VTL YOUJ I YV-1200ATC+C

[mirek1017]

Hello All ,can some one helping me how use G8d  drilling cycle on this machine ,this is our Vtl lathe 

when I am posting  

G83 Z-1 R.1 Q.1 F3 . for my drilling  cycle ,pecking  do not work ,so I am find out on internet use  Q 1000.

So when I am posting 

G83 Z-1 R.1 Q1000. F3 .

C90.

C180.

C270.

the pecking working only on 1st hole  do not work on 90 180  270   position 

there is some setting  on machine or I should use something else in G83 line 

 

thank you 

 

[AHarrison1]

Should the Z value not have a decimal too?

[mirek1017]

11 minutes ago, AHarrison1 said:

Should the Z value not have a decimal too?

I mean  

Z-1.

Just now, mirek1017 said:

I mean  

Z-1.

 

 

I cant find out ,how use pecking on this machine 

[gcode]

What control does that machine have ?

 

This is a drilling cycle for one of out VTL's running a Fanuc 31i control

G99 means return to Retract plane

 

N935 G0 G54 X21.5 Z3. C.52 T0202 M16
N940 Z2.4679 <------ retract plane
N945 G94
N950 G99 G83 Z2.2629 R0. F15.
N955 X23. C124.62
N960 C232.62
N965 C358.62
N970 G80
N975 Z3.
N980 G28 U0. W0. M05
N985 M16
N990 M0

 

[crazy^millman]

Try putting the redundant  G83 C90 Z-1 R.1 Q1000. F3 at each index.

[mirek1017]

52 minutes ago, crazy^millman said:

Try putting the redundant  G83 C90 Z-1 R.1 Q1000. F3 at each index.

I the will be option ,just use G83 line in every C position 

haw I can fixing this in my post ?

I use generic FANUC lathe post 

1 hour ago, gcode said:

What control does that machine have ?

 

This is a drilling cycle for one of out VTL's running a Fanuc 31i control

G99 means return to Retract plane

 

N935 G0 G54 X21.5 Z3. C.52 T0202 M16
N940 Z2.4679 <------ retract plane
N945 G94
N950 G99 G83 Z2.2629 R0. F15.
N955 X23. C124.62
N960 C232.62
N965 C358.62
N970 G80
N975 Z3.
N980 G28 U0. W0. M05
N985 M16
N990 M0

 

this is series oi-tc 

[Leon82]

in the subsequent cycles section under the drill cycles in the post

[crazy^millman]

4 minutes ago, mirek1017 said:

I the will be option ,just use G83 line in every C position 

haw I can fixing this in my post ?

I use generic FANUC lathe post 

this is series oi-tc 

Copy the logic from the first section into the second section and should be good to go.

[mirek1017]

16 hours ago, crazy^millman said:

Copy the logic from the first section into the second section and should be good to go.

Good morning  ,in this place of post 

# --------------------------------------------------------------------------
# Drilling
# --------------------------------------------------------------------------
pdrill0$         #Pre-drill postblock call
      if cuttype = five, #Don't allow 5 axis, rests at toolchange
        [
        usecandrill$ = zero
        usecanpeck$  = zero
        usecanchip$  = zero
        usecantap$   = zero
        usecanbore1$ = zero
        usecanbore2$ = zero
        usecanmisc1$ = zero
        usecanmisc2$ = zero
        ]
      else,
        [
        if abs(cuttype) < three, mdrl_dir = zero
        else, mdrl_dir = one
        x$ = xnci$
        y$ = ynci$
        z$ = refht$
        copy_x = vequ(x$)
        pshft_map_xa
        pxyzcout
        refht_x = vequ(xabs)
        z$ = depth$
        copy_x = vequ(x$)
        pshft_map_xa
        pxyzcout
        depth_x = vequ(xabs)
        z$ = zdrl$
        copy_x = vequ(x$)
        pshft_map_xa
        pxyzcout
        zdrl_x = vequ(xabs)
        z$ = initht$  #Initial is last
        copy_x = vequ(x$)
        pshft_map_xa
        pxyzcout
        initht_x = vequ(xabs)
        znci$ = initht$
        ps_inc_calc
        ]

pdrlcommonb     #Canned Drill Cycle common call, before
      if gcode$ = 81,
        [
        if drillcyc$ = three, drlgsel = fsg1 (-g_speed * spdir$) + drillcyc$ * two #Tap
        else, drlgsel = fsg2 (dwell$) + drillcyc$ * two
        if initht$ <> refht$, drillref = zero
        else, drillref = one
        prv_refht_a = c9k
        prv_refht_i = c9k
        prv_dwell$  = zero
        ]
      if mdrl_dir = zero, #Set Z to depth
        [
        zia = fmtrnd(depth_z)
        zinc = zia - prv_zia
        ]
      else,               #Set X to depth
        [
        xia = fmtrnd(depth_x)
        xinc = xia - prv_xia
        ]
      xabs = vequ (depth_x)
      comment$
      pcan

pgdrlout        #Drill Gcode output
      if mdrl_dir = zero, *sgdrillf
      else, *sgdrillc

prdrlout        #R drill position
      if mdrl_dir = zero, refht_a = refht_z
      else, refht_a = refht_x
      refht_i = refht$ - initht$
      if absinc$ = zero, refht_a, !refht_i
      else, refht_i, !refht_a

[gcode]

What control does that machine have ?

