----- Original Message -----

From: Tom Kerekes

To: DynoMotion@yahoogroups.com

Sent: Monday, November 25, 2013 6:04 PM

Subject: Re: [DynoMotion] Thread cutting issue w/ Mach3?

 

Hi Tapio,

What do you mean by "multiple starts?"

Regards
TK

Group: DynoMotion	Message: 8731	From: Tapio Larikka	Date: 11/26/2013
Subject: Thread cutting issue w/ Mach3?

 Hi Tom!   I'm still lost with my threading.   Editing the mach G76 did not help. Rollback from KMotion4.31c to 4.30 did not help   After changing the gcode to 4 consecutive lines of G32 I was able to verify that first two passes cut OK third pass starts off sync. Measuring the starting/return point gives no errors.   I have my machine set up so that spindle and A-axis are the same. encoder is 3600 pulses/14400 counts/rev Homing A to encoder index and and commanding a move of 14400 counts(1 rev) brings the axis/spindle precisely on the index mark.   For some reason, with mach pulley ratio set to 1 and SpindleMach3Jog.c factor set to 216000, the mach true rpm reports 10% smaller rpm(S300->trpm270)    I'll try to connect a second encoder in order to find out if there is a difference in pulse count on longer run which I doubt very much since even after hours of running the spindle a "G0 A0" command will bring the axis on the index mark.     I have pretty much done everything I can think of.   Do you, or anyone else, have any idea what to try next?   Is there any convinient way to change the thread timing to follow the index pulse?   Rgds, Tapio       ----- Original Message ----- From: Tapio Larikka To: DynoMotion@yahoogroups.com Sent: Monday, November 25, 2013 7:53 PM Subject: Re: [DynoMotion] Thread cutting issue w/ Mach3? Hi Tom!   By "multiple starts" I mean that thread starting point changes. First five passes cut on the spot but then I get passes that off sync, messing up the thread. While searching thru mach forum I found this http://www.machsupport.com/forum/index.php/topic,23999.30.html where this caught my eye: "The code generated from the Simple Threading Wizard ( M1076 configured for G32 output ) always had double G32's as shown in the format below. Use it whenever I do threading, never questioned the double G32's, but then, never had a problem when using it. (Decrement = 0.005 pass 1) G01 Z0 G32 X0.245 Z-0.0014 F0.025 G32 X0.245 Z-0.9969 F0.025 G01 X6.25 Z-1 F0.025 G00 X6.25 Z0 G00 X0.25 " I didn't have time to check the code but the cut looks a lot like the above would produce.   Rgds, Tapio     ----- Original Message ----- From: Tom Kerekes To: DynoMotion@yahoogroups.com Sent: Monday, November 25, 2013 6:04 PM Subject: Re: [DynoMotion] Thread cutting issue w/ Mach3?   Hi Tapio, What do you mean by "multiple starts?" Regards TK Group: DynoMotion Message: 8737 From: Tom Kerekes Date: 11/26/2013 Subject: Re: Thread cutting issue w/ Mach3? Hi Tapio, What do you have for your Mach3 | Config  Dynomotion Plugin | Spindle Settings set as? Regards TK Group: DynoMotion Message: 8738 From: tapiolarikka Date: 11/27/2013 Subject: Re: Thread cutting issue w/ Mach3? Hi Tom, I have the plugin spinde config as follows: Thread: 2 Variables: 0 Sensor:1 Axis:3 Counts/Rev: 14400 Tau: 0.1 Update: 0.2 I also still have the odd persisting problem I mentioned in one earlier thread/posting that I have to set the Mitsubishi servo drive to put out 4400 pulses(17600counts)/rev so that Kflop receives the expected 14400counts/rev and the axis stays on target. Rgds, Tapio ---In DynoMotion@yahoogroups.com, <tk@...> wrote: Hi Tapio, What do you have for your Mach3 | Config  Dynomotion Plugin | Spindle Settings set as? Regards TK Group: DynoMotion Message: 8742 From: Tom Kerekes Date: 11/27/2013 Subject: Re: Thread cutting issue w/ Mach3? Hi Tapio, What do you have for the Mach3 Pulley Speed for the Pulley you have selected? I don't understand what you would set the drive for 4400 pulses/rev.  Why would you do this? There is a Mach3 option called something like Spindle Averaging.  Please disable that. Regards TK Group: DynoMotion Message: 8743 From: Tapio Larikka Date: 11/27/2013 Subject: Re: Thread cutting issue w/ Mach3?  Hi Tom,   Mach pulley speed is 1000rpm, pulley ratio 1.   I'll have to re-check the spindle speed averaging, and pid and closed loop settings in mach tomorrow but I'm fairly sure they ar disabled.   I'll have to set the drive to put out 4400ppr for KFlop to read 3600ppr/14400 counts/rev. 800ppr gets lost on the way. Also, when commanding spindle speed 300 from mach, KFlop receives message 0.300 but with factor 216000 in SpindleMach3jog.c the true spindle speed reports 270rpm. I have the factor set so that truerpm is equal to commad.   