Results 1 to 12 of 12
  1. #1
    rnmmhunter is offline Cast Iron
    Join Date
    Oct 2012
    Location
    Menomonee Falls Wi
    Posts
    385

    Default Okuma Lathe program help.

    Can someone tell me how to edit the speeds of this program? I didn't write it looks Greek to me.I run a Fanuc controller.The boring bar starts at N0400 I would like to slow it down and there is no G50 where do I put it?

    $L531028.MIN%
    N0001 ()
    N0002 ()
    N0003 ( "L-2 ONLY" )
    N0004 (REVISED ON 06/05/10 J.J.)
    N0005 (1.250" DIA. BORE ID SIZE)
    N0006 (INSTALL P/N 999-102 JAWS)
    N0007 (X ZERO SET TO BE 559.040)
    N0008 (Z ZERO SET TO BE 283.740)
    N0009 (MAT:....ALUMINUM CASTING)
    N0010 (MACH. BASE 1ST,THRDS 2ND)
    N0011 (PROGRAM IS AT PEAK S.F.M)
    N0012 (CYCLE TIME:3 MIN.23 SEC.)
    N0013 PO=.1800 (0 SHIFT, SIDE 2)
    N0014 CLEAR
    N0015 DEF WORK
    N0016 PS LC,[-20,00],[20,21],4
    N0017 PS LC,[-09,00],[09,27],4
    N0018 PS LC,[-20,00],[20,11],0
    N0019 PS LC,[-20,00],[11,14],0
    N0020 END
    N0021 DRAW
    N0022 G50 S1200
    N0023 M216
    N0024 M01
    NAT02 (55 DEG. TURN & FACE TOOL)
    N0200 G00 X20 Z20 G95
    N0201 G97 M03 S1200 M42
    N0202 G00 X2.75 Z.1 T020202
    N0203 G96 S600 M08
    N0204 G00 Z.02
    N0205 G01 X.95 F.005
    N0206 G00 Z.05
    N0207 X2.75
    N0208 Z0
    N0209 G01 X.95 F.005
    N0210 G00 Z.05
    N0211 X2.65
    N0212 G85 N0213 D.125 F.012 U.025 W0
    N0213 G81
    N0214 G00 X2.4
    N0215 G01 Z0 F.01
    N0216 X2.5 Z-.05 F.003
    N0217 Z-1.015 F.008
    N0218 X2.292 F.005
    N0219 G04 F.25
    N0220 G01 X2.6 F.2
    N0221 G80
    N0222 G87 N0213
    N0223 G00 Z.1 M09
    N0224 G97 S1200
    N0225 X20 Z20 M05
    N0226 M01
    NAT04 (1.0" DIA. BORING BAR)
    N0400 G00 X20 Z20 G95
    N0401 G97 M04 S800 M42
    N0402 G00 X1.125 Z.1 T040404
    N0403 G96 S335 M08
    N0404 G85 N0405 D.1 F.012 U.025 W.005
    N0405 G81
    N0406 G00 X1.35
    N0407 G01 Z0 F.01
    N0408 X1.250 A225. F.003
    N0409 Z-.925 F.008
    N0410 X1.225 F.1
    N0411 G80
    N0412 G87 N0405
    N0413 G00 Z.1 M09
    N0414 G97 S800
    N0415 X20 Z20 M05
    N0416 M01
    N0417 (********************************)
    N0418 M00 (***** [FLIP PART OVER] *****)
    N0419 (********************************)
    NAT02 (55 DEG. TURN & FACE TOOL)
    N0226 VZSHZ=PO
    N0227 CLEAR
    N0228 DEF WORK
    N0229 PS LC,[-20,00],[20,20],4
    N0230 PS LC,[-13,00],[03,27],4
    N0231 PS LC,[-20,00],[20,14],0
    N0232 END
    N0233 DRAW
    N0234 G00 X20 Z20 G95
    N0235 G97 M03 S1200 M42
    N0236 G00 X2.8 Z.1 T020202
    N0237 G96 S600 M08
    N0238 G00 Z-1.02
    N0239 G01 X1.99 F.005
    N0240 G00 X2.8
    N0241 Z-1.048
    N0242 G01 X1.99 F.005
    N0243 G00 X2.8
    N0244 Z0
    N0245 X2.1
    N0246 G01 X1.225 F.005
    N0247 G00 Z.05
    N0248 X2.0
    N0249 G85 N0250 D.1 F.012 U.025 W0
    N0250 G81
    N0251 G00 X1.455
    N0252 G01 X1.575 Z-.06 F.003
    N0253 X1.66 Z-1.05 F.008
    N0254 X2.45 F.005
    N0255 X2.5 Z-1.1 F.003
    N0256 Z-1.435 F.008
    N0257 X2.292 F.005
    N0258 G04 F.25
    N0259 G00 X2.65
    N0260 G80
    N0261 G87 N0250
    N0262 G00 Z.1 M09
    N0263 G97 S1200
    N0264 G00 X20 Z20
    N0265 M01
    NAT10 (O.D. 60 DEG. THREAD TOOL)
    (1 1/4"-11.5 NAT. PIPE THREAD)
    N1000 G00 X20 Z20 G95
    N1001 G97 M03 S500 M42
    N1002 G00 X1.75 Z.1 T101010 M08
    N1003 G71 X1.475Z-.92A178B60D.02U.002H.07F1J11.5M22M32M73
    N1004 G00 X1.75 M09
    N1005 Z.1 M05
    N1006 X20 Z20
    N1007 M215
    N1008 V2=V2+1
    N1009 M01
    N1010 M30
    %

