Welcome To Signs101.com: Largest Forum for Signmaking Professionals

Signs101.com: Largest Forum for Signmaking Professionals is the LARGEST online community & discussion forum for professional sign-makers and graphic designers.

 


  1. This site uses cookies. By continuing to use this site, you are agreeing to our use of cookies. Learn More.

CNC Router Bits Keep Breaking

Discussion in 'CNC Routers & Engravers' started by nikdoobs, Dec 30, 2013.

  1. nikdoobs

    nikdoobs Active Member

    519
    0
    16
    Jun 4, 2013
    lafayette, la
    Hey Guys,

    I am using LMT onstrud bits (https://www.onsrud.com/product/Item/m/itemDetail.html?q=63-618&itemId=63-610)
    to cut .040 alumium on a Shop Bot. I was initially using 1/8"dia bits but have switched to 3/16"dia because the 1/8" bits kept breaking.

    Both sizes get clogged with melted metal shavings. (Sometimes it cuts great and other times it gets clogged like crazy, even with new bits).

    Do you guys have any suggestions? I'm going to try to use down-cut bits instead of up-cut bits. What do you guys find works best for you?

    I'm running .4 inches/second with a spindle speed of 8,000 rpm.

    I use this foot attachment (http://store.shopbottools.com/produ...ww.shopbottools.com/mproducts/accessories.htm)
    and have an air hose blowing as well.

    TIA
    -Nick
     
    Tags:
  2. Techman

    Techman Major Contributor

    8,553
    6
    38
    Jun 24, 2003
    michigan
    you have to lub it. I use tap magic for aluminum because it is cleaner and dries fast.
     
  3. tbullo

    tbullo Superunknown

    267
    10
    18
    Apr 5, 2012
    VA
    I use Onsrud 65-023 bit mostly. 1/4'' diameter at 10,000 RPM is what I use. I try not to use smaller bits unless I have to. These bits cut great and last.
     
  4. letterman7

    letterman7 Active Member

    977
    9
    18
    Nov 10, 2008
    Pennsylvania
    You should be able to cut .040 on a Bot with an 1/8" bit. Air isn't enough, though. Tap magic is good, WD40 works in a pinch, though it gets messy quick. Slow your feed rate and up your rpm's. Reverse your direction of cut if it's still clogging (if you're cutting with a climb cut, reverse it to a conventional. You'll see that option in the toolpath menu when you select the bit).
     
  5. nikdoobs

    nikdoobs Active Member

    519
    0
    16
    Jun 4, 2013
    lafayette, la
    Thanks for the advice. I'm going to get some tap magic.
     
  6. artbot

    artbot Very Active Member

    3,171
    2
    38
    Feb 18, 2010
    Houston TX
    i was cutting .040 5052 the other day with my shopbot. straight cut 1/4" (double flute) bosch bit, .7 inches per second, maybe 15,000 rpm? i get an old windex bottle full of soapy water and spritz the bit every so many seconds. the bit will pull the fluid into the cutting edge. there are sweetspots with fed/flute/rpms... but i just get a bit lazy and do the water bottle thing. if you are cutting 3003 AL that will be a bit trickier.
     
  7. Techman

    Techman Major Contributor

    8,553
    6
    38
    Jun 24, 2003
    michigan
    IF you have a way.
    Raising the panel a little off the bed works wonders for getting chips out of the way and air flowing to the cutter. Chips cause much pain.
    The lube will help cool the cutter, and will help keep the edge clean. An edge that accumulates heat allows microscopic particles to build up making more heat and a gob of a clog.
     
  8. nikdoobs

    nikdoobs Active Member

    519
    0
    16
    Jun 4, 2013
    lafayette, la
    Do you guys use down-cut or up-cut bits?
     
  9. I agree with artbot, soapy water in a spray bottle.
    Also wondering what grade of aluminum you're working with?
    Never had any issues with our Shopbots running Onsruds except for the harder grade aluminum.
    You might also consider posting this on the Shopbot forum http://www.talkshopbot.com/forum/
    There are guys on that board that know these machines inside-out. - Boyd
     
  10. Techman

    Techman Major Contributor

    8,553
    6
    38
    Jun 24, 2003
    michigan
    I wonder why professional machinists would use certain fluids such as Tap Magic?
    Well because they work. A machine shop working with metals as a profession would not use soapy water alone. The edges of a cutter are coated with a special substance that allows it to be magnitudes of higher efficiency. Why would someone spend big bux for an Onsrud cutter and use a fluid that does nothing to protect that coating. Onsrud spends big bux developing cutters and coatings for those cutters..

    In the old days machinists would use kerosene on their cutters when working with aluminum. It was messy. Then along came modern fluids such as tap magic for Aluminum that was a game changer. This product protected the cut edge and more importantly protected the coatings that were mere molecules in thickness.. The right fluid allows a tool to maintain wear resistance keeps the friction away and cools the cutter at high speeds. Coatings have aluminum in them. Albeit a very thin layer. Once that barrier is broken the cutter fails by filling with welded particles.