 

This is a drilling cycle for one of out VTL's running a Fanuc 31i control

G99 means return to Retract plane

 

N935 G0 G54 X21.5 Z3. C.52 T0202 M16
N940 Z2.4679 <------ retract plane
N945 G94
N950 G99 G83 Z2.2629 R0. F15.
N955 X23. C124.62
N960 C232.62
N965 C358.62
N970 G80
N975 Z3.
N980 G28 U0. W0. M05
N985 M16
N990 M0

 

[gcode]

try putting a G01 move prior to the G83 line

line this

N935 G0 G54 X21.5 Z3. C.52 T0202 M16
N940 G01 Z2.4679 F100.
N945 G94
N950 G99 G83 Z2.2629 R0. F15.
N955 X23. C124.62
N960 C232.62
N965 C358.62
N970 G80
N975 Z3.
N980 G28 U0. W0. M05
N985 M16
N990 M0

It is possible that G0 is remaining active and cancelling G83

after one cycle is complete

[mirek1017]

49 minutes ago, gcode said:

try putting a G01 move prior to the G83 line

line this

N935 G0 G54 X21.5 Z3. C.52 T0202 M16
N940 G01 Z2.4679 F100.
N945 G94
N950 G99 G83 Z2.2629 R0. F15.
N955 X23. C124.62
N960 C232.62
N965 C358.62
N970 G80
N975 Z3.
N980 G28 U0. W0. M05
N985 M16
N990 M0

It is possible that G0 is remaining active and cancelling G83

after one cycle is complete

My control i s  Fanuc  oi-tc  

I do not have problem with G83 line or  Z position ,my problem is when I want use G83 cycle  my machine pecking only on 1st hole the other C indexing position drilling without pecking 

so I think like Ron said I need to get G83 line with all index like this 

 C0 G83Z-1R.1Q1000.F3.

 C90. G83Z-1R.1Q1000.F3.

 C180. G83Z-1R.1Q1000.F3.

 C270. G83Z-1R.1Q1000.F3.

 

 

 

[crazy^millman]

57 minutes ago, mirek1017 said:

My control i s  Fanuc  oi-tc  

I do not have problem with G83 line or  Z position ,my problem is when I want use G83 cycle  my machine pecking only on 1st hole the other C indexing position drilling without pecking 

so I think like Ron said I need to get G83 line with all index like this 

 C0 G83Z-1R.1Q1000.F3.

 C90. G83Z-1R.1Q1000.F3.

 C180. G83Z-1R.1Q1000.F3.

 C270. G83Z-1R.1Q1000.F3.

 

 

 

In the drilling section of any Mastercam psot there is the mdrill$ and mdrill_2$ I am saying take the logic is mdrill$ and copy to mdrill_2$. From the Generic Right Turret VTL post. Notice in a Mill turn post we have 2 sections. We have a ldrill$ and mdrill$ in this case we are going to focus on mpeck$ and mpeck_2$:

mdrill$          #Canned drill cycle, mill
      pdrlcommonb
      pcan1, pbld, n$, *sgdrlref, pgdrlout, pxout, pyout, pzout,
        pcout, prdrlout, dwell$, pffr, strcantext, e$
      pcom_movea

mpeck_2$       #Canned peck drill cycle repeat, mill
      mdrill_2$

Now replace the mdrill_2$ in the mpeck_2$ section with what was in the first mpeck$ section like so. I also used the pfzout to force Z output verses pzout which will only output Z if the value changes. 

mpeck_2$       #Canned peck drill cycle repeat, mill
      pdrlcommonb
      pcan1, pbld, n$, *sgdrlref, pgdrlout, pxout, pyout, pfzout,
        pcout, prdrlout, *peck1$, dwell$, pffr, strcantext, e$
      pcom_movea

Now you should get exactly what I was saying from here one.

Note to anyone following along. Mastercam can output perfect code for any machine.

I will repeat myself Mastercam can output perfect code for any machine. Problem is to many people think one size fits all and sorry that is not the case. Every single machine has its own quirks and it is up to us to sort that out. If you have enough experience with posts then these are simple tweaks. More involved ones require a professional.

 

[mirek1017]

49 minutes ago, crazy^millman said:

In the drilling section of any Mastercam psot there is the mdrill$ and mdrill_2$ I am saying take the logic is mdrill$ and copy to mdrill_2$. From the Generic Right Turret VTL post. Notice in a Mill turn post we have 2 sections. We have a ldrill$ and mdrill$ in this case we are going to focus on mpeck$ and mpeck_2$:

mdrill$          #Canned drill cycle, mill
      pdrlcommonb
      pcan1, pbld, n$, *sgdrlref, pgdrlout, pxout, pyout, pzout,
        pcout, prdrlout, dwell$, pffr, strcantext, e$
      pcom_movea

mpeck_2$       #Canned peck drill cycle repeat, mill
      mdrill_2$

Now replace the mdrill_2$ in the mpeck_2$ section with what was in the first mpeck$ section like so. I also used the pfzout to force Z output verses pzout which will only output Z if the value changes. 

mpeck_2$       #Canned peck drill cycle repeat, mill
      pdrlcommonb
      pcan1, pbld, n$, *sgdrlref, pgdrlout, pxout, pyout, pfzout,
        pcout, prdrlout, *peck1$, dwell$, pffr, strcantext, e$
      pcom_movea

Now you should get exactly what I was saying from here one.

