Odd arc error today

[crazy^millman]

I am doing some deburring of some clevis bores before they are finished machined. I am using a double angle cutter to put a .01 x 45 chamfer on both faces. I have programmed a standard contour toolpath. Nothing special just 2 chains for each clevis face. The back side on is adjusted the difference of the width of the chamfer mill. I am running through Vericut and it starts giving me bad arc warnings. I dig into it and sure enough there is a .0001" Arc difference. I tried many different filter settings and even no filter and nothing was making them match. I had to go into my operation and change the amount of stock to leave by .0002" and that was how I got the arc error resolved. Remember at the end of the day math doesn't lie and due to a rounding error I was getting this issue. It might have run on the machine with no issues, but glad I had a 2nd verification to tell me there was an issue the Backplot, Verify and Machiensim blesses as good when in reality is it not 100% correct. Everyday is a school day in this profession.

Front side Clevis with .0002" difference in stock to leave.

N100 G00 G90 G17 G20 G40 G80
N110 G53 Z0.
N120 G53 X-30. Y0.
(CHAMFER FRONT CLEVIS HOLE .01 X 45)
(MAXIMUM TOOL DEPTH - 4.)
(MINIMUM TOOL DEPTH - 1.57)
(T26    - 5/16 X 90 DOUBLE ANGLE - H18    - D18    - DIA .3125")
N130 T26 M06
N140 G00 G17 G90 G54
N150 S8000 M03
N160 M13 (C-AXIS UNLOCK)
N170 M11 (B-AXIS UNLOCK)
N180 B90. C-90.
N190 G254
N200 B90. C-90.
N210 M12 (C-AXIS LOCK)
N220 M10 (B-AXIS LOCK)
N230 X.0485 Y0.
N240 G43 H18 Z4.
N250 M08
N260 Z2.04
N270 G01 G94 Z2. F40.
N280 G41 D18 X-.1265
N290 G03 X-.1265 Y0. I.1265 J0.
N300 G01 G40 X.0485
N310 Z1.57
N320 G41 D18 X-.1265
N330 G03 X-.1265 Y0. I.1265 J0.
N340 G01 G40 X.0485
N350 G00 Z4.
N360 M09
N370 M05
N380 G255
N390 G53 Z0.
N400 G53 X-30. Y0.
N410 M13 (C-AXIS UNLOCK)
N420 M11 (B-AXIS UNLOCK)
N430 G91 G28 B0. C0.
N440 M12 (C-AXIS LOCK)
N450 M10 (B-AXIS LOCK)
N460 M30

Back side without the .0002" different in stock to leave

N100 G00 G90 G17 G20 G40 G80
N110 G53 Z0.
N120 G53 X-30. Y0.
(CHAMFER BACK CLEVIS HOLE .01 X 45)
(MAXIMUM TOOL DEPTH - 4.)
(MINIMUM TOOL DEPTH - 1.57)
(T26    - 5/16 X 90 DOUBLE ANGLE - H18    - D18    - DIA .3125")
N130 T26 M06
N140 G00 G17 G90 G54
N150 S8000 M03
N160 M13 (C-AXIS UNLOCK)
N170 M11 (B-AXIS UNLOCK)
N180 B90. C90.
N190 G254
N200 B90. C90.
N210 M12 (C-AXIS LOCK)
N220 M10 (B-AXIS LOCK)
N230 X.0483 Y0.
N240 G43 H18 Z4.
N250 M08
N260 Z2.04
N270 G01 G94 Z2. F40.
N280 G41 D18 X-.1267 <---->0001" Error
N290 G03 X-.1268 Y0. I.1268 J0. <---->.001" Error
N300 G01 G40 X.0483
N310 Z1.57
N320 G41 D18 X-.1267 <---->0001" Error
N330 G03 X-.1268 Y0. I.1268 J0. <---->0001" Error
N340 G01 G40 X.0483
N350 G00 Z4.
N360 M09
N370 M05
N380 G255
N390 G53 Z0.
N400 G53 X-30. Y0.
N410 M13 (C-AXIS UNLOCK)
N420 M11 (B-AXIS UNLOCK)
N430 G91 G28 B0. C0.
N440 M12 (C-AXIS LOCK)
N450 M10 (B-AXIS LOCK)
N460 M30

Here is a different section of the part where I am deburring different clevis bores.

Here is the tool being used for reference. I define it as a slot mill and add the shank of the tool to the holder since we cannot correctly define these tools in Mastercam. Defining it in the holder is the workaround.

Double Angle Shank Cutters - Pointed, Specialty Profiles

 

[jpatry]

I use these Harvey DA chamfermills all the time.

15 hours ago, crazy^millman said:

I define it as a slot mill and add the shank of the tool to the holder since we cannot correctly define these tools in Mastercam. Defining it in the holder is the workaround.

Here's what I do for all double chamfermills, I define them as a chamfermill with the length of cut from the tip to the point of largest diameter.

Then in the toolpath I use the chamfer variant of Contour, I set offset type to top with a value of zero, and a chamfer width of zero, then I if I am cutting a chamfer with the front of the tool I set +.02 for floor stock to leave and -.025 for wall stock to leave.

If I am cutting a chamfer with the back of the tool the only difference is I set -.02 for floor stock to leave and -.025 for wall stock to leave.

One further recommendation for anyone doing this is to use entry point chaining to drop cleanly through the hole before making the backside cut.

 

Only downside is I need two separate toolpaths, on for all the fronts, and one for all the rears.

[Leon82]

i get these with circlemill sometimes mostly with 10mm holes. never found a solution. i usually draw a new hole a little bit different size.

[crazy^millman]

5 hours ago, jpatry said:

I use these Harvey DA chamfermills all the time.

Here's what I do for all double chamfermills, I define them as a chamfermill with the length of cut from the tip to the point of largest diameter.

Then in the toolpath I use the chamfer variant of Contour, I set offset type to top with a value of zero, and a chamfer width of zero, then I if I am cutting a chamfer with the front of the tool I set +.02 for floor stock to leave and -.025 for wall stock to leave.

If I am cutting a chamfer with the back of the tool the only difference is I set -.02 for floor stock to leave and -.025 for wall stock to leave.

One further recommendation for anyone doing this is to use entry point chaining to drop cleanly through the hole before making the backside cut.

 

Only downside is I need two separate toolpaths, on for all the fronts, and one for all the rears.

That is one toolpath for 4 different clevis tabs with 8 different chains. I offset the chains the difference and then can drive everything with wireframe and not have more than one operation.

2 hours ago, Leon82 said:

i get these with circlemill sometimes mostly with 10mm holes. never found a solution. i usually draw a new hole a little bit different size.

Adjust the diameter manually .0001 to .0002 and then repost.

[crazy^millman]

I got an answer to this and it has proven to be very helpful. Go into the MCD of your machine and turn the NC precision down to either 5 or 6 places in inch and 4 to 5 places in Metric. The defaults are 4 and 3 places. This fixed 10 different issues I was running into over the last 2 weeks.

[Leon82]

9 hours ago, crazy^millman said:

I got an answer to this and it has proven to be very helpful. Go into the MCD of your machine and turn the NC precision down to either 5 or 6 places in inch and 4 to 5 places in Metric. The defaults are 4 and 3 places. This fixed 10 different issues I was running into over the last 2 weeks.

I did that for the yasda we have it was cutting a line on an angle before it did it

[crazy^millman]

On 9/16/2023 at 6:53 PM, Leon82 said:

I did that for the yasda we have it was cutting a line on an angle before it did it

Yasda would get 8 places and output all the NC code in 6 places for running on the machine if it were mine.