[PETE1968]

trying to program this old beast with mastercam has anyone had any experience with this lathe or control :rainfro:

[Mike Mattera]

Why dont you tell us....
1) what you know.
2) what you need to know.

That way we dont have to guess what info your looking for.

Mike Mattera

[PETE1968]

with this machine a g96 (constant surface speed) has to have a R word . the r dimension

[PETE1968]

with this machine a g96 (constant surface speed) has to have a R word . the r dimension is the distance from the center line of the spindle to the tool point. I am having trouble getting my post to out put this

[Mike Mattera]

Are the current values for X in Radius or Diameter. If it's in Rad, create a variable in the post (cssr) and assign the value of the first X position. cssr = xout (or possibly x). Then on the line that outputs the G96 add the output of that variable.

pbld, n, "G96", cssr, e

[PETE1968]

hi mike
is this the area i should make the change doing something with pfxout


pcss #Output Constant surface speed
speed = c1_ss
result = nwadrs(strr,xabs)
result = nwadrs(strr,xinc)
if c1_css_actv = one, pbld, n$, *sg9697, pfxout, *speed, e$
result = nwadrs(strx,xabs)
result = nwadrs(strx,xinc)
!speed

[Mike Mattera]

Somewhere in the post you need to find the section where the "Formats" (fmt) are setup. You need to add the variable and tell it which letter to use (R in your case). So find a section similar to what is shown below and add this line...

fmt R 2 cssr # CSS Radius value.

Note the number "2" is the same as the "2" used below in to format the "xabs" output. Your number may be different.

So insert that line somewhere below.


# Toolchange / NC output Variable Formats
# --------------------------------------------------------------------------
fmt T 7 toolno #Tool number
fmt G 4 g_wcs #WCS G address
fmt P 4 p_wcs #WCS P address
fmt S 4 speed #Spindle Speed
fmt M 4 gear #Gear range
fmt S 4 maxss$ #RPM spindle speed
fmt R 2 cssr # CSS Radius value.
# --------------------------------------------------------------------------
fmt N 24 n$ #Sequence number
fmt X 2 xabs #X position output
fmt Y 2 yabs #Y position output


Then in the section you showed, you need to make "cssr" = the "X" position. Then add the "cssr" call to the output line.

pcss #Output Constant surface speed
speed = c1_ss
cssr = x
result = nwadrs(strr,xabs)
result = nwadrs(strr,xinc)
if c1_css_actv = one, pbld, n$, *sg9697, *cssr, *speed, e$
result = nwadrs(strx,xabs)
result = nwadrs(strx,xinc)
!speed


Mike Mattera

[PETE1968]

Hi Mike
Thanks for the help it seems to recongize the change but is outputting a R0 everytime??????????

[Mike Mattera]

First try this.....(add the $)

pcss #Output Constant surface speed
speed = c1_ss
cssr = x$


If that doesn't work, try this....

pcss #Output Constant surface speed
speed = c1_ss
cssr = nextx$

Mike Mattera

[PETE1968]

that didi it
thanks i,m new to the lathe end of it. some stuff looks similiar but i think the control is dated and that makes for alot of post mods . i am using the mastercam psot for the acramatic 850

[PETE1968]

Good morning Mike
i ran a test program at the machine and the changes you showed me work except i need the r value to = the value of the home position then as the tool approaches the part the chuck speeds up. I tried changing to (xout) but that didnt work. below is the area i think i need to be looking???



ltlchg$ #Tool change
if cycseq_wrt = zero, lrapid$, ex$ #exit for canned cycle
gcode$ = zero
toolchng = one
ptoolcommon
ptoolcomment

pcomread
toolcount = toolcount + 1
#if mi1 = zero, pg50call
#if mi1 = one, phomecall
phomecall
pbld, pcssg50
if c2_cycseq = zero, plath_tl_map
pcom_moveb
pbld, pcss
pbld, n$, psccomp, pfsgcode, pwcs, pfxout, pyout, pfzout, pfscool, pcan,e$
pcom_movea

toolchng = zero
!x$, !y$, !z$


pg50call #Toolchange g50 position call
sav_xa = vequ (xa)
pmap_home
pbld, n$, *sg28ref, "U0.", "W0.", e$
pbld, n$, "G50", pfxout, pfyout, pfzout, e$
prv_xabs = vequ (xabs)
xa = vequ (sav_xa)

phomecall #Toolchange home position call
sav_xa = vequ (xa)
pmap_home
pbld, *toolcount, pspindle, prpm,e$
pbld, n$, "G70" , e$
pbld, n$, "G90" , e$
pbld, n$, sg00_1, pfxout, pfyout, pfzout, e$
pbld, n$, "G95" , e$
toolno=t$ * 100 + tloffno$
pbld, n$, *toolno,"M06" , e$
prv_xabs = vequ (xabs)
xa = vequ (sav_xa)

[PETE1968]

hi mike
i got part figured out. just changed to cssr= vequ (c1_xh)$

[PETE1968]

no i got another problem LINE 0008 the x value is outputting zero ??????
O0001G97S239M03 lsof$ phomecall 80.
N0001G70 lsof$ phomecall 80.
N0002G90 lsof$ phomecall 80.
N0003G00X40000Z10000 lsof$ phomecall 80.
N0004G95 lsof$ phomecall 80.
N0005T0200M06 lsof$ phomecall 80.
N0006G92S1200 lsof$ pcssg50 80.
N0007G96R40000S500 lsof$ pcss 80.
N0008G00X0Z3201M08 ** lsof$ ltlchg$ 80. PROBLEM************
N0009G01X4120Z2201F100 llin$ plinout 82.
N0010X5428Z896F100 llin$ plinout 84.

[mariusborza]

Hy,

I'm from Romania. I have a Cincinnati Milacron, Acramatic 850 T equiped.
Does anyone know the procedure to see phe PLC program ?
Any information will be helpfully. Thanks.

You know... in electronics you can do a wrong thing only once ! ... and go home !

[RPrecision]

I got the same problem. Have an cincinnati cinturn lathe with the acramatic 850TC control and can't get it to communicate with mastercam.
Let me know if you have any luck. I will let you know if I do.

Rod

trying to program this old beast with mastercam has anyone had any experience with this lathe or control :rainfro:

[cadcam]

are you have trouble communicating (sending a program to the machine) or you do not have a correct post that plays nice with the control.

[RPrecision]

I am having trouble comunicating. Never got the machine to accept anything.
We tried all the settings. baud rate and so on, different ascci characters.
nothing. it keeps saying device not responding.
Have you had any experience like that before?

[cadcam]

are you sure for starters you have the correct cable and that it is configured correct?
I know you are using mastercam to send. are you able to see the settings on the machine' you need to have the same baud and Data bits.have you been able to connect to any machine and send code?

Are you connect form a desktop or a laptop?

I know that you can send to from mastercam or predator as I have in the past.

[RPrecision]

Pete,

I am getting a cycle time elapse when trying to run the machine.
Any idea what that might be.?