Page 1 of 2 12 LastLast
Results 1 to 10 of 11

Thread: 3D MOLD - Advice on Cutting

  1. #1
    Join Date
    May 2018
    Location
    Beacon, NY
    Posts
    7

    Default 3D MOLD - Advice on Cutting

    Hello All,

    I have been making 3D wooden molds for a few months now; and have learned alot about the shopbot and cutting techniques from this forum.

    I am currently working on a mold with 1/8" radiuses. Normally, I would rough out the mold with a 1/2" ball nose and finish with a 1/4" ball nose.

    Should I rough out the mold with the 1/2" or 1/4" ball nose? I am concerned about the difference in cutting diameter going from the 1/2" ball nose to the 1/8" ball nose.

    The 1/8" ball nose is 1/4" tapered shank end mill.

    Also, any advice on feed and speed for 1/8" ball nose in maple wood would be appreciated. I use an online chip load normally if I am cross checking myself.



    -Zach

  2. #2
    Join Date
    Mar 2016
    Location
    Brooklet, Ga
    Posts
    187

    Default

    Shouldn't have any problems roughing with a 1/2" and finishing with the 1/8"BN. 3D cutting at 3ips X,Y, and Z feeds at 12Krpm should do the trick.
    2006 PRTalpha 96x48
    3hp SEV spindle
    Vcarve Pro8
    Always eager to consume large amounts of info, tips, and techniques!

  3. #3
    Join Date
    May 2018
    Location
    Beacon, NY
    Posts
    7

    Thumbs up

    Quote Originally Posted by guitarwes View Post
    Shouldn't have any problems roughing with a 1/2" and finishing with the 1/8"BN. 3D cutting at 3ips X,Y, and Z feeds at 12Krpm should do the trick.
    Thanks! Saves me from going forward blind. Good to know I had the Feed and Speed on the money.

  4. #4
    Join Date
    May 2018
    Location
    Beacon, NY
    Posts
    7

    Thumbs down

    Had my first bit break.

    What would cause the roughing cut and finishing cut on a part not to line up properly? Assuming all temporary zeroing is the same, the Z is zero, and the part is held in place....

    The issue is only visible in the x axis, y axis seems fine.

    I have been having this issue with a number of the molds I work on, usually I am able to fix the issue with a second finishing cut slightly lowered. But today it cost me a new bit...

    What am I doing wrong?

    -Zach

  5. #5
    Join Date
    Jan 2004
    Location
    iBILD Solutions - Southern NJ
    Posts
    7,986

    Default

    What material, bit, RPM, feed rate and pass depth were you running?

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

  6. #6
    Join Date
    Jan 2011
    Location
    gleason, wi 54435
    Posts
    449

    Default

    add to Brady's questions what machine do you have?

  7. #7
    Join Date
    May 2018
    Location
    Beacon, NY
    Posts
    7

    Default

    Brady -

    I machine blocks of maple
    Roughing - Onsrud 1/2" BN > 8000RPM > 5.5 IPS > 25% - 50%
    Finishing - Onsrud 1/4" BN > 12000RPM > 4-5 IPS > 50%
    Broken Bit - Tapered CARBIDE END MILL, 1/8", 1/4" SHK > 12000RPM > 3 IPS > 50% (Finishing)

    Bob -

    ShopBot BT48 Buddy


    -Zach
    Thanks.

  8. #8
    Join Date
    Jan 2004
    Location
    iBILD Solutions - Southern NJ
    Posts
    7,986

    Default

    Hi Zach,
    In my experience with maple, those speeds are WAY too slow (RPM) and feedrate is way too high.

    3D carving maple with the larger bits, set your MS to something like 2,2 with the 1/2" bit and 12-13k RPM. The smaller the tool, the higher the RPM you need to properly machine things. As long as you are not burning anything, keep the RPM high. The smaller bits like/need higher RPM. I know maple can be finicky when it comes to burning, so adjust as needed.

    FYI - all spindles sold by SB are rated for full power at 12,000 RPM or higher. Putting a lot of strain on the motor at low RPM (like your roughing pass) - pulls a lot of amps and heats up the windings in the motor...It's like going uphill in overdrive.

    So...reduce the move speed and jack up the RPM on your roughing. Once that's out of the way and there isn't a lot of material left for finishing, crank up the RPM and adjust the move speed to something that is prudent for finishing.

