Page 1 of 19 12311 ... LastLast
  1. #1
    Getting near the end of my router/mini-mill build now and need to start looking at how to run jobs, i have a couple lined up already;)

    I'm not new to milling - been running a Bridgeport for some years now, not new to CNC - been using a plasma table for a year now, so that should all help. I use SheetCam to produce my G-Code and I think I have it pretty much sussed for the mill now, just looking for tips.

    This is the first job - pretty complex but what better way to learn;)
    Click image for larger version. 

Name:	untitled.jpg 
Views:	1043 
Size:	50.8 KB 
ID:	17925
    It's from 5mm 6061 Aluminium, has plenty of 3mm holes, slots, square features, its about 320mm long.

    So far I am looking at using a 2mm carbide 2-flute cutter, mist coolant, I have figured out how to get sharp corners, also how to spiral-down to cut the holes.

    Questions -

    1 - I have used a calculator for feeds and got 24,000rpm, 487mm/min feed, 1mm DOC, these seem reasonable?

    2 - I am unsure of DOC - this is input rather than output on the feed calculator - how do you know how much bite to take at one pass?

    3 - Holding tabs to keep it together on the outside cuts, I'm guessing three or four, 0.5mm thick or less?

    4 - Use the one cutter and go straight to dimension or split and do a roughing & finish passes?

    5 - Use a bigger cutter for the roughing outside then switch to the 2mm for the finish?

    6 - Features like the oval hole - leave it to fall out or use tabs again?

    Any suggestions appreciated, I realise this is fairly adventurous but I would like to get these made in-house to increase my profit margin considerably ;)

    Thanks

  2. #2
    How are you going to do the 90' corners?
    ..Clive

  3. #3
    Quote Originally Posted by Clive S View Post
    How are you going to do the 90' corners?
    There is a tool-path option in SheetCam that runs the cutter diagonally into the corner just enough to allow the resulting corner to accept a square cut object - a neat feature and with a 2mm cutter its barely noticeable.
    Last edited by Davek0974; 14-03-2016 at 06:19 PM.

  4. #4
    Hi Dave,

    Taking each point in turn:

    #1 Only ever used a 3mm carbide, nothing smaller. I think it would snap on my machine at those rates but possibly depends on how rigid your machine is.

    #2 DOC for 3mm carbide has been about 0.3mm for me. It's quite possible I'm shortening it's life doing this but it works well but I only use it occasionally and it's still going strong.

    #3 I'd use 4 holding tabs. Now in Vectric Cut2D the thickness is relative to the bottom of the cut. For that cut I would ask for 6mm total depth to make sure it went right through. Therefore 0.5mm tab would not actually hold the part and I'd need to input a tab depth of 1.5mm to get 0.5mm. I think I'd go for at least 2mm tab to make sure it did not vibrate on the last finish pass.

    #4 If the part is complex (long run time, chance of an e-stop or other problem) then I'd do a roughing cut leaving 0.1mm for the outside as a finish cut.

    #5 I would not attempt all that with 2mm cutter! Use 6mm or 8mm if possible to cut most of it out, then finish pass with the same bit, then go in again with the 2mm for the detail.

    #6 Don't leave the oval hole as a free cut. When the cutter gets to the end the oval part will jam against the bit and mark the work, then fly across the workshop. AMHIK.
    You can use tabs, but it is a pain to clean up by hand inside there, so better still is "pocket" it out (turn it all to swarf).

    As a strategy I think I would:
    Spot all the holes (leave finishing for the drill press)
    Pocket out all the internal holes and slots (i.e. not an internal profile)
    Rough profile the exterior with 6 or 8mm carbide, leaving 0.1mm
    Finish profile the exterior with 6 or 8mm carbide in one full depth pass (but still use same tabs as when roughing)
    Switch to 2mm cutter and profile the outside again to get the detail then profile the inside of the pockets
    Cut away the tabs and tidy up the edges by hand
    Building a CNC machine to make a better one since 2010 . . .
    MK1 (1st photo), MK2, MK3, MK4

  5. #5
    Quote Originally Posted by routercnc View Post

    As a strategy I think I would:
    Spot all the holes (leave finishing for the drill press)
    Pocket out all the internal holes and slots (i.e. not an internal profile)
    Rough profile the exterior with 6 or 8mm carbide, leaving 0.1mm
    Finish profile the exterior with 6 or 8mm carbide in one full depth pass (but still use same tabs as when roughing)
    Switch to 2mm cutter and profile the outside again to get the detail then profile the inside of the pockets
    Cut away the tabs and tidy up the edges by hand
    Thanks for that, interesting stuff, my response...

    I really don't want to drill the final holes, IMHO, spiralling down should work ok, will need to test it.

    Pocketing out the waste - brilliant point, probably never have thought of that one;)

    Rough profile exterior - makes sense but favour a 6mm rather than going bigger.

    Finish profile exterior with big cutter - if its only got 0.1mm to go, I'm not sure of the point, a 2mm solid carbide should handle that in one pass AFIK - test again.

    The smaller internal shape/pocket would need a smaller roughing cutter, probably 4mm, why not go to finish on the same tool?

    Tabs are the same in Sheetcam, bottom upwards. So if i have an aluminium bed, I would not want to request a 6mm cut on a 5mm sheet, I was thinking of using a sheet of stiff card or some-such between, I use a lot of 0.4mm hard card at work and that would likely work well, cut would then go to work plus 0.2mm.

