Sign in to follow this  
Bob W.

Drilling plastics

Recommended Posts

I have a large order of plastic parts to make (Acetal) and I was curious what the best drilling strategy is to avoid loading up the drill with material. Any drill recommendations would be great as well.

 

Thanks,

Bob

Share this post


Link to post
Share on other sites

i found full retract with lots of coolant the best for cooling so the plastic does not melt and weld up the holes. nice sharp parabolic flute split point drills. other then that its just plastic. cuts like butter.

Share this post


Link to post
Share on other sites

I've had really good luck with onsrud hss drills on acetal, running .2 drill 300 sfm .010 ipr 1 inch deep no peck, plenty of coolant.

Share this post


Link to post
Share on other sites

My main concern is the stringers wrapping around the shank. I have several hundred holes to drill in one shot and I don't want to have to be there to keep cleaning off the drill. I'd like to run the parts unattended.

Share this post


Link to post
Share on other sites

My main concern is the stringers wrapping around the shank. I have several hundred holes to drill in one shot and I don't want to have to be there to keep cleaning off the drill. I'd like to run the parts unattended.

 

 

Bob, Acetal cuts great. Here is a trick we use: At the end of the cycle, run the drill backwards before putting it aways - it will sling the chips off.

Share this post


Link to post
Share on other sites

Hi Bob,

 

If machining unattended is your main concern, I'd go with a really short peck depth. This should help keep the chips short, and keep them from wrapping up on your drill. Delrin (Acetal) is my all time favorite plastic to machine. It is very stable and doesn't deflect much. Make sure you use sharp drills, and brand doesn't matter as much. I would recommend staying on the heavier side for chip load. You need to take a good bite out of the material.

 

I'd recommend a Feed per Revolution of 2% of the diameter. So with a .250 Drill, .005 per revolution.

Share this post


Link to post
Share on other sites

We are machining quite alot of Acetal and we always use carbide drill with internal coolant, high feed and peck with full retract each 50% of drill diameter... For deeper holes I/K is really a must, else you'll need to go pretty slowly to avoid melting or very small dept at a time...

Share this post


Link to post
Share on other sites

when we drill that kind of stuff what works pretty good is to turn your spindle coolant on. holding the drill with collet,

then just let the coolant flow thru collet gaps, that blows out string of chips.

Share this post


Link to post
Share on other sites

Thanks for the replies. I'll try pecking and see how it goes.

Share this post


Link to post
Share on other sites
then just let the coolant flow thru collet gaps, that blows out string of chips

 

If you are using the right cutting speeds for the drills, that will turn the coolant into an umbrella of water, which will never reach the cutting tip... Except you have really high coolant pressure through, 10-15000 rpm or even higher if it's possible will only work with a closed collet and I/K drills... At least my experience...

Share this post


Link to post
Share on other sites

Create an account or sign in to comment

You need to be a member in order to leave a comment

Create an account

Sign up for a new account in our community. It's easy!

Register a new account

Sign in

Already have an account? Sign in here.

Sign In Now
Sign in to follow this  

  • 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