from below (cdm)

pcan #Moved up from below (cdm)

pbld, n, *sgcode, *sgplane, "G40", "G49", "G80", *sgabsinc, "G94", "G98", e # Added (cdm)

if mi1 = one, #Work coordinate system

[

pfbld, n, *sg28ref, "X0.", "Y0.", e

pfbld, n, "G92", *xh, *yh, *zh, e

]

# pbld, n, "M01", e

pcom_moveb

c_mmlt #Multiple tool subprogram call

# ptoolcomment

# comment

# pcan

result = newfs(15, feed) #Reset the output format for 'feed'

# Toolchange altered to 3 lines (cdm)

pbld, n, "G111", e

pbld, n, *t, e

pbld, n, "M06", e

pindex

sav_absinc = absinc

if mi1 > one, absinc = zero

pcan1, pbld, n, sgcode, *sgabsinc, pwcs, pfxout, pfyout, #Removed * from sgcode (cdm)

pfcout, *speed, *spindle, next_tool, pgear, strcantext, e #Added next_tool (cdm)

pbld, n, "G43", *tlngno, pfzout, scoolant, e #Removed next_tool (cdm)

absinc = sav_absinc

pcom_movea

toolchng = zero

c_msng #Single tool subprogram call

 

and works perfectly for my machine. I have a 3-line toolchange:

 

.

.

G111

T02

M06

.

.

 

because my machine requires the G111 preparatory code.

 

You should be able to modify ptlchg to give you

 

T02

M06

 

by doing what I showed in my earlier post, just make sure that the *t word is only on one line and it should work.

 

C

[rasmond]

very sorry follow your changed in the post is correct, I can get both T1,M06 & T2, M06 in 2 lines . I forget to exit my cam after the changed.start again it really post correctly.Thank you Chris, Actually I learn from mastercam from ver 5.0 running in windows 3.11. All on the very basic drawing, toolpath, mostly 2D , because it never support subprogram, so i move on to ver 9.0. Read alot in this forum , fantasty pick up alot of tips down here.

I ,m working as a cnc milling , our joB is quite plain , drilling , step, width , length , round. Only the material are quite hard easy to chip off, chrome, nickel , cobalt ,titanium etc.

what are u working as chris, is there anyway to correspond with you, talk to you in the net .

[chris m]

I'm glad that you got things to work; time for you to go to bed!

 

I've been using Mastercam only since V8, so you have a lot of experience over me. This forum is a good place to find answers so don't be shy if you are having trouble.

 

C

[rasmond]

Anyways thank alot Chris , and a happy new yrs to you and everybody in this forums, got to go & take sleep now, Tommorow morning , had go back to work & try it at my shop. Very happy to solved 2 of my problem. good nights

[rasmond]

I hope to corespond with you, maybe we can try the net using the new beta softwares call skype. which you will be able to talk to me thru the microphone & we can heard it other voice. Thank for the help Chris. Really appreciated,even it is a very small problem, cause I,m still learning cam & I,m learning the hard way,One of my junior colleage which he is good in drawing, toolpath etc.using ver 5.0 , he is not good at troubleshooting , whenever he post a nc text, always got to edit those addition text,G92x0y0 , need to key the G54 for every tools, that not the correct way. you know we asian pple don,t like to share their knowledge, so you know I got to learn the hard ways. If he is on leave, i got to used manual pgm to do my work, cause nobody knows how to do . Tht not the ways,.

good bye.

[Rekd™]

quote:

---

Love ya Chris - you make my day.

---

+1. That was classic! Chris

 

'Rekd

[Paul Decelles]

Sorry I didn't get back on this sooner, I was off on Friday and just popped on for a sec and answered. The new job is going well, CNC is a tremendous company to work for and they have a boat load of really talented people working here. One thing I can say is that it is very humbling to come into a company like this and to realise that you really know nothing in the big scheme of things.

Oh, and BTW, ver. X looks really really good. I am quite sure that everyone is going to be very impressed with it.

[chris m]

quote:

---

One thing I can say is that it is very humbling to come into a company like this and to realise that you really know nothing in the big scheme of things

---

This is toooo easy, so insert your own rips here:

 

________________________________________________

 

 

C

 

Chris teh You needed a new job to figure that out?

[Paul Decelles]

Ripping me for stating the obvious wouldn't be very sportsmanlike now would it?

 

My point was not that I feel inadequate or anything, it was more to the point that there are a lot of extremely brilliant people in this company that I feel would impress any new comers. You don't think the code in Mastercam gets written by itself do you?

[chris m]

Just like the programs that make parts are 'generated by the software', no?

 

C

[MetalMarvels]

quote:

---

You don't think the code in Mastercam gets written by itself do you?

---

WHAT! They don't have AI-driven auto-coding software for generating new versions of MasterCam??? I am crushed.......