Peck drilling question

This forum is for general discussion about Aspire
User avatar
scotttarnor
Vectric Wizard
Posts: 941
Joined: Fri Aug 30, 2019 11:40 pm
Model of CNC Machine: Piranha XL , Shark HD520
Location: La Crosse WI

Peck drilling question

Post by scotttarnor »

I am working on a cribbage board today peck drilling with a brand new .125 drill bit from Think & Tinker.
Is it normal to have a lot of clean up from drilling? What do I need to do to prevent all the fuzzies?
Attachments
A7BA3833-7472-49E6-B004-7F975F31BBD6.jpeg
Scott T

@scottscnc

User avatar
ohiolyons
Vectric Wizard
Posts: 1702
Joined: Wed May 27, 2009 7:16 pm
Model of CNC Machine: Laguna IQ
Location: Kettering, Ohio

Re: Peck drilling question

Post by ohiolyons »

I have their 1/16", 1/8" and 1/4" drill bits and fuzzies have never been an issue for me.

Funky wood???


EDIT 1

There website says RPM >20K

Are you running less than that and plunging too deeply?
John Lyons
CNC in Kettering, Ohio

User avatar
adze_cnc
Vectric Wizard
Posts: 4325
Joined: Sat Jul 27, 2013 10:08 pm
Model of CNC Machine: AXYZ 4008
Location: Vancouver, BC, Canada

Re: Peck drilling question

Post by adze_cnc »

ohiolyons wrote:
Sat Jun 25, 2022 8:04 pm
Funky wood???
Is that American Sycamore? It seems the one time I worked with it (20 years ago now) I found it to be very hairy.

User avatar
scotttarnor
Vectric Wizard
Posts: 941
Joined: Fri Aug 30, 2019 11:40 pm
Model of CNC Machine: Piranha XL , Shark HD520
Location: La Crosse WI

Re: Peck drilling question

Post by scotttarnor »

I was very conservative on the plunge at .0625. I only ran at 15000 RPM, I will try 20000 next time. The wood was maple.
Attachments
BFE70A16-2DB0-49E6-9027-4F4A6A45A790.jpeg
Scott T

@scottscnc

User avatar
ohiolyons
Vectric Wizard
Posts: 1702
Joined: Wed May 27, 2009 7:16 pm
Model of CNC Machine: Laguna IQ
Location: Kettering, Ohio

Re: Peck drilling question

Post by ohiolyons »

Since the drills are so short I have them completely retract on each pecking cycle.

It does add time, but since drills are so short I don't worry about it.
John Lyons
CNC in Kettering, Ohio

Robert L
Vectric Craftsman
Posts: 120
Joined: Sun Dec 21, 2014 7:32 pm
Model of CNC Machine: Multicam

Re: Peck drilling question

Post by Robert L »

John has a good tip. full retraction after each peck.
Worth the extra time

User avatar
ohiolyons
Vectric Wizard
Posts: 1702
Joined: Wed May 27, 2009 7:16 pm
Model of CNC Machine: Laguna IQ
Location: Kettering, Ohio

Re: Peck drilling question

Post by ohiolyons »

Of course I don't do cribbage boards either.

On second thought!!!!!!
If I drill that many holes I might skip fully retract.
John Lyons
CNC in Kettering, Ohio

Jimcad
Vectric Wizard
Posts: 314
Joined: Sun Feb 20, 2022 12:59 pm
Model of CNC Machine: Alpha CNC 6090 with 4th Axis
Location: Dorset, England

Re: Peck drilling question

Post by Jimcad »

I'm very new to this but have many years CNC turning under my belt.
Rather than drilling is it worth trying to pocket with a 2.5 or 3mm end mill?
Better control of the diameter and less likely to fluff up the hairy bits.

Or you could try a slightly smaller drill then change to the size you want and re drill the holes with no need for pecking?
This would give very accurate holes and may reduce the hairs.
As a turner I've never run at these sort of revs.
I worked with metal and the highest spindle speed I ever had was 4,000
Drilling at 20,000 could cause all sorts of "chatter" issues.
Good luck and I await an update on how you get on.

