No announcement yet.

Help reduce cutter wear

  • Filter
  • Time
  • Show
Clear All
new posts

  • Help reduce cutter wear

    Trying to figure what I'm doing wrong here. I'm cutting 1018 CRS on my CNC with a 0.500" carbide endmill. Spindle speed is 1500, IPM is 6.0 with 0.040" cleanup pass at 8.0 IPM. Depth of cut in the Z as well as X and Y is 0.100". I'm making simple molds for plastic panels, face each side and cut a pocket in one side 0.375" deep. The problem I'm having is tool wear and I've got double flood nozzles flooding the tool with coolant. The carbide tools are wearing down about 0.002-0.004" after just one mold.

    Here's the code (BP Boss 5.0)


    Line 70 includes a pause where I turn the plate over. The feeds at the end of the G78 pocket cycle are roughing and finishing. The BP software interprets F60 as 6 IPM. Each face pass takes about 2 hours, I left and came back while it was running the pocket pass. I've got my coolant sump setup in a 25 gallon carbouy and I've built splash shields around the table so I can run the coolant flow pretty high to help flush chips as well as cool the tool.

    This jobs a freebie for my company since they let me set up my shop there and they are paying for the tools and materials. My concern has to do more with learning as well as precision, a worn tool won't remove the metal it's told to do after all.

    Any and all suggestions are welcome.


  • #2
    Forgot to add, I'm trying to get a bunch of work done on the CNC before winter so I can finally install the new controls I bought over a year ago LOL. No laughing at me Dave! hehe, BTW glad to see you back around the board.


    • #3
      I can understand your confusion, I do not see any problems with your settings or method to cause that.
      Carbide just does not wear like that on 1018 on a single piece ????

      Is there substantial heat being generated at any time where the coolant may be then trashing the cutter by thermal shock?

      Is the cutter diameter actually worn or is the part out of tolerance by the .002 - .004 ?



      • #4
        Thanks Ken,

        The cutter is visibly worn at the tips where most of the cutting is done. The bottom edge of the wall of the pocket is out by the amount the cutter is worn. This is because the pocket is cut in four passes of increasing depth and each pass has a 0.040" finish pass, the result is the top three passes got finished by cutter flutes that had been previously untouched.

        I've been going over it in my head as well as looking at the thread about carbide tooling and think I have a partial clue. On my facing cycle (G77) the cutter partially exits the metal on each end so that half the cutter diameter is cutting air. I'm wondering if the resulting interrupted cut, although brief, isn't the culprit. Tommorrow (today, I'm up late) I'll adjust the code so that the cutter doesn't exit the metal on the facing pass and see what happens.

        Since this is just simple cycle programing there really aren't any areas where excessive heat would be generated. I was concerned about chip buildup in a 0.375 deep pocket but I had enough coolant flow to remove about 60-80% of the chips from the pocket which is pretty good and far better than my old coolant setup. Having two coolant nozzles ensures the cutter is always getting fresh coolant. I suppose I should examine the cutter under the microscope in my lab to determine if it's wear or chipping of the tool. If it's just wear I'm out of ideas but if the cutter is actually chipped then perhaps my theory about the facing pass is correct. Of course the only way to know for sure will be to adjust the code and run another part.
        Last edited by rsr911; 09-07-2006, 01:29 AM.


        • #5
          Drop the revs a bit and use a coated HSS cutter.
          Everyone thinks that carbide is the answer to everything but unless you have immense rigidity it isn't always so.

          I did a job a while ago, 1500 pieces of stainless stamping 1/16" thick, one edge had to be reduced to 1/32" thick by 1/8" wide, hardly hogging material.
          I made a jig to hold 12 pieces and one pass with a 12mm cutter would do 6 a side.

          First 100 or so went OK then I noticed that the corner was rounding off, no problem as that isn't critical but it got worse, swap cutters, I had bought 2 in for the job and the edges on the first cutter were rubbed round.

          Another 200 or so and this one was U/S, no spare cutters, no delivery until Monday so I swapped to a HSS cutter just to get me through.
          That one HSS cutter did the other 1200 or so with no edge degrading.

          Sir John , Earl of Bligeport & Sudspumpwater. MBE [ Motor Bike Engineer ] Nottingham England.


          • #6
            Originally posted by rsr911
            Thanks Ken,
            I've been going over it in my head as well as looking at the thread about carbide tooling and think I have a partial clue. On my facing cycle (G77) the cutter partially exits the metal on each end so that half the cutter diameter is cutting air. I'm wondering if the resulting interrupted cut, although brief, isn't the culprit.
            I'll add my two cents, on what I do with carbide on a daily basis. First, milling is an interrupted cut anyways, you aren't going to make it more or less interrupted.

            At 1500rpm, your at about 200sfm, which should last just about forever in 1018 running with a fairly high pressure coolant. The problems that I see are the fact that your coolant isn't able to blow all the chips out of a .375 pocket, and your concern over making a more interrupted cut, leading me to believe that you are using a very large stepover, which results in almost a conventional cut on the way in, which results in a ton of heat, which, unless you have a high pressure coolant, results in a steam pocket at the cutting edge, which then results in thermal shock and breakdown of your endmill.

            Another thing that I would look at is a feed of 6ipm is only .004" per rev, which isn't much of a feed, and could result in more pushing than cutting, the result of which is more heat, and more thermal shock, and less tool life.

