Mach3 Turn Feed Per Revolution problem


Page 1 of 2 12 LastLast
Results 1 to 20 of 35

Thread: Mach3 Turn Feed Per Revolution problem

  1. #1
    Member Azalin's Avatar
    Join Date
    Mar 2014
    Location
    Turkey
    Posts
    1131
    Downloads
    0
    Uploads
    0

    Default Mach3 Turn Feed Per Revolution problem

    Hi,
    I'm trying to setup the Mach3 turning post processor for SolidCAM that I found in the forum. It is the only post processor I could find so I have no other alternative. However, so far the post doesn't look bad except feed per revolution mode doesn't work. When I say feed per revolution will 0.3mm per revolution it runs as CSS at 0.3mm per minute. I'm not an g-code expert (at all) but maybe you guys can help me.


    Below is a sample gcode. Can you please help me find out how it should be for feed per revolution work?

    By the way, spindle indexing sensor is working and;


    - "Use Spindle Feedback in Sync Modes" option is selected.
    - "Closed Loop Spindle Control" is unchecked
    - "Spindle Speed Averaging" is checked


    Thanks in advance.
    Best


    %
    N1 T0101
    N2 G0 X30. Z30.
    N3 G97 S1000 M3
    N4 G0 X17.002 Z2. M8
    N5 (-----------------------)
    N6 (TR-TURN-ON-SOLID - TURN)
    N7 (-----------------------)
    N8 G97 S1000
    N9 G0 X17.002 Z2.
    N10 X14.062
    N11 G1 Z-25.377 F0.3
    N12 G2 X14.986 Z-27.778 R-15.4
    N13 G1 X15.002 Z-27.833
    N14 X15.202
    N15 G0 Z2.
    N16 X13.122
    N17 G1 Z-23.709
    N18 G2 X14.062 Z-25.377 R-15.4
    N19 G1 X14.262 Z-25.177
    N20 G0 Z2.
    N21 X12.182
    N22 G1 Z-22.413
    N23 G2 X13.122 Z-23.709 R-15.4
    N24 G1 X13.322 Z-23.509
    N25 G0 Z2.
    N26 X11.242
    N27 G1 Z-21.353
    N28 G2 X12.182 Z-22.413 R-15.4
    N29 G1 X12.382 Z-22.213
    N30 G0 Z2.
    N31 X10.302
    N32 G1 Z-20.465
    N33 G2 X11.242 Z-21.353 R-15.4
    N34 G1 X11.442 Z-21.153
    N35 G0 Z2.
    N36 X9.362
    N37 G1 Z-19.71
    N38 G2 X10.302 Z-20.465 R-15.4
    N39 G1 X10.502 Z-20.265
    N40 G0 Z2.
    N41 X8.422
    N42 G1 Z-19.067
    N43 G2 X9.362 Z-19.71 R-15.4
    N44 G1 X9.562 Z-19.51
    N45 G0 Z2.
    N46 X7.482
    N47 G1 Z-18.519
    N48 G2 X8.422 Z-19.067 R-15.4
    N49 G1 X8.622 Z-18.867
    N50 G0 Z2.
    N51 X7.542
    N52 G1 X6.542
    N53 Z-18.056
    N54 G2 X7.482 Z-18.519 R-15.4
    N55 G1 X7.682 Z-18.319
    N56 G0 Z2.
    N57 X6.602
    N58 G1 X5.602
    N59 Z-17.668
    N60 G2 X6.542 Z-18.056 R-15.4
    N61 G1 X6.742 Z-17.856
    N62 G97 S1000
    N63 G1 X6.967 Z-17.461 F0.15
    N64 G0 X7.603 Z-16.342
    N65 Z2.
    N66 X5.002
    N67 G1 Z-17.868
    N68 G2 X15.002 Z-32.256 R-15.4
    N69 G1 X17.002 Z-32.252
    N70 G97 S1000
    N71 G0 Z2.
    N72 X5.002
    N73 G1 Z-17.868 F0.15
    N74 G2 X15.002 Z-32.256 R-15.4
    N75 G1 X17.002 Z-32.252
    N76 G0 Z2.
    N77 G0 X30.1 Z30.
    N78 M30
    %

    Similar Threads:
    Suat
    Proud father, C# developer, Model heli pilot, newbie free time machinist for hobby


  2. #2
    Member
    Join Date
    Jun 2010
    Location
    Australia
    Posts
    4252
    Downloads
    4
    Uploads
    0

    Default Re: Mach3 Turn Feed Per Revolution problem

    I really don't think feed per rev is useful except for threading.
    In addition, 0.3 mm per rev is rather coarse - OK maybe for ripping stuff off but not for a good finish.

