G54.1

[Travis B]

How do I change G54 to G54.1 P1 ?

[Elad]

what post are you using??

mpfan is automaticlly use G54.1 54.2.....etc after using G54 to G57.

If you want to cancel G54 to G57 you'll have to do changes in your post.

[Guest CNC Apps Guy 1]

Work Offset 0 = G54

Work Offset 1 = G55

Work Offset 2 = G56

Work Offset 3 = G57

Work Offset 4 = G58

Work Offset 5 = G59

Work Offset 6 = G54.1

Work Offset 7 = G54.2

etc...

 

Hope that helps

 

DOH!!!!! Hate those typos.!!!!

 

Thanks for pointing that out.

 

[ 06-30-2002, 05:37 PM: Message edited by: James Meyette ]

[d0gFartz]

Workoffset 6 is the first G54.1 P1

workoffset 7 is G54.1 P7

so on and so on

[Hacsta]

so how can i change this in the post so it outputs g110 g111 etc.. instead of g54 p1, g54 p2 i'm useing mpmaster.pst

[Chip-pan]

Look at the Haas post. It uses extended WO's like you are asking for. You will have to look at the correct output range and adjust acordingly

 

Chip-pan

[Hacsta]

can anyone clue me in on what lookfor in the post?

[chris m]

Usually pwcs; here's the one from MPHAAS

 

pwcs #G54+ coordinate setting at toolchange

if mi1 > one,

[

sav_frc_wcs = force_wcs

if sub_level, force_wcs = zero

if workofs <> prv_workofs | (force_wcs & toolchng),

[

if workofs < 6,

[

g_wcs = workofs + 54

]

else,

[

g_wcs = workofs + 104

]

if workofs >= 0 & workofs <= 25, *g_wcs

else, "ERROR - Invalid Work Coordinate System", e

]

force_wcs = sav_frc_wcs

!workofs

]

[Hacsta]

SWEET , thanks for the help

[Hacsta]

got it workin thanks guys for the help here's to friday

[crazy^millman]

Well you could do like I did. I got the extra offsets so I set up my MPMASTER post for the HAAS to use the offsets this way:

 

1=G154 P1

2=G154 P2

..........

99=G154 P99

 

Here is how I did that in the Post:

code:

---

pwcs            #G154+ coordinate setting at toolchange

if wcstype = two | wcstype > three,

[

sav_frc_wcs = force_wcs

if sub_level, force_wcs = zero

if sav_mi9 = 1, workofs = sav_workofs

if workofs < 0, workofs = 0

if workofs <> prv_workofs | (force_wcs & toolchng),

[

p_wcs = workofs

"G154", *p_wcs

]

force_wcs = sav_frc_wcs

!workofs

]

---

I just dont use G54 to G59 this way but along as I got things in a format I like and is similar to our FADAL's at this point all is good.

 

Crazy Millman

 

[ 12-19-2003, 02:49 PM: Message edited by: Millman^Crazy ]

[Hacsta]

great thats another way i'll have to try out on the machine with the new software , crazy . the new haas software has the workoffsets named

 

g154 p1 (g110)

g154 p2 (g111)

etc..

 

i wonder if the older software will understand this format, only one way to find out, thanks mill man for the code

[crazy^millman]

Well not sure about the old controls but on the new controls all you need is the G154 P1-P99 and it will use these offsets. ON a Fadal they use offset 1-48 and if you are writing a program for the Fadal then you want ot put it on the HAAS depending on what number you used you would get on the Fadal 1=E1 and on the HAAS 1=G55 so what I wanted to do was make it the same for bothe machine soem what for the operators. If I call 1 now when I post for the HAAS i get the G154 P1 which is along the same line of E=1 which to me leands itself to ease for the operators to follwo between each machine and for us that have to program. If I write a program for the FADAL or The HAAS I can keep my workoffsets all the same it it fall right in line just pick which post which machine and go to town so to speak.

 

OH yeah Glad to share the code what this place is all about. I just return the Favor others have given me is all.

 

 

Crazy Millman

 

[ 12-21-2003, 03:42 PM: Message edited by: Millman^Crazy ]

[Hacsta]

mill man i tried your post mod, i get a g154 p0 that freaks my haas controller out, i guess i have to start at g55 which is p1

 

 

I was also tring to mod the post to go from g54 thru g59 then g154 p1 etc.. follow me? but i'm not that good yet

[crazy^millman]

Did you put 1 on the offset page. With my post mod you have ot put a number hwere as any other post you dont have too. With this post mod I dont have declaration in the post that if the workoffset=0 that you get p1 automatically. It is an easy fix look ta this if you dotn want to have to put soemthing in your workoffset box have not tried this so tell me if it works if it doesn't then I will work on it some more.

code:

---

pwcs            #G154+ coordinate setting at toolchange

if wcstype = two | wcstype > three,

[

sav_frc_wcs = force_wcs

if sub_level, force_wcs = zero

if sav_mi9 = 1, workofs = sav_workofs

if workofs < 0, workofs = 1

if workofs <> prv_workofs | (force_wcs & toolchng),

[

p_wcs = workofs

"G154", *p_wcs

]

force_wcs = sav_frc_wcs

!workofs

]

---

If you look at this line you see the difference

code:

---

      if workofs < 0, workofs = 1

---

Try that and see if it posts out the G154 P1 without anything in the Workoffset box.