    I'm generally against babying cutters, on the Bridgeport I find they are happier when taking a proper cut, within the abilities of the machine, but not tickling the metal, especially with carbide which has a larger edge radius than HSS and needs to 'cut' the metal.

    Some good points though, noted, thanks

  6. #6
    #1 With cutters less than 3mm I work on 30% diameter DOC.

    #3 Wouldn't use tabs I'd use Onion Skin of 0.1mm. This gets rid of any chance of bed damage and removes risk of lifting.

    #4 Rough and Finish passes. I'd use Large tool for Pocketing and Roughing then use small tool for Finish pass and corners cleanup etc.

  7. #7
    Thanks Jazz, more good tips.

    0.6mm DOC on a 2mm cutter sounds reasonable.

    I had seen onion skinning used on the woodworking forums but how do you go about cleaning it off on a job like this or is it easier than i think?

    Rough and finish - large and small makes sense, would use the same process for shapes like the large oval or just use the large tool staring to finish?

    Thanks

  8. #8
    Quote Originally Posted by Davek0974 View Post
    I had seen onion skinning used on the woodworking forums but how do you go about cleaning it off on a job like this or is it easier than i think?
    The part breaks out easy. Often it breaks out clean but even if the 0.1 skin is left on in places it just snaps off clean. Then quick whip round edge with De-bur tool and done.

    Quote Originally Posted by Davek0974 View Post
    Rough and finish - large and small makes sense, would use the same process for shapes like the large oval or just use the large tool staring to finish?
    Depends on Job really. If could get away with using same tool then I would but if Got to use small tool then it pays to use large tool to hog away material quickly then finish with small tool at full depth.
    Often people try to avoid tool change and use same small tool but this fasle economy in several ways.?
    Large tool will do it in fraction of time and with much less wear which more than offsets the tool change time. The small amount of material left also means the smaller tool is much less likely to break and also wear is less.

    All it means is you have to think a little differently when you Cam the part and order the toolpaths are generated when large amount of tools are used.
    Instead of having a operation which roughs then finishes in same toolpath before going to next area meaning lots tool changes. ie: Pocket operation then profile operation.
    Instead you just have each operation do the roughing with large tool then create a separate set of operations for the finish passes with small tool.
    This way when post processed all the Roughing passes are done before the Finish passes so only one tool change for all operations.

    Hope that makes sense.?

  9. #9
    Thanks JAZZ,

    I was unsure if the onion skin would be enough to hold the part for the finish op's, have been messing in sheet cam and running simulations etc, seem to have it sorted i think but i can now re-order the processes to do all the roughing first.

    What sort (if any) lube/coolant do you use on aluminium? I have enough parts in now to build a pressurised fog-less system but just wondering what people put in them :)

    Back to the CAM, shapes like the odd shaped internal part on my drawing, I have roughed out the bulk with a 5mm tool, that leaves of course 2.5mm rads in all the corners, are you saying to finish cut that with the 2mm tool in one pass?

    Do lead-ins and outs feature or forget them for the minute?
    Last edited by Davek0974; 15-03-2016 at 02:42 PM.

  10. #10
    Quote Originally Posted by Davek0974 View Post
    What sort (if any) lube/coolant do you use on aluminium? I have enough parts in now to build a pressurised fog-less system but just wondering what people put in them :)
    I use WD40 type lube but oil/parafin mix will work.

    Quote Originally Posted by Davek0974 View Post
    Back to the CAM, shapes like the odd shaped internal part on my drawing, I have roughed out the bulk with a 5mm tool, that leaves of course 2.5mm rads in all the corners, are you saying to finish cut that with the 2mm tool in one pass?
    Yes will be ok in this case because your now side cutting and the tiny amount left won't hurt anything. However it's not recommended to use same size tool as the radius. ie: 2mm Rad use use 1.9mm or smaller Dia tool. This means the tool won't be cutting on two sides in the corner so won't chatter or snag and break the tool. Which can happen on really small tools. Larger tools just usually leave mark in corners and make horrible noise.


    Quote Originally Posted by Davek0974 View Post
    Do lead-ins and outs feature or forget them for the minute?
    Well they are all part the process really so should happen anyway. For instance you'll ramp into pockets for roughing to safe tool wear but radius arc into the Finish pass if enough room for better finish. If cam program allows I always let the lead out go slightly past the lean In point as well to remove cross over point.

Page 1 of 19 12311 ... LastLast

Similar Threads

  1. Beginner Moving Gantry Build? Read This!
    By Tenson in forum Gantry/Router Machines & Building
    Replies: 1
    Last Post: 21-09-2015, 07:54 PM
  2. Garage CNC - A gantry style machine design
    By fandango in forum Gantry/Router Machines & Building
    Replies: 14
    Last Post: 21-03-2014, 12:38 AM
  3. Truss style Gantry
    By D.C. in forum Gantry/Router Machines & Building
    Replies: 28
    Last Post: 15-12-2012, 06:23 PM
  4. A few questions to start a DIY mini CNC
    By purple_rob in forum Gantry/Router Machines & Building
    Replies: 5
    Last Post: 03-08-2009, 10:08 PM
  5. Vertical moving gantry????
    By Ross77 in forum Gantry/Router Machines & Building
    Replies: 9
    Last Post: 03-06-2009, 07:34 PM

Bookmarks

Posting Permissions

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