584,860 active members*
4,928 visitors online*
Register for free
Login
Page 1 of 6 123
Results 1 to 20 of 101
  1. #1
    Join Date
    Dec 2003
    Posts
    673

    Tips to improve surface finish?

    Hi all. Cut my first part on my series III today, and would like to improve surface finish. Can you share some tips?

    Its a tiny part about .4x.7in. made from .125 thick 6061, fully contoured on the outside.
    - Kress 1050w motor
    - .125 2 flute solid carbide cutter
    - 11in/min feed
    - ~7000rpm speed (not sure, don't have a tach to check it, but minimum speed of the motor is 5000rpm)
    - Flood coolant, Tormach variety at 20:1 dilution
    - Cutter is "choked up" into the collet right to the start of the flutes to minimize unsupported length
    - Climb cut

    I experimented with feeds from 2-12ipm, and speeds from 6000-15000 rpm, coolant, no coolant, and air blast for coolant, but all the parts look about the same. Seeing a bit of taper top to bottom, tooth marks, and some recutting/burnishing. On my "homemade" Grizzly G1106, I got pretty nice finishes with the same cutter at about 3000rpm and ~2ipm with mist coolant. Would like to ramp up the speed a lot, but keep a decent finish. Its not horrible, but would like to get a cleaner cut I don't have to hand sand to look "eyeball" decent.

    Its hard to get a natural picture of something this small, and I exaggerated the finish in software, but you'll get the idea. The top surface is a good finish that I'd like to match. The wall thickness at the hole is .025 to give you some scale.
    Attached Thumbnails Attached Thumbnails IMG_0629.jpg  

  2. #2
    Join Date
    Oct 2008
    Posts
    103
    Glad to see you up and running.
    Try stacking them 3 levels high (3/8" depth of cut). Switch to a 3/16" carbide 2 flute EM, 5100RPM at about 7.5ipm (or about 9ipm if you have a TIN-coated EM). And use the Tormach spindle, not the Kress high speed.
    Looks like you're losing rigidity in the companion spindle.

  3. #3
    Join Date
    Aug 2006
    Posts
    143
    could be chips binding up in the pocket. I find the only way I can get a decent finish is to leave .010" stock on the part and then do a finish pass after I clean out the chip trough.
    I also second moving up to a 3/16" cutter. I made a fixture plate with a but-load of holes in it. I do all the interior machine work then rough the part out of the stock. Then I transfer it to the tooling plate and do a finish pass around the whole perimeter. A lot more setup work but I can get really good edge finishes that way.

    Derek

  4. #4
    Join Date
    Oct 2011
    Posts
    0
    Your feedrate is less than .001 per tooth and at 7k rpm you're just over 200sfm

    Not sure what machine you're running and how much of a concern rigidity is, but in my books that is very slow for aluminum.

    Make sure your cutter is plain and very sharp. I've got more cutters than I can count that most of the people on this board would drool over and tell me are sharp enough, but they're not.

    Picture didn't load for me, so I'm just giving an opinion based on what I read.

  5. #5
    Join Date
    Dec 2003
    Posts
    673
    Thanks guys.. .125 is as big as I can use without a tool change. Is there a guide somewhere on FPT by cutter and material? I thought AL at this size .011 FPT was about right? Since my old machine was so slow, I'm actually a bit chicken to run past the 11ipm I'm already at on this little part... seems to mow right through it pretty quick. I'll do some more experiments, and try the main spindle. I hope the Kress and brackets wasn't a huge waste of money....

  6. #6
    Join Date
    Oct 2011
    Posts
    0
    Picture loaded.

    Yikes.

    How are you holding the part? That is some serious chatter.. I definitely wouldn't be increasing the feed. It's hard to tell but is that the actual surface, or have chips welded to the surface? The angular nature of the finish tells me its a chatter issue, which boils down to rigidity.

    Are you conventional or climb cutting? You may want to switch to the opposite of what youre currently using just to give it a try with the same feeds/speeds to see if it helps, and then work with the speeds and feeds from there.

    You don't mention any dimensions other than it being really small.

    You could be overloading the cutter leading to deflection and vibration which would lead to your issues.

    Also remember, even if you leave a small finish pass, if the prior rough pass looks anything like the picture, no matter how slow you take it the surface variability will be transferred to the endmill and thus to the final finish pass.

    First id examine how you hold the part, then the concentrocoty of the endmill to the holder and the spindle, if its out of whack problems are only going to be amplified, which is why when you get into smaller tools this becomes very critical and you get into things like shrink fit holders and the likes.

  7. #7
    Join Date
    Dec 2003
    Posts
    673
    Quote Originally Posted by SirDenisNayland View Post
    Picture loaded.

    Yikes.

    How are you holding the part? That is some serious chatter.. I definitely wouldn't be increasing the feed. It's hard to tell but is that the actual surface, or have chips welded to the surface? The angular nature of the finish tells me its a chatter issue, which boils down to rigidity.

    Are you conventional or climb cutting? You may want to switch to the opposite of what youre currently using just to give it a try with the same feeds/speeds to see if it helps, and then work with the speeds and feeds from there.

