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: 

Milled Chamfer larger than expected

4 REPLIES 4
Reply
Message 1 of 5
DS_P
266 Views, 4 Replies

Milled Chamfer larger than expected

Hey,

 

I've setup to mill a chamfer that I want to be 0.2mm width (0.28mm across hypotenuse see cad file below).  It is as machined dimension coming out much wider, about ~1.2mm and I have no clue why.

 

I've checked everything I can think of, any suggestions for further checks?   I feel like its something wrong with how fusion is posting wear comp, because the path looks different if you post In Computer vs Wear but I cant quite place my finger on it (maybe a red herring).  It looks like it takes the 0.3mm compensation allowance and adds it to the lead in radius of 0.6 =0.9mm on the G01 G41 line, but maybe the control doesn't like something about how this is posted?? 

 

This happened on another part as well, similar checks to no avail.

 

 

Things I've checked:

1. G54 position and height in machine matches fusion

2. Tool height H01 of T1 (6mm 90deg spot drill) in control was correct.

3. Tool diameter matches program =6mm

4. Tool tip angle matches program = 90deg

5. Tool wear comp setting (currently set to 0mm in the control so should cut undersized if anything)

6. Boss height and diameter from previous operations is correct

7. Programmed cut diameter matches expected tip offset and cut width (e.g at Z - 1.2mm the tip should travel around an 8.25mm arc, e.g.  G02 Y-8.25 J-8.25; Y8.25 J8.25)

 

Machine details

Chevalier FTC1320V with Fanuc OI-MC

 

IMG20240331125851.jpg

IMG20240331130159.jpg

IMG20240331125743.jpg

   

 

 

 

 


(2D CONTOUR2 - Wear comp - as machined)
M09
M01
G91 G28 Z0.
G28 X0. Y0.
G90
N15 T1 M06
T12
S12000 M03
G17 G90 G94
G54
M08
G5.1 Q1 R7
G00 X-0.6 Y10.35
G43 Z15. H01
G00 Z5.
G01 Z1. F600.
Z-0.6
G19 G02 Y9.75 Z-1.2 J-0.6 F1800.
G17
G01 G41 X-0.9 Y9.15 D01
G03 X0. Y8.25 I0.9
G02 Y-8.25 J-8.25
Y8.25 J8.25
G03 X0.9 Y9.15 J0.9
G01 G40 X0.6 Y9.75
G19 G03 Y10.35 Z-0.6 K0.6
G00 Z15.
G17

 

 

(2D CONTOUR2 CONTROL COMP for comparison)
M01
G91 G28 Z0.
G28 X0. Y0.
G90
N10 T1 M06
S12000 M03
G17 G90 G94
G54
M08
G5.1 Q1 R7
G00 X-0.6 Y10.05
G43 Z15. H01
G00 Z5.
G01 Z1. F600.
Z-0.6
G19 G02 Y9.45 Z-1.2 J-0.6 F1800.
G01 Y8.85
G17 G03 X0. Y8.25 I0.6
G02 Y-8.25 J-8.25
Y8.25 J8.25
G03 X0.6 Y8.85 J0.6
G01 Y9.45
G19 G03 Y10.05 Z-0.6 K0.6
G00 Z15.
G17

 

danielsethpearl_0-1711843252569.png

 

danielsethpearl_1-1711843935077.png

 

danielsethpearl_2-1711845040595.png

 

danielsethpearl_3-1711845084868.png

 

 

 

 

Labels (3)
4 REPLIES 4
Message 2 of 5
a.laasW8M6T
in reply to: DS_P

The posted code looks fine to me

 

Just to check, you say the  wear value is 0 for that tool but you also need to have the D value at 0 to correctly use the wear comp mode.

 

Also looks like you are using a Spot drill, does the spot drill actually come to a sharp point? or is there a small flat at the end(this can be hard to tell on a spot drill)

Message 3 of 5
DS_P
in reply to: a.laasW8M6T

Thanks, yeah I do have a bit of a flat. Its quite possible thats whats
causing it. Dont have a good way to measure it (or the chamfers for that
matter) but maybe almost a mm flat by eyeball.

Did a quick sketch in CAD and its possibly enough to cause that issue.
Message 4 of 5
a.laasW8M6T
in reply to: DS_P

one thing you can do as a bit of a sanity check is.

 

position your 6mm tool directly above an edge, where the top of that edge is Z0, and the edge is say Y0, then jog across and down -3mm, the intersection of the 90° cone and the 6mm diameter should be aligned with the edge.

 

if this isn't the case then the tool geometry isn't going to a sharp theoretical point.

 

Message 5 of 5
programming2C78B
in reply to: DS_P

How I "calibrate" the tip is program it to go down -.05" then measure the diameter of the hole it makes. Let

say its .125"

Then in fusion, modify the tool tip to where when you program it to spot to a chamfer diameter of .125, the Z depth is .05". Since it's 90*, you can guess it'd be a .012" flat or so.

It's always safer to say the flat is bigger then it is in reality. 

Please click "Accept Solution" if what I wrote solved your issue!

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

Post to forums  

Autodesk Design & Make Report