    For Mach3 the instruction you want is g95. On some other machines it is g99 (stupid committees). I can't see either in your example, although I can see g97. All that does is specify a constant speed spindle - which is the default anyhow.

    Cheers
    Roger



  3. #3
    Member Azalin's Avatar
    Join Date
    Mar 2014
    Location
    Turkey
    Posts
    1131
    Downloads
    0
    Uploads
    0

    Default Re: Mach3 Turn Feed Per Revolution problem

    Thanks Roger.

    So the post processor doesn't support feed per rev mode.

    Suat
    Proud father, C# developer, Model heli pilot, newbie free time machinist for hobby


  4. #4
    Member mactec54's Avatar
    Join Date
    Jan 2005
    Location
    USA
    Posts
    15362
    Downloads
    0
    Uploads
    0

    Default Re: Mach3 Turn Feed Per Revolution problem

    Quote Originally Posted by Azalin View Post
    Hi,
    I'm trying to setup the Mach3 turning post processor for SolidCAM that I found in the forum. It is the only post processor I could find so I have no other alternative. However, so far the post doesn't look bad except feed per revolution mode doesn't work. When I say feed per revolution will 0.3mm per revolution it runs as CSS at 0.3mm per minute. I'm not an g-code expert (at all) but maybe you guys can help me.


    Below is a sample gcode. Can you please help me find out how it should be for feed per revolution work?

    By the way, spindle indexing sensor is working and;


    - "Use Spindle Feedback in Sync Modes" option is selected.
    - "Closed Loop Spindle Control" is unchecked
    - "Spindle Speed Averaging" is checked


    Thanks in advance.
    Best


    %
    N1 T0101
    N2 G0 X30. Z30.
    N3 G97 S1000 M3

    %
    Constant surface speed, you need to use a G96 a G97 cancels constant surface speed

    Feed per revolution is G99
    Feed per minute is G98

    Mactec54


  5. #5
    Member
    Join Date
    Jun 2010
    Location
    Australia
    Posts
    4252
    Downloads
    4
    Uploads
    0

    Default Re: Mach3 Turn Feed Per Revolution problem

    So the post processor doesn't support feed per rev mode.
    My understanding of post-processors is that YOU can add that instruction to the header section.

    Cheers
    Roger



  6. #6
    Member Azalin's Avatar
    Join Date
    Mar 2014
    Location
    Turkey
    Posts
    1131
    Downloads
    0
    Uploads
    0

    Default Re: Mach3 Turn Feed Per Revolution problem

    Quote Originally Posted by mactec54 View Post
    Constant surface speed, you need to use a G96 a G97 cancels constant surface speed

    Feed per revolution is G99
    Feed per minute is G98
    Thanks.

    Below is a simple gcode for 10mm dia 1.5mm module thread. I just replaced G97 with G99. I didn't try this yet. Does it look OK?

    %
    N1 T0101
    N2 G0 X10. Z10.
    N3 G99 S50 M3
    N4 G0 X14. Z4.84 M8
    N5 (--------------------------)
    N6 (TH-TURN-ON-SOLID1 - THREAD)
    N7 (--------------------------)
    N8 G99 S50
    N9 G0 X14. Z4.84
    N10 G76 P000000 Q100 R100
    N11 G76 X8.5 Z-25.16 P750 Q100 F1.5
    N12 G0 X10. Z10.
    N13 M30
    %

    Suat
    Proud father, C# developer, Model heli pilot, newbie free time machinist for hobby


  7. #7
    Member mactec54's Avatar
    Join Date
    Jan 2005
    Location
    USA
    Posts
    15362
    Downloads
    0
    Uploads
    0

    Default Re: Mach3 Turn Feed Per Revolution problem

    Quote Originally Posted by Azalin View Post
    Thanks.

