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:

Is it possible to drill 0.16mm hole 1.6mm deep on HAAS VF2?


CNC-ERIC
 Share

Recommended Posts

HI, there,

 

I have a job, material is SST 316, need drill 0.16mm and 0.26mm hole on it with depth of 1.6mm.

 

machine is VF2 with 10000 rpm spindle.

 

my question is can I make it on this machine or not.

 

my procedure:

 

face the surface as a reference,

use 0.5mm solidcarbide drill as a center drill to drill down to -.006"

0.16mm solidcarbide drill drill down -0.008" ,rpm10000, feed 0.99in/sec

0.16mm solidcarbide drill peck drill to -0.047"( the flute is 0.05"), rpm10000, feed0.99in/sec, peck0.025"

 

tried twice, both failed.

 

Can I ask you advice on the job?

 

thanks very much

MMC-1556B TEST.MCX-5

Link to comment
Share on other sites

Where is the drill failing? How deep is it making it before it gives out? Trial and error is going to be your only option I am afraid. Your speeds and feeds look about right, but you could try cutting your feed to 50% or even less to start. I see in the file the peck is actually .0025" which I would say is OK. But you state here you are pecking at .025". If you are in fact running this at a .025" peck that is way too much. Keep your rapid at 5%. Turn your coolant down and use a really fine nozzle and drizzle the coolant on the drill. Anything as strong as a stream from a bottle of Windex is going to break the drill ;) I have seen this happen a number of times where the coolant was actually what was breaking the drill. I really hope this helps, and wish you luck. Let us know what you figure out.

Link to comment
Share on other sites

The runout of the spindle and tool may be more than a drill that small can handle. What are you holding it with? For a tool that small I would use an integral BIG baby chuck and check the runout of the tool body with a micron clock. Even 5 microns runout is a big number as a percentage of the tool diameter.

 

Bruce

Link to comment
Share on other sites

thanks for your inputs.

 

pecking is 0.0025", I made a wrong typing.

 

the drill bit flute is about 0.050", shaft is 0.125", hold with ER 16 holder

 

drill bits were still broken after cutting both the feed to 0.5in/sec, looked like it broken at the last pecking.

 

checked the failed part under microscope, all the holes looked like concentric, I am not sure is if I can the 0.5mm drill as a center drill. the solidcarbide drills are for circurt board, is this the reason?

 

 

I also thought the carbide drill too ridgit, I change both drill bits from carbide to HSS, same RPM and FEED, still no luck on this job.

HSS drill bits are 1.0mm shaft, also holding with ER collet.

 

any ideas? or what are the proper equipments or device for this kind of micro holes? I may have many job like this coming soon.

 

I feel a lit headache.

 

thanks again.

 

Eric

Link to comment
Share on other sites

If using HSS drills you will need to cut your surface speed down quite a bit. Probably closer to 5 SFM would be better for HSS. Maybe even less. It all depends if they are breaking, or burning up. If you are making it to the bottom of the hole before they break then stop .010" from where they are breaking then create another toolpath to finish the last bit at a smaller peck. Leave the feed alone at this point. They are more than likely burning up from lack of coolant. So a quick feed and shallow peck might get ya through the last little bit.

Link to comment
Share on other sites

"...ER 16 holder..."

 

I bet my best beef that that run-out using this system is far from what is acceptable. High RPMs are good, but for a drill that small, the coolant never gets in the cutting zone anyway... so it's important to keep it cooled and with a low run-out so the tool wear is evenly distributed to the flutes...

 

Compressed air with the nozzle blowing parallel to the drill can help, but MQL is probably the best way...

 

In your shoes I'd be looking at a better tool holder, hydraulic or shrink-fit are good options... Haimer shrink-fit holders are kick xxxx for low run-out results... hard to find one for 0.125" though (You guys don't know yet, but the real world is metric... :smoke: )

 

Another excellent tool holder option is Schunk Tribos mini, but it is $$$... Like Bruce said, the run-out is extremely important... get rid of ER collets, even if they say the offer high accuracy versions. ER collets cannot reach the level you need for these jobs...

 

RPM is not as important as run-out and cooling... mineral oil as the coolant (Especially if spread through MQL) can help too...

 

Well, that's all I can remember now...

 

Good luck,

 

Daniel

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...