Welcome to Our Community

Some features disabled for guests. Register Today.

CBeam XL tolerance in MDF

Discussion in 'CNC Mills/Routers' started by Mouldy, Nov 27, 2017.

  1. Mouldy

    Mouldy New
    Builder

    Joined:
    Aug 23, 2017
    Messages:
    10
    Likes Received:
    0
    Hi all,
    recently finished and calibrated my CBeam XL and have made a few test pieces and parts in MDF.
    One test I did was to cut a 40mm square and a 40mm square hole to see how well the fit together.
    However they both seem to leave about .15mm on each edge so the square plugs is about .2-.3mm to big and the hole is about .2-.3mm too small.
    I don't think its calibration as I set and checked that over a 300mm jog. Also wouldn't that make hole AND plug either BOTH too large or BOTH too small??

    So is it most likely to be
    a) Flex in the machine
    b) flex in the bit (6mm 2 flute straight)
    c) play/flex in the router (Dewalt 26200)
    d) bad maths in Fusion 360?

    I tried to also include a leave stock at .1mm and did a final contour cut to try and reduce the load on the final cut. This didn't help.

    So is this normal? and if so how do you work around it. I'm aiming to make guitar necks, bodies and templates etc. So a few 10ths on a hole is not too bad but I need to know fret slots will be as accurate as possible. Cavity holes and covers only need to be within .5mm so again should be fine for me to simply make the sizes larger than the error.
    Where I do need an accurate fit is neck heal into neck pocket. This should be a snug fit just tight enough so that you can lift the guitar by the neck and the body not fall off.
     
  2. Flash22

    Flash22 Veteran
    Builder

    Joined:
    Sep 1, 2015
    Messages:
    159
    Likes Received:
    38
    did you allow for the tool offset and what type of cam process are you using for the cut? how many passes ?
     
  3. Mouldy

    Mouldy New
    Builder

    Joined:
    Aug 23, 2017
    Messages:
    10
    Likes Received:
    0
    Not sure about tool offset??
    I did 2d adaptive to rough out the hole leaving .3mm and then 2d contour to finish to dize. And on the outer of the square two sets of 2d contour. One leaving .3mm and then a second finishing one that goes round twice
     
  4. Mouldy

    Mouldy New
    Builder

    Joined:
    Aug 23, 2017
    Messages:
    10
    Likes Received:
    0
    Flass22 - What do you mean by tool offset? I did set teh x and y zero point allowing for half tool diameter..
    The over sizing seems consistent in both x and y axis and whether I cut a sqaure or a circle.. Will keep playing with some size offsets and also try different overall model lengths to see if its consistent.. Eg a 40mm part vs a 200mm part.
     
  5. David the swarfer

    David the swarfer OpenBuilds Team
    Staff Member Moderator Builder

    Joined:
    Aug 6, 2013
    Messages:
    795
    Likes Received:
    362
    I think you have a .25 inch bit which is .35mm bigger than a 6mm bit. that would make a cut around the outside too small and a cut around the inside too big.
     
  6. Mouldy

    Mouldy New
    Builder

    Joined:
    Aug 23, 2017
    Messages:
    10
    Likes Received:
    0
    Ah ok I see your point - and yes I did fall for that one early on as I do have a 6mm bit and a 1/4" bit
    and more confusingly the 6mm bit has a 1/4" shank!!
    I'll check again though as it does imply I have that issue but the other way round as though my bit is too small.

    Out of interest should a 6mm bit cut exactly 3mm from its centre? BTW I'm using a climb cut.. Though a test betwen Climb and Conventional didnt make any noticable difference
     
  7. David the swarfer

    David the swarfer OpenBuilds Team
    Staff Member Moderator Builder

    Joined:
    Aug 6, 2013
    Messages:
    795
    Likes Received:
    362
    a 6mm bit may be anything up to 0.2mm off nominal size, either large or small.
    and
    runout in your collet can account for another 0.2mm quite easily.
    and
    cutting a slot is never accurate, always cut a slot with an undersize tool and take a finishing cut on both sides
    and
    if you did not measure a difference between climb and conventional then your measuring tool or technique needs help, because there is always a difference (-:

    I would redo the test but do at least 2 cuts, first one leaving 0.5mm radial stock and then a finishing cut with 0 stock to leave.
    note that MDF swells quite a bit with humidity so you have to measure quickly. it will change size after cutting because the fresh edge will either dry out (in aircon?) or absorb moisture. (your 0.1mm is just fluff, it needs to have something to cut to make a finish pass work)

    of course that raises the question of your exact settings in Fusion because IIRC it defaults to having some radial stock to leave on the operations that are deemed roughing strategies.

     

Share This Page