User avatar
ohiolyons
Vectric Wizard
Posts: 1702
Joined: Wed May 27, 2009 7:16 pm
Model of CNC Machine: Laguna IQ
Location: Kettering, Ohio

Re: Peck drilling question

Post by ohiolyons »

The manufactures web page says 20-80K on these drills.

They also specify plunge rates too.

precisebits.com a great small American company based in Colorado.
They make everything in their Colorado shop.

Send them an email and Ron the president responds.
Their website has all sorts of formulas for calculating all things CNC.

My go to bit supplier.
John Lyons
CNC in Kettering, Ohio

User avatar
jimandi5000
Vectric Wizard
Posts: 1050
Joined: Wed Mar 11, 2015 6:50 pm
Model of CNC Machine: Home Made 60 x 120
Location: North Houston Tx.
Contact:

Re: Peck drilling question

Post by jimandi5000 »

scotttarnor wrote:
Sat Jun 25, 2022 6:22 pm
I am working on a cribbage board today peck drilling with a brand new .125 drill bit from Think & Tinker.
Is it normal to have a lot of clean up from drilling? What do I need to do to prevent all the fuzzies?
Hi Scott,

I did have the fuzzies issue on drilling then I started using Brad Point bits and I do not have them anymore.
Attachments
Brad Point Drill Bits
Brad Point Drill Bits
Thanks,
Jim

User avatar
ohiolyons
Vectric Wizard
Posts: 1702
Joined: Wed May 27, 2009 7:16 pm
Model of CNC Machine: Laguna IQ
Location: Kettering, Ohio

Re: Peck drilling question

Post by ohiolyons »

I'd be careful using normal drill bits in a CNC.

They are engineered for much slower RPMs that you normally see on a CNC.
John Lyons
CNC in Kettering, Ohio

Dan O
Posts: 35
Joined: Sun Dec 22, 2019 9:15 pm
Model of CNC Machine: Shapeoko XXL
Location: Wisconsin-USA

Re: Peck drilling question

Post by Dan O »

Scott,

I've done quite a few cribbage boards. I use a 2-flute .125 upcut end mill. 12,500 rpm @ 15 IPM feed .080 peck depth with a .05 retract.(not a full retract) (total depth is .300) It works really good for me. No fuzzies, nice clean holes. Cycle time is 20 mins.

Dan

User avatar
scotttarnor
Vectric Wizard
Posts: 941
Joined: Fri Aug 30, 2019 11:40 pm
Model of CNC Machine: Piranha XL , Shark HD520
Location: La Crosse WI

Re: Peck drilling question

Post by scotttarnor »

Thank You all for the information you provided, I was able to use a dental tool to remove the piece that was left at the top of each hole. I was doing a .5 retract which I will definitely make smaller on the next board, I believe I may try and end mill as Dan O suggested.
Maybe it was the wood? I did not get any in my practice run.
jimandi5000, there was mention of a brad point bit in one of the topics not too long ago, I will have to look it up, they also stated they had good results with one.

Again Thank You all for your input/suggestions.
Scott T

@scottscnc

User avatar
ohiolyons
Vectric Wizard
Posts: 1702
Joined: Wed May 27, 2009 7:16 pm
Model of CNC Machine: Laguna IQ
Location: Kettering, Ohio

Re: Peck drilling question

Post by ohiolyons »

FYI when you use an EM if your X and Y are not set up perfectly you will get an oval.
John Lyons
CNC in Kettering, Ohio

Tailmaker
Vectric Wizard
Posts: 699
Joined: Sun Jun 16, 2013 4:40 am
Model of CNC Machine: Home Built 4-axis Router
Location: Fort Collins, CO

Re: Peck drilling question

Post by Tailmaker »

scotttarnor wrote:
Mon Jun 27, 2022 2:34 pm
..... I believe I may try and end mill as Dan O suggested.
When using an end mill, try finding one with a "fishtail" tip (PreciseBits has such as well as various ebay sellers). The protruding flute ends will cut the perimeter of the hole first, minimizing the tear out.
A bottom cutting flat tip or a pointed drill bit will start cutting in the middle of the hole, allowing some fibers to be lifted out of the way before the actual flute can sever it.
Puzzle, Finger Joint, Maze and Guilloche freeware at https://fabrikisto.com/tailmaker-software/

Post Reply