How are people handling the lack of M00 Program Stop in PP - Page 2

Page 2 of 2 FirstFirst 12
Results 21 to 39 of 39

Thread: How are people handling the lack of M00 Program Stop in PP

  1. #21
    Member vmax549's Avatar
    Join Date
    Oct 2005
    Location
    Lady Lake
    Posts
    1145
    Downloads
    3
    Uploads
    0

    Default Re: How are people handling the lack of M00 Program Stop in PP

    HUM, so we can M01 run stop jog and resume along with M01 (message) and M01 (picture) and M01(document) and even M01(video). I guess that Tormach Path Pilot has it covered after all.

    (;-) TP



  2. #22

    Default Re: How are people handling the lack of M00 Program Stop in PP

    Having skimmed this thread to avoid wasting my time with the pissing match, now I'm confused. I would love to have the ability to jog the machine after a stop (m00 or m01, dont really care) as I have seen that done on my employer's Haas's. Is that really an option?



  3. #23
    Member vmax549's Avatar
    Join Date
    Oct 2005
    Location
    Lady Lake
    Posts
    1145
    Downloads
    3
    Uploads
    0

    Default Re: How are people handling the lack of M00 Program Stop in PP

    IT works here. at M01 press STOP then you can jog away and do what ever. When you are ready to return jog back close to the restart point , right click on the line AFTER the M01, the selected line will turn green and select restart with NO preparation. Then turn the spindle and coolant back on , next press CycleStart and you should be off and running. With the M01 you can also show a message to remind you why you stopped.

    M01(Check Tooling ) When the M01 runs it will display that message in the bottom of teh toolpath display . You can also display a picture M01(nameof pic.jpg) or even show a video M01(nameofvideo.mov) . Here I can also display a text file M01(name of text.txt) but that is not currently available in PP.

    Tormach is always looking for usefull functions to add to PathPilot . Yall really need to use the New function request page on the website. IF you don't ask for things you want/need you may NEVER get them. SPEAK UP they won't bite. THE worst they can say is NOPE. And so far hearing that has not hurt me or caused me to NOT eat a cheesburger for lunch........

    People were not bashfull of asking for things when Mach3 was king of the hill (;-). It is PathPilot's turn..

    (;-) TP



  4. #24
    Member mountaindew's Avatar
    Join Date
    Nov 2007
    Location
    earth
    Posts
    2151
    Downloads
    0
    Uploads
    0

    Default Re: How are people handling the lack of M00 Program Stop in PP

    Quote Originally Posted by popspipes View Post
    I use a .25 tool for roughing and a finish op for that reason, it will complete the roughing op and stop and wait for a tool change, the rough tool is say #10 and the finish tool is #11, its the same tool but does two different ops. I also use it for a stop to clean chips etc. before restarting.
    Might have to use this method on my lathe. Use same tool but different numbers between rough and finish. That way I can pull out birds nest if I have one. Dont know why I didn't think of this before ????. Simple and no extra tool setup. Just copy the tool offsets in table



  5. #25
    Member mountaindew's Avatar
    Join Date
    Nov 2007
    Location
    earth
    Posts
    2151
    Downloads
    0
    Uploads
    0

    Default Re: How are people handling the lack of M00 Program Stop in PP

    hi Vmax549
    The pictures I posted of parametric programs I often do, I mentioned I create a screen clip of each offset / setup in cam. I can then look at those to review how to fixture and position the part at each step. I use to include links in code to display them when you run program. Was cool to have it automatic. Any more I dont do the extra steps that requires and I just go to project location and load jpg's into viewer manually. Still I liked tormach added that option.
    The main idea is if I made another part days, weeks or months later all I had to do us look at setup clips. Load stock and run program. Super easy and no reason to go back to cam to look at what I did.



