1. This site uses cookies. By continuing to use this site, you are agreeing to our use of cookies. Learn More.
  2. PLEASE: Read the FORUM RULES BEFORE registering!

    Dismiss Notice

How Should I Machine This?

Discussion in 'CNC IN THE HOME SHOP' started by Metal, Aug 24, 2016.

  1. Metal

    Metal United States Active Member Active Member

    Likes Received:
    80
    Trophy Points:
    28
    City:
    Buffalo
    State:
    New York

    -Return to Top-

    Just a quick question really
    apparently image didn't post, here
    https://s10.postimg.org/hy9c8gjp5/dive.jpg

    upload_2016-8-24_8-22-23.png

    I'm still figuring out the new CNC, I've noticed that when coming around a corner, the bit has a tendency of being pulled up into the work exactly how I assume it would be due to the forces on the bit (note this is all roughing passes)

    I "assume" this is unavoidable with a machine that has backlash since the mill moves upwards, then the torque from the cutter is what is dragging the table across the backlash zone and into the work before the cnc compensates. if I was doing this manually I'd lock the table, which the cnc can't do.

    So my questions are
    1: is this avoidable (I'm guessing not)
    2: again assuming not, how much stock should I leave around the part for a finishing pass, My assumption again is around 2x the depth of the "dive" or .05", which ever is more, since passes less than .05" in aluminium tend to not cut it very well.
     
    Last edited by a moderator: Aug 24, 2016
  2. dlane

    dlane Active User H-M Supporter-Premium

    Likes Received:
    618
    Trophy Points:
    113
    Location:
    Lake oroville
    City:
    Oroville
    State:
    California

    -Return to Top-

    I'll guess you are useing tapatalk camera icon , not paper clip , all I see is the infamous red "X"
     
  3. jbolt

    jbolt United States Active User H-M Supporter-Premium

    Likes Received:
    856
    Trophy Points:
    113
    City:
    Mountain View
    State:
    California

    -Return to Top-

    What is the machine, material, cutter, depth of cut, width of cut, feed rate?
     
  4. JimDawson

    JimDawson Global Moderator Staff Member Director

    Likes Received:
    3,769
    Trophy Points:
    113
    City:
    Sandy
    State:
    Oregon

    -Return to Top-

    I fixed the picture for you!

    The first thing I notice from your picture is you are conventional cutting, if your machine will do it, climb cutting is the prefered method.

    The next thing I notice is that your feed speed looks a little fast for the spindle speed. Maybe bump up the spindle speed or slow down the feed. Your cutter could be a bit dull also, maybe try a different cutter. Are you keeping the tool wet with coolant, I see what looks like fuzz ''welded'' to the surface.

    Maybe try taking smaller bites, both depth and step over, it takes longer to make the part, but the quality generally goes up. In the home hobby shop time is not normally an issue. If you are doing this for profit, then some maintenance on your machine might be in order. Maybe just snugging the gibs a bit would be helpful.

    I normally leave 0.010 for the finish cut.
     
    dlane likes this.
  5. Metal

    Metal United States Active Member Active Member

    Likes Received:
    80
    Trophy Points:
    28
    City:
    Buffalo
    State:
    New York

    -Return to Top-

    Thanks for the advice, this was purposely roughing to test the cnc's accuracy at a higher load and with an old dull cutter since I wasn't sure if it was going to snap at this speed, I was just looking to address the dive issue circled at this time.

    This is with a 3/8" endmill @ 1100 or so rpm, ~14ipm .1" doc. 6061 aluminium These servos could easily exceed 100ipm so I'm being gentle, I'm trying to resolve issues as I move up to a hopeful 20ipm cutting rate rather than just start at that rate and break a bunch of things figuring it out.

    I am conventionally milling because the bridgeport doesn't have ball screws and its going to be less problematic.
     
    ncf250sd likes this.
  6. Billh50

    Billh50 Active User H-M Supporter-Premium

    Likes Received:
    947
    Trophy Points:
    113
    City:
    New Britain
    State:
    Connecticut

    -Return to Top-

    Jim is quite right in what he said. If your machine is not rigid enough you may want to take several passes conventional milling and leave about .015 for a final pass climb milling. Climb milling tends to leave a much better finish with the right speed and feed. But definitely use either a spray or flood coolant to keep chips from welding themselves to side as the cutter passes.
     