    Below is a simple gcode for 10mm dia 1.5mm module thread. I just replaced G97 with G99. I didn't try this yet. Does it look OK?

    %
    G54 G18 G40 G80 (Safe start line )
    N1 T0101
    N2 G0 X10. Z10.
    N3 G97 S50 M3
    N4 G0 X14. Z4.84 M8
    N5 (--------------------------)
    N6 (TH-TURN-ON-SOLID1 - THREAD)
    N7 (--------------------------)
    N8 G97 S50
    N9 G0 X14. Z4.84
    N10 G76 P000000 Q100 R100
    N11 G76 X8.5 Z-25.16 P750 Q100 F1.5
    N12 G0 X10. Z10.
    N13 M30
    %
    You don't want that G99 in there the G76 canned cycle is all you need, this is when you would have the G97 in place so put it back in N3 and N8 for threading add a start line as well to all your programs

    Mactec54


  8. #8
    Member Azalin's Avatar
    Join Date
    Mar 2014
    Location
    Turkey
    Posts
    1131
    Downloads
    0
    Uploads
    0

    Default Re: Mach3 Turn Feed Per Revolution problem

    Quote Originally Posted by mactec54 View Post
    You don't want that G99 in there the G76 canned cycle is all you need, this is when you would have the G97 in place so put it back in N3 and N8 for threading add a start line as well to all your programs
    What is a start line? In the end of this page, mentioned R and K (X and Z start). Is this what you mean?

    Sorry I'm very new to turning programming.

    Suat
    Proud father, C# developer, Model heli pilot, newbie free time machinist for hobby


  9. #9
    Member mactec54's Avatar
    Join Date
    Jan 2005
    Location
    USA
    Posts
    15362
    Downloads
    0
    Uploads
    0

    Default Re: Mach3 Turn Feed Per Revolution problem

    Quote Originally Posted by Azalin View Post
    What is a start line? In the end of this page, mentioned R and K (X and Z start). Is this what you mean?

    Sorry I'm very new to turning programming.
    A safety start line, is a line of code that either cancels codes used in the program that have not been canceled before the start of a new run, or activates new codes at the start of a program, that should be in place for the program you are running
    some are needed all the time, like X and Z is G18 this tells the control that it is working in the X and Z plane G80 cancels any canned cycle like your threading cycle G54 tells the control what work offset you are using G90 will set it up to run in absolute

    There is not difference with Mill or lathe, you should have a safety line in both programs

    Mactec54


  10. #10
    Member Azalin's Avatar
    Join Date
    Mar 2014
    Location
    Turkey
    Posts
    1131
    Downloads
    0
    Uploads
    0

    Default Re: Mach3 Turn Feed Per Revolution problem

    It's a little confusing. I don't know what code should be where so I guess understanding gcode will take some time. Maybe I should find some gcodes and try to understand how it works.

    Sent from my MI 5s Plus using Tapatalk

    Suat
    Proud father, C# developer, Model heli pilot, newbie free time machinist for hobby


  11. #11
    Member mactec54's Avatar
    Join Date
    Jan 2005
    Location
    USA
    Posts
    15362
    Downloads
    0
    Uploads
    0

    Default Re: Mach3 Turn Feed Per Revolution problem

    Quote Originally Posted by Azalin View Post
    It's a little confusing. I don't know what code should be where so I guess understanding gcode will take some time. Maybe I should find some gcodes and try to understand how it works.

    Sent from my MI 5s Plus using Tapatalk
    You can do a program without a safety line, a lot do, but they are mostly experienced programmers

    Having a safety line is something that the post processor can do every time you do a program, it has no negative affect on your program, it can be peace of mind

    This is how you would use a G80 for a Mill / Router Drill Canned cycle, Z move after being, either the end of the program or just moving out the way for the next operation


    G73G98X0.Y0.Z-1.1R.1Q.030F10.
    X1.Y0.
    X2.Y1.
    X4.Y2.
    G80G0Z3.
    G0X5.Y7.

