I need to cut out a small object out of plastic and I need a chamfer on the bottom of it.
No problem...I can cut it upside down and cut the chamfer first.
My question is what is the best way to position the 90° tool in order to cut eh chamfer. ( Chamfer is 45° )
My first thought was to just use the outer edge of the job as the centre of the tool and make incemental cuts dwn until teh correct sized chamfer was cut.
Would this work or is there a better way?
If I move the tool outwards and down, I would have to draw a perimeter around the job for the tool to follow.....?
Steve
How to cut a chamfer on a job
-
- Vectric Wizard
- Posts: 1592
- Joined: Sun Sep 16, 2007 2:59 pm
- Model of CNC Machine: Custom DIY
- Location: Lake St Clair, MI, USA
- Contact:
Re: How to cut a chamfer on a job
My preference would be to offset the vector outward by 1/8", then cut a profile, on the line, with the depth being 1/8 + chamfer width.
Gerry - http://www.thecncwoodworker.com
-
- Posts: 18
- Joined: Sun Jun 28, 2015 10:12 am
- Model of CNC Machine: X6-1500GT re-built with ESS and MB2
- Location: Bunbury, Western Australia
Re: How to cut a chamfer on a job
Thanks Ger21...as per the 2nd pic?
-
- Vectric Craftsman
- Posts: 277
- Joined: Mon Apr 29, 2013 3:37 am
- Model of CNC Machine: Tormach PCNC770
- Location: Cobourg, ON, Canada
Re: How to cut a chamfer on a job
An easy way (rather than creating an offset path for every edge to be chamfered) is to setup the chamfer tool as having a smaller diameter than it actually is. For example, if you are using a 1/4-inch chamfer tool define it in your tool database as being 3/16 in diameter.
- mtylerfl
- Vectric Archimage
- Posts: 5896
- Joined: Thu Jan 29, 2009 3:54 am
- Model of CNC Machine: -CarveWright CNC -ShopBot Buddy PRSAlpha
- Location: Brunswick, GA
Re: How to cut a chamfer on a job
Interesting alternative. Personally, I wouldn’t recommend that method - too much room for confusion. Better to layout the project correctly and keep the Tool Database specs matching actual bits used.
Michael Tyler
facebook.com/carvebuddy
-CarveWright CNC
-ShopBot Buddy PRSAlpha CNC
facebook.com/carvebuddy
-CarveWright CNC
-ShopBot Buddy PRSAlpha CNC
- Martin Reid
- Vectric Apprentice
- Posts: 93
- Joined: Wed May 18, 2016 6:00 pm
- Model of CNC Machine: Shopbot
- Location: Lancashire UK
- Contact:
Re: How to cut a chamfer on a job
Dear Steve
My two penn’orth is on option 2.
If the pieces are quite big then I may do the 'chamfer' after doing the profile cut - I get a really good finish and there is less work on the cutter as most of it is in the gap created with the profile cutter. If the pieces are small then I will do the chamfer before the profile cut so the pieces don't move. Also if there is some vCarving then I will do the chamfer while the cutter is in.
Doing the profile cut after doing a chamfer on the line (option 1) always leaves a quirk or raised arris that needs sanding.
Sincerely and in good faith
Martin
My two penn’orth is on option 2.
If the pieces are quite big then I may do the 'chamfer' after doing the profile cut - I get a really good finish and there is less work on the cutter as most of it is in the gap created with the profile cutter. If the pieces are small then I will do the chamfer before the profile cut so the pieces don't move. Also if there is some vCarving then I will do the chamfer while the cutter is in.
Doing the profile cut after doing a chamfer on the line (option 1) always leaves a quirk or raised arris that needs sanding.
Sincerely and in good faith
Martin
-
- Posts: 18
- Joined: Sun Jun 28, 2015 10:12 am
- Model of CNC Machine: X6-1500GT re-built with ESS and MB2
- Location: Bunbury, Western Australia
Re: How to cut a chamfer on a job
@Martin
The job is quite small, so I think it would be easier to do the chamfer before the profile cut, as you say.
No VCarving. The job is a guide and a support for a charging connector, so it doesn't damage the device.
I suspected chamfering 'on the line' would leave some sort of artifact behind, but not a real problem.
I think offsetting the tool has too many avenues for math errors ( ok if I was doing lots but I only need to cut one )
The chamfer is only to allow the max surface area for gluing the guide in place.
Steve
The job is quite small, so I think it would be easier to do the chamfer before the profile cut, as you say.
No VCarving. The job is a guide and a support for a charging connector, so it doesn't damage the device.
I suspected chamfering 'on the line' would leave some sort of artifact behind, but not a real problem.
I think offsetting the tool has too many avenues for math errors ( ok if I was doing lots but I only need to cut one )
The chamfer is only to allow the max surface area for gluing the guide in place.
Steve
-
- Vectric Wizard
- Posts: 1013
- Joined: Fri May 15, 2015 1:10 pm
- Model of CNC Machine: 3 axis small size machine
- Location: France
Re: How to cut a chamfer on a job
Steve,
To avoid cutting on the vector (your first drawing in your initial post), which does not give the best cutting condition (the linear cutting speed of the tip is 0), with a 90° V-Bit set these parameters for the 2D profile toolpath:
-machine vectors Outside/ right (or inside / left for an internal chamfer, not tested)
-set the allowance offset to - chamfer value. For example, for a 2mm chamfer (top view), set the allowance to -2
-set the cut depth to a value > chamfer value
The software will set the depth cut and the offset of the tooltip in order to get these values and cut as in your 2nd drawing. No need to do any math.
Tested on Aspire trial 9.5
To avoid cutting on the vector (your first drawing in your initial post), which does not give the best cutting condition (the linear cutting speed of the tip is 0), with a 90° V-Bit set these parameters for the 2D profile toolpath:
-machine vectors Outside/ right (or inside / left for an internal chamfer, not tested)
-set the allowance offset to - chamfer value. For example, for a 2mm chamfer (top view), set the allowance to -2
-set the cut depth to a value > chamfer value
The software will set the depth cut and the offset of the tooltip in order to get these values and cut as in your 2nd drawing. No need to do any math.
Tested on Aspire trial 9.5
Best regards
Didier
W7 - Aspire 8.517
Didier
W7 - Aspire 8.517
-
- Posts: 18
- Joined: Sun Jun 28, 2015 10:12 am
- Model of CNC Machine: X6-1500GT re-built with ESS and MB2
- Location: Bunbury, Western Australia
Re: How to cut a chamfer on a job
Cut2D will do that?LittleGreyMan wrote:Steve,
To avoid cutting on the vector (your first drawing in your initial post), which does not give the best cutting condition (the linear cutting speed of the tip is 0), with a 90° V-Bit set these parameters for the 2D profile toolpath:
-machine vectors Outside/ right (or inside / left for an internal chamfer, not tested)
-set the allowance offset to - chamfer value. For example, for a 2mm chamfer (top view), set the allowance to -2
-set the cut depth to a value > chamfer value
The software will set the depth cut and the offset of the tooltip in order to get these values and cut as in your 2nd drawing. No need to do any math.
Tested on Aspire trial 9.5
Thanks, I will check it out and have a play.