  7. Metal

    Metal United States Active Member Active Member

    Likes Received:
    80
    Trophy Points:
    28
    City:
    Buffalo
    State:
    New York

    -Return to Top-

    so how would that address the dive issue illustrated above?
     
    rdean likes this.
  8. jbolt

    jbolt United States Active User H-M Supporter-Premium

    Likes Received:
    856
    Trophy Points:
    113
    City:
    Mountain View
    State:
    California

    -Return to Top-

    Your spindle speed is too slow for a 3/8" 2-flute cutter in aluminum for that feed rate. Would be okay for a 4-flute but with aluminum they don't evacuate chips well and tend to load up even running flood coolant.

    I wouldn't recommend experimenting with a dull cutter. I don't think you will learn much other than dull cutters produce poor finishes.

    I suspect the over run issue is the backlash on the lead screws. Are your gibs snug?
     
  9. JimDawson

    JimDawson Global Moderator Staff Member Director

    Likes Received:
    3,769
    Trophy Points:
    113
    City:
    Sandy
    State:
    Oregon

    -Return to Top-

    Using a dull cutter will increase the dive. The cutting pressures are much greater and much more spring in everything. The cutter is doing more rubbing than cutting, especially when conventional cutting.

    Here is a staged picture of a bearing mount I machined last night just to put things in perspective. Material is 6061-T6
    upload_2016-8-24_10-53-35.png

    I still had the G code loaded so I fired up the machine and grabbed a screen capture of the running machine cutting air.

    The DOC is 0.125, a sharp solid carbide 3/8 end mill, climb cutting. Kerosene in the fogless coolant system. Finishing passes were at 0.010

    This is real time cutting parameters. The inputs come from the G code, actual spindle speed, and actual axis vector speed. The cutting speed and chip load are calculated from the inputs. Also accepts manual inputs for calculating feeds and speeds when not running.

    upload_2016-8-24_10-52-46.png

    This may help a bit getting you started in the right direction to address the issues.:)
    .
    .
     
  10. Boswell

    Boswell United States Hobby Machinist since 2010 H-M Supporter-Premium

    Likes Received:
    89
    Trophy Points:
    28
    City:
    Cedar Park
    State:
    Texas

    -Return to Top-

    I'm not sure I understand your initial post. Are you implying that you have 0.05 backlash? If that is the case, you probably need to figure that out before making parts. No amount of optimizing feeds and speeds or coolant will fix a 0.05" backlash. I also tend to leave 0.015" for a finnish pass and use climb milling most of the time. For a 0.375 two flute cutter. 0.1 DOC at 1100RPM and full cutter width slotting, GWizard sayd that a very aggressive rough cut would be 7.9 IPM and (as a hobbyist with more time than money) I never use the most aggressive end and for roughing using go about midway between aggressive and conservative, in this case GWizard recommends 4.8 IPM . I typically cut using 2750 RPM and in this case that would allow the 4.8ipm to increase to 12.3 ipm. Also note that GWizard assumes you have proper chip removal in place (Flood coolant, or Misting system etc).
     
  11. Metal

    Metal United States Active Member Active Member

    Likes Received:
    80
    Trophy Points:
    28
    City:
    Buffalo
    State:
    New York

    -Return to Top-

    adjusting gibs, stepping up the rpm a tad (48 to 50 hrtz on vfd) and reducing lead in speed seems to have helped (and adding the finishing pass), the features are slightly trapezoidal so I have backlash over compensating or leadscrew wear to address but I think we're okay at that point.

    I was under the impression you don't want to climb cut in a machine with leadscrews unless taking very small cuts (or I could adjust the gibs /really/ tight(?) so what is the story there?
     
  12. TomS

    TomS Active User H-M Supporter-Premium

    Likes Received:
    409
    Trophy Points:
    83
    City:
    Redding
    State:
    California

    -Return to Top-

    I climb mill on my RF-30 all the time but with a bit of caution. I adjust the depth and width of cut to minimize the chance the cutter will grab and pull the work piece into the cutter. My gibs are not adjusted tight but not loose either.

    I use climb milling almost exclusively on my CNC mill leaving about .010" for the finish pass.

    Tom S.
     
    JimDawson likes this.
  13. JimDawson

    JimDawson Global Moderator Staff Member Director

    Likes Received:
    3,769
    Trophy Points:
    113
    City:
    Sandy
    State:
    Oregon

    -Return to Top-

    It is related to backlash, when climb cutting the work is being pulled toward the cutter. The heavier the cut the harder it is being pulled. The machine has to be rigid enough to overcome this force. If there is backlash the table can move uncontrolled for the distance of the backlash on a transition, this can cause the tool to grab. Tightening the gibs will help by adding friction to the system, but you can only go so far with this. The way to really fix the problem is to eliminate the backlash.

    Does your machine have acme lead screws or ball screws?
     
