Adventures in cutting steel

New Home Forum Mostly Printed CNC – MPCNC Advice – MPCNC Adventures in cutting steel

This topic contains 16 replies, has 6 voices, and was last updated by  Bruh 2 months ago.

Viewing 17 posts - 1 through 17 (of 17 total)
  • Author
    Posts
  • #99403

    Bruh
    Participant

    Thought I’d share my progress with cutting steel bar. I’ll update this thread with progress as I keep tweaking things.

    I got so far as to cut 3/16″ steel bar in a single pass using trochoidal milling. I’m also blasting the part with quite a bit of air though the nozzle that’s built into my lower mount ~50psi for both chip removal and cooling. All of the cuts here are made with a single flute 1/8″ cutter. It’s slow going so I wouldn’t expect to cut anything large and I don’t think I’ll get much more aggressive than the settings below without cooking cutters.

    5mm DOC (material is 4.8mm, however)
    1.25% trochoidal step
    50% trochoidal width
    9mm/s feed

    IMG_20190504_202654
    IMG_20190504_202714
    IMG_20190504_170555

    I haven’t played around with plunge speeds yet. That’s next.

     

    #99413

    Ryan
    Keymaster

    WOW!!

    #99428

    Guffy
    Participant

    How long was a time of that trochoidal milling?

    Trochoidal path has a disadvantage – it takes too much time and if you will try to increase feed rate too much you may get geometric distortions because our cnc machines aren’t stiff enough.

    And when i had tried to mill steel i used wd40 as lubricant. It was pretty helpful especially for engraving with ball end bit.

    #99436

    Bruh
    Participant

    How long was a time of that trochoidal milling?
    Trochoidal path has a disadvantage – it takes too much time and if you will try to increase feed rate too much you may get geometric distortions because our cnc machines aren’t stiff enough.

    A little over 4min if I remember correctly.

    It’s definitely slow going and the MPCNC/DW660 certainly isn’t the best setup for the job. To be clear, I don’t have a part that I intend to cut this way. I’m really just curious as to what we could expect with good CAM.

    I’ll have to give WD40 a go as well.

    1 user thanked author for this post.
    #99454

    Bruh
    Participant

    I was able to do a little bit of plunging and cut a 1″ square test part.

    To @guffy‘s point this is much like carving Mt Rushmore with a pocket knife 😉 That said, I was able to speed up the trochoidal cut time by decreasing the trochoidal width from 50% to 40%. My gut says I can take this even lower to speed things up more. (Less wasted movement by using smaller arcs). I don’t think we need nearly the width used during aluminum cutting because the chips aren’t as gummy and we’re removing less material on each pass. The cut in the video below used both oil and compressed air and took a hair under 35m to complete.

    DOC 4.7mm
    Trochoidal width: 40%
    Trochoidal step: 1.4%
    X/Y feed: 9 mm/s
    Plunge: 1.5 mm/s

    NOTE: I noticed a bit of chatter during plunge at the start of the video and dialed the speed back to 80% in repetier during the initial plunge and left it there for the remainder of the cut.

    I suspect that things can be sped up slightly by decreasing trochoidal width. You can see a failed cut on the opposite side of the work piece from me getting a little too impatient.

    Edit: Image uploads keep timing out for me.

    1 user thanked author for this post.
    #99503

    Ryan
    Keymaster

    Have you tried not using trichoidal? Your plunge went much better than mine in steel, so I will look into that for sure but I think you can really speed that up with a standard slot and finishing pass.

    #99596

    Bruh
    Participant

    Have you tried not using trichoidal? Your plunge went much better than mine in steel, so I will look into that for sure but I think you can really speed that up with a standard slot and finishing pass.

    I haven’t tried regular slotting yet. I assumed that trochoidal would be the most forgiving and give better tool life since it’s using more of the cutter. I’ll have to give it a go.

    I think it’s probably best for us not to plunge into steel at all if we can avoid it. Definitely do a helical plunge into the material if you must. Better yet, use the machine to mark areas to drill out on a manual press and then use those holes for plunging.

    #99727

    Tim Ross
    Participant

    Alright, I am humbled once again. I’ve been trying to cut aluminum and can’t get good consistent results yet, and you are knocking out steel with good results. My machinist friend keeps telling me that the DW660 is running way too fast to cut aluminum. I’ve tried putting cutting oil on the cut, etc. but still poor results. Great job for you! Back to the drawing board for me. /Tim

    #99732

    Barry
    Participant

    Tim, single flute end mill?