    You don't mention any dimensions other than it being really small.

    You could be overloading the cutter leading to deflection and vibration which would lead to your issues.

    Also remember, even if you leave a small finish pass, if the prior rough pass looks anything like the picture, no matter how slow you take it the surface variability will be transferred to the endmill and thus to the final finish pass.

    First id examine how you hold the part, then the concentrocoty of the endmill to the holder and the spindle, if its out of whack problems are only going to be amplified, which is why when you get into smaller tools this becomes very critical and you get into things like shrink fit holders and the likes.
    Thanks... Its about .7x.4in, with a .025 wall at the thinnest part and .125 thick. climb milled, and finish accentuated in photoshop, so it looks more extreme than it is. The top face is mill finish with a scuff of 320 for reference. On my very non-rigid previous machine with the same cutter and same fixture, stick out etc... I got a better finish, with certainly less accurate tool holding and less rigidity. Maybe I'll just slow the whole thing way down, like my old setup, and work from there... will try that tomorrow.

  8. #8
    Join Date
    Feb 2007
    Posts
    1041
    I cut small pieces like this all the time and can tell you use the machines spindle. The larger the cut diameter, the better. I design most of my parts around my tool library. I spiral rough (carbide coarse 3FL) cut and finish with a ZRN carbide coated 2 - 3 FL EM. Here's a few to show







    Final




    I also design a lot of fixtures to hold the parts for 2nd, 3rd, 4th, etc.. mop. I use to cut these with a .125" cutter but wanted more speed, so I dropped one part to save 5 mins or so on each plate. Anyway hope this helps, let me know if you need anymore help










    .

  9. #9
    Join Date
    Mar 2009
    Posts
    1863
    When you're profile cutting there are three things that are really, really important. They are RIGIDITY, RIGIDITY AND RIGIDITY, OH, and did I mention RIGIDITY.

    It looks to me that with that Kress spindle you ain't got it.

    I use cutters as small as 1/16 diameter in my PCNC 1100, and have never had a finish like that. I typically run 4,000 to 4,500 RPM 12 to 15 IPM feed. If I want a really good finish on the sides, I will slow the RPM down to 3,000 and leave the feed at no less than 12 IPM.

    When I have large amounts of material to remove, I'll use a larger end mill and leave .005 to .010 stock for finish.
    You can buy GOOD PARTS or you can buy CHEAP PARTS, but you can't buy GOOD CHEAP PARTS.

  10. #10
    Join Date
    Jan 2012
    Posts
    789
    I agree with Steve. Something isn't rigid. It's either your work holding, your spindle, or your tool. I recently had to do some 1.25" deep slotting with a 1/4 EM. The surface looked just like that, and that was with a 1/4" EM. I knew I was going to get chatter, and boy, did I! Thankfully the surface quality didn't matter at all on that slot, I needed it quickly.

    A rule of thumb, is that if your cut is squealing, it is vibrating, and you will get a bad finish.

  11. #11
    Join Date
    Dec 2003
    Posts
    673
    Thanks...

    I took off the kress, put a fresh cutter in a TTS collet, choked it up so just the flutes are showing and put the cutter down as far as possible in the cut (the material is in free air, so can go past the floor of the stock).

    I'm at 1.25 DOC (full material thickness), 5000rpm but only 4ipm in a single pass. It practically makes no noise in the cut, and the finish is ok now. Could the finish actually improve by a higher feed rate? Seems I'm balancing reweld with tool marks. May need to experiment more. Unfortunately I'm only making a few parts at a time, so elaborate fixtures just don't make sense. I'd also like to do a single pass - the finish doesn't have to be perfect.

    There's a drop of coolant on the part so it distorts the picture a little bit and its hard to get it to show what my eyes see, but compare the finish to the as shipped surface finish. Seem ok? The only chatter seems to be on the visible 1/4 diameter which I'm attributing to a bit of backlash (backside is fine) Other thoughts?
    Attached Thumbnails Attached Thumbnails Tormach He-111 Oleo Stay.jpg  

  12. #12
    Join Date
    Feb 2006
    Posts
    7063
    Seeing that last picture, I can tell you for certain part of your problem is the part is very poorly supported, which will make getting a really good surface finish near impossible. You should leave as much support as you possibly can to do the bulk of the cutting and finishing, then do a final op to remove the support. Cutting on that piece as it is, cantilevered way out into thin air, the workpiece will be able to move around a LOT, while you're doing even a very light pass.

    You'd be much better off cutting it on a fixture that would allow you to mill out that center hole, then lock the piece to the fixture with a bolt so it's fully supported, THEN cut the outside profile.

    Regards,
    Ray L.

  13. #13
    Join Date
    Dec 2003
    Posts
    673
    Quote Originally Posted by HimyKabibble View Post
    Seeing that last picture, I can tell you for certain part of your problem is the part is very poorly supported, which will make getting a really good surface finish near impossible. You should leave as much support as you possibly can to do the bulk of the cutting and finishing, then do a final op to remove the support. Cutting on that piece as it is, cantilevered way out into thin air, the workpiece will be able to move around a LOT, while you're doing even a very light pass.

