Ball nose plunge cutting

This forum is for general discussion about Aspire
Post Reply
vgraves
Vectric Craftsman
Posts: 122
Joined: Sat Sep 29, 2012 2:04 am
Model of CNC Machine: CNC Router Parts PRO4848 w/LinuxCNC
Location: Knoxville, TN

Ball nose plunge cutting

Post by vgraves »

I'm making some marble-based games for Christmas (think Chinese Checkers for instance), so I need to make numerous plunge cuts into MDF. I'm using a Drilling toolpath along with a 0.5-inch 4-flute ball nose end mill. I've started with 12000 rpm, 10 ipm feed rate and can see deflection in my Z axis (3HP PC router on a CNCRP PRO4848). I understand that plunge cuts put some vertical loading on the bit and router, which isn't preferred but can't be helped in this case.

For those who might do this kind of operation regularly, any suggestions as to feed/speeds?

Thanks,
Van

LittleGreyMan
Vectric Apprentice
Posts: 918
Joined: Fri May 15, 2015 1:10 pm
Model of CNC Machine: 3 axis small size machine
Location: France

Re: Ball nose plunge cutting

Post by LittleGreyMan »

Hi Van,

Can you post a screenshot of your toolpath settings?
Best regards

Didier

W7 - Aspire 8.517

Paul Z
Vectric Wizard
Posts: 517
Joined: Sun Apr 30, 2006 10:04 pm
Model of CNC Machine: shopbot PRT Alpha 96x48
Location: New Hampshire, USA
Contact:

Re: Ball nose plunge cutting

Post by Paul Z »

Can you make a first cut with a 1/4" end mill and then make the final cut with the 1/2" ball? Using a 1/4" end mill as a drill is not a great idea but it is better than using a 1/2" ball as a drill.

Paul Z

vgraves
Vectric Craftsman
Posts: 122
Joined: Sat Sep 29, 2012 2:04 am
Model of CNC Machine: CNC Router Parts PRO4848 w/LinuxCNC
Location: Knoxville, TN

Re: Ball nose plunge cutting

Post by vgraves »

Here's my tool path settings. I was hoping to do the dishes with a single tool but may have to look at splitting it into two.
Attachments
drill toolpath.PNG

User avatar
Turtle49
Vectric Wizard
Posts: 1482
Joined: Mon Aug 27, 2007 9:11 pm
Model of CNC Machine: 4' EZ-Router and Blurry customs SK25
Location: Holland, MI. U.S.A
Contact:

Re: Ball nose plunge cutting

Post by Turtle49 »

I wonder, if you were to set up a 0.501 circle and use a pocket toolpath with the 1/2" ball nose ramping in...perhaps that would help with your issue.
Tim Hornshaw
www.HornshawWoodWorks.com

User avatar
scottp55
Vectric Wizard
Posts: 3810
Joined: Thu May 09, 2013 11:30 am
Model of CNC Machine: ShopbotDesktop 5.5"Z/spindle/VCP10
Location: Kennebunkport, Maine, US

Re: Ball nose plunge cutting

Post by scottp55 »

Tim,
That actually works quite well with an inside profile/spiral ramped.
All files and pics on other computer, but tested 2 buttons with 2F .5" BN and quite fast even with many passes as I was very cautious on protos in Hard Maple.
Bit stayed cool with good chips on my test blocks with a very good finish.
I'll check control computer for feeds/speeds that worked if OP wants, and can probably still go a lot faster.
It was only several seconds for the toolpath if I remember right.
scott
"Flatness is King"
Brady W.

scott

User avatar
Ms Wolffie
Vectric Wizard
Posts: 2689
Joined: Sat Mar 31, 2012 10:41 pm
Model of CNC Machine: Blue Elephant 1325, Shark HD Pro
Location: Tully Heads, Wet Tropics, Queensland, Australia

Re: Ball nose plunge cutting

Post by Ms Wolffie »

According to your tool setting picture, you have ticked Dwell at bottom but time =0.0, so why have you ticked dwell?
I also notice that you are not using peck drilling, doing the whole cut in one cut.
Peck drilling lifts your bit up to get rid of the drill dust and puts less strain on your bit.
For the depth you are doing, I would use at least but preferably 3 passes, that would ease the deflection on your Z axis.
Hope this helps.
Cheers
Wolffie

Whatshammacallit
Cut3D, VCarvePro 6.5, Aspire4, PhotoVCarve, Corel Graphics Suite X6

vgraves
Vectric Craftsman
Posts: 122
Joined: Sat Sep 29, 2012 2:04 am
Model of CNC Machine: CNC Router Parts PRO4848 w/LinuxCNC
Location: Knoxville, TN

Re: Ball nose plunge cutting

Post by vgraves »

Wolffie, dwell is ticked and =0 by default as far as I know. Since dwell = 0, it really doesn't dwell, so having dwell ticked doesn't do anything. I haven't tied peck drilling with the ball nose, may try that and see if it helps. Thanks.

vgraves
Vectric Craftsman
Posts: 122
Joined: Sat Sep 29, 2012 2:04 am
Model of CNC Machine: CNC Router Parts PRO4848 w/LinuxCNC
Location: Knoxville, TN

Re: Ball nose plunge cutting

Post by vgraves »

Instead of trying a spiral profile with a bit diameter close to the "divot" diameter, which would nearly be the same as a straight drill tool path, I actually removed the center material using a 0.25 drill bit. This has issues in itself because drill bits aren't really designed to rotate at router speeds. I have a SuperPID on my router, which allows me to lower the spindle speed down to 5000 rpm, but this is still faster than most drill presses and recommended speeds for drill bits.

The original ball nose drill path was to a depth of 0.216; I went down to 0.2 inches using the drill bit, and I did use peck drilling (0.1 deep per peck). Then I reran the original ball nose tool path, and since the tip of the ball nose didn't have to remove material except at the very bottom of the divot, it worked much better.

This will be my new default mode, but maybe I'll try using a flat end mill instead of a drill bit for hogging more of the divot out. Bottom line is that these routers don't really like drilling.

LittleGreyMan
Vectric Apprentice
Posts: 918
Joined: Fri May 15, 2015 1:10 pm
Model of CNC Machine: 3 axis small size machine
Location: France

Re: Ball nose plunge cutting

Post by LittleGreyMan »

A flat end mill with peck drilling will probably give good results. We often use this technique, or a spiral if the hole diameter doesn't match a standard end mill diameter. As you noticed, drill bits require very low rpm.

Keep the peck drilling option for the ball nose tool path.
Best regards

Didier

W7 - Aspire 8.517

Post Reply