    Keep in mind the laws of physics - that is to say, imagine going say 5 inches per second across the part with a hand router. If the part is 24" wide, it WILL get up to that speed after it ramps up. BUT if the part is say only 8" wide, it will NEVER get up to 5 IPS and SB3 will ramp things down to compensate. The problem with this is SB3 does a pretty good job trimming speed back but it results in abrupt moves in comparison to setting a reasonable MS value of something like MS,2,1 for that same 8" part. Setting the MS too high CAN result in movements so abrupt it loses steps - which may have been what happened in your situation.

    Try the slower speed and higher RPM. Make some adjustments at the tool (speed things up by hitting space bar and Insert command, then MS and enter new value. Adjust RPM as you see fit. Every part is different & each can benefit from fine tuning via the machine operator.

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

  9. #9
    Join Date
    May 2018
    Location
    Beacon, NY
    Posts
    7

    Default

    Brady -

    I will put this advice into practice immediately, should greatly improve the quality of parts and my process.

    I am aware of the speed ramping issue, particularly with the process I use, making parts that are negatives with all internal cutting. Does the issue of speed ramping and in-turn the abrupt movements explain the increased material left from roughing in the x+ direction, and the decreased material (over cutting ) in the x- direction? Or is this the effect of deflection? Chatter?

    I am still relatively new to the editing of parameters at the tool through commands and shortcuts. What should I know before I try learning by doing? I am hesitant to stop / pause a part file and end up having to start over.

    This information is touched on in ShopBot Tools - video tutorials. What can I search for on the forum?

    Again, Thank You Brady.

    -Zach

  10. #10
    Join Date
    Jan 2004
    Location
    iBILD Solutions - Southern NJ
    Posts
    7,986

    Default

    Hi Zach,
    In terms of learning, take a look at the article I did on VR and Ramping settings for SB3 some years ago. You can find it here It should give you a pretty good understanding of how to fine tune your tool for the task at hand. I remember at the time I was doing a lot of 3D work and wanted to really get a handle on commanding the machine for quality finishes. I spent a few weeks of back and forth with help from Ted on what each parameter does and how to tweak things in a meaningful way.

    The take away is that you're going to get the most bang for your buck in the obvious difference department by changing the Slow Corner Speed. Be sure to change your Minimum Distance to Check and 3D Ramp Threshold to the numbers I suggest. SCS works in both the XY plane AND the XZ and YZ planes for 3D stuff. The main thing with 3D raster toolpaths is to eliminate 'banging' or abrupt direction changes at the start and end of the raster. SCS will cushion this, but also influence how quickly the tool traverses a pyramid profile etc in actual 3D cutting.

    As for your deviation between the roughing and finishing cuts at the extents of the design, most of the time this is a 3D toolpath boundary issue (in CAD/CAM) and not so much the tool itself. I learned early on that not completely roughing out the perimeter of the design often results in that horrid 'nernt' sound at the end of each raster pass. This is usually because CAM prevents the larger dia tool from gouging outside of the toolpath boundary vector and lets the smaller tool resolve the portions that were left on by roughing.

    So...It isn't uncommon for me to have a distinct boundary vector for roughing and another one that is offset a bit inward for 3D finishing. For many reliefs I tend to also create a profile toolpath that matches the outside profile of the part to be cut and run that down either full depth or enough to hog away those annoying bits of material that make the 'nernt' sound. It's not the sound so much that is the issue - it's the shock load of the tool suddenly engaged in a much deeper volume of material. What that does from a 'physics' standpoint if you want to call it that, is it loads the tool and unloads it very quickly. This causes vibration, whether it is the bit or the gantry deflecting, it rings like a bell and telegraphs into your finish cut...which if you're making molds or masters is NOT what we want!

    Spend the time on the front end to generate toolpaths that are going to eliminate the finishing tool from entering ambient/scrap material. Hammer on that previewer in CAM until it looks like it should. Just pretend you're at the tool and try to mentally anticipate what will or could happen & program for it. For the 3D finishing pass a lot of times I'll make one that just does the first few lines very slowly (in case the bit is cutting on BOTH sides initially - because that's where bits snap!) until it is only shaving off material on one side of the bit. It's sometimes better to use an offset 3D toolpath for this and then stop it when you're where you need to be. You can even run it high (.02") in the Z, then run your real finishing pass at the right Z. The major thing to focus on with all of this stuff is this: Consistent, smoothness. Sometimes that also means turning your move speed way down to minimize machine reverberations and keeping your chipload light. If I have something that is really important - where surface finish is paramount - I care little about speed...because that means less time sanding or no sanding at all!

    Good luck - chime back in after you've done some tweaks and let us know how you made out.

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

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
  •