pocket hole problem

This forum is for general discussion regarding VCarve Pro
Post Reply
gareth52
Posts: 4
Joined: Thu Aug 08, 2019 3:21 pm
Model of CNC Machine: 3 axis home built cnc machine
Location: Anglesey , Wales

pocket hole problem

Post by gareth52 »

Hi, I have been testing cutting rebates in ply and the results I’m getting are bemusing Can anyone please explain the differences I am getting in size. I am using the pocketing function in V carve. In this program there are 3 possible settings for the profile cut (1st, last, none). I was getting a ragged edge when using the default setting of last. So I tried setting the profile cut to 1st. Whilst it was a clean cut, the pocket was wider than the pocket cut with the profile at the end. I have listed various details below: –

PROFILE CUT LAST (inch)
0.432
0.438
0.444
PROFILE CUT 1st (inch)
0.485
0.489
0.492

Is there a reason for this?
Cheers,
Gareth

User avatar
TReischl
Vectric Wizard
Posts: 3569
Joined: Thu Jan 18, 2007 6:04 pm
Model of CNC Machine: 8020 Build 48X36X10 RP 2010 Screenset
Location: Leland NC

Re: pocket hole problem

Post by TReischl »

Where are those numbers coming from?

If those are measurements you took then I would venture that your bit is deflecting.

Another couple of questions:

What size bit are you using to do that cut?

How far out of the collet is it hanging?

The real answer to your question is in the gcode. I would bet dollars to donuts that the machine is being commanded to the exact same locations in both strategies. Hint: We have all been cutting pockets for years and years, so think like tens of thousands of pockets having been cut. If this were a software issue we would have all been talking about it long ago.
"If you see a good fight, get in it." Dr. Vernon Jones

ger21
Vectric Wizard
Posts: 1555
Joined: Sun Sep 16, 2007 2:59 pm
Model of CNC Machine: Custom DIY
Location: Shelby Township, MI, USA
Contact:

Re: pocket hole problem

Post by ger21 »

Is there a reason for this?
My guess would be machine deflection.
Gerry - http://www.thecncwoodworker.com

gareth52
Posts: 4
Joined: Thu Aug 08, 2019 3:21 pm
Model of CNC Machine: 3 axis home built cnc machine
Location: Anglesey , Wales

Re: pocket hole problem

Post by gareth52 »

Thanks for your replies. I measured the pockets with a pair of digital calipers. Like you, I’ve cut hundreds pockets, but I’ve never used the profile cut 1st option before. I’m using a 3 mm bit and it protrudes from the collet about three quarters of an inch.
Since you have both offered the possibility of deflection, I will try again using a shorter bit.

thanks again

User avatar
Adrian
Vectric Archimage
Posts: 10470
Joined: Thu Nov 23, 2006 2:19 pm
Model of CNC Machine: ShopBot PRS Alpha 96x48
Location: Surrey, UK

Re: pocket hole problem

Post by Adrian »

Thing to bear in mind is that if you're using the profile 1st option then there will be more load on the bit (more likelihood of deflection) as there is material on both sides of it. Cutting the profile last means less load because the "inside" material has already been removed.

User avatar
TReischl
Vectric Wizard
Posts: 3569
Joined: Thu Jan 18, 2007 6:04 pm
Model of CNC Machine: 8020 Build 48X36X10 RP 2010 Screenset
Location: Leland NC

Re: pocket hole problem

Post by TReischl »

Adrian wrote:Thing to bear in mind is that if you're using the profile 1st option then there will be more load on the bit (more likelihood of deflection) as there is material on both sides of it. Cutting the profile last means less load because the "inside" material has already been removed.
Hmmmm, Adrian. . . . There may be less load on the last pass option, but that load is all on one side with nothing on the opposite side to resist it. Obviously more of a problem with smaller bits.
"If you see a good fight, get in it." Dr. Vernon Jones

gareth52
Posts: 4
Joined: Thu Aug 08, 2019 3:21 pm
Model of CNC Machine: 3 axis home built cnc machine
Location: Anglesey , Wales

Re: pocket hole problem

Post by gareth52 »

After thinking about the 1st 2 answers last night, I had also thought that there was more chance of deflection using the profile can’t last option. This would force the bit inwards, creating a smaller pocket.
I’ll try again next week using a shorter bit and also a 0.25-inch bit.

sharkcutup
Vectric Wizard
Posts: 681
Joined: Sat Mar 26, 2016 3:48 pm
Model of CNC Machine: Shark HD3 Pro Extended Bed with Spindle
Contact:

Re: pocket hole problem

Post by sharkcutup »

Maybe feedrate being too fast causing unnecessary deflection!

Just an additional Thought!

Sharkcutup
Facebook: Hogan's CNC Crafts
www.hoganscnccrafts.com
V-Carve Pro 10.022

User avatar
TReischl
Vectric Wizard
Posts: 3569
Joined: Thu Jan 18, 2007 6:04 pm
Model of CNC Machine: 8020 Build 48X36X10 RP 2010 Screenset
Location: Leland NC

Re: pocket hole problem

Post by TReischl »

I'll try not to go into a long winded dissertation here but. . .

Sometimes I need to cut quite deep with a very small endmill, think .5 deep with a 1.5mm (.059) end mill to get good detail and crisp edges. I have found that if I make that cut after clearing out material I have all sorts of problems, deflection, bit breakage, etc. What does work is to make those cuts first. I use bits that have a very high spiral that helps pull the chips out and prevent packing. Also make sure the dust collector is running for the same reason. At the same time that technique helps prevent chipout at the surface by larger bits.
"If you see a good fight, get in it." Dr. Vernon Jones

gareth52
Posts: 4
Joined: Thu Aug 08, 2019 3:21 pm
Model of CNC Machine: 3 axis home built cnc machine
Location: Anglesey , Wales

Re: pocket hole problem

Post by gareth52 »

After some experimentation, I finally determined that using a shorter bit length, making the profile cut 1st and slowing the feed rate down to 50 in/min was the best way to go on my machine. It produced much better repeatable results.
Thanks for the help and advice you gave me.

Post Reply