Community
Fusion Manufacture
Talk shop with the Fusion (formerly Fusion 360) Manufacture Community. Share tool strategies, tips, get advice and solve problems together with the best minds in the industry.
cancel
Showing results for 
Show  only  | Search instead for 
Did you mean: 

2d contour chamfer issues

2 REPLIES 2
Reply
Message 1 of 3
mmharris
154 Views, 2 Replies

2d contour chamfer issues

should be simple but isn't

 

the goal is a .030 chamfer around a simple part using 2d contour

 

tip offset is .15 to get good surface footage 

in the attached pic of simulation the Gcode has the tip at -.18 ( tip offset+ chamfer ?) or 

which MIGHT be tip offset from bottom of chamfer  or ?

 

but clearly is not like the illustration if you hover over CHAMFER TIP OFFSET while editing the toolpath

until the window pops up

the drawing clearly shows tip offset from top of chamfer

 

the BIGGEST PROBLEM is the actual chamfer on the cut part in the machine is WAY bigger than .030

the simulation looks like a .030 chamfer with the tip at -.180 but the real part might have a .070 + chamfer

 

anybody know what is going on?

and how to program the size of the chamfer?

 

thanks

mark

 

 

 

 

 

 

here's a link to a test file 

https://a360.co/3MwzQCf

2 REPLIES 2
Message 2 of 3
engineguy
in reply to: mmharris

@mmharris 

 

The G Code looks to be correct according to your settings, a 0.03 Chamfer plus a tip offset of 0.15 does give a Z-0.18 which is correct as measured from the top of the part, likewise a 0.015 chamfer plus a tip offset of 0.1 gives a Z-0.115, again correct.

 

So, if the code is correct then it must be something at the CNC that is not correct, for example, in Fusion you have the Chamfer tool with an exact point, most chamfer tools have either a small flat or radius, not a perfect point, if your tool is like that then when you set the tool at the CNC it will certainly cut deeper than you expect so you get too large a Chamfer. Right now I can`t see anything that would cause the CNC to cut too deep in the code.

Below is the G Code generated here and there is nowhere in the code where the tool is programmed to go deeper than your settings 🙂

%
O1001
(T20 D=0.375 CR=0. TAPER=45DEG - ZMIN=-0.18 - CHAMFER MILL)
N1 G90 G94 G17
N2 G20
N3 G28 G91 Z0.
N4 G90

(2D CONTOUR1)
N5 T20 M6
N6 S2800 M3
N7 G4 P64
N8 M8
N9 G0 E1 X-0.54 Y-1.16
N10 G43 Z2.4 H20
N11 Z0.1
N12 G1 Z0.0394 F30.
N13 Z-0.015
N14 G18 G2 X-0.44 Z-0.115 I0.1 F15.
N15 G1 X0.06
N16 G17 G3 X0. Y-1.1 I-0.06
N17 G2 X-0.1 Y-1. J0.1 F25.
N18 G1 Y0.
N19 G2 X0. Y0.1 I0.1
N20 G1 X1.
N21 G2 X1.1 Y0. J-0.1
N22 G1 Y-1.
N23 G2 X1. Y-1.1 I-0.1
N24 G1 X0.
N25 G3 X-0.06 Y-1.16 J-0.06 F15.
N26 G1 X0.44
N27 G18 G2 X0.54 Z-0.015 K0.1
N28 G0 Z2.4
N29 G17

(2D CONTOUR1 (2))
N30 G1 X-0.54 Y-1.21 F100.
N31 G0 Z2.4
N32 Z0.1
N33 G1 Z0.0394 F30.
N34 Z-0.08
N35 G18 G2 X-0.44 Z-0.18 I0.1 F15.
N36 G1 X0.06
N37 G17 G3 X0. Y-1.15 I-0.06
N38 G2 X-0.15 Y-1. J0.15 F25.
N39 G1 Y0.
N40 G2 X0. Y0.15 I0.15
N41 G1 X1.
N42 G2 X1.15 Y0. J-0.15
N43 G1 Y-1.
N44 G2 X1. Y-1.15 I-0.15
N45 G1 X0.
N46 G3 X-0.06 Y-1.21 J-0.06 F15.
N47 G1 X0.44
N48 G18 G2 X0.54 Z-0.08 K0.1
N49 G0 Z2.4
N50 G17

N51 M9
N52 G28 G91 Z0.
N53 G90
N54 G0
N55 G53 X0. Y0.
N56 M30
%

 

Message 3 of 3
mmharris
in reply to: mmharris

Thank you

I guess the point of the cutter dragging due to the tip offset being from the bottom edge of the chamfer. 

 

Can't find what you're looking for? Ask the community or share your knowledge.

Post to forums