more that one fixture offset (newbie)

[benji]

Hi all.

 

I am currently programming a Fadal 3-axis VMC. I have had good luck so far with using just one fixture offset (E1=G54). What I would like to do is learn how to program multiple fixture offsets.

 

The questions that I have are:

 

1) do I need to draw each part in it's exact location in mastercam?

 

2) how do I tell mastercam that I want to use a diferent fixture offset number.

 

What I'm doing is six of the same parts in chick vises. I want tool one to do all six, then tool two, then tool three....

 

 

Thanks in advance guys!

[heeler]

Multiple ways to do this. We would just do transform toolpath and use increament the fixture offsets. Then you can set your g54, g55 ect. offsets in the machine.

 

HTH

Glenn

[Rekd™]

benji, some posts are set up for subs. Or you could use transform, or or or.

 

Several years ago I made a VB program for post post processing the NC files to do this. It reads your g-code file and splits it up to run multiple parts, with either 1 tool running all parts, or running 1 part with all tools.

 

If you don't get the results you need via a .pst, let me know and I'll run one of your g-code files thru it and see how it does. (It's designed around the structure of my NC code, so may not work properly for yours.)

[MACHINEMASTERG]

also the mpsubrep .pst available on this site works great!!!ill do one pc go to machine run and fine tune if needed then back in mcam fix it up to what i did on the shop floor then in misc inter on the first op set for how many parts and what offset #'s to start with it may need some tweeking to run for a fadel(e1-e2-e3) but check it out or what the others have said work good too!!!

[Tom Szelag]

The shop I work in we have a Fadal 3016VMC. Our post is set up so that the 1st Misc integer is the fixture offset. Therefore, you just draw your geometry, write your toolpaths, and when you do you tell it which fixture to operate on.

[benji]

So far I have been able to:

-find and download the mpsubrep.pst

-find and use transform

 

It seems that in "transform" I am limited in the number of fixture offests that will post (I'm geting 4 different fixture offset numbers)

 

There had been a reference to some "misc integer" which I am unfamiliar with.

 

Your help and suggestions are greatly appreciated!

[HevyMetl]

I would also recomend using the e-codes over the G50's. E's will allow you to use up to I believe 99 fixture offsets. Depending on your files size subprograms will keep the size to a minimum and allow you to download to the machine and not have to drip feed. I havent't used a fadal in about a year but they were greatly limited in file memory unless you spent a large sum of money to upgrade.

[Bill Craven]

On the first page of your toolpath parameters, there is an option box called Misc values. If it is grayed out, click on the check box next to it and then you can get into it and see what is available for the post that is currently active.

The misc. integers are often used as switches (turn on and off otpions) and are specific for the post processor that you are using. On the Mpfadal post, misc integer 1 is used to change between using G92, if set to 0 or 1, or E values if set to 2. Using the Mpfadal post you can get a lot more than 4 fixture offsets.

[dabrow]

Benji,

you can also just post for one fixture and use macro "B" format for all additional locations by making your fixture offset a variable and updating in the program with a counting macro.This will also save you lots of memory.

[Tim Johnson]

+1 to dabrow,

 

That's how I do it all the time.

 

code:

---

N0010T01M06S10000

N0020G90M03

N0030#V40=V41

N0040#:1

N0050#V40=V40+1

N0060#R9=V40

N0070G00X1.13Y-.56E+R9

N0080Z2.1H01M08

N0090G99G82R.85Z.602P6F40.

N0100G98X1.63

N0110G80

N0120#IF V40<V42 THEN GOTO :1

 

N0130T02M06S9958

N0140G90M03

N0150#V40=V42+1

N0160#:2

N0170#V40=V40-1

N0180#R9=V40

N0190G00X1.63Y-.56E+R9

N0200Z2.1H02

N0210G99G83R.85Z-.096P.02Q.036F16.41

N0220G98X1.13Z.194

N0230G80

N0240#IF V40>V41+1 THEN GOTO :2

---

[dabrow]

tim,

do you have your post set up for this format?I haven't been able to do it and I just post the straight g-code then modify it to suit my fixture arrangement.It can be a pain since we program by tool here , not by individual part.One tool program can contain code for 50 seperate jobs.Any one else use this format?

[Tim Johnson]

Yes I do, (mpfadal)

I'll post what you need during lunch.

[medaq]

I would follow the advice of checking misc value. But I have had varying success in getting my posts to output the right E1 or G54 #. But I have always had good success using the misc and t/c plane option. I turn on tool plane once inside, and turn on work offset.

 

-1 =G54,E1

1=G55,E2

2=G56,E3

 

and so on.

 

Medaq

[Tim Johnson]

Multi part Macro for Fadal;

 

In the .txt file;

code:

---

[misc integers]

1. "Work system [0-1=G92,2=E's,3-4macro]"

2. "Misc. integer [2]"

3. "Misc. integer [3]"

4. "Misc. integer [4]"

5. "Misc. integer [5]"

6. "Misc. integer [6]"

7. "Misc. integer [7]"

8. "Misc. integer [8]"

9. "Absolute or Incremental [0=ABS, 1=INC]"

10. "Reference Return [0=G28, 1=G30]"

---

in the .pst file;

 

mics variable section (may have to add one)

code:

---

#Misc variables

processcount : 0 # Counter start for toolpath macro calls

processcountend : 0 # Counter end for toolpath macro calls

---

format section

code:

