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:

Cutting a part hardened to Rc60 with Dynamic Milling (feedback welcomed)


WOODS7
 Share

Recommended Posts

Hi folks! I am cutting a 3/4" deep pocket into a gear that I have been told is hardened to a hardness of Rc60 by one of our customers.  I made my first attempt today and no bueno! :thumbdown:  Was wondering if anyone on here has had any experience with using the dynamic motion in Mastercam X9 and would care to share their thoughts on this? :help: I have attached pictures of my fixture, how far I got into the part before the bit broke the tip, the broken bit and the tool path image. I will list below the machine, bit, feeds, speeds, ect, ect. What I am hoping to gain from this post is your thoughts on what went wrong and any suggestions if you have machined material this hard before. Any feedback is welcomed and thank you in advance for your help on this matter. :smoke:
 
 
MACHINE = HAAS VF3
 
PROGRAMED WITH = MASTERCAM X9
 
BIT USED = KENNAMETAL 1/2" ENDMILL 6 FLUTE (HPFDM500S6175)
 
(ap) = .75
(fz) = .002
(Vc) = 250
(n) = 1910
(ae) = .015
MasterCam with the RCTF box checked set the (vf) to = 67
 
 
 
post-70001-0-48551600-1466195025_thumb.jpgpost-70001-0-59082300-1466195044_thumb.jpgpost-70001-0-23550800-1466195062_thumb.jpgpost-70001-0-05798300-1466195075_thumb.jpgpost-70001-0-77240700-1466194995_thumb.jpg

Link to comment
Share on other sites

I have found the numbers from Helical tool's milling advisor are usually pretty good. For 60Rc material with good work holding and tooling it recommends;

 

431 SFM

3292 RPM

.0041 IPT

.035 stepover

 

It seems to me that your feed may be kind of light and you may be overheating the tool. However, I am a novice when it comes to hard milling, I do not do it that often. 

Link to comment
Share on other sites

Tool holding will be important here and I would use a mill chuck, hydraulic, or shrink fit.  It looks like you were running coolant and I'm not sure at RC60, but we run production parts at RC54 (4140) with air blast.  Coolant cuts the tool life in half, at least with the speeds and feeds we are running.  Do you know the exact alloy?

Link to comment
Share on other sites

Another thing that might help is to put the machine into roughing more (G187 P1) as this will speed up the tool and reduce pauses and dwells.  When in roughing mode make sure to leave enough extra material for finishing.  I'd guess .010-.015" should be fine at those feed rates.

Link to comment
Share on other sites

Tool holding will be important here and I would use a mill chuck, hydraulic, or shrink fit.  It looks like you were running coolant and I'm not sure at RC60, but we run production parts at RC54 (4140) with air blast.  Coolant cuts the tool life in half, at least with the speeds and feeds we are running.  Do you know the exact alloy?

 

None of those are going to work great on a 40 taper Haas for roughing hardened steel. Switch to a quality sidelok if you want good tool life and some rigidity.

Link to comment
Share on other sites

I'd start with Doug's parameters.

I've found a sweeter spot with my VF-3 @ .02 to .025" radial stepover with under 40Rc steel. I'd imagine it would be even more sensitive at your hardness. Need a shorter tool, for sure.

 

I wonder if Peel or Blend would be ideal here.

 

 

Might want to consider a High feed cutter from Sandvik or similar . controlling z depths might be easier for a newbie to hard milling.

Link to comment
Share on other sites

Definitely low axial depth of cut style hardmilling will work better than the high axial depth of cut style of high speed machining. Judging by the amount of chatter that I can see on the part, and the fixture, I'd bet you have a lot of fretting on your tool and spindle taper.

Link to comment
Share on other sites

None of those are going to work great on a 40 taper Haas for roughing hardened steel. Switch to a quality sidelok if you want good tool life and some rigidity.

I avoid those holders like the plague as we have had nothing but trouble from them.  We gave all ours to the local high school...  My #1 preference for this application would be a hydraulic chuck like the Schunk Tendo-E compact.  Great damping characteristics and cuts like butter.  I would also use a smaller tool and run faster.  Heck, I hated running 1/2" tools in my Haas in ALUMINUM because the rigidity was so bad.  I'd try a 3/8" tool and just replace them more often.

  • Like 3
Link to comment
Share on other sites

Looks like your tool is too long.  What I found under that part number has a  1.75" LOC, you only need 0.75".  IIRC if you double the stickout of a tool you multiply the deflection by four; it makes a huge difference.

 

I do dynamic roughing in 17-4 H900 in my Haas VF-3SS with a 3/8" bull, and traditional roughing with a 3/4" indexable.

Link to comment
Share on other sites

I avoid those holders like the plague as we have had nothing but trouble from them.  We gave all ours to the local high school...  My #1 preference for this application would be a hydraulic chuck like the Schunk Tendo-E compact.  Great damping characteristics and cuts like butter.  I would also use a smaller tool and run faster.  Heck, I hated running 1/2" tools in my Haas in ALUMINUM because the rigidity was so bad.  I'd try a 3/8" tool and just replace them more often.

 

Well there isn't any legitimate reason to not use a quality sidelok, they have the best tool retention and the best rigidity for roughing. Some of the is because they are 2" or more shorter in gage length than your suggested holders (and that makes a huge difference on 40 tapers), some is due to the fact there is nothing in a sidelok assembly to cause vibration.

 

If you are getting more than a few tenths of runout on a sidelok, it's not a quality sidelok. If you are having problems with the tool pulling out of a sidelok, you didn't tighten it correctly.

 

I use hydraulic and shrink fit as well, but they are much better served for finishing applications.

Link to comment
Share on other sites

Looks like your tool is too long.  What I found under that part number has a  1.75" LOC, you only need 0.75".  IIRC if you double the stickout of a tool you multiply the deflection by four; it makes a huge difference.

 

I do dynamic roughing in 17-4 H900 in my Haas VF-3SS with a 3/8" bull, and traditional roughing with a 3/4" indexable.

I'm with Matt. If it were me, I would go with a 3/8 with .75 LOC. the smaller tool will put less pressure on your  spindle, lowering chatter, with the same percentage radial depth of cut.

2:1 is length to dia. is pretty reasonable. Or, a 1/2 with 1" LOC.

I'm not a fan of side locks either. Especially with the flat grinding skills I see. :laughing:  Also, with a weak machine like a HAAS, the balance can be an issue, even at lower speeds, causing you to cut with fewer flutes.

A quality holder in a Haas 40 taper is still a mediocre holder.

Which.... leads me to make sure your tool is running dead true. you want each flute cutting the exact radial depth. Otherwise, instead of a .015 ae, you will have some flutes at .018 and some at .012 or so...

Link to comment
Share on other sites

That aluminum plate is not helping you situation at all. I would also get away from those hex head bolts and go to an Allen head cap screw. They provide more clamping force per square inch tan hex head bolts IMHO. Go to a heavy washer.

 

I agree with everything everyone else said, but might step up to a 7 flute if you can get one that same or down to a 5 flute. The even flutes have always been an issue I have seen and the odd numbers of flutes helps to break up harmonics.

 

I also agree with Bob on the hydraulic chuck as they in my experience do help dampen the tool and I understmadwhat Sticky is thinking, but seeing what I see there have to think you done have top of the line best money can get side lock holders. Not trying to be dispectful to your efforts, but in this case I would thinking using one would greatly improve your efforts here. Issue will be probably not enough money in this job to even purschase the endmill. Hopefully someone knew what they were getting you into and quoted that job accordingly and you don't end up wrapping $100 bills around the part to give it to the customer.

Link to comment
Share on other sites

Thank you everyone for your input! My Kenntametal reps contacted me this weekend and said they will be by the shop Monday morning to see what is going on. I will have to say the support we have received with this company has been very hands on and helpful. I will post the results to let you folks know what happens.

 

Unfortunately I'm not sure how to respond to everyone's post on here where you can show the quote and then answer it. So I will do it this way instead:

 

@ YoDoug - I have never used that but will definitely look it up and give it a try.

 

@ Liegh @ Kodiak - It is just a VF3 but I am using the micro lifts to clear when it's back feeding.

 

@ Bob W. - I am using a Solid tool holder and running coolant because our machine isn't set up for air blast and needed something to flush the chips out.

 

@ Mathew - it is a long tool but reason being is the final cut on this will be a little deeper than 1.5".

 

@ 5th-axis - Lots of helpful advise! My shop teacher told me on a facing project one time about removing one of the inserts to have an odd tooth count for better harmonics and it worked like a champ. This bit is what my Kenntametal reps suggested so trusted they would give me the best tool for the job.

Link to comment
Share on other sites

I had another look at the pictures and noticed the tool failed at the flute corners so I looked up the tool data and it appears to be a sharp corner tool.  Given your finishing depth of cut I would do this job with two tools.  A rougher with a .030-.060 corner radius and a finisher with the sharp corner if that is what is needed.  Running coolant will require than you back off the speeds and feeds which will make this take much longer.  It might be worth rigging up a quick and dirty air blast depending on the anticipated cycle time (zip tie an air hose with adjustable nozzle in there).  So to summarize, bolt the fixture plate directly to the mill table, get a tool with a corner radius for roughing, see if you can rig up an air blast system, check the quality of your side lock holder, and you're good to go.

Link to comment
Share on other sites

 

 

@ Mathew - it is a long tool but reason being is the final cut on this will be a little deeper than 1.5". 

 

I'd recommend then using a short tool for what it can reach, then having the long one do only what it's needed for.  The long tool will need to take lighter cuts than the short one can.

Link to comment
Share on other sites

Once again thank you for all the input on here. :unworthy: The project is finished and the only casualty was the end mill that was broke the first go around.  We were able to cut the part with no problems with the following adjustments made. :thumbsup:

 

 

 

Macgyver'd up an air blast system to clear the chips.

 

Used a shorter Kennametal (cxer0500nn4-f) endmill to remove all the material in the pocket down to the 3/4" depth.

 

Used different feeds and speeds

 

Inserted a plate jack In between the fixture and the table to reduce vibration.

 

 

Below is the finished product. :smoke:

 

 

 

 

post-70001-0-01188900-1466539294_thumb.jpg

post-70001-0-41356500-1466539338_thumb.jpg

  • Like 6
Link to comment
Share on other sites

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...