502,512 active members
4,705 visitors online
Register for free
Login
Page 1 of 2 12
Results 1 to 12 of 14
  1. #1
    Junior Member
    Join Date
    Jun 2014
    Posts
    1462

    Does Path Pilot support G64?

    On the parts I run the cutter seems to stop at certain points in an arc, this leaves a mark in the finish, the feedrates seem to vary a lot, I didnt notice this so much in Mach 3.

    I am wondering if I need to specify a G64 to run in constant velocity mode?

    any info on this would be appreciated.

    thanks
    mike sr

  2. #2
    Registered
    Join Date
    Dec 2008
    Posts
    626

    Re: Does Path Pilot support G64?

    Hello Mike
    I'm experiencing what sounds to be the same issue. I' in the middle of writing an e-mail to Tormach but I can't get around to remaking some screenshots...
    I haven't detected any issues on circular cuts but on compound curves the travel stops between curve segments - maybe PP has problems when the radius changes? I checked all the values prior to, and after the Sprutcam post and found nothing other than small rounding errors in the least significant position (which I hope PP can cope with).
    Presumably you're generating the code with Sprut so the first line of G-code should look something like mine:
    N10 G90 G64 G50 G54 G80 G17 G40 G49
    G64 is included but it isn't performing as I would expect. I played around with the blending tolerance values and found that a value of P0 worked wonders. This surprised me because the LinuxCNC docu implies (presuming I'm understanding it correctly) that this is only retained for backwards compatibility and should be the same as without the P option.
    Try G64 P0 and let me know if your issue improves.
    Regards
    Step

  3. #3
    Junior Member
    Join Date
    Jun 2014
    Posts
    1462

    Re: Does Path Pilot support G64?

    Step,
    I tried to take a pic of the anomaly, that takes a bit of doing as well ha! I use Rhino for CAD and Sprut for CAMhave for a few years, 7 for CAM, the latest version, and have been using both for a few years now, so I dont think its in the cad/cam software.

    I can see the anomaly with the naked eye in two different ops, both 2d contour, these appear at four different points on the contour. Watching the feedrate window, it is not constant or even close to it, and appears to stop momentarily at certain points during the cut.
    I use the tangent and arc functions in Sprut, so it isnt that but appears similar in the finished parts.
    I am using a fixture that holds 4 parts and the anomaly is in the exact same places on all the parts.

    This doesnt affect the functionality of the parts,its just cosmetic.


    I will try the G64 P0 in the program line and see if that has an effect on the blemish, thanks for the tip!

    Attachment 301156Attachment 301158
    mike sr

  4. #4
    Registered
    Join Date
    Jul 2003
    Posts
    1670

    Re: Does Path Pilot support G64?

    If I understand it correctly the pathpilot tolerance for path following defaults to something like .005". So setting G64P0 effectively (I don't have a system up to test at the moment so going by memory) tells linuxcnc to go as fast as it can while touching every segment.

    Could you post an example of your program?

  5. #5
    Junior Member
    Join Date
    Jun 2014
    Posts
    1462

    Re: Does Path Pilot support G64?

    Samco,

    I have the .tap file for the parts, but it is rather lengthy, I could try to post that, but I think it is too large for the forum attachments.

    Maybe post a snip of the first few lines??
    mike sr

  6. #6
    Registered
    Join Date
    Jul 2003
    Posts
    1670

    Re: Does Path Pilot support G64?

    where it is pausing would be great.

    sam

  7. #7
    Registered
    Join Date
    Dec 2008
    Posts
    626

    Re: Does Path Pilot support G64?

    Quote Originally Posted by samco View Post
    If I understand it correctly the pathpilot tolerance for path following defaults to something like .005". So setting G64P0 effectively (I don't have a system up to test at the moment so going by memory) tells linuxcnc to go as fast as it can while touching every segment.
    A quote from the LinuxCNC pages- is this perhaps outdated or are Tormach implementing this differently?

    G64 - (Blend Without Tolerance Mode) G64 is the default setting when you start LinuxCNC. G64 is just blending and the naive cam detector is not enabled. G64 and G64 P0 tell the planner to sacrifice path following accuracy in order to keep the feed rate up. This is necessary for some types of material or tooling where exact stops are harmful, and can work great as long as the programmer is careful to keep in mind that the tool’s path will be somewhat more curvy than the program specifies. When using G0 (rapid) moves with G64 use caution on clearance moves and allow enough distance to clear obstacles based on the acceleration capabilities of your machine.

