Ballnose not cutting to depth
-
- Posts: 2
- Joined: Wed Feb 01, 2017 9:55 pm
- Model of CNC Machine: Camaster Stinger II
Ballnose not cutting to depth
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?
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?
- Leo
- Vectric Wizard
- Posts: 4092
- 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
How are you touching off the cutters?
Imagine the Possibilities of a Creative mind, combined with the functionality of CNC
-
- Posts: 2
- Joined: Wed Feb 01, 2017 9:55 pm
- Model of CNC Machine: Camaster Stinger II
Re: Ballnose not cutting to depth
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,
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,
- dwilli9013
- Vectric Wizard
- Posts: 1237
- 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
I would check the lengths of the bits in your tool holder. Is is possible maybe one slipped? Just a thought.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,
D-Dub
Dwayne
Dwilli
Dwayne
Dwilli
-
- Vectric Wizard
- Posts: 413
- 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
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?
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?
Connor Bredin
Distinctive Dimensional Concepts Ltd.
www.distinctive-concepts.ca
Distinctive Dimensional Concepts Ltd.
www.distinctive-concepts.ca
- SteveNelson46
- Vectric Wizard
- Posts: 2310
- Joined: Wed Jan 04, 2012 2:43 pm
- Model of CNC Machine: Camaster Stinger 1
- Location: Tucson, Az.
Re: Ballnose not cutting to depth
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
- adze_cnc
- Vectric Wizard
- Posts: 4380
- Joined: Sat Jul 27, 2013 10:08 pm
- Model of CNC Machine: AXYZ 4008
- Location: Vancouver, BC, Canada
Re: Ballnose not cutting to depth
I would suggest they are in error.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?
-
- Vectric Craftsman
- Posts: 164
- Joined: Wed Sep 28, 2016 4:51 pm
- Model of CNC Machine: Laguna MCNCIQ
Re: Ballnose not cutting to depth
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.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?
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.
-
- 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
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
Microsystems World CNC (WinCNC)
https://www.youtube.com/user/cncMike304
-
- Vectric Craftsman
- Posts: 240
- Joined: Sun May 15, 2011 4:19 pm
- Model of CNC Machine: Camaster Stinger II
Re: Ballnose not cutting to depth
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.
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.
- ChrisInEstes
- Vectric Wizard
- Posts: 841
- 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
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
Chris
Aspire 9.5 - FlexiEXPERT 11 - Vytek Rebel 4' x 8' - 5HP Perske Spindle
-
- Vectric Craftsman
- Posts: 298
- 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
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.
Try cutting outside the line and see what happens.
"Out of my mind. Back in 5 Minutes."