1. #1
    Hi guys simple question , when you are setting the origin do you set it to the outside of the bit or to the centre of the bit ?

    Fiction is far more plausible when wrapped around a thread of truth

    Nothing great was ever achieved without enthusiasm.
    Ralph Waldo Emerson

  2. #2
    centre then the Cam system works all the offsets out for 1/2 the diameter.
    If you don't use a CAM system then draw your part out, add the off set and follow that.
    John S -

  3. #3
    That is not a simple question...

    Outside

  4. #4
    It depends...
    Old router build log here. New router build log here. Lathe build log here.
    Electric motorbike project here.

  5. #5
    In which case we need more clarification.
    Thinking about this I set the origin point in CAD at the point I want to start or top left which for me is the fixed point on my machine, left hand side of the fixed vise jaw.

    Many use bottom left because then all moves up and right are positive but it doesn't matter to a CNC what is positive or negative.

    I don't use bottom left because that's the moving jaw and if your blank material differs in depth, Y+, Y-, then the parts come out different.

    Next step is CAM just uses this point.

    However it's not something that's written in stone, like many machining operations there is never a laid down right way and wrong way, just different ways of doing things.
    John S -

  6. Have to agree with it depends and John S pointing out some of the reasons. If it setting up a part on the deck that is NOT going on a preset jig I set up to the material and then add offset to get the bit where I want it (usually .5 to .75 diameter of the largest bit being used) unless there is a built in offset in the project or I have to put in a larger offset due to needing material edge that needs to be remaining. I use G55 to G57 for most of these and they get changed as needed. For Jig stations where the Jig has been placed and is squared and the material is a fixed to the jig; then I use the preset G59P# depending on which station I am using (start at P7). This probably is as clear as mud and hope I am not just making it worse.

    Tool offset I deal with in my CAM programs so that issue does not become a problem when dealing with the machining side of the item. CAD wise it depends if I am planning to offset the item and we are back to same issue as above. I tend to work from 0,0,0 in CAD and then adjust once in my CAM program IF I am going or need to.

    Michael

  7. #7
    Thanks for the replys guys I was just wondering how you guys set it up.
    It’s not absolutely vital I get it perfect as I don’t do anything that is precision, but I have found if I’m using a 6mm roughing bit and set it to the outside it tends run down the first line with the centre of the bit on the edge of the material rather than 3mm in per say, but it still completes the piece with the last outside pass at opposite edge at the centre of the bit, just wondering if that is normal?

    Fiction is far more plausible when wrapped around a thread of truth

    Nothing great was ever achieved without enthusiasm.
    Ralph Waldo Emerson

  8. #8
    Ger21's Avatar
    Lives in Detroit, United States. Last Activity: 10 Hours Ago Has been a member for 5-6 years. Has a total post count of 508. Received thanks 68 times, giving thanks to others 0 times. Referred 1 members to the community.
    There is no normal. Machines do exactly what you tell them to do.
    What you need to do is set your 0,0 position on your machine to the same position relative to your stock that it is in your CAM program.
    On my router, 0,0 is the lower left corner of the table.
    In AutoCAD, I have my table drawn with the lower left corner at 0,0.
    I draw my parts exactly where I'll be placing them on the table, and never change my origin. (Well, almost never, but that just complicates things. )
    Gerry
    ______________________________________________
    UCCNC 2017 Screenset

    Mach3 2010 Screenset

    JointCAM - CAM for Woodworking Joints

  9. #9
    Quote Originally Posted by Fivetide View Post
    but I have found if Iím using a 6mm roughing bit and set it to the outside it tends run down the first line with the centre of the bit on the edge of the material rather than 3mm in per say, but it still completes the piece with the last outside pass at opposite edge at the centre of the bit, just wondering if that is normal?
    This is more to do with cutter compensation than the Origin point.? Cutter comp will place the cutter half the cutter dia either to the left or right of the toolpath and often your CAM will deal with this, often it will be called offset.
    If your writing code by hand then you'll need to Tell the machine using the G41/42 G-codes which side to apply comp which it then does according to the specified tool IE T1 and the data held for it in the tool table of the control.

    The origin is often thought of has just the 0,0,0 or start point of the part being cut. But this really is only the Origin of the WORK coordinate which is located at some point in relation to the Machine coordinate Origin.
    Where to place this Work Origin on the bed is totally up to you. The 0,0,0 WORK coordinate is the start point and will never change in relation to the part unless you change it's location in CAD or by writing new G-code.
    Where you place it on the bed is entirely upto you and so long has theres enough room for the complete part it doesn't matter because you set the 0,0,0 in WORK coordinates by zeroing the DRO's. The WORK coordinate then has an offset from the MACHINE coordinate Origin which you can not change unless you move the HOME switches. This is how you can get back into position if something goes tits up because the control knows the WORK coordinate 0,0,0 offset point in relation to MACHINE coordinate FIXED Origin.