    #99734

    kd2018
    Participant

    Either of you, Bruh or Tim, using a router speed control like this?

    https://m.harborfreight.com/router-speed-control-43060.html?utm_referrer=direct%2Fnot%20provided

    #99762

    Bruh
    Participant

    Either of you, Bruh or Tim, using a router speed control like this?
    https://m.harborfreight.com/router-speed-control-43060.html?utm_referrer=direct%2Fnot%20provided

    No speed control for my cuts. I did just order a superpid, however.

    #99810

    Tim Ross
    Participant

    I’ve tried single flute, double, and quad. I didn’t have a speed control, so I removed the floor pedal from my Foredom Flex shaft and plugged into it. Then I put a C-clamp on the attenuator to slow down the unit. There still seems to be too much wobble and flex in the system. My MPCNC legs are 6″ long, and the unit is 24″ square. Maybe I will cut some at 3″ and reduce the outside to 18″ to see if I get better results at those dimensions. I’ve even thought about printing the corner holding units in low fill rate and using lost PLA casting to cast the end pieces in aluminum, but I’m not quite there yet.

     

     

    #99813

    Ryan
    Keymaster

    My MPCNC legs are 6″ long

    Biggest issue here.

    1 user thanked author for this post.
    #99829

    Tim Ross
    Participant

    I will cut some shorter legs and try them. Also, I will insert the bit further into the 660. my protrudes out quite a bit. And if it won’t go in further, I will cut the upper end off enough to get it in further, and/or buy some shorter endmills. Maybe the double ended ones are shorter. IF I need to cut further than have the length for, I plan to later add a subtable in some way. But first things first. Get the damn thing working correctly. I want to mill and aiplane door handle when I get milling aluminum correctly.

    Ryan, the 182 is running great and anxiously awaiting to take you for a flight. North Las Vegas airport.

    1 user thanked author for this post.
    #99832

    Bruh
    Participant

    I will cut some shorter legs and try them. Also, I will insert the bit further into the 660. my protrudes out quite a bit. And if it won’t go in further, I will cut the upper end off enough to get it in further, and/or buy some shorter endmills. Maybe the double ended ones are shorter. IF I need to cut further than have the length for, I plan to later add a subtable in some way. But first things first. Get the damn thing working correctly. I want to mill and aiplane door handle when I get milling aluminum correctly.

    Ryan, the 182 is running great and anxiously awaiting to take you for a flight. North Las Vegas airport.

    Good luck cutting down those Carbide end mills 😉

    Once you shorten your machine’s legs and get shorter end mills you should also raise the work piece up as close to the gantry as possible. The closer the you work to your max Z height the more rigid the setup will be.

    I likely wouldn’t bother with cast corners unless you’re just really itching to try it out. My gut says the corners aren’t where your issues are coming from.

    1 user thanked author for this post.
    #100279

    Tim Ross
    Participant

    Glorius day in Las Vegas. My first complete aluminum cut is shown in the picture. It’s about a 11x11mm square cut of aluminum about 3/8″ thick.

    1. Bought the Harbor Freight router speed control that kd2018 posted above.
    2. Cut 3″ uprights out of conduit and replaced my 6″ uprights with the shorter 3″.
    3. Tightened all corner holding screws (I think I heard a few cracks as I tightened them)
    4. Broke the spindle mount holding the DW660 by overtightening, so I connected a few large cable ties and bound it into place tighter.
    5. Used a single flute upcut bit, plunge rate 2mm sec, DOC .3mm, feed rate 2mm sec.
    6. Sprayed WD40 with left hand and 40lbs air from air compressor from time to time to clear the chips as it cut.

    The first few tries went along ok, but it jumped around and chatter forced me to stop the cut. This appears to be due to the motor mount not being tight enought (before I tightened it and broke it). Finally after about 4 tries the 5th was successful.  I filed it down a little so you may see file marks in the picture. (coin shown to compare size). I have to find ways to tighten the unit, making it more rigid, without breaking all the parts, but hey, now “I’ve now cut aluminum”. Making progress as time permits. /Tim

     

     

    #100327

    Bruh
    Participant

    @trosslv; The feet certainly don’t take that much clamping force to hold the conduit in place. If you’re having to tighten them to the point of cracking the plastic then you might double check your printers calibration to make sure your holes aren’t over sized.

    2mm/s feeds seem a little on the low side but it’s tough to say without knowing exactly what RPM you’re running. One issue with the type of speed control that you’re using is that they also reduce the power of the cutter. The more you lower the cutting speed the less power the cutter will have.

    Zip ties holding your router in place are almost certainly allowing the router to deflect which is hell on cutters. I’d get that fixed and give things another go. Here’s some inspiration for you.

    1 user thanked author for this post.
Viewing 17 posts - 1 through 17 (of 17 total)

You must be logged in to reply to this topic.