Ballnose not cutting to depth

Post Reply
nickgless@gmail.com
Posts: 2
Joined: Wed Feb 01, 2017 9:55 pm
Model of CNC Machine: Camaster Stinger II

Ballnose not cutting to depth

Post by nickgless@gmail.com »

Yesterday we experienced a challenge when cutting a pocket using the pocket toolpath using a larger area clearance tool (.5 endmill) along with a .5 ballnose to finish with a radius in the inside corner. The ballnose is not cutting to the specified depth. The endmill (clearing tool) cuts to correct depth. Aspire 8.514, WinCNC

I will try to attach photos of the setup and resulting cut.

This morning we did some testing to try and isolate the cause for the issue:

same file, same board, no clearing cut

Cut 4 pockets 1.25" in diameter at .3 deep (Z at bottom of material)
.25 endmill cut to .3
.25 ballnose cut to .28
.5 endmill cut to .3
.5 ballnose cut to .25


Repeated the test using same file and parameters cutting with the Z at the top of the material:
.5 endmill cut to .3
.5 ballnose cut to .27

Any ideas on cause/resolution?

**It has been suggested in another forum that Aspire Pocket Toolpath with large area clearing tool is only for flat cutters and cannot work with a ballnose. Is this true?
Attachments
Toolpath settings
Toolpath settings
Resulting cut
Resulting cut

User avatar
Leo
Vectric Wizard
Posts: 3101
Joined: Sat Jul 14, 2007 3:02 am
Model of CNC Machine: 1300 x 1300 x 254 Chinese Made
Location: East Freetown, Ma.
Contact:

Re: Ballnose not cutting to depth

Post by Leo »

How are you touching off the cutters?
Imagine the Possibilities of a Creative mind

www.leosworkshop.com

nickgless@gmail.com
Posts: 2
Joined: Wed Feb 01, 2017 9:55 pm
Model of CNC Machine: Camaster Stinger II

Re: Ballnose not cutting to depth

Post by nickgless@gmail.com »

Leo,
We are using the fast tool change on our Camaster. We just spoke with Vectric support and they verified our g-code is correct, so it looks like the next step is to contact Camaster.

Thanks,

User avatar
dwilli9013
Vectric Wizard
Posts: 1232
Joined: Mon Sep 30, 2013 12:45 am
Model of CNC Machine: 3 axis Self Designed Self Built
Location: Machesney Park Illinois

Re: Ballnose not cutting to depth

Post by dwilli9013 »

nickgless@gmail.com wrote:Leo,
We are using the fast tool change on our Camaster. We just spoke with Vectric support and they verified our g-code is correct, so it looks like the next step is to contact Camaster.

Thanks,
I would check the lengths of the bits in your tool holder. Is is possible maybe one slipped? Just a thought.
D-Dub
Dwayne
Dwilli

Mobius
Vectric Wizard
Posts: 408
Joined: Wed Jul 09, 2014 1:19 am
Model of CNC Machine: CRP Pro 4848 Custom Build
Location: Drumheller, Alberta, Canada
Contact:

Re: Ballnose not cutting to depth

Post by Mobius »

It is hard to judge scale from the picture, but where does the center line of the ballnose bit end up with regards to the lip you see in the picture? It should be dead center on the edge of the end mill cut, otherwise the cut will start to move up the radius of the ballnose and create a lip.

Something like the picture? Have you tried offsetting the cut inwards? Or is the opposite true? Is the center line of the cut too far inboard?
Attachments
ballnose.jpg
Connor Bredin
Distinctive Dimensional Concepts Ltd.
www.distinctive-concepts.ca

SteveNelson46
Vectric Wizard
Posts: 909
Joined: Wed Jan 04, 2012 2:43 pm
Model of CNC Machine: Camaster Stinger using WinCNC
Location: Tucson, Az.

Re: Ballnose not cutting to depth

Post by SteveNelson46 »

I have never worked with a tool changer so I'm kind of stabbing in the dark. Is it possible to swap the position of the bits in the changer to see if the problem is the changer? Of course you would have to change the tool number position in the tool setup also.
Steve

User avatar
adze_cnc
Vectric Apprentice
Posts: 981
Joined: Sat Jul 27, 2013 10:08 pm
Model of CNC Machine: AXYZ 4008
Location: Vancouver, BC, Canada

Re: Ballnose not cutting to depth

Post by adze_cnc »

nickgless@gmail.com wrote:It has been suggested in another forum that Aspire Pocket Toolpath with large area clearing tool is only for flat cutters and cannot work with a ballnose. Is this true?
I would suggest they are in error.