---

fmt     4   processcount    #Counter start for toolpath macro calls

fmt 4 processcountend #Counter start for toolpath macro calls

---

string definitions area

 

code:

---

#Address string definitions

strm "M"

strn "N"

stro "O"

strp "P"

srad "R"

srminus "R-"

sblank

se+r9 "E+R9" #<<<<<<<<<<<< add this line only

---

psof section

code:

---

      if mi1 > one, absinc = zero  #<<<<< after this line

processcount = processcount + 1

if mi1 = 3,

[

pbld, n, 35, no_spc, "V40=V41-1", e

pbld, n, 35, no_spc, ":", no_spc, processcount, e

pbld, n, 35, no_spc, "V40=V40+1", e

pbld, n, 35, no_spc, "R9=V40", e

]

if mi1 = 4,

[

pbld, n, 35, no_spc, "V40=V42+1", e

pbld, n, 35, no_spc, ":", no_spc, processcount, e

pbld, n, 35, no_spc, "V40=V40-1", e

pbld, n, 35, no_spc, "R9=V40", e

]

---

And in peof after the "check for rigid tap" area

code:

---

      if mi1 > one, absinc = zero

if mi1 = 3,

[

pbld, n, 35, no_spc, "V40=V41", e

pbld, n, 35, no_spc, ":", no_spc, processcount, e

pbld, n, 35, no_spc, "V40=V40+1", e

pbld, n, 35, no_spc, "R9=V40", e

]

if mi1 = 4,

[

pbld, n, 35, no_spc, "V40=V42+1", e

pbld, n, 35, no_spc, ":", no_spc, processcount, e

pbld, n, 35, no_spc, "V40=V40-1", e

pbld, n, 35, no_spc, "R9=V40", e

]

---

pwcs section;

code:

---

        force_wcs = sav_frc_wcs

!workofs

] # <<<<<<<<<<<<<<< add after this line

if mi1 = 3 | mi1 = 4,

[

force_wcs = zero

workofs = zero

se+r9

]

---

ptoolend section

code:

---

      !speed, !spdir2 #<<<<<<<<< after this line

if nextop = 1002, processcountend = processcountend + 1

if nextop = 1002 & mi1 = 3, pbld, n, 35, "IF V40<V42 THEN GOTO :", no_spc, processcountend, e

if nextop = 1002 & mi1 = 4, pbld, n, 35, "IF V40>V41+1 THEN GOTO :", no_spc, processcountend, e

---

ptlchg section

code:

---

      if mi1 > one, absinc = zero #<<<<<<<<< after this line

processcount = processcount + 1

if mi1 = 3,

[

pbld, n, 35, no_spc, "V40=V41-1", e

pbld, n, 35, no_spc, ":", no_spc, processcount, e

pbld, n, 35, no_spc, "V40=V40+1", e

pbld, n, 35, no_spc, "R9=V40", e

]

if mi1 = 4,

[

pbld, n, 35, no_spc, "V40=V42+1", e

pbld, n, 35, no_spc, ":", no_spc, processcount, e

pbld, n, 35, no_spc, "V40=V40-1", e

pbld, n, 35, no_spc, "R9=V40", e

]

---

peof section

code:

---

      processcountend = processcountend + 1 #<<<<< this is first line in postblock

if mi1 = 3, pbld, n, 35, "IF V40<V42 THEN GOTO :", no_spc, processcountend, e

if mi1 = 4, pbld, n, 35, "IF V40>V41+1 THEN GOTO :", no_spc, processcountend, e

" ", e

---

That should be it.

 

Notes;

In the FADAL control variables section;

V41 = "E" value of first part

V42 = "E" value of last part

 

mi1 controls the macro choices

 

Happy macroing

[Reece L Gibson]

If you break a tool in the middle of a fixture run, can you pick up where it broke without drilling a bunch of air?

[dabrow]

Reece,

you can but you have to have a statement at the beginning of the tool code to allow the operator to choose the fixture he wants to start at. EX:

 

 

IF[#520EQ1]GOTO1(SKIP FIXTURE 3)

IF[#520EQ2]GOTO2(SKIP FIXTURE 2 AND 3)

IF[#520EQ0]GOTO3(MACHINE ALL FIXTURES)

 

N1#118=17

GOTO4

 

N2#118=21

GOTO4

 

N3#118=13

N4WHILE[#118LE24]DO2

 

 

G0G90G54J#118X-11.0Y-10.25S#19M3

G43H7Z5.M8

G1Z-4.8F2000.

X11.0F#9

G0Z5.

X-11.0

G01Z-4.99F2000.

X11.0F[#9*2]

G0Z5.0

X11.0Y-14.73

G1Z-3.71F2000.

X-11.0F200.

G0Z20.

X11.0Y15.30

G1Z-8.30F2000.

X-11.0F150.

G0Z20.

 

 

G100

#118=[#118+1]

END2

GOTO9990

END1

 

 

By entering a value in variable #520,the operator can start at any fixture.You can be very creative with macro B programming using conditional statements.

[Tim Johnson]

quote:

---

If you break a tool in the middle of a fixture run, can you pick up where it broke without drilling a bunch of air?

---

V41 = "E" value of first part

V42 = "E" value of last part

 

 

The operator can type any value. If you want to start at part 5 end end at 11, just go to the variable screen on the control type 5 in variable 41 and 11 in variable 42.

Setting mi1 in you toolpath manager to 3 will run the parts from the first part to the last. Set it at 4 and and the toolpaths will go fron the last part to the first.

No tranforming toolpaths are required.