    Soapy water alone will not lubricate the cutting edges and protect the coatings. The use of soap in a water based cutting fluid is to emulsify oil that is the actual tool protector. The fact is for aluminum.. water should be mixed with an oil using soap as an emulsifier. However that is usually a messy way to go. Using a product such as Tap Magic for Aluminum is much cleaner and it works.. How does it work? It has mineral oil and a fast drying emulsifier and no water. It evaporates fast. Much faster than water and is how it carries away the heat. The oil lubs the cutter.
     
  11. artbot

    artbot Very Active Member

    3,171
    2
    38
    Feb 18, 2010
    Houston TX
    i only use the water because my pieces will then need to be brushed, printed, and coated which requires clean metal. the easiest thing to clean off is the soapy water. there are some really advanced bits out there but i prefer a straight cut for metal....no spiral up or down.
     
  12. CES020

    CES020 Very Active Member

    2,893
    2
    38
    Oct 16, 2008
    VA
    As a machinist by trade (30 years in that trade), the reasoning you used carbide verses high speed steel was because one sheared the material off and the other actually ripped the material off. You could look at the actual cutting under a high power microscope (we had photos of it all), and you could see the plastic deformation happening (that's the process where the friction is so great that the metal becomes soft enough to start peeling away from itself), and the different between the two was huge. High Speed Steel really did shear the material while carbide was tearing it off through brute strength. That was prior to the advent of micro grain carbide. But all in all, CNC routers aren't the best machine for running carbide. Carbide hates, and I mean hates 2 things, vibration and flex. Since the work is typically held down by vacuum, and the machines are gantry based, it's not exactly the ideal circumstances for carbide. A lot of people use it and a lot of people will tell you they have great success, but if you want to see the difference, order yourself a 2 flute high speed end mill (high helix, right hand spiral would be best, but the high helix will want to peel the work off the table more than the standard flute geometry), and put some tap magic on that. You can push it a lot more and you can run far less RPM. You can run 6500 or so with 1" per second pretty safely. High speed steel doesn't mind vibration or flex, so it works well. Plus they are a fraction of the cost of carbide. You can buy 3-4 high speed steel end mills for the price of one onrud bit.

    We use a synthetic coolant, Tri-Cool MD-7 in a spray mist system. It's synthetic so it doesn't mess up our spoil board (water based will swell a Trupan spoil board in minutes).

    The grade, as mentioned earlier, is also paramount. Some aluminum is made to be formed and it's very gummy and wants to stick to itself like mad. Other is harder and the chips come off clean. A lot of times you have no idea what grade it is, so you are just stuck with it. That's why you can get it dialed in perfect and then 2 weeks later, the same settings don't work at all.

    People in this business tend to wrestle with it until they find some magic combination that works for them and they stick with it. I've seen settings from 5000-18000 RPM, and people at both ends said how well it worked for them.

    I'd try the high speed steel and lower RPM and see how that works for you. And I'd always ramp into the cut.

    Just my opinion, your milage may vary.
     
  13. Techman

    Techman Major Contributor

    8,553
    6
    38
    Jun 24, 2003
    michigan
    ^^^^ This times two..
     
  14. letterman7

    letterman7 Active Member

    977
    9
    18
    Nov 10, 2008
    Pennsylvania
    Interesting and good information there ^. I didn't know the difference in cutting between the two types of bits, other than the carbide was much more brittle. I'll have to get a couple HSS and play with them to compare!
     
  15. Jester1167

    Jester1167 Premium Subscriber

    Monitoring chip size is important as well, probably hard to do with .040. The chips carry away alot of the heat and will give you feedback on speed and feed. Thin needle size chips tell you that your spindle speed is too fast or you feed rate is too slow and your building up too much heat. Eventually the chips will start to weld back to the material and then the heat will eventually dull and break the bit. On 1/8" aluminum you should see approximately 1/8" x 1/8" thin (potato chip) size chips.

    Your speed and feed rates will be dependent on your router. Bigger heavier routers dampen vibrations leading to faster feed rates and bits lasting longer. If you cut a lot of aluminum a mister will pay for itself in no time otherwise a spray bottle will work.

    I used to cut a lot of aluminum and really like the 3/16" bits. The 1/8" bits would break to easily and we didn't like the radius on the inside corners on the 1/4" bits.
     
  16. artbot

    artbot Very Active Member

    3,171
    2
    38
    Feb 18, 2010
    Houston TX
    the limac i used last year had some kind "air coolant sytem" type of thing that blew very cold high velocity air at the bit. it worked really well. the
    fluid system on the prior multicam being used was inferior for the 1/8" and thinner aluminum that we were cutting.
     
  17. nikdoobs

    nikdoobs Active Member

    519
    0
    16
    Jun 4, 2013
    lafayette, la
    Very valuable info. Thanks guys. Just to update everyone, I've run 3/16" down cut carbide bits for the last two jobs with great success. Down cut bits make a huge difference. I may pick up a few steel bits to do some comparison.
     
Loading...

Share This Page

Loading...