  14. Metal

    Metal United States Active Member Active Member

    Likes Received:
    80
    Trophy Points:
    28
    City:
    Buffalo
    State:
    New York

    -Return to Top-

    It has lead screws which is why I was sticking to conventional
     
  15. JimDawson

    JimDawson Global Moderator Staff Member Director

    Likes Received:
    3,769
    Trophy Points:
    113
    City:
    Sandy
    State:
    Oregon

    -Return to Top-

    In that case, maybe the best bet is to do the roughing conventional, then climb cut the finishing pass(es) Or just take smaller bites so the mass of the machine helps to overcome the tendency of the tool to grab. Lighten up the DOC and stepover rather than reducing the feed. The cutter needs to cut rather than rub, sharp cutters will help.

    For any really serious work the only solution is to install ball screws, preferably double ball nut so they can be preloaded. Unfortunately it's impossible to have a zero lash acme screw / nut. If there was zero clearance it wouldn't turn.

    I wish I had a better answer for you.
     
  16. Metal

    Metal United States Active Member Active Member

    Likes Received:
    80
    Trophy Points:
    28
    City:
    Buffalo
    State:
    New York

    -Return to Top-

    I've had a backlash laden mini mill cnc'd for about a year, it hasn't been a huge issue for me, the bridgeport cnc is just proving much harder to tune up to where I want it.
     
    brino likes this.
  17. JimDawson

    JimDawson Global Moderator Staff Member Director

    Likes Received:
    3,769
    Trophy Points:
    113
    City:
    Sandy
    State:
    Oregon

    -Return to Top-

    One totally crazy idea comes to mind, you could preload your lead screws with air springs. Connect air cylinders to the X & Y axis on the table and it would eliminate the backlash. I'm doing this with my Z axis, but I never thought of trying it on the table. Probably not really practical.:confused:
     
    brino likes this.
  18. Metal

    Metal United States Active Member Active Member

    Likes Received:
    80
    Trophy Points:
    28
    City:
    Buffalo
    State:
    New York

    -Return to Top-

    Well that certainly is one way of increasing resistance!

    I could push the machine more softly, but truth be told I just don't want to run the bridgeport at full speed (over 3k rpm) until I get it tuned in, and have a shield of some sort in place since this is quite a bit scarier than my little hobby mill. But I've picked up a handful cheap of 3 flute hss 12mm endmills that I'm not afraid of breaking that I'm going to try tonight probably with some new code to be a little more gentle once I properly setup backlash comp again.

    I also need to rebuild the head as low gear is noisy and I'm getting grey oil at the base of the spindle probably because of it but that is for another day.
     
  19. jbolt

    jbolt United States Active User H-M Supporter-Premium

    Likes Received:
    856
    Trophy Points:
    113
    City:
    Mountain View
    State:
    California

    -Return to Top-

    For projects that require a lot of material to be removed I've become a big fan of using roughing end mills for removing most of the material and only using standard end mills for finish cuts. Smaller chips, deeper cuts and faster feed rates.
     
    countryguy and brino like this.
  20. JimDawson

    JimDawson Global Moderator Staff Member Director

    Likes Received:
    3,769
    Trophy Points:
    113
    City:
    Sandy
    State:
    Oregon

    -Return to Top-

    I had the same problem when I first got my CNC. Was scared to death of all that new fangled stuff. I used it for about a year as a manual machine with a fancy DRO before I had the guts to actually run it as a CNC. It just takes some time to work up to that. :) It's a learning curve. Now after about 3 or so years I have confidence in me and the machine;)
     
    brino likes this.
  21. Metal

    Metal United States Active Member Active Member

    Likes Received:
    80
    Trophy Points:
    28
    City:
    Buffalo
    State:
    New York

    -Return to Top-

    Absolutely, in getting it working I had one servo runaway with the belts attached, magmotors at full spin are terrifying fast, I was luckily able to estop before the axis hit its endstop but in my mind that could have cracked the cast iron and I"d have a 3000lb paperweight in my basement.

    I'm putting /huge/ rubber bumpers at the ends of travel due to being paranoid, but this thing is /awesome/ compared to the hobby mill, even at the above "conservative" 15ipm / .1 doc / less than half cutter engagement I can make the run for that part in the first post in under 5 minutes, that was like a 20 minute job before, plus fixtures/indicating because I could never get a big enough vice in the little one, and I'm not even going /fast/ yet.
    It is pretty exciting that I am this close to getting it running, I'm close to a year in on this project, hah.
     
    brino and JimDawson like this.
  22. Metal

    Metal United States Active Member Active Member

    Likes Received:
    80
    Trophy Points:
    28
    City:
    Buffalo
    State:
    New York

    -Return to Top-

    I've got this tuned out now, I went to a larger, sharp, 3 flute cutter which seems to have removed the dive

    Did some experimentation climb cutting, and even with a 1/4" ballnose not cutting much at all it wanders a little, so i'll stick to only using it for the final finishing pass. but moving on to more complex cuts and all is going well!
    I'm having some minor accuracy issues with some parts, but I believe that is leadscrew wear which I can't correct for until I get good home switches.
     

