. .
Page 2 of 4 FirstFirst 1234 LastLast
  1. #11
    Got you.
    I home left ! (obviously)

  2. #12
    Like Doddy I'm using LinuxCNC so cannot comment on how you set up UCCNC but my limit switches are set to be at X and Y = (-15, -15). The spindle then moves to (0, 0) with soft limits set to (-10, -10). This gives 5mm of deceleration space between the soft limit and the switches to avoid an accidental switch activation which will disable the motor drivers and un-calibrate the machine and also allows space for the spindle to move into negative values which it will need to do if you want to do an external profile of an object that touches X or Y = 0 using any tool with a diameter greater than 0.0mm.

    This arrangement makes it easier to use fixed guides along the X=0 and Y=0 axes which will put your stock in a position which often needs the spindle to go into 'negative' space.

    Kit
    Last edited by Kitwn; 29-07-2020 at 07:41 AM.
    An optimist says the glass is half full, a pessimist says the glass is half empty, an engineer says you're using the wrong sized glass.

  3. #13
    I suppose we all have differences in the way we need to set up . I had not considered this when I originally posted . And it is not surprising that the woodcarvers have different needs to The Heavy metal brigade
    Mine is a milling machine of course.

    And it had not occurred to me either that having a profiling tool run past zero (obvious once pointed out) could be useful in milling an external profile too, but I suppose that applying an offset overcomes that need.

    My next need is to allow for a touch of backlash on my Z motion . Its not much but I would like to figure out how to apply it .
    I have ball-screws on X and Y but for my Z axis I am driving the quill through mechanical gears with a 6/1 reduction. As I say it is not a massive amount as there is little wear but If I understand how to cater for it it will assist my next project.

  4. #14
    Quote Originally Posted by John11668 View Post
    I suppose we all have differences in the way we need to set up . I had not considered this when I originally posted . And it is not surprising that the woodcarvers have different needs to The Heavy metal brigade
    Mine is a milling machine of course.

    And it had not occurred to me either that having a profiling tool run past zero (obvious once pointed out) could be useful in milling an external profile too, but I suppose that applying an offset overcomes that need.

    My next need is to allow for a touch of backlash on my Z motion . Its not much but I would like to figure out how to apply it .
    I have ball-screws on X and Y but for my Z axis I am driving the quill through mechanical gears with a 6/1 reduction. As I say it is not a massive amount as there is little wear but If I understand how to cater for it it will assist my next project.
    Will backlash be a problem in Z as I would have thought the weight of the spindle would always keep the tool at the lowest position possible thereby eliminating backlash?

  5. I'm a bit concerned that anyone thinks that "going past zero" is in any way relevant when you are using Mach3/UCCNC. Maybe in the days of archaic controllers that did not have any homing/work offset capability this might have mattered but not today.

    The point here is that homing sets machine zero, either directly by putting home switches at the zero point, or somewhere else with an appropriate offset (at the right-hand end of travel, in the most extreme case). But that is absolutely nothing to do with where the zero point is on the work. First thing you do when you plonk the stock on the bed and clamp (assuming that you have already homed the machine) is to move the spindle to where you want (0,0) to be, and then set "work coordinate zero" to that point. Maybe x and y at the same time, maybe separately. Effectively you are doing the same thing when you set tool height - this is setting z coordinate zero, indirectly. Your gcode will, if generated by any modern CAM package, be working in terms of work coordinates. Nothing at all to do with machine coordinates. For example, recently, I have been machining work where the X zero work coordinate is at the right hand side and most of the machining is done with negative X coordinates. I told my CAM software where I wanted X=0, set the spindle to the RH edge of the stock and set work coord X to zero, and away it all went.

    This machine/work coordinate confusion is a bit complicated to follow at first sight but it soon becomes second nature and you won't even think about it, but it is absolutely critical to using CAM and the machine in harmony. I sorry if I have misunderstood what was being said, but the idea that you need to set machine zero somewhere on to the bed just so that you can move to negative coordinates could be very misleading to anyone new coming to this.

  6. #16
    Quote Originally Posted by ngwagwa View Post
    Will backlash be a problem in Z as I would have thought the weight of the spindle would always keep the tool at the lowest position possible thereby eliminating backlash?
    The quill has a return spring , a bit like a pedestal drill but in an exercise the cutting depth is often increasing so backlash wont be a problem there. But lots of exercises where the quill is being driven up and down frequently so lost motion in each direction in that case . I am presuming if you enter a backlash figure , then a number of steps will be discounted before the Display registers movement. Is that so?

  7. #17
    Quote Originally Posted by Neale View Post
    I'm a bit concerned that anyone thinks that "going past zero" is in any way relevant when you are using Mach3/UCCNC. Maybe in the days of archaic controllers that did not have any homing/work offset capability this might have mattered but not today.

    The point here is that homing sets machine zero, either directly by putting home switches at the zero point, or somewhere else with an appropriate offset (at the right-hand end of travel, in the most extreme case). But that is absolutely nothing to do with where the zero point is on the work. First thing you do when you plonk the stock on the bed and clamp (assuming that you have already homed the machine) is to move the spindle to where you want (0,0) to be, and then set "work coordinate zero" to that point. Maybe x and y at the same time, maybe separately. Effectively you are doing the same thing when you set tool height - this is setting z coordinate zero, indirectly. Your gcode will, if generated by any modern CAM package, be working in terms of work coordinates. Nothing at all to do with machine coordinates. For example, recently, I have been machining work where the X zero work coordinate is at the right hand side and most of the machining is done with negative X coordinates. I told my CAM software where I wanted X=0, set the spindle to the RH edge of the stock and set work coord X to zero, and away it all went.