  2. #2
    metlmunchr is offline Diamond
    Join Date
    Jul 2004
    Location
    Asheville NC USA
    Posts
    8,339

    Default

    G50 is at line 22 and currently clamped at 1200 rpm. G50 is modal on an Okuma control, so if another program is run that doesn't contain a G50 speed clamp, the S1200 will still be in effect on the new program.

  3. #3
    angelw is online now Stainless
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    1,655

    Default

    As Metlmunchr states, the G50 is specified in your program as follows "N0022 G50 S1200", and will clamp the speed at that unless otherwise specified. Rather than have one overriding G50 for all tools, I prefer to specify a G50 for each and every tool. In that way you're able to tailor the RPM limit for each tool. You only make comment regarding slowing the boring bar down; accordingly, you must be happy with the max speed for OD tool. Programming a slower speed in the N0022 block will affect the max speed for the OD tool and the boring bar.

    With the constant surface speed specified for the boring bar in "N0403 G96 S335", the maximum speed the boring bar will reach is 1137 RPM. If you want the boring bar only to use a slower speed, edit the "N0403" block, or insert a G50 block with an "S" value less than S1137, after the N0400 block.

    Regards,

    Bill

  4. #4
    rnmmhunter is offline Cast Iron
    Join Date
    Oct 2012
    Location
    Menomonee Falls Wi
    Posts
    385

    Default

    You are correct Bill when I write a program on the Fanuc I put a G50 on every tool.I am not happy with the way these programs are written it sounds like the lathe is going to take off to the moon.No need to be at max spindle speed.On the Okuma how or what does the G97 do?

  5. #5
    angelw is online now Stainless
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    1,655

    Default

    Quote Originally Posted by rnmmhunter View Post
    You are correct Bill when I write a program on the Fanuc I put a G50 on every tool.I am not happy with the way these programs are written it sounds like the lathe is going to take off to the moon.No need to be at max spindle speed.On the Okuma how or what does the G97 do?
    The same as the Fanuc control, constant RPM.

    Regards,

    Bill

  6. #6
    rnmmhunter is offline Cast Iron
    Join Date
    Oct 2012
    Location
    Menomonee Falls Wi
    Posts
    385

    Default

    Can I change this line N0401 G97 M04 S800 M42 just put a G50 where the G97 is? Or do I need the G97.

  7. #7
    angelw is online now Stainless
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    1,655

    Default

    Quote Originally Posted by rnmmhunter View Post
    Can I change this line N0401 G97 M04 S800 M42 just put a G50 where the G97 is? Or do I need the G97.
    The general format is the same as a Fanuc control. The biggest differences between the two controls are the G codes and syntax used for the various cycles.