  6. #26
    Member popspipes's Avatar
    Join Date
    Jun 2014
    Location
    United States
    Posts
    1777
    Downloads
    0
    Uploads
    0

    Default Re: How are people handling the lack of M00 Program Stop in PP

    Hello MD

    I just number the same tool with a different number. The problem with this is that my rough op is mainly .130 deep so it takes two passes to rough the part, this wears the first .130 more than the upper .130 of the tool, this is more noticeable as the tool wears.
    I am thinking about just using a carbide cutter for finish alone or resharpen the flutes on the HSS cutter and learn to use wear in PP.

    This also helps with finding the tool if you just need to run from here the finish op etc.

    mike sr


  7. #27

    Default Re: How are people handling the lack of M00 Program Stop in PP

    Quote Originally Posted by vmax549 View Post
    IT works here. at M01 press STOP then you can jog away and do what ever. When you are ready to return jog back close to the restart point , right click on the line AFTER the M01, the selected line will turn green and select restart with NO preparation. Then turn the spindle and coolant back on , next press CycleStart and you should be off and running. With the M01 you can also show a message to remind you why you stopped.

    M01(Check Tooling ) When the M01 runs it will display that message in the bottom of teh toolpath display . You can also display a picture M01(nameof pic.jpg) or even show a video M01(nameofvideo.mov) . Here I can also display a text file M01(name of text.txt) but that is not currently available in PP.

    Tormach is always looking for usefull functions to add to PathPilot . Yall really need to use the New function request page on the website. IF you don't ask for things you want/need you may NEVER get them. SPEAK UP they won't bite. THE worst they can say is NOPE. And so far hearing that has not hurt me or caused me to NOT eat a cheesburger for lunch........

    People were not bashfull of asking for things when Mach3 was king of the hill (;-). It is PathPilot's turn..

    (;-) TP
    Ah, ok. I knew that process worked, there seemed to be some implication that it could be done without actually stopping the program and doing the manual RFH steps.



  8. #28
    Member vmax549's Avatar
    Join Date
    Oct 2005
    Location
    Lady Lake
    Posts
    1145
    Downloads
    3
    Uploads
    0

    Default Re: How are people handling the lack of M00 Program Stop in PP

    HI Soofle, No you cannot do it with the pathpilot version of M00 directly . It would work IF they changed a few lines of code in teh M00. But I don't think that will ever happen . I am working on a new button to automate the RSJC process in PathPilot. At M00, stop, then do whatever, to continue press the White button Prep your machine (spindle on, coolant ON) then press CycleStart . That is the way I have it working here . Just testing the white button more to make sure it does not OOPS in any odd machine conditions. I do know that if you are using INC mode gcode that the process changes slightly. You would need to add a G28.1 in front of teh M00 and a G28 after the M00 THEN it runs fine.

    IT would be nice to know if anyone else ever had a problem with RUN FROM HERE in PathPilot. OR is it rock stable ????

    (;-) TP



  9. #29
    Member vmax549's Avatar
    Join Date
    Oct 2005
    Location
    Lady Lake
    Posts
    1145
    Downloads
    3
    Uploads
    0

    Default Re: How are people handling the lack of M00 Program Stop in PP

    OK further testing reveils a flaw. As long as you do not use any offsetting in your Gcode it seems stable BUT the moment I introduced an offset things tend to fall apart (;-) I am talking G52 G92 G10 L2 G10 L20 . It seems that LinuxCNC does NOT reset the offsets at a M30 or STOP. At times they can become cumulative when you rerun the Gcode. LinuxCNC warns you about the problem in teh manual but no one fixed it from what I can see.

    OR it is an optical illusion with the toolpath display. Please use with Caution.

