9 replies to this topic

[Mr. Dayshift]

Hi all, I've made a return to mastercam and the forum after a couple year absence. Started at a new job and we are using X3 and the Mplmaster X3 lathe post for a 2 axis lathe with Fanuc 0i-TC. I'd like to suppress the work offset from the posted code. Near as I can tell, this cannot be done from the tool path parameters page or control defns.


Also, why does this post output a G97 command at the end of the tool sequence (occurs when that sequence is not the last in program)? What sets this G97 value.

Sample of code below. Thanks in advance for any input here.



O0001(LATHE TEST OP1)
(DATE:09-02-12 - TIME:12:50)
(MCX FILE - C:\USERS\MSHOP_2\DESKTOP\TEST PART LATHE.MCX)
(T1   - OD ROUGH RIGHT - 80 DEG. - OFFSET - 1   - INSERT - CNMG-432 - HOLDER - DCGNR-164D)
(T223 - A08-SCLPR2 - CPMT-21.51LF - OFFSET - 223 - INSERT - CPMT-21.51LF - HOLDER - A08-SCLPR2)
G20
(T1 OFFSET - 1)
(OD ROUGH RIGHT - 80 DEG. INSERT - CNMG-432)
G54
N1T0101
G99
M24
G97S347M03
G0X2.2Z.005
G50S3600
G96S200
G1X-.0625F.01
G0Z.105
G97S3600
G28U0.W0.
M01
(T223 OFFSET - 223)
(A08-SCLPR2 - CPMT-21.51LF INSERT - CPMT-21.51LF)
G54
N223T22523
G99
M8
G97S3600M03
G0X1.3892Z.2
G50S3600
...

[gcode]

Try the Mics Values tab and set  Work Position to 0

this should get rid of the G54

Attached Files

•  lathe home.png   75.15K   25 downloads

[Bryan Johnson]

The G97 at start and end, will prevent the spindle from having to ramp up/down during the rapid moves to and from home.

[Mr. Dayshift]

Gcode,

The misc values tab is(was) already set to zero. Any other suggestions?


Bryan,

Can this RPM be set lower? I work at an educational facility, so are requirements aren't always the same as a commercial shop.

[Mr. Dayshift]

Located more suitable post file. Issue resolved.

[Bryan Johnson]

The S values on the G97 line is driven by the CSS and MAX RPM speed you set at Mastercam toolpath parameter page.
In your example, I think it would be the MAX RPM that you are wanting to adjust.

G97S347M03 ----- 347 RMP = 200 CSS @ X2.2<br style="color: rgb(255, 255, 255); font-family: 'Trebuchet MS', Arial; font-size: 14px; line-height: 21px; background-color: rgb(61, 61, 61); ">G0X2.2Z.005<br style="color: rgb(255, 255, 255); font-family: 'Trebuchet MS', Arial; font-size: 14px; line-height: 21px; background-color: rgb(61, 61, 61); ">G50S3600<br style="color: rgb(255, 255, 255); font-family: 'Trebuchet MS', Arial; font-size: 14px; line-height: 21px; background-color: rgb(61, 61, 61); ">G96S200<br style="color: rgb(255, 255, 255); font-family: 'Trebuchet MS', Arial; font-size: 14px; line-height: 21px; background-color: rgb(61, 61, 61); ">G1X-.0625F.01<br style="color: rgb(255, 255, 255); font-family: 'Trebuchet MS', Arial; font-size: 14px; line-height: 21px; background-color: rgb(61, 61, 61); ">G0Z.105<br style="color: rgb(255, 255, 255); font-family: 'Trebuchet MS', Arial; font-size: 14px; line-height: 21px; background-color: rgb(61, 61, 61); ">G97S3600 ---- 3600 RPM = 200 CSS @ X-.0625 (MAX RPM)

[Bryan Johnson]

not sure what happened to my previous post format.




G97S347M03 ----- 347 RPM = 200 CSS @ X2.2

G0X2.2Z.005

G50S3600

G96S200

G1X-.0625F.01

G0Z.105

G97S3600 ---- 3600 RPM = 200 CSS @ X-.0625 (MAX RPM)

[roland_1]

Mr. Dayshift, on 10 February 2012 - 01:04 PM, said:

Gcode,

The misc values tab is(was) already set to zero. Any other suggestions?


Bryan,

Can this RPM be set lower? I work at an educational facility, so are requirements aren't always the same as a commercial shop.

Hi, I just started to write posts and I know much in theory but I didn't see much different posts formats. But I am just trying to accommodate generic fanuc for one 5-ax machine. I see in this type of post that on  a beginning of post you have post switches. The one with name: "force_wcs    : yes$  #Force WCS output at every toolchange?" should post G54 only on a beginning and suppress all others at toolchanges. So you can try to put "no" or "0" in the post.

[Mr. Dayshift]

Yep Roland, that is what I changed. MPLmaster X3 is working nice now.

Force_wcs $
css_start_rpm $
css_end_rpm $

[Russh67]

Mr. Dayshift, on 10 February 2012 - 01:04 PM, said:

Gcode,

The misc values tab is(was) already set to zero. Any other suggestions?

I use fanuc Oi also.

Try setting setting misc integer to -1, meaning minus 1. I do this on all lathe programs.  I also add -1 misc integer to any c-axis milling ops. -1  will not post any work offsets....Try it.. assuming you are running the machine incrementally and do not use a predefined home position that would be set in the machine def.

The g97 is not required at the end of an op if the spindle gets turned off this is what mine posts with misc int -1.

G28U0.W0.
G0T0500
G0T0505
G97S1300M03
G0X2.7Z.005
G50S1300
G96S1000
G99G1X-.0313F.004
G0Z.105
X2.7
Z0.
G1X-.0313
G0Z.1
T0500
G28U0.W0.M05
M00

I always like to go home before a tool change.