Olle
Vectric Craftsman
Posts: 151
Joined: Wed Sep 28, 2016 4:51 pm
Model of CNC Machine: Laguna MCNCIQ

Re: Ballnose not cutting to depth

Post by Olle »

Mobius wrote:It is hard to judge scale from the picture, but where does the center line of the ballnose bit end up with regards to the lip you see in the picture? It should be dead center on the edge of the end mill cut, otherwise the cut will start to move up the radius of the ballnose and create a lip.

Something like the picture? Have you tried offsetting the cut inwards? Or is the opposite true? Is the center line of the cut too far inboard?
That's what I was thinking when I saw this: It may be cutting to the right depth, but a bit offset. There is no reason for the cut depth to change just because you change tools, unless you're using a quick change system that's not properly set up and don't zero between the tool changes.

I have run into similar problems, and it's almost always turns out being me screwing up by specifying an offset somewhere, picking the wrong vector etc. Like you said, I would go back to the drawing board and make sure that the center of the cut is located at the edge of the end mill cut before doing anything else.

BTW: I have a cheap depth gauge I use to verify depths and trouble shoot problems like this: http://www.ebay.com/itm/SHARS-0-4-Elect ... xykmZTK0Qc . It's a very handy tool when you run into problems with multiple cuts, or when you need to verify cut depths in general. If you have one of those, run the ball nose cut only and check the depth, then run the end mill cut and check again.

M Queen
Vectric Apprentice
Posts: 86
Joined: Tue Jul 29, 2014 9:25 pm
Model of CNC Machine: WinCNC Hybrid
Location: Buckhannon, WV, USA
Contact:

Re: Ballnose not cutting to depth

Post by M Queen »

Fast tool change isn't really a tool changer. With this method, it allows the user to output files using a tool changer setup (multiple tools in the same file). When one toolpath finishes, the machine moves to a set location and prompts the user to put in the next tool. Once the user changes out the tool and hits Enter, it moves to a touch off switch or measuring pad, measures the tool, and continues with the file (sets a spindle speed, starts the spindle, and sets a feedrate just like a tool changer). It is quicker than creating and loading multiple files to do the same job.
Mike Queen
Microsystems World CNC (WinCNC)
https://www.youtube.com/user/cncMike304

Pete Cyr
Vectric Craftsman
Posts: 199
Joined: Sun May 15, 2011 4:19 pm
Model of CNC Machine: Camaster Stinger II

Re: Ballnose not cutting to depth

Post by Pete Cyr »

Are you sure you spindle is trammed ? (the axis of the spindle must be perpendicular to the table in the X and Y axis)
If it is off axis I could see a flat end mill and a ball end mill measuring differently on the FTC. I would not expect to see as large a difference in the depth of cut you listed but I would expect to see the different profile measuring differently.

User avatar
ChrisInEstes
Vectric Wizard
Posts: 835
Joined: Fri Jul 17, 2009 8:00 pm
Model of CNC Machine: Vytek 4' X 8' - Perske Spindle - Mach3
Location: Estes Park, Colorado, USA

Re: Ballnose not cutting to depth

Post by ChrisInEstes »

I saw the OP's post on a Vectric related Facebook group asking about the same issue, & I believe they found their issue to be a loose Z axis coupler nut.

Chris
Aspire 9.5 - FlexiEXPERT 11 - Vytek Rebel 4' x 8' - 5HP Perske Spindle

nicksilva
Vectric Craftsman
Posts: 295
Joined: Thu Aug 21, 2014 8:13 pm
Model of CNC Machine: ULS M300, Rockler 60th Ann. Shark
Location: Dallas, TX USA
Contact:

Re: Ballnose not cutting to depth

Post by nicksilva »

when cutting a vector you get to choose whether to run ON the light or INSIDE or OUTSIDE. Since a ball nose curves rather than cut on a flat that could be affecting the cut.
Try cutting outside the line and see what happens.
"Out of my mind. Back in 5 Minutes."

Post Reply