    You will note that in the code for OD and ID turning tools, the spindle is started in Constant RPM Mode (G97), then once the tool has been moved to the machining start diameter, Constant Surface Speed Mode (G96) is selected. You should also note that Constant RPM has been programmed again before the slides are sent back to the Tool Change Position. Many programmers do this, and its a good practice, so that there isn't a rapid revving up and slowing down of the spindle as the tool moves from Tool Change Position (large diameter) to Machining Start Position (small diameter) and then back to Tool Change Position (large diameter). Normally the RPM for the given CSS and Machining Start Position of the next tool is calculated and the spindle set to rev at that speed, but in your listed program, ball park RPM has been used.

    To answer your question directly, yes you could replace the G97 with G50. However, at a CSS of 335 sfm, and with the profile the boring bar is cutting, the spindle revs will never be slower than the 800 RPM you're proposing to clamp the spindle speed at. Accordingly, you could just leave the "N0401 G97 M04 S800 M42" as is, and delete the "N0403 G96 S335". The resulting spindle speed will be the same if you limit the RPM with G50 to S800, and keep the G96 block.

    As Metlmunchr points out, the speed clamped by G50 is Modal. Therefore, if you clamp the RPM at 800, and you want a higher limit for another tool, you must remember to include the new clamp RPM for the particular tool and operation.

    Regards,

    Bill
    Last edited by angelw; 01-10-2013 at 02:17 PM.

  8. #8
    rnmmhunter is offline Cast Iron
    Join Date
    Oct 2012
    Location
    Menomonee Falls Wi
    Posts
    385

    Default

    No wonder what ever I tried didn't change the speed.Thanks starting to make sense
    Now what the heck is this
    N0016 PS LC,[-20,00],[20,21],4
    N0017 PS LC,[-09,00],[09,27],4
    N0018 PS LC,[-20,00],[20,11],0
    N0019 PS LC,[-20,00],[11,14],0

  9. #9
    angelw is online now Stainless
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    1,655

    Default

    Quote Originally Posted by rnmmhunter View Post
    No wonder what ever I tried didn't change the speed.Thanks starting to make sense
    Now what the heck is this
    N0016 PS LC,[-20,00],[20,21],4
    N0017 PS LC,[-09,00],[09,27],4
    N0018 PS LC,[-20,00],[20,11],0
    N0019 PS LC,[-20,00],[11,14],0
    That's related to the graphic representation of the part for the purpose of verifying the tool path.
    All the following can be deleted and it will have no affect on the machining process. The program was likely created with Okuma's IGF programming system, or a CAM system.

    Regards,

    Bill

    N0014 CLEAR
    N0015 DEF WORK
    N0016 PS LC,[-20,00],[20,21],4
    N0017 PS LC,[-09,00],[09,27],4
    N0018 PS LC,[-20,00],[20,11],0
    N0019 PS LC,[-20,00],[11,14],0
    N0020 END
    N0021 DRAW

  10. #10
    rnmmhunter is offline Cast Iron
    Join Date
    Oct 2012
    Location
    Menomonee Falls Wi
    Posts
    385

    Default

    Thanks for explaining that they have IGF on one lathe. Now can you explain how the work shift works on a two sided part.N0013 PO=.1800 (0 SHIFT, SIDE 2)
    N0014 CLEAR
    On the Fanuc I run I use G55 and G54.

  11. #11
    litlerob's Avatar
    litlerob is offline Hot Rolled
    Join Date
    Jun 2009
    Location
    PDX, OR
    Posts
    547

    Default

    Quote Originally Posted by rnmmhunter View Post
    Thanks for explaining that they have IGF on one lathe. Now can you explain how the work shift works on a two sided part.N0013 PO=.1800 (0 SHIFT, SIDE 2)
    N0014 CLEAR
    On the Fanuc I run I use G55 and G54.
    This machine works in an absolute work coordinate system, unlike some other inferior systems. Meaning that there is one Zero and one Home, you need to use a Macro to shift the work zero offset.

    N0013 PO=.1800 (0 SHIFT, SIDE 2)
    N0226 VZSHZ=PO

    These 2 lines are working together to shift the Zero offset .1800, so once the program gets to line 226 it reads the shift of PO value in line 13.

    Robert

  12. #12
    rnmmhunter is offline Cast Iron
    Join Date
    Oct 2012
    Location
    Menomonee Falls Wi
    Posts
    385

    Default

    I would think that would be a -.180?

Bookmarks

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •