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:

Kennametal KOR-5 worth it?


Recommended Posts

I recently purchased the Kennametal KOR-5 in 1/2" and 3/8" through our tooling rep using the discounted promo code from Titans of CNC. I am going to try it out once one of our mills opens up. Has anyone tried it? Thoughts? I have had much success using 3 flute aluminum roughers (with chip breakers) from Helical tool, so I am interested in giving this 5 flute a shot. By the way, running on a HAAS VF2 with no internal coolant.

  • Like 1
Link to comment
Share on other sites

Are you going to be running the tool in aluminum? I would try it, but I would be super aggressive on my feedrate and less on my Radial. Maybe I would run a 3 flute at 10k rpms, 15%-25% ROC and .008 to .015 per tooth 150% to 200% DOC with 1000 psi TSP. 1/2 4 Flute endmill at 10k RPMs 25% ROC, 200% DOC with a .015 feed per tooth that is 56.25 in3 16.88 hp with a .0014 deflection.

Without TSP. Might try 10% ROC, 100% DOC with .015 to .025 per tooth feed rate at 8k rpms. You biggest concern on Aluminum is sticking to the tool to loading up with a 5 flute, but pushing past the normal is crazy talk, but I like crazy land so I like to see how hard I can push things. You can start very mild and just keep kicking it up till you find the sweet spot for the tool. Problem would be need to feed at 1000 ipm to support such crazy feed rates per tooth. You would be a 50 in3 and have .0015 tool deflection and need only 15 HP to pull off such a cut. I know of a few machines on the Market capable of such work. 

  • Thanks 1
Link to comment
Share on other sites

Calculate things for as fast as you can feed.  Then increase the radial until you run out of horsepower.  I am guessing your sweet spot will be about 15%-20% RDOC, at full depth.  The tool will gladly handle 40% stepover at full flute length, but your setup and tool holding need to be perfect to make that work long term.  Make sure you use dynamic tool paths, or if not be very conscious not to create radial engagement spikes.  You will be limited more by the machine than the tool.  A half inch KOR 5 is plenty of tool for a Cat 40 spindle.  It is a very stiff tool and will absolutely match or beat the performance of what you have ran in the past.

What do you plan to hold it with?  If you plan to max out what your machine can handle you will need to be in a Hyrdoforce HT chuck or equivalent milling chuck.  If you grind a flat and put it in a weldon holder, that would work as well, but is not recommended due to balance issues.

Avoid ramping into a pocket without internal coolant.  If you do, don't exceed a 4 degree ramp angle.  With internal coolant you could go 8 degrees, but doesn't sound like you have it.   Full slot don't exceed .5xd depth.

Oh and if you do load it up through poor coolant or unintended misapplication.  Drain cleaner (muriatic acid, drano or zep work well) works very well to dissolve the aluminum and make it good as new again.  Just drop the tool in a bucket of that stuff for a little while and then knock the pieces out, rinse it off and get back to work...

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

I will also state my preference for the Helical 3 flute with chip breakers. We have good results with them, especially in chip control. Our mills are robot/FMS fed and the smaller chips are more easily washed away with coolant. As for the Kore5, for me it would really depend on a few factors; part geometry, Spindle HP, and machine ACC/DEC times. If the part geometry is to intricate and/or the machines ACC/DEC are not going to get up the desired feedrate I will opt for less flutes and more engagement, as long as the machine has the HP to handle it. I see a lot of those videos that Titan puts out and it just looks like the machine is going really fast but not a lot of material coming off. IMO the goal is MMR, not just going fast. 

  • Thanks 1
  • Like 1
Link to comment
Share on other sites
On 8/29/2020 at 8:51 AM, CNC programming questions said:

Thanks for the feedback. I am using 6061 Aluminum and plan on holding it in a Shunk hydraulic holder. I generally use dynamic tool paths with a 15% stepover as a starting point for roughing operations in aluminum. The Haas has 500IPM maximum. I am excited to see how hard I can push it.

I have been reading that Schunk hydraulic holders are failing on very aggressive cuts. Tools are pulling out.

 

Paul

Link to comment
Share on other sites
27 minutes ago, PAnderson said:

I have been reading that Schunk hydraulic holders are failing on very aggressive cuts. Tools are pulling out.

 

Paul

We had that issue with them. We also had the same issue with Iscar hydraulics in aggressive cuts. We also found them to have more chatter issues. I don't know if there is some sort of resonance issue from the hydraulic fluid in the holder or just from the thinner sections because of the fluid cavities. We switched to shrink fits for most of our tooling now and only use the hydraulics we have for finishing tools or drill/reamers. 

Link to comment
Share on other sites
4 hours ago, PAnderson said:

I have been reading that Schunk hydraulic holders are failing on very aggressive cuts. Tools are pulling out.

 

Paul

Had that once about 5 years ago. 14mm MA Ford Type 134 (knuckle).

Never used them again for roughing from that day.

 

Edit - Doug, I found that the tool was quieter in a Schunk hydraulic. Oil dampened!

 

Link to comment
Share on other sites

That is interesting. We have used them for roughing and finishing operations for a couple of years now with no issues. We do moderate amounts of stainless steel and titanium but primarily aluminum and plastics. My current alternatives are ER collets or Weldon shank holders. I have seen tools pulled out of our ER collets on multiple occasions.

Link to comment
Share on other sites

The Hamier Reverse spiral lock is hands down the best way on the market to prevent tool pull out for Solid Carbide Endmills. Next is a Weldon tool perfectly balanced and used with the correct holder for Solid Carbide tooling. They exist and keep the tool runout less than .0001".  Now we look to the head style tools and that changed things drastically. Dollar for Dollar the inserted head tools in a production environment are what I am seeing make the best return on money spent.  

  • Like 2
Link to comment
Share on other sites
On 8/28/2020 at 7:21 PM, crazy^millman said:

Are you going to be running the tool in aluminum? I would try it, but I would be super aggressive on my feedrate and less on my Radial. Maybe I would run a 3 flute at 10k rpms, 15%-25% ROC and .008 to .015 per tooth 150% to 200% DOC with 1000 psi TSP. 1/2 4 Flute endmill at 10k RPMs 25% ROC, 200% DOC with a .015 feed per tooth that is 56.25 in3 16.88 hp with a .0014 deflection.

Without TSP. Might try 10% ROC, 100% DOC with .015 to .025 per tooth feed rate at 8k rpms. You biggest concern on Aluminum is sticking to the tool to loading up with a 5 flute, but pushing past the normal is crazy talk, but I like crazy land so I like to see how hard I can push things. You can start very mild and just keep kicking it up till you find the sweet spot for the tool. Problem would be need to feed at 1000 ipm to support such crazy feed rates per tooth. You would be a 50 in3 and have .0015 tool deflection and need only 15 HP to pull off such a cut. I know of a few machines on the Market capable of such work. 

How are you calculating the tool deflection?

Link to comment
Share on other sites
  • 4 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...