    Step

  8. #8
    Junior Member
    Join Date
    Jun 2014
    Posts
    1462

    Re: Does Path Pilot support G64?

    Quote Originally Posted by samco View Post
    where it is pausing would be great.

    sam
    It happens on most all 2d contour curves and waterline finishing ops, when the cutter slows down it leaves a blemish in the finish.

    I am no whiz on G code, so I will work on eliminating all the ops except the ones in question. I think if there was a constant velocity setting it would fix the problem, the accuracy may suffer but cosmetically it would be better.
    mike sr

  9. #9
    Registered
    Join Date
    Dec 2008
    Posts
    626

    Re: Does Path Pilot support G64?

    Quote Originally Posted by samco View Post
    Could you post an example of your program?
    Here's a snippet of the code that I used :
    Code:
    %
    OPlug_V2
    
    (Tool) (23) (Diameter)(9.525) (3/8  3Fl Rougher 25L/32 Maritool) (Operation) (Roughing waterline)
    
    N10 G90 G64 G50 G54 G80 G17 G40 G49
    N20 G21 (Metric)
    (Roughing waterline)
    N30 M998
    N40 T23 G43 H23 M6
    (3/8  3Fl Rougher 25L/32 Maritool)
    N50 S5000 M3 M8
    N60 G0 G94 X-20.444 Y-0.062 Z6.
    N70 Z4.
    N80 Z0.5
    N90 G1 X-19.844 F1000.
    N100 G3 X-19.297 Y0.166 Z0.5 I-0.156 J1.146
    N110 X-18.003 Y1.816 Z0.5 I-7.684 J7.358
    N120 G1 X-17.421 Y2.75
    N130 X-15.622 Y5.868
    N140 G2 X-12.575 Y10.071 Z0.5 I23.125 J-13.562
    N150 X-5.905 Y14.715 Z0.5 I13.197 J-11.842
    N160 X10.332 Y11.961 Z0.5 I5.826 J-14.896
    N170 X6.381 Y-14.452 Z0.5 I-10.351 J-11.954
    N180 X-14.147 Y-7.016 Z0.5 I-6.369 J14.472
    N190 X-14.565 Y-4.871 Z0.5 I5.093 J2.105
    N200 X-14.169 Y-1.904 Z0.5 I13.153 J-0.245
    N210 X-10.825 Y5.312 Z0.5 I20.625 J-5.174
    N220 X-5.827 Y9.69 Z0.5 I12.065 J-8.732
    N230 X2.525 Y10.73 Z0.5 I5.562 J-10.611
    N240 X10.957 Y0.109 Z0.5 I-2.622 J-10.74
    N250 X6.945 Y-8.482 Z0.5 I-11.041 J-0.076
    N260 X-6.678 Y-8.668 Z0.5 I-6.928 J8.497
    N270 X-8.324 Y-6.444 Z0.5 I3.246 J4.124
    N280 X-8.842 Y-3.608 Z0.5 I7.129 J2.768
    N290 X-8.576 Y-1.33 Z0.5 I9.118 J0.087
    N300 X-7.571 Y0.497 Z0.5 I4.747 J-1.421
    N310 X-6.218 Y1.968 Z0.5 I22.255 J-19.117
    N320 X-4.83 Y3.111 Z0.5 I11.019 J-11.968
    N330 X-2.775 Y4.133 Z0.5 I5.477 J-8.43
    N340 X-0.609 Y4.424 Z0.5 I1.826 J-5.379
    N350 X0.661 Y4.156 Z0.5 I-1.071 J-8.212
    N360 X2.886 Y2.517 Z0.5 I-1.731 J-4.678
    N370 X3.642 Y0.174 Z0.5 I-3.38 J-2.384
    N380 X3.243 Y-1.366 Z0.5 I-4.336 J0.301
    N390 X0.547 Y-3.223 Z0.5 I-3.151 J1.69
    N400 G0 Z15.525
    N410 M5 M9
    
    N1250 M998
    N1260 M30
    %
    The following image was taken shortly after a feed discontinuity. The path at this point looks quite round. The Halscope shows the x axis velocity and the disturbance is clear to see. Adding G64 P0 reduces this disturbance to just a small "blip".
    Attachment 301296

    Step

  10. #10
    Junior Member
    Join Date
    Jun 2014
    Posts
    1462

    Re: Does Path Pilot support G64?