    Mactec54


  12. #12
    Member Azalin's Avatar
    Join Date
    Mar 2014
    Location
    Turkey
    Posts
    1131
    Downloads
    0
    Uploads
    0

    Default Re: Mach3 Turn Feed Per Revolution problem

    Hi,

    I used Mach3's threading wizard and created the same threading. M10x1.5 threads. 10mm long. When I start the program it stays at block "M03 S300". It seems like Mach3 waiting for something at that line.

    G0 G40 G18 G80 G50 G90
    G00 G53 X10 Z10
    T202M6
    G00 X10.025
    G00 Z0
    G00 X10
    M03 S300
    G76 X8.2 Z-10 Q5 P1.5 J0.006 L45 H0.1 I29 C0.025 B0.0001 T0
    M9
    M5
    M30

    When I uncheck "Use Spindle Feedback In Sync Mode" and try it would run fine and complete the program. So, maybe the index reading is not constant as it should? Mine, say it reads 300 +-10 RPM.

    Also I ran the "Spindle Calibration" but it couldn't finish it. The problem is the curve is not very flat but I don't know if this affects the threading operation.

    I have set Debounce Interval to 500 and Index Debounce to 2.

    Suat
    Proud father, C# developer, Model heli pilot, newbie free time machinist for hobby


  13. #13
    Member
    Join Date
    Jun 2010
    Location
    Australia
    Posts
    4252
    Downloads
    4
    Uploads
    0

    Default Re: Mach3 Turn Feed Per Revolution problem

    This is a bit complex, so I am guessing.
    If the screen display sits at the line BEFORE the G76 command, that means Mach is trying to execute the G76 command. That's just how the Mach display works.
    If it is not proceeding with the G76 command, that could mean it is waiting for the Spindle Index pulse.
    When you uncheck the "Use Spindle Feedback In Sync Mode" switch, Mach will no longer wait for the spindle index pulse, but I am not sure what would drive Mach then. I would have thought that Mach would refuse to do the G76 in that case.

    All of that initially suggests to me that Mach cannot see the Index pulses. They may be too short, in which case try setting Index Debounce to 0. They may be coming in on a different pin to what you have told Mach.BUT if Mach reads " 300 +-10 RPM" as you say under normal spinning, then ... um.

    Do you have spindle averaging switched on? That may or may not matter.

    If you turn OFF the "Use Spindle Feedback In Sync Mode" switch, does Mach cut a respectable thread? If so, it almost seems that this switch is being inverted inside Mach.That would be VERY strange.

    Cheers
    Roger



  14. #14
    Member Azalin's Avatar
    Join Date
    Mar 2014
    Location
    Turkey
    Posts
    1131
    Downloads
    0
    Uploads
    0

    Default Re: Mach3 Turn Feed Per Revolution problem

    In this video the index reading is very constant. 552 +-1 RPM. Maybe the index slot of the wheel is not wide enough on my lathe. Or maybe I can try a hall sensor like the guy uses in his lathe.



    Suat
    Proud father, C# developer, Model heli pilot, newbie free time machinist for hobby


  15. #15
    Member Azalin's Avatar
    Join Date
    Mar 2014
    Location
    Turkey
    Posts
    1131
    Downloads
    0
    Uploads
    0

    Default Re: Mach3 Turn Feed Per Revolution problem

    Quote Originally Posted by RCaffin View Post
    Do you have spindle averaging switched on? That may or may not matter.

    If you turn OFF the "Use Spindle Feedback In Sync Mode" switch, does Mach cut a respectable thread? If so, it almost seems that this switch is being inverted inside Mach.That would be VERY strange.

    Cheers
    Roger
    Yes, "Spindle Speed Averaging" is checked but I also did a try while it is unchecked. Nothing changed.

    When I uncheck "Use Spindle Feedback In Sync Mode" and give a try it completes the operation but the thread is not what I want. Pitch of the thread is supposed to be 1.5mm but the actual thread is something like 0.5mm or so.