    Just a thought, (;-) TP



  10. #30
    Member machinehop5's Avatar
    Join Date
    Aug 2009
    Location
    United States
    Posts
    1567
    Downloads
    5
    Uploads
    2

    Default Re: How are people handling the lack of M00 Program Stop in PP

    ...very intrusting this thing CALL Mo



  11. #31
    Member mountaindew's Avatar
    Join Date
    Nov 2007
    Location
    earth
    Posts
    2151
    Downloads
    0
    Uploads
    0

    Default Re: How are people handling the lack of M00 Program Stop in PP

    Quote Originally Posted by vmax549 View Post
    OK further testing reveils a flaw. As long as you do not use any offsetting in your Gcode it seems stable BUT the moment I introduced an offset things tend to fall apart (;-) I am talking G52 G92 G10 L2 G10 L20 . It seems that LinuxCNC does NOT reset the offsets at a M30 or STOP. At times they can become cumulative when you rerun the Gcode. LinuxCNC warns you about the problem in teh manual but no one fixed it from what I can see.

    OR it is an optical illusion with the toolpath display. Please use with Caution.

    Just a thought, (;-) TP
    I guess maybe I dont understand what your trying to do or your style of programs!

    Whatever it is I hope they dont change the behavior of the "run from here" menu options much from the way they are now.
    I find it easy to use with confident results every time. By just stopping the program at predefined points then setting the rfh position at that point. Then repositioning stock, probing the new offset g54-g59x and continue running program from the predefined stopping point using the rfh menu options. Repeating this for each side or offset of the program until I get a finished part. At this point the machine has all the offsets located so all I have to do is reposition the stock for that offset and continue program and make parts. No stopping required after the first complete run of the program "it learned all the offset". This program format can also be run a number of different ways depending on strategy and need! Maybe just do one side for a pile of stock. then repeat for each side or offset until pile of stock is gone and you have a pile of completed parts. Or one at a time if your doing a short run. And or sorted by tool and offset or mix and match. The cam I use now has this type of workflow optimized and will generate code a couple of different ways.

    example of predefined stopping point

    (Set G58 Workspace 0 x,y,z pp)
    (Template Design by Me All rights reserved)
    N9120 G58 <<<<<<<<<<<<<<<<<< this line changes to reflect what offset is to be active
    N9130 T1 G43 H1 M6 <<<<<<<<<<<<<<<<<<<this sets my hamier probe tool so if required I can probe the new offset.
    N9140 M1 <<<<<<<<<<<<<<<<<<<<where I stop and start programs with rfh menu! My cam puts the same 3 lines of code at the start of each new offset or side of part for as many as I have programmed.

    (Roughing plane) <<<<<<<<<<<<<<<<<<<<Run from here then starts with this code when I start program again. Safe to use and works every time
    N9150 T8 G43 H8 M6
    (0.375 End Mill HSS 3 flute alumax)
    .



  12. #32
    Member vmax549's Avatar
    Join Date
    Oct 2005
    Location
    Lady Lake
    Posts
    1145
    Downloads
    3
    Uploads
    0

    Default Re: How are people handling the lack of M00 Program Stop in PP

    It would depend on how many and what type offsets you may have in your program. You just have to remember that Pathpilot does NOT clear offsets on a Stop ,M30, etc and it is possible for an offset to be additive in nature if it is not cleared. Then each time you run the same part in a row it works its way off the table. There are 2 main type of how controllers work. On a Haas you can select either the Haas way or the Fanuc way. The haas way is similar to PathPilot. The fanuc way is to auto clear offsets on stop.

    IF you are in for a kick try doing a RFH with INC programed Gcode or offsets . And there IS a lot of it out in the real world.

    I don't see Tormach changing anything with their RFH as it suites their purpose with CAM programming. Here I have a real button setup to run the RFH the way I see it needs to be. And so far it works great with everything I have thrown at it. But that is just my opinion. In cnc there is always a 100 different ways to setup and machine the same part.

    Here with PathPilot I also have a G31 , G68/69 G15/16 to work with that matches how the rest of the world does those functions. That keeps it simple to use already existing programs.

    (;-) TP

    Last edited by vmax549; 02-26-2022 at 10:15 AM.


  13. #33
    Member mountaindew's Avatar
    Join Date
    Nov 2007
    Location
    earth
    Posts
    2151
    Downloads
    0
    Uploads
    0

    Default Re: How are people handling the lack of M00 Program Stop in PP

    Quote Originally Posted by vmax549 View Post

    IF you are in for a kick try doing a RFH with INC programed Gcode or offsets . And there IS a lot of it out in the real world.