    Micheal mentioned G55/6/7 etc work offsets.? These are just programmable WORK offsets that are a set amount from the MACHINE coordinate origin. These OFFSETS are set in the control. So say your table is 4ft sqr you can effectively divide the table into segments each with it's own 0,0,0 work coordinate.
    So say we break it into 4 segments then X0Y0 in MACHINE coords will be first offset, often the Default G54.
    X24Y0 will be next offset G55.
    X0Y24 will be 3rd offset called G56,
    X24Y24 will be 4th G57.
    Now Lets say we want to cut a different part in each segment then we would just select G54 for 1st part and the 0,0,0 WORK coordinate starts there at 0,0,0 in MACHINE coords.
    Then we select G55 for our next part and the WORK 0,0,0 point shifts to X24Y0 in MACHINE coords and so on for each WORK OFFSET.
    So to cut 4 individual parts at the same time each with there own 0,0,0 point we just combine the code in one file with a G54,55,56,57 before the code relating to each part and the control automaticly offsets to that point and uses it has WORK coordinate origin.

    Hope this helps and doesn't confuse.??

  10. #10
    No Jazz it makes perfect sense, I tend to set my Origin at the time I'm going to Mill it, mainly because nothing I have done so far is of any identical proportions. The problem was with the cutter compensation was that it began to mill through my clamps ! But I have set it now to compensate for this, however some of my blank wood pieces are not exactly square so it sometimes mills inside the line, but I'm not bothered I'm not making scientific equipment designed to measure things at quantum levels ! I'm making ART lol ! But I was curious to see if its normal, as explained, "it is", and once one knows what is normal one can then change the behavior by specific predictable amounts giving specific predicable results as I have done.

    Quote Originally Posted by JAZZCNC View Post
    This is more to do with cutter compensation than the Origin point.? Cutter comp will place the cutter half the cutter dia either to the left or right of the toolpath and often your CAM will deal with this, often it will be called offset.
    If your writing code by hand then you'll need to Tell the machine using the G41/42 G-codes which side to apply comp which it then does according to the specified tool IE T1 and the data held for it in the tool table of the control.

    The origin is often thought of has just the 0,0,0 or start point of the part being cut. But this really is only the Origin of the WORK coordinate which is located at some point in relation to the Machine coordinate Origin.
    Where to place this Work Origin on the bed is totally up to you. The 0,0,0 WORK coordinate is the start point and will never change in relation to the part unless you change it's location in CAD or by writing new G-code.
    Where you place it on the bed is entirely upto you and so long has theres enough room for the complete part it doesn't matter because you set the 0,0,0 in WORK coordinates by zeroing the DRO's. The WORK coordinate then has an offset from the MACHINE coordinate Origin which you can not change unless you move the HOME switches. This is how you can get back into position if something goes tits up because the control knows the WORK coordinate 0,0,0 offset point in relation to MACHINE coordinate FIXED Origin.

    Micheal mentioned G55/6/7 etc work offsets.? These are just programmable WORK offsets that are a set amount from the MACHINE coordinate origin. These OFFSETS are set in the control. So say your table is 4ft sqr you can effectively divide the table into segments each with it's own 0,0,0 work coordinate.
    So say we break it into 4 segments then X0Y0 in MACHINE coords will be first offset, often the Default G54.
    X24Y0 will be next offset G55.
    X0Y24 will be 3rd offset called G56,
    X24Y24 will be 4th G57.
    Now Lets say we want to cut a different part in each segment then we would just select G54 for 1st part and the 0,0,0 WORK coordinate starts there at 0,0,0 in MACHINE coords.
    Then we select G55 for our next part and the WORK 0,0,0 point shifts to X24Y0 in MACHINE coords and so on for each WORK OFFSET.
    So to cut 4 individual parts at the same time each with there own 0,0,0 point we just combine the code in one file with a G54,55,56,57 before the code relating to each part and the control automaticly offsets to that point and uses it has WORK coordinate origin.

    Hope this helps and doesn't confuse.??

    Fiction is far more plausible when wrapped around a thread of truth

    Nothing great was ever achieved without enthusiasm.
    Ralph Waldo Emerson

Similar Threads

  1. Setting my table up...
    By Davek0974 in forum Plasma Table Machines
    Replies: 23
    Last Post: 10-03-2014, 08:24 PM
  2. setting up a business
    By dstivens in forum Opportunities Available & Sought
    Replies: 5
    Last Post: 16-05-2013, 10:28 PM
  3. hi i nead help please with setting up dsp control
    By cockneyrebel in forum Machine Control Software
    Replies: 1
    Last Post: 19-01-2013, 01:18 AM
  4. Setting a start point.
    By jrob3rts in forum Computer Software
    Replies: 14
    Last Post: 17-06-2012, 12:36 PM
  5. Need help setting up a CNC router machine please
    By 1albobs in forum Gantry/Router Machines & Building
    Replies: 4
    Last Post: 27-02-2012, 06:16 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
  •