 

Crazy Millman

[crazy^millman]

Nope that didn't help. I will have to play with it to see what works.

 

Crazy Millman

 

Ok try this that should keep the P0 out and still work for any plugged in vaule as well as Trnasform I just tested all three seemed fine.

code:

---

pwcs            #G154+ coordinate setting at toolchange

if wcstype = two | wcstype > three,

[

sav_frc_wcs = force_wcs

if sub_level, force_wcs = zero

if sav_mi9 = 1, workofs = sav_workofs

if workofs < 0, workofs = 0

if workofs <> prv_workofs | (force_wcs & toolchng),

[

p_wcs = workofs

if p_wcs = 0, #This will keep P1 if workoff is 0

[

p_wcs = 1

]

"G154", *p_wcs

]

force_wcs = sav_frc_wcs

!workofs

]

---

Crazy Millman

 

One Thing I added to the end of my post since I am using the P offset I went to P99 on the Machine and made that my bring table to me position so here is what I did in my post to get posted code everytime and works on the VF2 and VF4 so sohuld work on all VF mills and this is with the MPMASTER Post. You would have to see what works on other posts.

code:

---

peof            #End of file for non-zero tool           

pretract

if lock_codes = 1 & rot_on_x, pbld, n, *sunlock, "(UNLOCK)", e

rotretflg = 1

pbld, n, *sg90, "G154 P99", "X0.", "Y0.", e

rotretflg = 0

if lock_codes = 1 & rot_on_x, pbld, n, *slock, "(LOCK)", e

comment

#Remove pound character to output first tool with staged tools

#if stagetool = one, pbld, n, *first_tool, e

#n, *sg90, e

n, "M30", e

mergesub

clearsub

mergeaux

clearaux

"%", e

---

Crazy Millman

 

[ 12-22-2003, 10:29 AM: Message edited by: Millman^Crazy ]

[chris m]

If you want to do this:

 

quote:

---

I was also tring to mod the post to go from g54 thru g59 then g154 p1 etc.. follow me? but i'm not that good yet

---

Try a change to the MPFAN pwcs:

 

pwcs #G54+ coordinate setting at toolchange

if mi1 > one,

[

sav_frc_wcs = force_wcs

if sub_level, force_wcs = zero

if workofs <> prv_workofs | (force_wcs & toolchng),

[

if workofs < 6,

[

g_wcs = workofs + 54

*g_wcs

]

else,

[

p_wcs = workofs - five

"G54.1", *p_wcs

]

]

force_wcs = sav_frc_wcs

!workofs

]

 

Just change the 'G54.1' to 'G154' and it might work

 

C

 

[ 12-22-2003, 12:19 PM: Message edited by: chris m ]

[Hacsta]

dang you the code master general or what its gonna take me a little while to get this but i will definetly give it shot

 

thanks crazy man

 

[crazy^millman]

Chris it will work that way just fine if you look at my post Mods I have the G154 instead of the G54.1. I just wanted a standard format for MC programs that the opertors could follow is all from the FADAL's to the HAAS's.

 

Crazy Millman

 

One thing i didn't say and this is the most important!!! Make back-up of your post before doing any post modfications. If you make the post unsable and it is your olny post well then you are the creek without a paddle.

 

[ 12-22-2003, 01:19 PM: Message edited by: Millman^Crazy ]

[chris m]

Yes Ron I did see what you had, looks like it would work fine; just throwing up the option to have the 'regular' work offsets followed by the 'expanded' sort of like the vanilla Fanuc way to do it is all.

 

C

[crazy^millman]

Yeah I figured that Chris. I am too off the wall to do the thing vanilla thing.

 

I guess I just got so use to not even having them with the PC-Fusion MAZAK's that I got out of the Habit of even using a G54. Then I go to Fadal's with the E offsest so for me it is kinda what work best for here and would be easy on everyone.

 

I had one fo the owners tell me Saturday that I am Crazy and must have CNC fuilds pumping through my viens to work as hard as I do. I didn't know wheter to take it as a complimant or an insult.

 

Crazy Millman

[Hacsta]

i tried both ways they work good, mill man keep it pumping through it's a good thing

 

thanks for the help you guys

 

p.s. i used the g154 p99 at the end to bring the table forward and to center works SWEET

 

 

thanks again and again and again

[chris m]

quote:

---

I had one fo the owners tell me Saturday that I am Crazy and must have CNC fluids pumping through my viens to work as hard as I do

---

I'd tell him 'Thanks for noticing; how about a f_cking raise?'

 

How are the wife and baby doing?

 

C

[crazy^millman]

Wife and Kids are great.

 

Hacsta that is what I like to hear glad to be of help. Rekd has a good little trick for the G187

 

Yeah I am taking the next 12 days off will be here next Monday for the 5 axis Thermwood showing up. Help the riggers get it where i want it and then off till the 5th.

 

Crazy Millman teh infusion of coolant, tapping fluid, and way oild and I am as good as new.

 

[ 12-23-2003, 02:20 PM: Message edited by: Millman^Crazy ]

[Hacsta]

quote:

---

Yeah I am taking the next 12 days off

---

sweet !!! after tomorrow i'll be off till the 5th

gotta love it

 

merry christmas

 

[ 12-24-2003, 10:07 AM: Message edited by: Hacsta ]