    (;-) TP
    My Tormach 24r router using the 24r sprutcam post for code behaves pretty much this way!
    Run from here for the most part does not work like the mill or as expected.

    It requires a different strategy to work best. All offsets need to be defined before starting. In this case you have say 12 pieces of stock in 12 fixture positions with 12 offsets. with 1-12 of the same or different parts. User needs to locate all 12 offsets first to get program to work best. This strategy also allows sorting by tool then offset. That way tool #8 can be used at all 12 offset locations and then tool 9 and so on until the program is finished. the cam software will sort and post code this way. no hand editing. Stopping the program to locate a offset and restarting does not work the same way as I mentioned in the above comment.

    To be honest, I found the only way to safely restart a 24r router program that had to be stopped and has run for hours is to go back to cam and create a new code file to start at the point i stopped it, at the machine or as close as possible. Restarting a program willy nilly after say the material moved or tool needed replacement is not easy because of the way the code is posted and formatted.

    Edit: Im guessing there are ways to do it but i have not mastered the process or method. I hate to trash material and crash machines. so I often use the safest possible method I can come up with.

    Also passing note: As long as the behavior is a machine standard then I see no reason not to use it in pp or any control bloatware!

    Last edited by mountaindew; 02-26-2022 at 11:06 AM.


  14. #34
    Member vmax549's Avatar
    Join Date
    Oct 2005
    Location
    Lady Lake
    Posts
    1145
    Downloads
    3
    Uploads
    0

    Default Re: How are people handling the lack of M00 Program Stop in PP

    IF you have a program I can try I would like to see IF anything I know will make it safe to restart. . I know how to restart INC code but not sure if it will work in your case.

    Here they have a couple of MOLD and PLUG routers that can run for days at a time. IF it OOPS about 12hours in it can be painfull to recover. ALSO from time to time they have to rebuild the plugs or molds so it NEEDS to be able to restart mid program.

    (;-) TP

    Last edited by vmax549; 02-26-2022 at 07:41 PM.


  15. #35
    Member vmax549's Avatar
    Join Date
    Oct 2005
    Location
    Lady Lake
    Posts
    1145
    Downloads
    3
    Uploads
    0

    Default Re: How are people handling the lack of M00 Program Stop in PP

    OK Guys , I have a RSJC (run, stop. jog away. return continue) button working just like the way the HAAS JSRC button does it. Running gcode feedhold, stop, jog away and do what ever. Then move back close to the restart point , press F5 turn back on Spindle,Coolant,etc Press CYCLESTART and away it goes. It goes BACK to the beginning of the block you stopped on LOWERS down to the Zpos and restarts motion.

    AND there was not a mouse harmed in the use of this function as it is a MOUSE FREE function (;-)

    It works here but your mileage may vary due to local conditions. (;-)

    (;-)TP

    Last edited by vmax549; 03-03-2022 at 11:43 AM.


  16. #36
    Member kstrauss's Avatar
    Join Date
    Apr 2013
    Location
    Canada
    Posts
    1788
    Downloads
    0
    Uploads
    0

    Default Re: How are people handling the lack of M00 Program Stop in PP

    Will you post the necessary changes? Does your enhancement survive PP updates?

    - - - Updated - - -

    Does your enhancement survive PP updates? Will you post the necessary changes?



  17. #37
    Member vmax549's Avatar
    Join Date
    Oct 2005
    Location
    Lady Lake
    Posts
    1145
    Downloads
    3
    Uploads
    0

    Default Re: How are people handling the lack of M00 Program Stop in PP

    Well here is the situation. IF I publish the code and you install it AND it crashes your system you will be mad at me. THEN if you call Tormach for help THEY will be mad at you for hacking the system and ME for giving you the code. And it does give them cause to deny you support for ever. When you hack PP it makes it almost impossible for them to trouble shoot it because they have NO idea what you have done. They WILL know you have been inside the code because PP will tell on you. The files are check sumed and IF you so much as change one dot or tidle they will know about it. It tells them in the report you send in for support. ALSO PP if it gets the chance DOES call home and asks mom what's for supper if you get my drift. There is code in there now that may change how PP is used. But that is for them to disclose not me.