    Hello Step,

    Where do you put the G64 P0? My code has a G64 in it already from Sprutcam, but I am wondering if Pathpilot recognizes it or just ignores it?

    If I were to add the G64 P0 command, should it be entered on the MDI line or edited into the .tap file?

    The reason I ask is that I have tapping cycles in other programs written in sprut 7 that throw a caution on the P0 command, and it says that it will be ignored.
    mike sr

  11. #11
    Junior Member
    Join Date
    Jun 2014
    Posts
    1462

    Re: Does Path Pilot support G64?

    I tried the G64 P0 edited into the first line of the program, it ran fine and seemed to be more constant on the feedrate, may be wishful thinking, mind over matter, or whatever, but it seemed to work better.

    I have some long contours coming up, that was a problem with the cutter stopping during the cut, I will see if it helps there.

    It was also making anomalys in my waterline finishing ops in one section, they were hard to see unless you were looking for them.

    Hopefully the G64 P0 will cure the problem, or maybe it will be changed in later updates of PathPilot, it has a few rough edges yet but it hasnt made an unprogrammed move yet and thats a very good thing!!!
    mike sr

  12. #12
    Registered
    Join Date
    Dec 2008
    Posts
    626

    Re: Does Path Pilot support G64?

    Quote Originally Posted by popspipes View Post
    I tried the G64 P0 edited into the first line of the program, it ran fine and seemed to be more constant on the feedrate, may be wishful thinking, mind over matter, or whatever, but it seemed to work better.

    I have some long contours coming up, that was a problem with the cutter stopping during the cut, I will see if it helps there.

    It was also making anomalys in my waterline finishing ops in one section, they were hard to see unless you were looking for them.

    Hopefully the G64 P0 will cure the problem, or maybe it will be changed in later updates of PathPilot, it has a few rough edges yet but it hasnt made an unprogrammed move yet and thats a very good thing!!!
    Hi Mike, sorry for not getting back to you, I've been "out of action" for a while...
    The G64 was discussed some time ago on this forum but for just the opposite reason:
    http://www.cnczone.com/forums/tormac...ml#post1662938
    I thought perhaps Tormach had since modified the G64 behaviour (without a P parameter) to be more like G64 P0.005 as "samco" indicated above, so I ran a test with a fresh installation of PathPilot V1.4, the earliest version I have, to see if the behavior was originally different but my test code showed the exact same behaviour. Shred did however point out that he was using an early Beta version so perhaps something was changed prior to V1.4.
    This is not how I expect G64 to behave per default (but then I'm no G-Code expert). I can see the advantages of both variants but I don't want the feed to stop unexpectedly for several reasons - not only does the finish suffer but the chipload drops briefly to almost zero during roughing ops!
    It would be interesting to find out how Mach3 compares when running the same code but I don't have time to play with Mach again.
    Sorry, not much help - perhaps we should raise an issue with Tomach and reference this thread (I'm sure they read them all anyway - I know I would!).
    Step

Page 1 of 2 12

Similar Threads

  1. Networking Path Pilot
    By RA-Bowtie in forum Tormach PathPilot™
    Replies: 6
    Last Post: 12-29-2015, 05:39 PM
  2. What comes with Tormach's path pilot?
    By 1abrat in forum Tormach PathPilot™
    Replies: 7
    Last Post: 11-26-2015, 08:23 PM
  3. --Unlocking Path Pilot--
    By Jim Anderson in forum Tormach PathPilot™
    Replies: 7
    Last Post: 09-19-2015, 04:32 PM
  4. Path Pilot - wish list
    By RA-Bowtie in forum Tormach PathPilot™
    Replies: 34
    Last Post: 07-13-2015, 12:12 AM
  5. Path Pilot Sub Routine
    By csm-Guy in forum Tormach PathPilot™
    Replies: 5
    Last Post: 04-08-2015, 05:23 PM

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
  •