Can not drill a hole straight

[CNC-ERIC]

Hi,there,

2.35mm dia, 20mm deep hole on plastic(PET-P).

 

First,I use 2.30mm solid carbid drill goes to 9.5mm, then use 2.35mm solid carbid drill peck to 20mm, rpm 3037 feed 10.5in/m, the holes I measured are not straight, off 0.05mm,I did not use coolant,is this a problem?I notice the drill bit very hot.

 

thanks

 

eric

[htm01]

need coolant or plastic melts and sticks to drill

[CNC-ERIC]

hi,htm01

there are 12 holes on 2 lines, I add coolant on, the first is good, the second line still are not good, I can not figure out why?

 

thanks for help

 

eric

[Programinator]

What is your peck value?

[CNC-ERIC]

HI,programinator,

 

peck 0.03"

[RobertELee]

I was just going to bring up peck length also. You may want to lengthen and shorten it and see what happens.

[Kevangel]

are you checking straightness on the machine? If not, is the part buckled in vise from clamping pressure?

[GoetzInd]

quote:

---

is the part buckled in vise from clamping pressure?

---

Me thoughts exactly.

[RobertELee]

Also, are you using a drill specifically made for plastic? Ones made for cutting steel uses tool pressure to cut and with plastic there obviously isn't any tool pressure and may drift.

[billystein]

slow the rpm to 2000 and raise the feed to 20.

start the peck at .1 if it wraps around the drill then make it smaller.

the thicker chip should clear the hole better.

[PeterM]

If the chip wraps around the drill it can prevent the coolant from getting to the part. You can spin the drill backwards to clear the chips between holes.

[Jim at Gentex]

Agreed with everything said thus far.

 

Getting the speed and feed just right is the key with plastics.

 

I do alot of 5-axis swarf milling on polycarbonate lenses. If the speed and feed is just right, you get a great finish and you hardly even have to deburr the edges. A bit too slow or fast on the speed / feed and the tool either loads up, or you get chatter marks.

 

Unfortunately, it's all trial and error to find the ideal speed / feed for any particular job.

 

One thing I will say for sure is that I have had the best results using high helix drills and end mills. They seem to pull the chips away quicker so they don't load up on the tool.

[CNC-ERIC]

HI,GUYS,

 

THANKS FOR YOUR INPUTS.

ADD COOLANT,( LOOKS A9 IS BETTER), AFTER PECK DRILING, ADDING A DIRECT DRILLING(G81,RMP3000,F20. P0.2),THE HOLES ARE GOOD.

 

THANKS FOR YOUR HELP.

 

ERIC

[bigjohn]

Long time ago I read that drilling bar stock behave differently than flat stock plastic due to internal stresses from rolling or extruding.

 

 

John

[Tyler Robertson]

Awesome thread - you guys rock