            My suggestion, dump the coolant(an airblast doesn't hurt to clear chips), I was scared of running carbide endmills dry for a long time, but they really like it and as long as you aren't recutting chips, you'll be fine. With an uncoated carbide endmill, you can easily run 350-400sfm(2600-3000rpms), and feed at least .002 per tooth(the heat has to go with the chip), with a 50-65% stepover. If you're using a standard 4 flute, you might run into chatter, in that case I would go with either a carbide rougher, or a variable flute, in which case you can increase the feed up to .003 or .004 per tooth. If you're TiAlN coated you can push up the RPMs even further also.

            Its hard to give good advice without standing in front of the machine and seeing what the situation is. Another thing to realize, cheap carbide can be really really crappy, money spent on good tools is never a mistake, there are times when a single $50 endmill can easily outlast and outperform 10 $25 endmills.


            • #7
              I don't know that any carbide endmill can take 8 hours cut time.

              I would get a 3/4" cobalt hss hog mill, rough the whole thing out in one pass, and save the carbide for a finish pass.




              • #8
                Thanks for the additional input guys. A few notes,

                I'm using high quality endmills, my stepover is 0.100, depth of cut for the facing pass is 0.050, depth of cut in the pocket is 0.100 for the first 3 passes and 0.075 on the final pass. I have an air mist system but my shield around the mill isn't enough to contain the chips when blasting out of a pocket so I elected to use coolant on this project. I can put smaller nozzles on the flood system and open the flow all the way, this would likely remove 90% or more of the chips. While not ultra rigid, my CNC is a Bridgeport Boss 5 Rigid Ram which makes a manual BP look like a flimsy toy in comparison. I have faced plates with an indexable 2" endmill and gotten a beautiful finish with this mill, in this case I wanted to do it all with one tool as the machine is largely unattended hence the small stepover and reduced feed rate. I haven't had much luck pushing feedrates on similar jobs in the past so I tend to go a little conservative to insure the job gets done without a broken tool. One job I run each part takes 45 minutes and includes a circular pocket as well as a 0.5" deep slot around the outside and several drilled holes, the same 5/16" endmill is still in great shape after 48 parts (36 hours run time). Cleaning up the mill this morning I examined the chips and all are uniform with no blueing as would be the case with overheating (usually). I'm going to examine the bit next and I'll go ahead and up the feed rate as suggested. This time I'll start the program at such a time that I'll be able to watch the pocket cycle so I can check for any clues. I'll report back what I've found.

                John, I'm clean out of HSS endmills but since they are buying I'll pick some up.


                • #9
                  {I would get a 3/4" cobalt hss hog mill, rough the whole thing out in one pass, and save the carbide for a finish pass.} My thoughts, exactly.


                  • #10
                    OK, I know when to accept advice LOL. However wouldn't I be better off with a 1/2" rougher? My concern is the inside corners of the pocket, with a 3/4" I'll have a lot of material in the corners to remove on a finish pass. Or should I use a 3/4 rougher, then rough the corners with the 1/2 carbide, then finish? Should I even use carbide on the finish pass, wouldn't I get a better finish with coated HSS if all I'm doing is a 0.020-0.040 finish pass?


                    • #11
                      What little CNC experience I've had; I'd say the cutter slows down, but not dwell in the corners. All that depends on the rigidity of the machine, spindle, cutter, ways, and a million other things that we just can't see on the net.
                      Last edited by Millman; 09-07-2006, 09:36 AM.


                      • #12
                        Don't know your machine, but why are you using .020-.040 for a finishing pass? Your machine must be awful rigid to hold a tight tolerance using a finish pass that deep. That could cause cutter flex.


                        • #13
                          Originally posted by Millman
                          Don't know your machine, but why are you using .020-.040 for a finishing pass? Your machine must be awful rigid to hold a tight tolerance using a finish pass that deep. That could cause cutter flex.
                          What would you recommend for a finish pass? Default for the machine control on a pocket cycle is 0.020" I'm open to any ideas.


                          • #14
                            Like I said, I don't know your machine; I would think .005-.010 for finish. Cut some deep pockets in hard materials using .002 for finish. All depends on the rigidity and sharpness of the cutting edges.


                            • #15
                              I know very little about CNC and am certainly no expert, but I would offer a general thought. The information comes from talking to folks much wiser than I about the use of carbide tooling.

                              1. There is a tendancy to think that straw or blue chips are bad. In point of fact, they represent heat *in the removed material* which is the desired effect. If you don't take enough material to heat the chip, you heat just the contact point of the cutter and heat kills cutting surfaces.

                              2. Shallow cuts with carbide tend to wear out the tool before you get the job done. The rigidity and wear characteristics of carbide are such that it is happiest doing plenty (but not *too* much) work. Chipload needs to be high enough that you are not just burnishing the cutter

                              In reality, 2 and 1 are related. The cutter wears whether fed to the point of creating what would be considered a "normal" chipload, or set to cut a fraction of that amount. If it takes many more "passes" of a given cutting surface to get the job done, then making light passes may be counter-productive in terms of tool life.

                              I would think I would be tempted to work on using a larger tool for the surfacing you indicate takes 2 hours. If you think of 2 hours of cutter wear per part for that operation alone, that seems like you are well on your way to wearing out the small cutter doing a large job.

                              Paul Carpenter
                              Mapleton, IL