Page 1 of 1

How to cut a chamfer on a job

PostPosted: Sun Dec 30, 2018 12:56 pm
by sterob
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

Re: How to cut a chamfer on a job

PostPosted: Sun Dec 30, 2018 2:30 pm
by ger21
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.

Re: How to cut a chamfer on a job

PostPosted: Mon Dec 31, 2018 6:21 am
by sterob
Thanks Ger21...as per the 2nd pic?

Re: How to cut a chamfer on a job

PostPosted: Mon Dec 31, 2018 1:38 pm
by ger21
yes

Re: How to cut a chamfer on a job

PostPosted: Tue Jan 01, 2019 7:59 pm
by kstrauss
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.

Re: How to cut a chamfer on a job

PostPosted: Tue Jan 01, 2019 8:44 pm
by mtylerfl
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.

Re: How to cut a chamfer on a job

PostPosted: Wed Jan 02, 2019 4:04 pm
by Martin Reid
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

Re: How to cut a chamfer on a job

PostPosted: Sun Jan 06, 2019 4:04 am
by sterob
@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

Re: How to cut a chamfer on a job

PostPosted: Sun Jan 06, 2019 11:51 am
by LittleGreyMan
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

Re: How to cut a chamfer on a job

PostPosted: Sun Jan 06, 2019 12:30 pm
by sterob
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.