Note to anyone following along. Mastercam can output perfect code for any machine.

I will repeat myself Mastercam can output perfect code for any machine. Problem is to many people think one size fits all and sorry that is not the case. Every single machine has its own quirks and it is up to us to sort that out. If you have enough experience with posts then these are simple tweaks. More involved ones require a professional.

 

BEST OFF THE BEST AND ONLY ONE !!!!!!!!!!!!!!!!!

 

 

Thank you RON 

 

 

[crazy^millman]

9 minutes ago, mirek1017 said:

BEST OFF THE BEST AND ONLY ONE !!!!!!!!!!!!!!!!

Thank you RON

Glad to offer any help I can offer. Always someone better and smarter and we are only one mistake away from being the worst any given day of the week.

[mirek1017]

3 hours ago, crazy^millman said:

Glad to offer any help I can offer. Always someone better and smarter and we are only one mistake away from being the worst any given day of the week.

That is what I am looking for 

(MATERIAL - STEEL INCH - 1030 - 200 BHN)
G20
(TOOL - 1 OFFSET - 1)
(0.875 DRILL)
G0 T0101
M66
G0 G54 X-12.875 Z-1.9048
C-30.
G97 S286 M33
G83 Z-3.1757 R-2.0548 Q3000. F1.43
G83 C-180. Q3000. F1.43
G83 Q3000. F1.43
G83 C60. Q3000. F1.43
G83 Q3000. F1.43
G80
G28 W0. H0. M55
T0100
M30
%

 

 

 

Thank you  Ron one more time 

 

[crazy^millman]

53 minutes ago, mirek1017 said:

That is what I am looking for 

(MATERIAL - STEEL INCH - 1030 - 200 BHN)
G20
(TOOL - 1 OFFSET - 1)
(0.875 DRILL)
G0 T0101
M66
G0 G54 X-12.875 Z-1.9048
C-30.
G97 S286 M33
G83 Z-3.1757 R-2.0548 Q3000. F1.43
G83 C-180. Q3000. F1.43
G83 Q3000. F1.43
G83 C60. Q3000. F1.43
G83 Q3000. F1.43
G80
G28 W0. H0. M55
T0100
M30
%

 

 

 

Thank you  Ron one more time 

 

Are you getting what you are looking for? Sorry the posting is to vague for me to know if you got the results you are looking for or not. If not then you would use pzout and not pfzout. feed already has the * to force that output. If the R is not being forced then just add the * before the prdrlout or the pffr and see if either one of them give you the forced output you need.

As always please make sure you have a backup copy of your post before doing any post modifications. I have some posts backed up 20 times and with memory cheap as it today I have no problem being that redundant.

I just picked up a 990 M2 Samsung Pro 2TB drive for $130 off Amazon. My laptop will not have 7Tb of room on it. The new drive will be my Windows 11 drive. The laptop will have 3 bootable drives. I learned how to disable and enable the Mastercam license between each drive. Vericut doesn't care since it used the MAC address of the Ethernet port. Maybe next year when this laptop hits the 5 year mark I will replace it. Been rough year, but still keeping a roof over our heads and food on the table.

[mirek1017]

36 minutes ago, crazy^millman said:

Are you getting what you are looking for? Sorry the posting is to vague for me to know if you got the results you are looking for or not. If not then you would use pzout and not pfzout. feed already has the * to force that output. If the R is not being forced then just add the * before the prdrlout or the pffr and see if either one of them give you the forced output you need.

As always please make sure you have a backup copy of your post before doing any post modifications. I have some posts backed up 20 times and with memory cheap as it today I have no problem being that redundant.

I just picked up a 990 M2 Samsung Pro 2TB drive for $130 off Amazon. My laptop will not have 7Tb of room on it. The new drive will be my Windows 11 drive. The laptop will have 3 bootable drives. I learned how to disable and enable the Mastercam license between each drive. Vericut doesn't care since it used the MAC address of the Ethernet port. Maybe next year when this laptop hits the 5 year mark I will replace it. Been rough year, but still keeping a roof over our heads and food on the table.

 

 

I will testing this somettime this week ,I thing this should work 

 

G83 Z-3.1757 R-2.0548 Q3000. F1.43
G83 C-180. Q3000. F1.43
G83 Q3000. F1.43   -------------------------  may be  I need to remove this  lines ,but I let you know when I start testing 
G83 C60. Q3000. F1.43
G83 Q3000. F1.43                                  remove this line 

 

Thank you so much ,every day I learn something new from you ,you are NYMBRER ONE !!!!!!