I haven't yet been able to find anyone familiar enough with Mitsubishi mr-j2 drives who could tell where to look for cause and cure for this. This is why I started today with installing a second encoder on the spindle. I want to see if there is any difference in counts per rev. Driving the servo with +/-10V there should not be any issue af drive doing gearing. the drive goes up to full 1000rpm when requested.   Rgds, Tapio       ----- Original Message ----- From: Tom Kerekes To: DynoMotion@yahoogroups.com Sent: Wednesday, November 27, 2013 7:27 PM Subject: Re: Re: [DynoMotion] Thread cutting issue w/ Mach3?   Hi Tapio, What do you have for the Mach3 Pulley Speed for the Pulley you have selected? I don't understand what you would set the drive for 4400 pulses/rev.  Why would you do this? There is a Mach3 option called something like Spindle Averaging.  Please disable that. Regards TK Group: DynoMotion Message: 8745 From: Tom Kerekes Date: 11/27/2013 Subject: Re: Thread cutting issue w/ Mach3? Hi Tapio, With a Max Pulley Speed of 1000 RPM the Factor in SpindleMach3Jog.c should be: 1000 / 60 x 14400 = 240000 not 216000 Regards TK Group: DynoMotion Message: 8748 From: tapiolarikka Date: 11/28/2013 Subject: Re: Thread cutting issue w/ Mach3? Hi Tom, The spindle speed averaging is/was disabled. so that is not the cause. I set the factor to 240000. It is close to what I had, but made no difference in cutting the thread. cut starts 4 pitches from stock. I tried cutting/scribing single passes homing, the spindle in between. cutting speed is 300rpm. homing hits constantly on the index pulse but the threading passes do not align. mach version is 3.042.040 Rgds, Tapio ---In DynoMotion@yahoogroups.com, <tk@...> wrote: Hi Tapio, With a Max Pulley Speed of 1000 RPM the Factor in SpindleMach3Jog.c should be: 1000 / 60 x 14400 = 240000 not 216000 Regards TK Group: DynoMotion Message: 8749 From: TK Date: 11/28/2013 Subject: Re: Thread cutting issue w/ Mach3? Hi Tapio, Did the 240000 factor make the commanded speed correct? After each threading pass stop the spindle and move to the closest multiple of 14400 counts. You can determine this by taking the current spindle encoder count, divide by 14400,  make it an integer, multiply by 14400,  move there. Is the spindle at home every time? Regards TK On Nov 28, 2013, at 5:27 AM, <tapio.larikka@...> wrote:   Hi Tom, The spindle speed averaging is/was disabled. so that is not the cause. I set the factor to 240000. It is close to what I had, but made no difference in cutting the thread. cut starts 4 pitches from stock. I tried cutting/scribing single passes homing, the spindle in between. cutting speed is 300rpm. homing hits constantly on the index pulse but the threading passes do not align. mach version is 3.042.040 Rgds, Tapio ---In DynoMotion@yahoogroups.com, <tk@...> wrote: Hi Tapio, With a Max Pulley Speed of 1000 RPM the Factor in SpindleMach3Jog.c should be: 1000 / 60 x 14400 = 240000 not 216000 Regards TK Group: DynoMotion Message: 8750 From: tapiolarikka Date: 11/28/2013 Subject: Re: Thread cutting issue w/ Mach3? Hi Tom, Yes, teh factor 240000 sets the trpm equal to commanded speed. I also checked the speed with a rev gauge and it is correct. I added int gohome=0; gohome=ch3->position/14400; MoveAtVel(A,gohome*14400,500); to my homing program under flag 16 (B axis) so that I can execute it with mach ref B button. starting with homing A/Spindle I cut 8 single passes of equal diameter and executed refB between each pass. Spindle stops every time on the index pulse, input bit 41 either on, blinking or turns on when manually turning spindle by what Kflop reports 1/2 to 1 count. Last pass&gohome ended to 17150400 counts= 1191 revs total. Second pass landed app half rev off the first and consecutive passes seemingly randomly around the perimeter. I'll try to get the second encoder (160cpr) working tomorrow to see if it makes any difference but I don't have very high hopes on that. If that does not work out the last thing I can try is to change the KFlop/Kanalog combo to the other I received end of September Rgds, Tapio ---In DynoMotion@yahoogroups.com, <tk@...> wrote: Hi Tapio, Did the 240000 factor make the commanded speed correct? After each threading pass stop the spindle and move to the closest multiple of 14400 counts. You can determine this by taking the current spindle encoder count, divide by 14400,  make it an integer, multiply by 14400,  move there. Is the spindle at home every time? Regards TK On Nov 28, 2013, at 5:27 AM, <tapio.larikka@...