    Attached Files:

    • wat.jpg
      wat.jpg
      File size:
      28.7 KB
      Views:
      24
    brino likes this.
  23. JimDawson

    JimDawson Global Moderator Staff Member Director

    Likes Received:
    3,769
    Trophy Points:
    113
    City:
    Sandy
    State:
    Oregon

    -Return to Top-

    Sounds like you are on the right track. :encourage: That is a complex part, looking good!

    I'm not sure how home switches will help compensate for lead screw wear. Can you explain what you have in mind?
     
  24. Metal

    Metal United States Active Member Active Member

    Likes Received:
    80
    Trophy Points:
    28
    City:
    Buffalo
    State:
    New York

    -Return to Top-

    In mach3 you can create a grid basically, pick a spot on the table, tell it to move 1", then measure how far it actually moved in order to measure the wear on your leadscrew/nuts, off the top of my head I don't remember what the menu was (screw mapping?), but once you create the measurements mach3 can compensate for them so your parts dont end up slightly squished or stretched.

    But anyways, in order to map out that grid and have mach3 know its relative position according to it, you need a home position for mach3 to reference. Right now I don't have a home position at all so it has no idea where it actually is on the table, just from its work home reference point.

    Ive also noticed that I get a "moan" from the right side of the y axis at a certain point in its travel, only when moving in one direction... which I need to figure out.
     
    Last edited: Aug 30, 2016
    JimDawson likes this.
  25. JimDawson

    JimDawson Global Moderator Staff Member Director

    Likes Received:
    3,769
    Trophy Points:
    113
    City:
    Sandy
    State:
    Oregon

    -Return to Top-

    Ahhhh.... That makes sense. :eagerness: I remember seeing that screen.

    Strange. It is possessed? :cautious:
     
  26. TomS

    TomS Active User H-M Supporter-Premium

    Likes Received:
    409
    Trophy Points:
    83
    City:
    Redding
    State:
    California

    -Return to Top-

    I may be wrong but I thought I read where Mach3 has a limitation on backlash compensation. In other words if your backlash exceeds the maximum allowable then BL compensation doesn't work at all or Mach ignores the incremental backlash that exceeds the maximum allowable.

    Tom S.
     
  27. JimDawson

    JimDawson Global Moderator Staff Member Director

    Likes Received:
    3,769
    Trophy Points:
    113
    City:
    Sandy
    State:
    Oregon

    -Return to Top-

    Do a Google search for 'mach3 backlash compensation'. A lot of info on it.

    I see double nut ball screws in your future :)
     
  28. Metal

    Metal United States Active Member Active Member

    Likes Received:
    80
    Trophy Points:
    28
    City:
    Buffalo
    State:
    New York

    -Return to Top-

    I dont think its haunted, I think its the ways binding or some stuff got into them or wear on the ways (but they still had scrape marks so that would be strange), weird that its only in one direction.

    Backlash compensation is /fine/ I have it setup and it works great, the only issues I ran into was I had a mm indicator and imperial screws so I ended up with too many significant figures doing the conversion and ended up having to round it for mach3 to work right.

    What i'm (vaguely" seeing is my parts end up being a few thou longer than they should be, even if only traveling in one direction, its not really a big deal for the kind of stuff I make, but I should probably fix it.
     
  29. Metal

    Metal United States Active Member Active Member

    Likes Received:
    80
    Trophy Points:
    28
    City:
    Buffalo
    State:
    New York

    -Return to Top-

    May have figured out the noises, adjusting the gib appeared to do nothing, but adjusting the y axis belt did, it appears the servo belt drive is putting too much downards strain on the leadscrew or somesuch, i'll see if i can order a belt with one more tooth
     
    JimDawson likes this.
  30. JimDawson

    JimDawson Global Moderator Staff Member Director

    Likes Received:
    3,769
    Trophy Points:
    113
    City:
    Sandy
    State:
    Oregon

    -Return to Top-

    Cool! One little step at a time, but you're getting there :encourage: One of these days some pictures of your machine would be a good thing. :)
     

Share This Page