    IF you guys WANT these functions simply ASK tormach for them. Heck that function only took 12 lines of code added in the correct spot. IF needed I can show them how I did it. THEY know my email address or it is IN the profile (;-)

    SO no I will not publish any PP internal hacking code on the web. (;-) TP

    NOW whith all that said IF you want to do it without using the MOUSE run feedhold jog away get close and from the MDI type

    SET START linenumber you want to restart from PLUNGE . Then turn the spindle and coolant back on and then press CYCLESTART. NOTE: the uppercase MUST be uppercase in the MDI line.

    I just automated all that into a F5 button press (;-).and my button knows if you stopped on a M0/M1 or did a feedhold stop. Also it knows HOW to deal with INC gcode.

    Last edited by vmax549; 03-03-2022 at 09:53 PM.


  18. #38
    Member kstrauss's Avatar
    Join Date
    Apr 2013
    Location
    Canada
    Posts
    1788
    Downloads
    0
    Uploads
    0

    Default Re: How are people handling the lack of M00 Program Stop in PP

    Vmax549, I understand your concerns and obviously sharing is your choice. If we report an issue to Tormach it is unreasonable to expect their help on other than a virgin system. That said, it is better for everyone if we share our insights instead of each of us having to independently improve things. Don't forget that PP is open source!



  19. #39
    Member mountaindew's Avatar
    Join Date
    Nov 2007
    Location
    earth
    Posts
    2151
    Downloads
    0
    Uploads
    0

    Default Re: How are people handling the lack of M00 Program Stop in PP

    Quote Originally Posted by mountaindew View Post
    My Tormach 24r router using the 24r sprutcam post for code behaves pretty much this way!
    Run from here for the most part does not work like the mill or as expected.

    It requires a different strategy to work best. All offsets need to be defined before starting. In this case you have say 12 pieces of stock in 12 fixture positions with 12 offsets. with 1-12 of the same or different parts. User needs to locate all 12 offsets first to get program to work best. This strategy also allows sorting by tool then offset. That way tool #8 can be used at all 12 offset locations and then tool 9 and so on until the program is finished. the cam software will sort and post code this way. no hand editing. Stopping the program to locate a offset and restarting does not work the same way as I mentioned in the above comment.

    To be honest, I found the only way to safely restart a 24r router program that had to be stopped and has run for hours is to go back to cam and create a new code file to start at the point i stopped it, at the machine or as close as possible. Restarting a program willy nilly after say the material moved or tool needed replacement is not easy because of the way the code is posted and formatted.

    Edit: Im guessing there are ways to do it but i have not mastered the process or method. I hate to trash material and crash machines. so I often use the safest possible method I can come up with.

    Also passing note: As long as the behavior is a machine standard then I see no reason not to use it in pp or any control bloatware!
    After taking the time and testing a number of different reasons and methods for using the run from here command. I found it works very well and as expected!
    Not clear if something has changed from when I had the problem I mention above or what I was doing wrong before when I run into this problem on a router project.
    In short it works very well as is! I could do just about anything I wanted and as long as I found the highlighted line of code I stopped on and set the run from here with the appropriate choice the machine takes off and goes to the correct position and engages tool and completes the program. What ever problem I run into before that I remember creating a second code file for is no longer a problem.

    I keep thinking it was a Sprutcam code format problem, but I could not recreate the problem during any testing. So its good to go and 2tu or two thumbs up!



Page 2 of 2 FirstFirst 12

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

How are people handling the lack of M00 Program Stop in PP

How are people handling the lack of M00 Program Stop in PP