How to cut a chamfer on a job

Post general information and questions relating to Cut2D in this Forum.

How to cut a chamfer on a job

Postby sterob » Sun Dec 30, 2018 12:56 pm

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
Attachments
Chamfer.JPG
Chamfer2.JPG
sterob
 
Posts: 18
Joined: Sun Jun 28, 2015 10:12 am
Location: Bunbury, Western Australia
Model of CNC Machine: X6-1500GT re-built with ESS and MB2

Re: How to cut a chamfer on a job

Postby ger21 » Sun Dec 30, 2018 2:30 pm

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
ger21
Vectric Wizard
 
Posts: 1473
Joined: Sun Sep 16, 2007 2:59 pm
Location: Shelby Township, MI, USA
Model of CNC Machine: Custom DIY

Re: How to cut a chamfer on a job

Postby sterob » Mon Dec 31, 2018 6:21 am

Thanks Ger21...as per the 2nd pic?
sterob
 
Posts: 18
Joined: Sun Jun 28, 2015 10:12 am
Location: Bunbury, Western Australia
Model of CNC Machine: X6-1500GT re-built with ESS and MB2

Re: How to cut a chamfer on a job

Postby ger21 » Mon Dec 31, 2018 1:38 pm

yes
Gerry - http://www.thecncwoodworker.com
ger21
Vectric Wizard
 
Posts: 1473
Joined: Sun Sep 16, 2007 2:59 pm
Location: Shelby Township, MI, USA
Model of CNC Machine: Custom DIY

Re: How to cut a chamfer on a job

Postby kstrauss » Tue Jan 01, 2019 7:59 pm

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.
kstrauss
Vectric Craftsman
 
Posts: 129
Joined: Mon Apr 29, 2013 3:37 am
Location: Cobourg, ON, Canada
Model of CNC Machine: Tormach PCNC770

Re: How to cut a chamfer on a job

Postby mtylerfl » Tue Jan 01, 2019 8:44 pm

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

carvebuddy.com

facebook.com/carvebuddy

-CarveWright CNC
-ShopBot Buddy PRSAlpha CNC
User avatar
mtylerfl
Vectric Wizard
 
Posts: 3941
Joined: Thu Jan 29, 2009 3:54 am
Location: Brunswick, GA
Model of CNC Machine: -CarveWright CNC -ShopBot Buddy PRSAlpha

Re: How to cut a chamfer on a job

Postby Martin Reid » Wed Jan 02, 2019 4:04 pm

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
Attachments
Chamfer.png
Chamfer
User avatar
Martin Reid
Vectric Apprentice
 
Posts: 90
Joined: Wed May 18, 2016 6:00 pm
Location: Lancashire UK
Model of CNC Machine: Shopbot

Re: How to cut a chamfer on a job

Postby sterob » Sun Jan 06, 2019 4:04 am

@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
Attachments
20180924_152909 (Small).jpg
Charging Guide Size.JPG
sterob
 
Posts: 18
Joined: Sun Jun 28, 2015 10:12 am
Location: Bunbury, Western Australia
Model of CNC Machine: X6-1500GT re-built with ESS and MB2

Re: How to cut a chamfer on a job

Postby LittleGreyMan » Sun Jan 06, 2019 11:51 am

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
Best regards

Didier

W7 - Aspire 8.517
LittleGreyMan
Vectric Apprentice
 
Posts: 918
Joined: Fri May 15, 2015 1:10 pm
Location: France
Model of CNC Machine: 3 axis small size machine

Re: How to cut a chamfer on a job

Postby sterob » Sun Jan 06, 2019 12:30 pm

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


Cut2D will do that?
Thanks, I will check it out and have a play.
sterob
 
Posts: 18
Joined: Sun Jun 28, 2015 10:12 am
Location: Bunbury, Western Australia
Model of CNC Machine: X6-1500GT re-built with ESS and MB2


Return to Cut2D - General

Who is online

Users browsing this forum: No registered users and 4 guests