Jump to content

Welcome to eMastercam

Register now to participate in the forums, access the download area, buy Mastercam training materials, post processors and more. This message will be removed once you have signed in.

Use your display name or email address to sign in:

deep pocket in aluminum (continued)


Recommended Posts

I made a post about this before and it seemed like the general consensus is that I was doing it right, but it is still one of my least favorite jobs to run. It is a 4x5x3in deep cavity (in Al 6061) that I need to machine. The way we have been doing it is, " 3/4 x 3.5" solid carbide rougher (with chip breakers) from Helical tool and finished the walls with a 1/2 reduced neck EM. With the rougher, I did a helical plunge with a dynamic toolpath and 2 passes axially (1.5" depths of cut). " The main issue I am having is recutting of chips. We are running flood coolant and the coolant and chips are stuck in the cavity. Any ideas on how I can Improve this process (tools, methods, whatever..?)

I appreciate any help.

Link to comment
Share on other sites

Best options would be TSC or put it on a horizontal.  Failing that, maybe find a way to increase your coolant pressure and aim it down along the tool to blast the chips out.  Maybe put a couple parts on a 4 axis fixture, cut partway and then rotate, work on the next part while dumping the chips out of the first?

Or put a coolant inducer on your toolholder, so you can pipe your flood coolant through the tool.

Or mount the machine on the ceiling.

  • Like 1
  • Haha 4
Link to comment
Share on other sites
11 hours ago, Matthew Hajicek - Conventus said:

Best options would be TSC or put it on a horizontal.  Failing that, maybe find a way to increase your coolant pressure and aim it down along the tool to blast the chips out.  Maybe put a couple parts on a 4 axis fixture, cut partway and then rotate, work on the next part while dumping the chips out of the first?

Or put a coolant inducer on your toolholder, so you can pipe your flood coolant through the tool.

Or mount the machine on the ceiling.

If you ceiling-mount, you also increase the floor-space! Win-win.

  • Like 1
  • Haha 4
Link to comment
Share on other sites
2 hours ago, CNC programming questions said:

12k. I will see about a ceiling mount. I think that makes the most sense.

You could try a high rake insert (ala Big Kaiser or Dapra) cutter with an air blast. With12K you should be able to get as much material removal rate as with your  solid carbide, and replacing inserts is definitely cheaper, those 3/4" solid carbides don't get given away.

You will need a .625 loc insert  to get the MRR.

You should be able to eject most of the chips and the air should take care of anything else

  • Like 1
Link to comment
Share on other sites

Dapra 1" Diameter Insert Body, with 4" Effective Length (they don't make a 3" reach, unfortunately). 16mm Insert Length (.600 Max DOC)

20570 1.000” SSER1000-4000-R55-2C .600” 2 1.250” 6.28” 4.00”

XPET Inserts. 

XPET160404-ALU > .015”-Corner Radius

       Plain (uncoated) > DMK25 (29912)

       Coated (recommended) > DMK25-GLH (29914)

(They also have 0.031-CR, 0.047-CR, 0.062-CR, and 0.120-CR Available)

They also have PCD Tipped, but only in 0.031" - Corner Radius

 

  • Thanks 1
  • Like 2
Link to comment
Share on other sites
11 minutes ago, nickbe10 said:

I might go for something a bit smaller depending on available horse power.

The problem is lack of reach, with the 16mm insert. They have a .750, but not in a deep-reach option. (2" is about the deepest you can go with the 0.750 diameter cutter.)

If you have the Horsepower, you could easily obtain the following:

  • 9550 RPM (2,500 SFM)
  • 0.022" per tooth (0.044 IPR)
  • Feedrate = 420 IPM
  • 30% Radial DOC (0.3")
  • 0.6" Axial DOC

This should equate to roughly 18-20 HP.

I plugged this into a Dynamic 2D Path, using 5 depth cuts, to go the full 3" deep. That is 5 passes. Backplot time was about 1.5 minutes.

So if you have the available ponies, and can hook up an airline, that cutter will make very short work of the roughing. Of course you'll still need to finish with the 0.750 Diameter carbide tool, but at least you won't be recutting any chips...

pocket.PNG

  • Like 2
Link to comment
Share on other sites

I tried running it with a shear hog and it did okay but the MRR was not good enough (plus the noise was an issue). I will look into the Dapra tool. The method I am using is holding up and works for 60+ parts per run but I just cringe when I hear the sound because I can hear it recutting chips. I can try to hookup an air blast and see if it improves. I programmed a stop in between the axial cuts to blow out chips but didnt help much. Unfortunately, we do not have TSC or air blast on the machine. Thanks again for the help guys!

Link to comment
Share on other sites
2 hours ago, CNC programming questions said:

Collin- can you shoot me a part number? Dont want to ask too much, but I am not good at navigating these sites.

I put part #'s for the Cutter Body, and 2 different inserts (one coated, one without coating). Look up a couple of posts, earlier in the thread. Copy/Paste the string after [1.000"], into Google. I enjoy helping where I can, but I already listed the part #'s, speeds/feeds, and even made a collage of the Operation Parameters. I thought it was a pretty good roadmap. That said; you'll have to do the driving.

Link to comment
Share on other sites

The other option to consider would be to add a secondary coolant pump to your coolant tank, and to run a beefy supply line go the spindle, and then use 2 big loc-lines (3/8" or 1/2"), to flush out the chips from the pocket. Hook up a relay to the existing Coolant relay (M08), so you can drive the auxiliary pump.

 

https://product-selection.grundfos.com/us/products/mt-tank-mounted-pumps/mta?tab=models

 

  • Like 2
Link to comment
Share on other sites

Does your machine have air blast??? Last resort if you still have to stop the machine to remove chips maybe instead of an M00 that requires operator interaction keep it all automated? Tool change to a small diameter empty holder (whatever diameter holder provides good air pressure, empty collet holder would work as well) and air blast your chips out. After good air blast and chips are gone pull the 3/4 back out and continue roughing. 

 

Also, that 3/4 should have no problem roughing at full depth in 6061 with a good dynamic routine. Depending on machine HP, reduce your step over amount. Try the non chip breaker style if you have it. This will create longer skinnier chips and actually utilize most of the 3.5" flutes your end mill.  

  • Thanks 1
  • Like 1
Link to comment
Share on other sites

Did you look into Guhring Diver mills? I am not sure they have that length/reach but they do make solid carbide with thru coolant in the flutes. That would get more coolant pressure to the tip of your tool to evac chips easier.

Link to comment
Share on other sites
  • 2 weeks later...

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

Guest
Reply to this topic...

×   Pasted as rich text.   Paste as plain text instead

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.

 Share

  • Recently Browsing   0 members

    • No registered users viewing this page.

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Follow us

×
×
  • Create New...