    You'd be much better off cutting it on a fixture that would allow you to mill out that center hole, then lock the piece to the fixture with a bolt so it's fully supported, THEN cut the outside profile.

    Regards,
    Ray L.
    Thanks Ray.. Yep, I get that. I make lots of little parts, but only a few any given part, making a bunch of fixtures not practical... Maybe I'm close enough, and will just bead blast or run through the vibe'.. Most of the parts should get painted too. Similar to your suggestion, I guess I could take a strip of material, and then just bore the holes and cut the slot on the end, then cut off, and do one at a time in a fixture with a screw in the main hole and a pin in the slot to cut the outer profile.. I've done that on my old machine, but it was a time consuming way to do it. Another idea - I suppose I could do like I have it, but have a pause in the program to put a support post through the hole before cutting the profile.. hmm.. that might be a good compromise that's easy to do.

  14. #14
    Join Date
    Jan 2012
    Posts
    789
    Looking much better. Pretty much all your gains to be had now are in your fixturing, like Himy says.

  15. #15
    Join Date
    Feb 2006
    Posts
    7063
    Quote Originally Posted by Spinnetti View Post
    Thanks Ray.. Yep, I get that. I make lots of little parts, but only a few any given part, making a bunch of fixtures not practical... Maybe I'm close enough, and will just bead blast or run through the vibe'.. Most of the parts should get painted too. Similar to your suggestion, I guess I could take a strip of material, and then just bore the holes and cut the slot on the end, then cut off, and do one at a time in a fixture with a screw in the main hole and a pin in the slot to cut the outer profile.. I've done that on my old machine, but it was a time consuming way to do it. Another idea - I suppose I could do like I have it, but have a pause in the program to put a support post through the hole before cutting the profile.. hmm.. that might be a good compromise that's easy to do.
    The "fixture" doesn't need to be anything more than a scrap piece of aluminum plate with a few threaded holes in it. I rarely make parts without making such a fixture, and have several plates with numerous holes in them to accommodate many different parts.

    Regards,
    Ray L.

  16. #16
    Join Date
    Dec 2003
    Posts
    673
    Quote Originally Posted by HimyKabibble View Post
    The "fixture" doesn't need to be anything more than a scrap piece of aluminum plate with a few threaded holes in it. I rarely make parts without making such a fixture, and have several plates with numerous holes in them to accommodate many different parts.

    Regards,
    Ray L.
    Hmm. Only bit remaining is how to index that fixture quickly... The wall thickness is <.025 on that hole, so its real easy to see if the hole is not concentric with the outer radius... You guys got me thinking though, and I'll figure out some simple fixture.

  17. #17
    Join Date
    Oct 2011
    Posts
    0
    Personally id mill the entire thing out of a block, and then flip it and flycut the top off.

  18. #18
    Join Date
    Apr 2006
    Posts
    439
    Quote Originally Posted by SirDenisNayland View Post
    Personally id mill the entire thing out of a block, and then flip it and flycut the top off.

    +1

    If you do not want to make fixtures this is the way to do it. You get to machine 5 sides of a block with one set up. Then flip it and deck it to the proper thickness. Or even use a slitting saw to liberate them from the base material.

    Scott
    www.sdmfabricating.com

  19. #19
    Join Date
    Dec 2003
    Posts
    673
    Ok, thanks for the ideas... I'll work on fixturing... what kinds of feeds should I be able to get? 11ipm? I'm at 4 now.... I also "finished" for the moment anyway, my initial setup and here's my cheapie version of the "shower curtain" mod... the little shield box was pretty much a waste for me as it didn't fit the 4th axis and was kind of a nuisance.
    Attached Thumbnails Attached Thumbnails IMG_1541.JPG  

  20. #20
    Join Date
    Oct 2011
    Posts
    0
    Quote Originally Posted by Scott_M View Post
    +1

    If you do not want to make fixtures this is the way to do it. You get to machine 5 sides of a block with one set up. Then flip it and deck it to the proper thickness. Or even use a slitting saw to liberate them from the base material.

    Scott
    I actually can't really think of any other way to do it.. not sure how the threadstarter was. I mean, you have to start with the block anyway
    Hmm.

    You will need a fixture of some sort to hold it on the flipside to remove the remaining material though. Id probably use some sort of a stationary arbor mounted in a vice.

Page 1 of 6 123

Similar Threads

  1. Tips on a really nice side milled finish in aluminum
    By Kerry Harrison in forum Bridgeport / Hardinge Mills
    Replies: 5
    Last Post: 12-29-2009, 04:29 PM
  2. how to improve surface quality?
    By davidsutton in forum Uncategorised CAM Discussion
    Replies: 4
    Last Post: 07-15-2008, 01:27 PM
  3. Replies: 22
    Last Post: 06-30-2008, 05:42 PM
  4. Surface Finish
    By life3970 in forum Mini Lathe
    Replies: 2
    Last Post: 11-07-2007, 07:00 PM
  5. surface finish
    By fadalman in forum BobCad-Cam
    Replies: 2
    Last Post: 03-03-2007, 08:30 AM

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •