Results 1 to 8 of 8

Thread: Rest machining too deep

  1. #1
    Join Date
    Mar 2004
    Location
    Lenox High School, Lenox MA
    Posts
    818

    Default Rest machining too deep

    I have done a a fair number of family crests similar to the one attached. Typically I will do a roughing cut with a .5" ball nose, then a finishing cut on the entire model with a .25" ball nose followed up with two rest machining cuts. The rest machining cuts are where I have a problem. I use a .125" ball nose, Beckwith coated carbide bit. One cut is for the banner, the second is for the shield and flourish. I always z-zero with a Shopbot provided zero plate and I always use the same location on the material to zero. Frequently the rest machining cut is too deep. I wind up with a shallow trough around the banner and the flourish. This leaves a lot of hand work to blend away the shallow trough.
    Any help will be appreciated.

    Thanks,

    Phil
    Attached Images Attached Images

  2. #2
    Join Date
    Jan 2004
    Location
    iBILD Solutions - Southern NJ
    Posts
    7,925

    Default

    Phil - run a simulation on the rest machining - post a pic zoomed in @ the problem areas. My best guess with the info you've given so far is that A) The vector boundaries are too loose and the tool is dropping down - or B) One of the component combine options is off, causing there to be a deviation in Z in comparison to the rest of the model.

    -B
    High Definition 3D Laser Scanning Services - Advanced ShopBot CNC Training and Consultation - Vectric Custom Video Training IBILD.com

  3. #3
    Join Date
    Mar 2004
    Location
    Lenox High School, Lenox MA
    Posts
    818

    Default

    Brady,
    here is a preview zoomed in to show the areas that I am discussing, the perimeter of the flourish and the banner. The cut appears fine in the preview but the actual cut has a trough around the perimeter of both about 1/8" wide and 1/32" deep.
    Attached Images Attached Images

  4. #4
    Join Date
    May 2009
    Location
    Philadelphia PA
    Posts
    90

    Default

    I had the same issue previously ( see attached pictures ) and the response from Brian of Vectric was as follows...

    "The Aspire preview I believe shows the artifacts I would expect from the boundary between a large tool (and hence large cusps) and a small tool (and presumably smaller stepover and smaller cusps).

    The real world image I believe shows the result from changing the tool with a very slight z height difference and very possibly slight movement in the material.

    This does illustrate why I've never been a big fan of automated 'rest machining' for materials like wood, foam etc. There are always witness marks at the boundary between two different tools and these often require more finishing effort than is saved by using the two tools. As the marks usually occur in areas of fine detail (the reason for using the 2nd tool) they are usually particularly difficult to sand.

    Michael
    Attached Images Attached Images

  5. #5
    Join Date
    Jan 2011
    Location
    gleason, wi 54435
    Posts
    429

    Default

    I would try to shim under the new bit maybe .010" or so and then nudge down to the preferred height a little at a time until satisfied, then run the part.

  6. #6
    Join Date
    Jan 2004
    Location
    iBILD Solutions - Southern NJ
    Posts
    7,925

    Default

    Not sure what to tell you about rectifying the issue. I'll repeat what I've always said - that it is absolutely imperative to Zzero at the exact same XY position when changing tools. Let's say your material is exactly 2" thick and you Zzero on the top of the block. In reality, I would pick a spot on the bed, off the work that I could Zzero to with the plate. I would then pencil in the X,Y coordinate numbers and label it "ZZ here, MZ,2.00 ". Of course you could also zero off the bed and set that up in CAM - but the numbers can be confusing for those who normally work from the top down.

    When you ZZ on the table, DON'T forget to MZ,2.00 and ZZ again or it'll be a sad day. If done correctly, this should eliminate all mechanical error in the Z, unless the material moves.

    I personally never liked Rest Machining in ANY CAM software. I always make my own vector toolpath boundaries and use those with another toolpath with the smaller tool. In the even't that there IS a step from the smaller tool where it transitions into the rest of the part, it is possible to work a little black magic by either making a component that feathers the toolpath at that lower depth out to the face of the surrounding relief or to modify the SBP. If you used an offset 3D toolpath, it wouldn't be too hard to gradually eek the Z UP every few passes along the entire length of the toolpath. Yes - it's a pain - yes, it DOES work, but it all depends on how much time you have into it and how precious the material is. Just don't move it off the bed until you are TOTALLY sure it's all good. It's also possible to do this at the tool with the nudge command every so often, evenly from the low to high spots. Just creep it up .002" each time and resume. Repeat until it's feathered out.

    Another option in terms of recovery would be to just raster over the entire thing .015" deeper with the smaller tool. It'll take a long time, but it'll get you there.

    -B
    High Definition 3D Laser Scanning Services - Advanced ShopBot CNC Training and Consultation - Vectric Custom Video Training IBILD.com

  7. #7
    Join Date
    Jan 2004
    Location
    Marietta GA
    Posts
    448

    Default

    I've found that on long 3d cuts the wood will sometimes "move" due to the relief you are machining.

    But, yeah, what Brady says too.

  8. #8
    Join Date
    Mar 2004
    Location
    Lenox High School, Lenox MA
    Posts
    818

    Default

    I appreciate the responses.

    Thanks,

    Phil

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •