Jump to content

Welcome to eMastercam

Register now to participate in the forums, access the download area, buy Mastercam training materials, post processors and more. This message will be removed once you have signed in.

Use your display name or email address to sign in:

CNC Software OSP Lathe Post

Mick

By Mick,
in Post Processor Development Forum

 Share

Recommended Posts

Mick Contributor

Mick

Posted
Posted

I'm catching up on something I have been meaning to do for a long time, and that is set up a decent machine definition/post for the Okuma OSP series of 2 axis lathes, to output LAP cycles. One thing I've found, in using the CNC Software supplied OSP lathe post, is that it outputs the roughing feedrate within the canned roughing cycle, but doesn't have an option for the finishing feedrate within the contour. When the G87 is called up, it cuts using the roughing feedrate.

 

The finishing feedrate is output if the canned finishing cycle is called immediately after the canned roughing cycle, but if the finishing cycle is called later (for example, after roughing and grooving), then the finishing feedrate isn't output.

 

Is there are variable for the finishing feedrate as per the toolpath parameters page?

Link to comment
Share on other sites
Colin Gilchrist Proficient

Colin Gilchrist

Posted
Posted

Hi Mick,

 

I'm actually looking at some of the Lathe Canned Cycle stuff for the Okuma OSP Posts. Could you send me a Zip2Go file with an example? I'm outputting some test code here using the Okuma OSP7000 2X Lathe Post. I can see the issue you are describing. My only question is: where do you want the finish feed value output?

 

Here is some sample NC Code from a test file. I created a simple profile and used a Canned Rough, Canned Groove, and Canned Finish Cycle. Where would you expect the finish feedrate value to be?

 

$T.MIN%
O0001
(PROGRAM NAME - T)
(DATE=DD-MM-YY - 14-11-11 TIME=HH:MM - 09:06)
(MCX FILE - T)
(NC FILE - C:\USERS\CMG\DOCUMENTS\MY MCAMX5\LATHE\NC\T.NC)
(MATERIAL - ALUMINUM MM - 2024)
(TOOL - 1 OFFSET - 1)
(OD ROUGH RIGHT - 80 DEG.  INSERT - CNMG 12 04 08)
N10 G0 X250. Z250.
N20 T0101
N30 G97 S604 M03 M41
N40 G0 X145.018 Z0. M09
N50 G50 S3600
N60 G96 S275
N720 G85 NAT01 U.4 W.2 U4. F.8
N730 NAT01 G81
N740 G0 X-4. Z0.
N750 G1 X94.166
N760 G3 X95.454 Z-.326 K-.8
N770 G1 X144.706 Z-33.757
N780 G3 X145.018 Z-34.231 I-.644 K-.474
N790 G1 Z-76.002
N800 Z-92.523
N810 Z-147.521
N820 G80
N830 G0 Z0.
N920 G0 X250. Z250.
N930 M05
N940 M01

(TOOL - 43 OFFSET - 43)
(OD GROOVE CENTER - WIDE  INSERT - N151.2-600-4E)
N950 G0 X250. Z250.
N960 T4343
N970 G97 S645 M03 M41
N980 G0 X149.018 Z-81.402 M09
N990 G50 S3600
N1000 G96 S302
N1350 G73 X114.246 Z-91.523 K1. F.1
N1360 G0 X149.018
N1370 Z-79.787
N1380 X147.846
N1390 G1 X145.018 Z-81.202
N1400 X113.846
N1410 X114.446 Z-81.502
N1420 G0 X147.846
N1430 Z-93.137
N1440 G1 X145.018 Z-91.723
N1450 X113.846
N1460 Z-86.402
N1470 G0 X147.846
N1480 G0 X250. Z250.
N1490 M05
N1500 M01

(TOOL - 1 OFFSET - 1)
(OD ROUGH RIGHT - 80 DEG.  INSERT - CNMG 12 04 08)
N1510 G0 X250. Z250.
N1520 T0101
N1530 G97 S604 M03 M42
N1540 G0 X145.018 Z0. M09
N1550 G50 S3600
N1560 G96 S275
N1570 G87 NAT01
N1660 G0 Z0.
N1670 G0 X250. Z250.
N1680 M05
N1690 M02
%

 

Thanks,

Link to comment
Share on other sites
Mick Contributor

Mick

Posted
  • Author
Posted

Hi Mick,

 

I'm actually looking at some of the Lathe Canned Cycle stuff for the Okuma OSP Posts. Could you send me a Zip2Go file with an example? I'm outputting some test code here using the Okuma OSP7000 2X Lathe Post. I can see the issue you are describing. My only question is: where do you want the finish feed value output?