    This machine/work coordinate confusion is a bit complicated to follow at first sight but it soon becomes second nature and you won't even think about it, but it is absolutely critical to using CAM and the machine in harmony. I sorry if I have misunderstood what was being said, but the idea that you need to set machine zero somewhere on to the bed just so that you can move to negative coordinates could be very misleading to anyone new coming to this.
    As you say Neale it is not at all intuitive to begin with, and I dont believe I have seen a clear explanation in the manuals . ( and some of the videos are even less helpful)
    I think I have got it now though.
    So by homing and setting soft limits you are defining the extremities of the working area, within which you will place your job.
    You then choose a point on your workpiece which you will define as 0,0,0 for you starting point, traverse your tool to that point and you will then set the work coordinates to zero on all axes.
    The G code routine will then move the tool in whatever positive or negative directions are needed to complete the work.

    I suppose it becomes particularly clear when doing say an engraving job where conventionally you will set z=0 when the tool is touching the surface, then any movement to Z negative involves a cutting depth and movement to Z positive gives a clearance for tool repositioning.

  8. #18
    Quote Originally Posted by ngwagwa View Post
    So to clarify on my machine with a back off of minus 5mm after machine has been homed the DRO will display -5mm when displaying machine co-ordinates.
    I'm not sure that it works quite like that. It's been a few months since I set up a UCCNC machine but I think it Backoff works like most other controllers.? Which is that it looks for the Home switch then after hitting the switch Zero's the DRO, then backs off the set amount and Re-Zero's DRO again. When finished the MACHINE coordinates will show Zero.

    It does this so you can have your HOME position or MACHINE ZERO at any point on the machine ie: Centre of travel, away from where the switch is physically located.

    SOFT LIMITS are ALWAYS taken from MACHINE ZERO and limit the travel in the + & - directions. So in my Centre of travel example above with 1000mm of total travel, you would have Min soft limit = -500 and Max soft limit =+500.

    If MACHINE ZERO was at the switch then soft MIN =0 Softmax =1000

    Hope that helps clear a little of the confusion.!
    .
    -use common sense, if you lack it, there is no software to help that.

    Email: [email protected]

    Web site: www.jazzcnc.co.uk

  9. #19
    Quote Originally Posted by Neale View Post
    I'm a bit concerned that anyone thinks that "going past zero" is in any way relevant when you are using Mach3/UCCNC. Maybe in the days of archaic controllers that did not have any homing/work offset capability, this might have mattered but not today.
    The Problem here Neale is that word HOME confuses people. They mix it up with WORK ZERO and think that HOME is where the JOB starts.
    99% of new users fall foul of this so when I deliver machines to new users I always spend at least 30mins or more explaining and showing how the COORDINATE SYSTEM's and WORK OFFSETS relate to each other and how they relate to CAD etc.

    Now John11668: and anyone else who doesn't quite understand. This is where SOFT LIMITS can come into play to save the day.? Let us say your HOME (machine zero)position is at the end of travels on each axis and you have 1000mm of travel.

    You ZERO the WORK coordinate 100mm from the MACHINE ZERO. The job is drilling holes in a 1000mm long piece of stock with the last hole located 990mm from 0. What do think will happen .?.....Yep CRASH.!! . . Because your last hole would actually be located 1090mm from MACHINE ZERO. . . . But not if you have SOFTLIMTS turned on because the controller will pre-run through the G-code when you first load it and will warn you that you are going to exceed the SOFT LIMITS and the day is saved...

    So hopefully this shows how MACHINE ZERO and WORK OFFSETS play together.
    -use common sense, if you lack it, there is no software to help that.

    Email: [email protected]

    Web site: www.jazzcnc.co.uk

  10. #20
    Hi Jazz and thanks for your response .
    I dont think however you have quite clarified things for me.
    So ignoring backoff for now .
    I home to machine zero in all axes and the machine defines its position as 0,0,0
    I have set soft limits X of 0 and 400.
    Soft limits Y of 0 and 200,
    and Soft limits Z of 0 and -50
    So I have now defined a box 400x 200 x50 which is the envelope within which all work MUST be done .

    We now come to the workpiece which I have to plant on the table completely within that envelope and clamp it. I have to bear in mind if I am doing an outside profile that I must consider the cutter and allow at least a cutter radius all round.

    I am guessing that my workpiece origin or start point is defined somewhere within it , whether it is right hand end, middle, or wherever so I identify that origin, jog to it , and set all my work parameters to zero at that point.

    So really it is only if I have placed my job wrongly and that the toolpath will stray outside the envelope that a soft limits alarm should arise .
    Are you saying that it should arise prior to hitting the start button . or will it only arise when the work zero position is defined .

Page 2 of 4 FirstFirst 1234 LastLast

Thread Information

Users Browsing this Thread

There are currently 1 users browsing this thread. (0 members and 1 guests)

Similar Threads

  1. mach3 soft limits
    By Daveo in forum Control Hardware & Systems
    Replies: 12
    Last Post: 25-06-2020, 05:24 PM
  2. Lichuan "Easy Servo" closed loop stepper question
    By Voicecoil in forum Stepper & Servo Motors
    Replies: 15
    Last Post: 09-10-2019, 09:33 PM
  3. "Hacking" and "Modding"
    By magicniner in forum General Discussion
    Replies: 15
    Last Post: 07-01-2015, 08:59 PM
  4. Setting up "System 45" 3 axis unit by DIYCNC
    By StevenT in forum LinuxCNC (EMC)
    Replies: 2
    Last Post: 15-10-2014, 03:22 PM
  5. "Racks" VS "ball screw"
    By C.AlveSilva in forum Linear & Rotary Motion
    Replies: 1
    Last Post: 17-04-2012, 11:53 PM

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
  •