> wrote:   Hi Tom, The spindle speed averaging is/was disabled. so that is not the cause. I set the factor to 240000. It is close to what I had, but made no difference in cutting the thread. cut starts 4 pitches from stock. I tried cutting/scribing single passes homing, the spindle in between. cutting speed is 300rpm. homing hits constantly on the index pulse but the threading passes do not align. mach version is 3.042.040 Rgds, Tapio ---In DynoMotion@yahoogroups.com, <tk@...> wrote: Hi Tapio, With a Max Pulley Speed of 1000 RPM the Factor in SpindleMach3Jog.c should be: 1000 / 60 x 14400 = 240000 not 216000 Regards TK Group: DynoMotion Message: 8751 From: Tom Kerekes Date: 11/28/2013 Subject: Re: Thread cutting issue w/ Mach3? Hi Tapio, I'm not sure I understand what you are describing. I think you are saying that you cut 8 passes.  After each pass the RefB test (very clever) showed the encoder worked perfectly, no loss of counts, and the index was always at exactly the same 14400 multiple.  But the physical thread cut was random, starting at random spindle angles.  Is this correct? You do have the Mach3 "Use Spindle Feedback in Sync Modes" Selected - Correct? Your GCode didn't seem to have a G95 to select feed rate in units/rev.  Please add this. Please perform a sanity check by extreme slowing or stopping of the spindle while thread cutting.  Does the Z motion slow accordingly? I doubt if it could be a hardware or encoder problem if the RefB test works perfectly. Regards TK Group: DynoMotion Message: 8752 From: Tapio Larikka Date: 11/28/2013 Subject: Re: Thread cutting issue w/ Mach3?  Hi Tom,   Yes, that i what I mean.   The G95 is there I posted just the effective part of the code.   The Mach3 "Use Spindle Feedback in Sync Modes" however is not selected :-( When I originally deselected the "Spindle speed averaging" on converting from parport to Kflop I disabled all 3 items in this group. So these "Special functions" should be: "Use Spindle Feedback in Sync Modes"  - enabled "Closed Loop Spindle Control" - disabled "spindle speed averaging" - disabled   I'll test this tomorrow morning and let you know what happens :-(?   Rgds, Tapio     ----- Original Message ----- From: Tom Kerekes To: DynoMotion@yahoogroups.com Sent: Thursday, November 28, 2013 6:49 PM Subject: Re: Re: [DynoMotion] Thread cutting issue w/ Mach3?   Hi Tapio, I'm not sure I understand what you are describing. I think you are saying that you cut 8 passes.  After each pass the RefB test (very clever) showed the encoder worked perfectly, no loss of counts, and the index was always at exactly the same 14400 multiple.  But the physical thread cut was random, starting at random spindle angles.  Is this correct? You do have the Mach3 "Use Spindle Feedback in Sync Modes" Selected - Correct? Your GCode didn't seem to have a G95 to select feed rate in units/rev.  Please add this. Please perform a sanity check by extreme slowing or stopping of the spindle while thread cutting.  Does the Z motion slow accordingly? I doubt if it could be a hardware or encoder problem if the RefB test works perfectly. Regards TK Group: DynoMotion Message: 8753 From: Tapio Larikka Date: 11/29/2013 Subject: Re: Thread cutting issue w/ Mach3?  Hi Tom,   I finally got the thread cutting to work this morning. It turned out to be as easy as enabling the spindle feedback.   thank you for your time and patience again.   Rgds, Tapio     ----- Original Message ----- From: Tom Kerekes To: DynoMotion@yahoogroups.com Sent: Thursday, November 28, 2013 6:49 PM Subject: Re: Re: [DynoMotion] Thread cutting issue w/ Mach3?   Hi Tapio, I'm not sure I understand what you are describing. I think you are saying that you cut 8 passes.  After each pass the RefB test (very clever) showed the encoder worked perfectly, no loss of counts, and the index was always at exactly the same 14400 multiple.  But the physical thread cut was random, starting at random spindle angles.  Is this correct? You do have the Mach3 "Use Spindle Feedback in Sync Modes" Selected - Correct? Your GCode didn't seem to have a G95 to select feed rate in units/rev.  Please add this. Please perform a sanity check by extreme slowing or stopping of the spindle while thread cutting.  Does the Z motion slow accordingly? I doubt if it could be a hardware or encoder problem if the RefB test works perfectly. Regards TK