 

Here is some sample NC Code from a test file. I created a simple profile and used a Canned Rough, Canned Groove, and Canned Finish Cycle. Where would you expect the finish feedrate value to be?

 

$T.MIN%
O0001
(PROGRAM NAME - T)
(DATE=DD-MM-YY - 14-11-11 TIME=HH:MM - 09:06)
(MCX FILE - T)
(NC FILE - C:\USERS\CMG\DOCUMENTS\MY MCAMX5\LATHE\NC\T.NC)
(MATERIAL - ALUMINUM MM - 2024)
(TOOL - 1 OFFSET - 1)
(OD ROUGH RIGHT - 80 DEG.  INSERT - CNMG 12 04 08)
N10 G0 X250. Z250.
N20 T0101
N30 G97 S604 M03 M41
N40 G0 X145.018 Z0. M09
N50 G50 S3600
N60 G96 S275
N720 G85 NAT01 U.4 W.2 U4. F.8
N730 NAT01 G81
N740 G0 X-4. Z0.
N750 G1 X94.166  F.15 <---- Finishing Feedrate should be here
N760 G3 X95.454 Z-.326 K-.8
N770 G1 X144.706 Z-33.757
N780 G3 X145.018 Z-34.231 I-.644 K-.474
N790 G1 Z-76.002
N800 Z-92.523
N810 Z-147.521
N820 G80
N830 G0 Z0.
N920 G0 X250. Z250.
N930 M05
N940 M01

(TOOL - 43 OFFSET - 43)
(OD GROOVE CENTER - WIDE  INSERT - N151.2-600-4E)
N950 G0 X250. Z250.
N960 T4343
N970 G97 S645 M03 M41
N980 G0 X149.018 Z-81.402 M09
N990 G50 S3600
N1000 G96 S302
N1350 G73 X114.246 Z-91.523 K1. F.1
N1360 G0 X149.018
N1370 Z-79.787
N1380 X147.846
N1390 G1 X145.018 Z-81.202
N1400 X113.846
N1410 X114.446 Z-81.502
N1420 G0 X147.846
N1430 Z-93.137
N1440 G1 X145.018 Z-91.723
N1450 X113.846
N1460 Z-86.402
N1470 G0 X147.846
N1480 G0 X250. Z250.
N1490 M05
N1500 M01

(TOOL - 1 OFFSET - 1)
(OD ROUGH RIGHT - 80 DEG.  INSERT - CNMG 12 04 08)
N1510 G0 X250. Z250.
N1520 T0101
N1530 G97 S604 M03 M42
N1540 G0 X145.018 Z0. M09
N1550 G50 S3600
N1560 G96 S275
N1570 G87 NAT01
N1660 G0 Z0.
N1670 G0 X250. Z250.
N1680 M05
N1690 M02
%

 

Thanks,

 

Hi Colin,

 

I've marked in the text above where the finish feedrate should go. Any feedrates within the finish contour (within the LAP cycle) are recognised by the G87 cycle. I guess the problem is that the LAP cycle uses a roughing feedrate (generated on the G85/G86 line), which is pulled from the Roughing Feedrate in the Canned Rough parameters. However, there is no setting on the Rough Canned Cycle for the finish pass feedrate. I initially thought that the best option was to output a feedrate on the G87 line for the canned finishing cycle, however I dont think that would work. Also, if a change in feedrate part way through the finishing is required, there would be no option to do so, so the best option is to put the feedrate on the first linear feed (G1) of the contour, as above.

 

I'll sort a zip2go file out today for you :)

Link to comment
Share on other sites
Mick Contributor

Mick

Posted
  • Author
Posted

i run this post since 5 years, i always create a different operation for finish for that reason

 

I was thinking the same thing last night. The easiest way is to just create a seperate finishing cycle. However, it would be nice to use the G87 option.

Link to comment
Share on other sites
  • 2 weeks later...

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

Guest
Reply to this topic...

×   Pasted as rich text.   Paste as plain text instead

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.

×
 Share
Go to topic listing

  • Recently Browsing   0 members

    • No registered users viewing this page.

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Useful Links

Contact Info

Subscribe to eMastercam News

 

Legal

Privacy Policy

Store Terms & Conditions

Forum Guidelines

Follow us

×
×
  • Create New...