    Suat
    Proud father, C# developer, Model heli pilot, newbie free time machinist for hobby


  16. #16
    Member
    Join Date
    Jun 2010
    Location
    Australia
    Posts
    4252
    Downloads
    4
    Uploads
    0

    Default Re: Mach3 Turn Feed Per Revolution problem

    Hi Azalin

    That video is appalling! Next time, clamp the camera to something solid and keep it still!
    I will take you word for it that the spindle sits at 552 rpm - I could not tell from the video.

    If you don't use sync mode and the pitch is horribly wrong - fair enough. But I am not sure what to suggest.
    What version of Mach, and what hardware (PP, ESS, ??)

    Cheers
    Roger



  17. #17
    Member mactec54's Avatar
    Join Date
    Jan 2005
    Location
    USA
    Posts
    15362
    Downloads
    0
    Uploads
    0

    Default Re: Mach3 Turn Feed Per Revolution problem

    Quote Originally Posted by Azalin View Post
    Hi,

    I used Mach3's threading wizard and created the same threading. M10x1.5 threads. 10mm long. When I start the program it stays at block "M03 S300". It seems like Mach3 waiting for something at that line.

    G0 G40 G18 G80 G50 G90
    G00 G53 X10 Z10
    T202M6
    G00 X10.025
    G00 Z0
    G00 X10
    M03 S300
    G76 X8.2 Z-10 Q5 P1.5 J0.006 L45 H0.1 I29 C0.025 B0.0001 T0
    M9
    M5
    M30

    When I uncheck "Use Spindle Feedback In Sync Mode" and try it would run fine and complete the program. So, maybe the index reading is not constant as it should? Mine, say it reads 300 +-10 RPM.

    Also I ran the "Spindle Calibration" but it couldn't finish it. The problem is the curve is not very flat but I don't know if this affects the threading operation.

    I have set Debounce Interval to 500 and Index Debounce to 2.
    The G76 line is not correct it won't run it like that

    Mactec54


  18. #18
    Member
    Join Date
    Jun 2010
    Location
    Australia
    Posts
    4252
    Downloads
    4
    Uploads
    0

    Default Re: Mach3 Turn Feed Per Revolution problem

    Hi Mactec

    Ah - what is the matter with the g76 line?
    It runs on Mach on my desktop (simulation), with just one small problem. The minimum depth of cut H0.1 causes the number of passes to exceed the limit of 200 set in the 1076.m1s macro, so it halts before it is finished. But if I change it to H0.3 then it runs to completion OK.

    This probably does not solve the OP's problem though.

    Cheers
    Roger



  19. #19
    Member mactec54's Avatar
    Join Date
    Jan 2005
    Location
    USA
    Posts
    15362
    Downloads
    0
    Uploads
    0

    Default Re: Mach3 Turn Feed Per Revolution problem

    Try your program like this, fill in the blanks
    %
    G0G53X10Z10

    T0202 G99 G97 M03 S318

    G0______

    G0_______

    G76 P010060 Q0.020 R0.0200
    G76 X8.160 Z-10.000 P0.920 Q0.300 F1.500 R0.000 P1

    M30
    %

    Mactec54


  20. #20
    Member mactec54's Avatar
    Join Date
    Jan 2005
    Location
    USA
    Posts
    15362
    Downloads
    0
    Uploads
    0

    Default Re: Mach3 Turn Feed Per Revolution problem

    Quote Originally Posted by RCaffin View Post
    Hi Mactec

    Ah - what is the matter with the g76 line?
    It runs on Mach on my desktop (simulation), with just one small problem. The minimum depth of cut H0.1 causes the number of passes to exceed the limit of 200 set in the 1076.m1s macro, so it halts before it is finished. But if I change it to H0.3 then it runs to completion OK.

    This probably does not solve the OP's problem though.

    Cheers
    Roger
    If it is a single line G76 it should look like this

    G76 X8.160 Z-10.000 K0.920 D0.300 F1.500 I0 A60 P1

    Mactec54


Page 1 of 2 12 LastLast

Tags for this Thread

Posting Permissions

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


About CNCzone.com

    We are the largest and most active discussion forum for manufacturing industry. The site is 100% free to join and use, so join today!

Follow us on


Our Brands

Mach3 Turn Feed Per Revolution problem

Mach3 Turn Feed Per Revolution problem